Abaqus Example Problems Manual

bottom,3, *output,field *node output u, *node file,global=yes u, *end step

1-377

Static Stress/Displacement Analyses

Listing 1.2.6-3 *heading Input file for the postbuckling analysis. *parameter # # filenames # buckle_file = 'file1.dat' imperf_file = 'file2.dat' # # workaround to allow parametrization of a # filename read with *INCLUDE # line1 = '*include, input='+imperf_file # # geometric/load parameters # radius = 5.0 length = 2.0 thickness = 0.01 # # this is the pcritical for the 1st value from # the linear eigenvalue analysis # eig1_load = 1.18305e+4 # # elastic material properties # young = 30e+06 poisson=0.3 # # internal pressure # int_press = 0.0 # # mesh parameters # node_circum = 240 node_length = 21 ## ## dependent parameters (do not modify) ##

1-378

Static Stress/Displacement Analyses

chn = node_circum*node_length-node_circum node_ang = -360.0/float(node_circum) node_tot = node_circum*node_length node_tmp = node_tot-node_circum+1 node_int = node_length-1 node_circum1 = node_circum+1 node_circum2 = node_circum+2 node_circum0 = node_circum-1 e1 = node_circum*2 p = -eig1_load/float(node_circum) pn = eig1_load/float(node_circum) # # end of parameter list # *node,system=c 1,,0.0,0.0 ,,,0.0 ,,0.0, ,,, *ngen,line=c,nset=bottom 1,,1,,0.0,0.0,0.0,0.0,0.0,1.0 *ncopy,new set=top,old set=bottom,shift,change number= 0.0,0.0, 0.0,0.0,0.0,0.0,0.0,1.0,0.0 *nfill bottom,top,, **specify the imperfection as a function of modeshape amplitude *imperfection,file=,step=2 *element,type=s4 1,1,2,, ,,1,, *elgen,elset=cylinder 1,,1,1,,, ,1,,,,, *shell section, elset=cylinder, material=mat_1 , *material,name=mat_1 *elastic , *nset,nset=ends bottom,top *transform,type=c,nset=ends

1-379

Static Stress/Displacement Analyses

0.0,0.0,0.0,0.0,0.0,1.0 *boundary ends,1,2 ends,4,4 ends,6,6 1,3 ** *step,nlgeom,inc=10 static preload for internal pressure *static 1.0,1.0 *monitor,node=, dof=3 *dload cylinder,p, *end step ** *step,nlgeom,inc=60 postbuckling (riks) analysis *static,riks 0.05,1.0,,0.05,,,3,-0.1 *monitor,node=,dof=3 *controls,parameter=field,field=global 1.e-5, *cload top,3,

bottom,3, *node file,freq=1,nset=top u,cf *output,field,variable=preselect,freq=10 *output,history,freq=1 *node output,nset=top u,cf *end step

1.3 Forming analyses 1.3.1 Upsetting of a cylindrical billet in ABAQUS/Standard: quasi-static analysis with rezoning Product: ABAQUS/Standard This example illustrates the use of the rezoning capabilities of ABAQUS/Standard in a metal forming application. The same problem is analyzed using the coupled temperature-displacement elements in

1-380

Static Stress/Displacement Analyses

``Upsetting of a cylindrical billet: coupled temperature-displacement and adiabatic analysis, '' Section 1.3.17. Coupled temperature-displacement elements are included in this example only for rezoning verification purposes; no heat generation occurs in these elements for this example. The same test case is done with ABAQUS/Explicit in ``Upsetting of a cylindrical billet in ABAQUS/Explicit,'' Section 1.3.2. When the strains become large in geometrically nonlinear analysis, the elements often become so severely distorted that they no longer provide a good discretization of the problem. When this occurs, it is necessary to "rezone": to map the solution onto a new mesh that is better designed to continue the analysis. The procedure is to monitor the distortion of the mesh--for example, by observing deformed configuration plots--and decide when the mesh needs to be rezoned. At that point a new mesh must be generated using the mesh generation options in ABAQUS or some external mesh generator. The results file output is useful in this context since the current geometry of the model can be extracted from the data in the results file. Once a new mesh is defined, the analysis is continued by beginning a new problem using the solution from the old mesh at the point of rezoning as initial conditions. This is done by including the *MAP SOLUTION option and specifying the step number and increment number at which the solution should be read from the previous analysis. ABAQUS interpolates the solution from the old mesh onto the new mesh to begin the new problem. This technique provides considerable generality. For example, the new mesh might be more dense in regions of high-strain gradients and have fewer elements in regions that are distorting rigidly--there is no restriction that the number of elements be the same or that element types agree between the old and new meshes. In a typical practical analysis of a manufacturing process, rezoning may have to be done several times because of the large shape changes associated with such a process. The interpolation technique used in rezoning is a two-step process. First, values of all solution variables are obtained at the nodes of the old mesh. This is done by extrapolation of the values from the integration points to the nodes of each element and averaging those values over all elements abutting each node. The second step is to locate each integration point in the new mesh with respect to the old mesh (this assumes all integration points in the new mesh lie within the bounds of the old mesh: warning messages are issued if this is not so, and new model solution variables at the integration point are set to zero). The variables are then interpolated from the nodes of the element in the old mesh to the location in the new mesh. All solution variables are interpolated automatically in this way so that the solution can proceed on the new mesh. Whenever a model is rezoned, it can be expected that there will be some discontinuity in the solution because of the change in the mesh. If the discontinuity is significant, it is an indication that the meshes are too coarse or that the rezoning should have been done at an earlier stage before too much distortion occurred.

Geometry and model The geometry is the standard test case of Lippmann (1979) and is defined in ``Upsetting of a cylindrical billet: coupled temperature-displacement and adiabatic analysis, '' Section 1.3.17. It is a circular billet, 30 mm long, with a radius of 10 mm, compressed between two flat, rigid dies that are defined to be perfectly rough.

1-381

Static Stress/Displacement Analyses

The mesh used to begin the analysis is shown in Figure 1.3.1-1. The finite element model is axisymmetric and includes the top half of the billet only since the middle surface of the billet is a plane of symmetry. Element type CAX4R is used: this is a 4-node quadrilateral with a single integration point and "hourglass control" to control spurious mechanisms caused by the fully reduced integration. The element is chosen here because it is relatively inexpensive for problems involving nonlinear constitutive behavior since the material calculations are only done at one point in each element. The contact between the top and lateral exterior surfaces of the billet and the rigid die is modeled with the *CONTACT PAIR option. The billet surface is defined by means of the *SURFACE option. The rigid die is modeled as an analytical rigid surface with the *SURFACE option in conjunction with the *RIGID BODY option. The mechanical interaction between the contact surfaces is assumed to be nonintermittent, rough frictional contact. Therefore, two suboptions are used with the *SURFACE INTERACTION property option: the *FRICTION, ROUGH suboption to enforce a no slip constraint between the two surfaces, and the *SURFACE BEHAVIOR, NO SEPARATION suboption to ensure that separation does not occur once contact has been established. No mesh convergence studies have been done, but the agreement with the results given in Lippmann (1979) suggests that the meshes used here are good enough to provide reasonable predictions of the overall force on the dies.

Material The material behavior is similar to that used in ``Upsetting of a cylindrical billet: coupled temperature-displacement and adiabatic analysis,'' Section 1.3.17, except that rate dependence of the yield stress is not included. Thermal properties are not needed in this case since the analysis is mechanical only (we assume the loading is applied so slowly that the response is isothermal).

Boundary conditions and loading Kinematic boundary conditions are symmetry on the axis (nodes at r =0, in node set AXIS, have ur =0 prescribed), symmetry about z =0 (all nodes at z =0, in node set MIDDLE, have uz =0 prescribed). The node on the top surface of the billet that lies on the symmetry axis is not part of the node set AXIS to avoid overconstraint: the radial motion of this node is already constrained by a no slip frictional constraint (see ``Common difficulties associated with contact modeling,'' Section 21.10.1 of the ABAQUS/Standard User's Manual). The uz -displacement of the rigid body reference node for the die is prescribed as having a constant velocity in the axial direction so that the total displacement of the die is -9 mm over the history of the upsetting. The first analysis is done in two steps so that the first step can be stopped at a die displacement corresponding to 44% upsetting. The second step carries the first analysis to 60% upsetting. The second analysis restarts from the first step of the first analysis with a new mesh. A FORTRAN routine is used to extract the coordinates of the nodes along the outer boundary of the original mesh at 44% upsetting. These coordinates are then used to define the outer boundary of the new mesh.

Results and discussion The results from the first mesh are illustrated in Figure 1.3.1-2. This figure shows the configuration

1-382

Static Stress/Displacement Analyses

and plastic strain magnitude that are predicted at 44% upsetting (73.3% of the total die displacement). The folding of the top outside surface of the billet onto the die is clearly visible, as well as the severe straining of the middle of the specimen. At this point the mesh is rezoned. The new mesh for the rezoned model is shown in Figure 1.3.1-3. It is based on placing nodes on straight lines between the outer surface of the billet and the axis of the billet. The final configuration and plastic strain magnitudes predicted with rezoning are shown in Figure 1.3.1-4. Figure 1.3.1-5 shows the predictions of the total upsetting force versus displacement of the die. The results shown on the plot include the results for the analysis that includes the rezoning and the data obtained when the original mesh is used for the entire analysis. The results show that the rezoning of the mesh does not have a significant effect, in this case, on the overall die force. The results compare well with the rate independent results obtained by Taylor (1981).

Input files rezonebillet_cax4r.inp Original CAX4R mesh. rezonebillet_cax4r_rezone.inp Rezoned CAX4R mesh; requires the external file generated by rezonebillet_fortran_cax4r.f. rezonebillet_fortran_cax4r.f FORTRAN routine used to access the results file of rezonebillet_cax4r.inp and generate a file containing the nodal coordinates of the outer boundary at 44% upsetting. rezonebillet_cax4i.inp Original CAX4I mesh. rezonebillet_cax4i_rezone.inp Rezoned CAX4I mesh. The FORTRAN routine given in file rezonebillet_fortran_cax4r.f is not used as part of this analysis sequence. rezonebillet_cgax4r.inp Original CGAX4R mesh. rezonebillet_cgax4r_rezone.inp Rezoned CGAX4R mesh; requires the external file generated by rezonebillet_fortran_cax4r.f. rezonebillet_cgax4t.inp Original CGAX4T mesh. rezonebillet_cgax4t_rezone.inp Rezoned CGAX4T mesh; requires the external file generated by rezonebillet_fortran_cgax4t.f. rezonebillet_fortran_cgax4t.f FORTRAN routine used to access the results file from file rezonebillet_cgax4t.inp and generate a

1-383

Static Stress/Displacement Analyses

file containing the nodal coordinates of the outer boundary at 44% upsetting. rezonebillet_deftorigid.inp Rigid die simulated by declaring deformable elements (SAX1) as rigid. The billet is meshed with CAX4R elements. rezonebillet_deftorigid_rezone.inp Rezoned CAX4R mesh. The rigid die is simulated by declaring deformable elements (SAX1) as rigid.

References · Lippmann, H., Metal Forming Plasticity, Springer-Verlag, Berlin, 1979. · Taylor, L. M., "A Finite Element Analysis for Large Deformation Metal Forming Problems Involving Contact and Friction," Ph.D. Thesis, U. of Texas at Austin, 1981.

Figures Figure 1.3.1-1 Axisymmetric upsetting example: initial mesh.

Figure 1.3.1-2 Deformed configuration and plastic strain at 44% upset.

1-384

Static Stress/Displacement Analyses

Figure 1.3.1-3 New mesh at 44% upset.

1-385

Static Stress/Displacement Analyses

Figure 1.3.1-4 Deformed configuration and plastic strain of original mesh at 60% upset.

Figure 1.3.1-5 Force-deflection response for cylinder upsetting. (Results from the rezoned mesh start at 73.6% of applied displacement.)

1-386

Static Stress/Displacement Analyses

Sample listings

1-387

Static Stress/Displacement Analyses

Listing 1.3.1-1 *HEADING AXISYMMETRIC UPSETTING PROBLEM REZONING *RESTART,WRITE,FREQUENCY=30 *NODE,NSET=RSNODE 9999,0.,.015 *NODE 1, 13,.01 1201,0.,.015 1213,.01,.015 *NGEN,NSET=MIDDLE 1,13 *NGEN,NSET=TOP 1201,1213 *NFILL MIDDLE,TOP,12,100 *NSET,NSET=AXIS,GENERATE 1,1201,100 *NSET,NSET=OUTER,GENERATE 13,1013,100 *NSET,NSET=NAXIS,GENERATE 1,1101,100 *ELEMENT,TYPE=CAX4R,ELSET=METAL 1,1,2,102,101 *ELGEN,ELSET=METAL 1,12,1,1,12,100,100 *ELSET,ELSET=ECON1,GENERATE 1101,1112,1 *ELSET,ELSET=ECON2,GENERATE 12,1112,100 *RIGID BODY,ANALYTICAL SURFACE=BSURF,REF NODE=9999 *SURFACE,TYPE=SEGMENTS,NAME=BSURF START,.020,.015 LINE,-.001,.015 *SURFACE,NAME=ASURF ECON1,S3 ECON2,S2 *CONTACT PAIR,INTERACTION=ROUGH ASURF,BSURF *SURFACE INTERACTION,NAME=ROUGH

1-388

Static Stress/Displacement Analyses

*FRICTION,ROUGH *SURFACE BEHAVIOR,NO SEPARATION *SOLID SECTION,ELSET=METAL,MATERIAL=EL *MATERIAL,NAME=EL *ELASTIC 200.E9,.3 *PLASTIC 7.E8,0.00 3.7E9,10.0 *BOUNDARY MIDDLE,2 NAXIS,1 *STEP,INC=200,AMPLITUDE=RAMP,NLGEOM 73.3 PERCENT OF DIE DISPLACEMENT *STATIC 0.015,1. *BOUNDARY 9999,1 9999,6 9999,2,,-.0066 *MONITOR,NODE=9999,DOF=2 *CONTACT PRINT,SLAVE=ASURF,FREQUENCY=40 *CONTACT FILE,SLAVE=ASURF,FREQUENCY=40 *EL PRINT, ELSET=METAL,FREQUENCY=40 S,MISES E, PEEQ, *NODE PRINT, FREQUENCY=10 *NODE FILE,NSET=RSNODE U,RF *NODE FILE,FREQUENCY=999 COORD, *OUTPUT, FIELD, OP=NEW, FREQUENCY=9999 *NODE OUTPUT U, *END STEP *STEP,INC=200,AMPLITUDE=RAMP,NLGEOM 100 PERCENT OF DIE DISPLACEMENT *STATIC 0.015,1. *BOUNDARY 9999,1 9999,6

1-389

Static Stress/Displacement Analyses

9999,2,,-.009 *MONITOR,NODE=9999,DOF=2 *EL PRINT, ELSET=METAL,FREQUENCY=40 S,MISES E, PEEQ, *NODE PRINT, FREQUENCY=10 *NODE FILE,NSET=RSNODE U,RF *END STEP

1-390

Static Stress/Displacement Analyses

Listing 1.3.1-2 *HEADING AXISYMMETRIC UPSETTING PROBLEM REZONED *RESTART,WRITE,FREQUENCY=30 *NODE,NSET=RSNODE 9999,0.,.0084 *NODE 1, 1001,0.,.0084 *NODE,NSET=OUTER,INPUT=BOUNDARY.OUT *NGEN,NSET=AXIS 1,1001,100 *NSET,NSET=NAXIS,GENERATE 1,901,100 *NSET,NSET=MIDDLE,GENERATE 1,13 *NSET,NSET=TOP,GENERATE 1001,1013 *NFILL AXIS,OUTER,12,1 *ELEMENT,TYPE=CAX4R,ELSET=METAL 1,1,2,102,101 *ELGEN,ELSET=METAL 1,12,1,1,10,100,100 *ELSET,ELSET=ECON1,GENERATE 901,912,1 *ELSET,ELSET=ECON2,GENERATE 12,912,100 *RIGID BODY,ANALYTICAL SURFACE=BSURF,REF NODE=9999 *SURFACE,TYPE=SEGMENTS,NAME=BSURF START,.020,.0084 LINE,-.001,.0084 *SURFACE,NAME=ASURF ECON1,S3 ECON2,S2 *CONTACT PAIR,INTERACTION=ROUGH ASURF,BSURF *SURFACE INTERACTION,NAME=ROUGH *SURFACE BEHAVIOR,NO SEPARATION *FRICTION,ROUGH *SOLID SECTION,ELSET=METAL,MATERIAL=EL

1-391

Static Stress/Displacement Analyses

*MATERIAL,NAME=EL *ELASTIC 200.E9,.3 *PLASTIC 7.E8,0.00 3.7E9,10.0 *BOUNDARY MIDDLE,2 NAXIS,1 *MAP SOLUTION,STEP=1,INC=16 *STEP,INC=200,AMPLITUDE=RAMP,NLGEOM *STATIC .03,1. *BOUNDARY 9999,1 9999,6 9999,2,,-.0024 *MONITOR,NODE=9999,DOF=2 *CONTACT PRINT,SLAVE=ASURF *CONTACT FILE,SLAVE=ASURF,FREQUENCY=40 *EL PRINT, ELSET=METAL,FREQUENCY=40 S,MISES E, PEEQ, *NODE PRINT, FREQUENCY=10 *NODE FILE,NSET=RSNODE U,RF *END STEP

1-392

Static Stress/Displacement Analyses

Listing 1.3.1-3 SUBROUTINE HKSMAIN C C C

PROGRAM

READSETS

INCLUDE 'aba_param.inc' C PARAMETER (MAXNODES = 500) DIMENSION ARRAY(513), JRRAY(NPRECD,513), NMEMS(MAXNODES) EQUIVALENCE (ARRAY(1), JRRAY(1,1)) C INTEGER LRUNIT(2,1) LOGICAL READNODES CHARACTER FNAME*80, ASET*8 C C C C C C C C C C C C C C

THIS PROGRAM WILL EXTRACT THE CURRENT COORDINATES OF THE NODES OF THE "OUTER" AT THE STEP/INC DEFINED BY THE PARAMETERS K STEP AND K INC. TH NUMBERS AND COORDINATES ARE WRITTEN TO THE OUTPUT FILE BOUNDARY.OUT IN SUITABLE FOR INPUT INTO AN ABAQUS INPUT FILE. FOR EXAMPLE rezonebillet_cax4r: PARAMETER (K_STEP = 1, K_INC = 16, FNAME = 'rezonebillet_cax4r') FOR EXAMPLE rezonebillet_cgax4t: PARAMETER (K_STEP = 1, K_INC = 17, FNAME = 'rezonebillet_cgax4t') THIS MAY BE USED TO EXTRACT COORDINATES FROM EXA rezonebillet cax4i U PARAMETER (K_STEP = 1, K_INC = 40, FNAME = 'rezonebillet_cax4i') LRUNIT(1,1)=8 LRUNIT(2,1)=2 LOUTF=0 NRU = 1

C CALL

INITPF (FNAME, NRU, LRUNIT, LOUTF)

C JOUT = 6 KEYPRV= 0 KSTEP = 0 KINC = 0 READNODES = .FALSE. NUMMEM= 0

1-393

Static Stress/Displacement Analyses

C JUNIT = LRUNIT(1,1) CALL DBRNU (JUNIT) C OPEN (UNIT=6,STATUS='UNKNOWN',FILE='BOUNDARY.OUT') C C C

READ RECORDS FROM RESULTS FILE, UP TO 100000 RECORDS: DO 50 IXX = 1, 99999 CALL DBFILE(0,ARRAY,JRCD) IF (JRCD .NE. 0 .AND. KEYPRV .EQ. 2001) THEN WRITE(0,*) 'END OF FILE' CLOSE (JUNIT) GOTO 100 ELSE IF (JRCD .NE. 0) THEN WRITE(0,*) 'ERROR READING FILE' CLOSE (JUNIT) GOTO 100 ENDIF

C KEY=JRRAY(1,2) C C C

RECORD 2000: INCREMENT START RECORD IF(KEY.EQ.2000) THEN KSTEP = JRRAY(1,8) KINC = JRRAY(1,9) END IF

C C C

RECORD 1931: NODE SET DEFINITION RECORD IF(KEY.EQ.1931) THEN

C 110

WRITE(ASET,110) array(3) FORMAT(a8) IF (ASET(1:5).EQ.'OUTER') THEN NUMMEM = JRRAY(1,1) - 3 IF (NUMMEM.GT.MAXNODES) THEN WRITE(0,*)'ERROR: TOO MANY NODES ON RECORD' WRITE(0,*)' INCREASE MAXNODES TO ',NUMMEM CLOSE (JUNIT) GOTO 100 END IF

1-394

Static Stress/Displacement Analyses

DO KMEM = 1,NUMMEM NMEMS(KMEM)=JRRAY(1,3+KMEM) END DO READNODES = .TRUE. END IF END IF C C C

RECORD 107: NODAL COORDINATES RECORD IF (KEY.EQ.107 .AND. READNODES) THEN IF (KSTEP.EQ.K_STEP .AND. KINC.EQ.K_INC) THEN KNODE = JRRAY(1,3) DO KMEM = 1,NUMMEM IF (KNODE.EQ.NMEMS(KMEM)) THEN WRITE(JOUT,70)KNODE,ARRAY(4),ARRAY(5) FORMAT(I5,2(',',D18.8)) END IF END DO END IF END IF

70

C KEYPRV = KEY C 50

CONTINUE

C 100 CONTINUE C STOP END

1.3.2 Upsetting of a cylindrical billet in ABAQUS/Explicit Product: ABAQUS/Explicit The example illustrates the forming of a small, circular billet of metal that is reduced in length by 60%. This is the standard test case that is defined in Lippmann et al. (1979), so some verification of the result is available by comparing the results with the numerical results presented in that reference. The same test case is done with ABAQUS/Standard in ``Upsetting of a cylindrical billet in ABAQUS/Standard: quasi-static analysis with rezoning,'' Section 1.3.1. The same problem is analyzed using the coupled temperature-displacement elements in ``Upsetting of a cylindrical billet: coupled temperature-displacement and adiabatic analysis,'' Section 1.3.17.

Problem description The specimen is a circular billet, 30 mm long with a radius of 10 mm, compressed between flat, rough,

1-395

Static Stress/Displacement Analyses

rigid dies. The finite element model is axisymmetric and includes the top half of the billet only, since the middle surface of the billet is a plane of symmetry. Axisymmetric continuum elements of types CAX4R and CAX6M are used to model the billet. The rigid die is modeled in several different ways, as described below. 1. The die is modeled as an analytical rigid surface using the *SURFACE, TYPE=SEGMENTS and the *RIGID BODY options. The rigid surface is associated with a rigid body by its specified reference node. 2. Axisymmetric rigid elements of type RAX2 are used to model the rigid die. Three input files that use progressively finer meshes to model the billet exist for this case. 3. The die is modeled with RAX2 elements, as in Case 2. However, the die is assigned a mass by specifying point masses at the nodes of the RAX2 elements. The reference node of the rigid die is repositioned at its center of mass by specifying POSITION=CENTER OF MASS on the *RIGID BODY option. 4. The die is modeled with RAX2 elements, as in Case 2. The rigid elements are assigned thickness and density values such that the mass of the die is the same as in Case 3. 5. The die is modeled with RAX2 elements, as in Case 2. The NODAL THICKNESS parameter is used on the *RIGID BODY option to specify the thickness of the die at its nodes. The same thickness value is prescribed as in Case 4. 6. Axisymmetric shell elements of type SAX1 are used to model the die, and they are included in the rigid body by referring to them on the *RIGID BODY option. The thickness and the material density of the SAX1 elements is the same as that of the rigid elements in Case 4. 7. The die is modeled with axisymmetric shell elements of type SAX1 and with axisymmetric rigid elements of type RAX2. The deformable elements are included in the rigid body by referring to them on the *RIGID BODY option. Both element types have the same thickness and density as in Case 4. A coefficient of friction of 1.0 is used between the rigid surface and the billet. This value is large enough to ensure a no-slip condition so that, when the billet comes in contact with the rigid surface, there is virtually no sliding between the two. The material model assumed for the billet is that given in Lippmann et al. (1979). Young's modulus is 200 GPa, Poisson's ratio is 0.3, and the density is 7833 kg/m 3. A rate-independent von Mises elastic-plastic material model is used, with a yield stress of 700 MPa and a hardening slope of 0.3 GPa. Kinematic boundary conditions are symmetry on the axis (all nodes at r = 0 have ur = 0 prescribed) and symmetry about z = 0 (all nodes at z = 0 have uz = 0 prescribed). The rigid body reference node for the rigid body is constrained to have no rotation or ur -displacement. In Case 1 and Case 2 the uz -displacement is prescribed using a velocity boundary condition whose value is ramped up to a velocity of 20 m/s and then held constant until the die has moved a total of 9 mm. In the remaining cases a concentrated force of magnitude 410 kN is applied in the z-direction at the reference node. The

1-396

Static Stress/Displacement Analyses

magnitude of the concentrated force is such as to ensure that the resulting displacement of the die at the end of the time period is the same as in Case 1 and Case 2. The total time of the analysis is 0.55 millisec and is slow enough to be considered quasi-static. For Case 1 several different analyses are performed to compare section control options and mesh refinement for the billet modeled with CAX4R elements. Table 1.3.2-1 lists the analysis options used. A coarse mesh (analysis COARSE_SS) and a fine (analysis FINE_SS) mesh are analyzed with the pure stiffness form of hourglass control (HOURGLASS=STIFFNESS). A coarse mesh (analysis COARSE_CS) is analyzed with the combined hourglass control. The default section controls, using the integral viscoelastic form of hourglass control (HOURGLASS=RELAX STIFFNESS), are tested on a coarse mesh (analysis COARSE). Since this is a quasi-static analysis, the viscous hourglass control option (HOURGLASS=VISCOUS) should not be used. All other cases use the default section controls. In addition, Case 1 of the above problem has been analyzed using CAX6M elements with both coarse and fine meshes.

Results and discussion Figure 1.3.2-1 through Figure 1.3.2-4 show results for Case 1, where the billet is modeled with CAX4R elements. The rigid die is modeled using an analytical rigid surface, and the pure stiffness hourglass control is used. Figure 1.3.2-1 shows the original and deformed shape at the end of the analysis for the coarse mesh. Figure 1.3.2-2 shows the original and deformed shape at the end of the analysis for the fine mesh. Figure 1.3.2-3 and Figure 1.3.2-4 show contours of equivalent plastic strain for both meshes. Corresponding coarse and fine mesh results for the billet modeled with CAX6M elements are shown in Figure 1.3.2-5 to Figure 1.3.2-8. The number of nodes used for the coarse and fine CAX6M meshes are the same as those used for the coarse and fine CAX4R meshes. However, the analysis using CAX4R elements performs approximately 55% faster than the analysis using CAX6M elements. The equivalent plastic strain distributions obtained from each analysis compare closely for both the coarse and fine meshes; the CAX6M elements predict a slightly higher peak value. In both analyses the folding of the top outside surface of the billet onto the die is clearly visible, as well as the severe straining of the middle of the specimen. Figure 1.3.2-9 is a plot of vertical displacement versus reaction force at the rigid surface reference node for Case 1 with the section control options identified in Table 1.3.2-1. Results for an analysis run with ABAQUS/Standard (labeled COARSE_STD) are included for comparison. The curves obtained using CAX4R and CAX6M elements are very close and agree well with independent results obtained by Taylor (1981). The results from analysis COARSE_SS are virtually the same as the results from analysis COARSE, but at a much reduced cost; therefore, such analysis options are recommended for this problem. The results for all the other cases (which use the default section controls but different rigid surface models) are the same as the results for Case 1 using the default section controls.

Input files upset_anl_ss.inp

1-397

Static Stress/Displacement Analyses

Coarse mesh (CAX4R elements) of Case 1 using STIFFNESS hourglass control. upset_fine_anl_ss.inp Fine mesh of Case 1 (CAX4R elements) usingSTIFFNESS hourglass control. upset_anl_cs.inp Coarse mesh of Case 1 (CAX4R elements) using COMBINED hourglass control. upset_anl.inp Coarse mesh of Case 1 (CAX4R elements) using the default section control options. upset_fine_anl.inp Fine mesh of Case 1 (CAX4R elements) using the default section control options. upset_case2.inp Coarse mesh of Case 2 (CAX4R elements). upset_fine_case2.inp Fine mesh of Case 2 (CAX4R elements). upset_vfine_case2.inp An even finer mesh of Case 2 (CAX4R elements) included to test the performance of the code. upset_case3.inp Case 3 using CAX4R elements. upset_case4.inp Case 4 using CAX4R elements. upset_case5.inp Case 5 using CAX4R elements. upset_case6.inp Case 6 using CAX4R elements. upset_case7.inp Case 7 using CAX4R elements. upset_anl_cax6m.inp Case 1 using the coarse mesh of CAX6M elements. upset_fine_anl_cax6m.inp Case 1 using the fine mesh of CAX6M elements.

References

1-398

Static Stress/Displacement Analyses

· H. Lippmann, editor, Metal Forming Plasticity, Springer-Verlag, Berlin, 1979. · Taylor, L. M., "A Finite Element Analysis for Large Deformation Metal Forming Problems Involving Contact and Friction," Ph. D. Dissertation, U. of Texas at Austin, 1981.

Table Table 1.3.2-1 Analysis options for Case 1 using CAX4R elements. Analysis Mesh Hourglass Label Type Control COARSE_SS coarse STIFFNESS FINE_SS fine STIFFNESS COARSE_CS coarse COMBINED COARSE coarse RELAX

Figures Figure 1.3.2-1 Undeformed and deformed shape for the coarse mesh (CAX4R) of Case 1 (using the STIFFNESS hourglass control).

Figure 1.3.2-2 Undeformed and deformed shape for the fine mesh (CAX4R) of Case 1 (using the STIFFNESS hourglass control).

1-399

Static Stress/Displacement Analyses

Figure 1.3.2-3 Contours of equivalent plastic strain for the coarse mesh ( CAX4R) of Case 1 (using the STIFFNESS hourglass control).

Figure 1.3.2-4 Contours of equivalent plastic strain for the fine mesh ( CAX4R) of Case 1 (using the STIFFNESS hourglass control).

1-400

Static Stress/Displacement Analyses

Figure 1.3.2-5 Undeformed and deformed shape for the coarse mesh (CAX6M) of Case 1.

Figure 1.3.2-6 Contours of equivalent plastic strain for the coarse mesh ( CAX6M) of Case 1.

Figure 1.3.2-7 Undeformed and deformed shape for the fine mesh (CAX6M) of Case 1.

1-401

Static Stress/Displacement Analyses

Figure 1.3.2-8 Contours of equivalent plastic strain for the fine mesh ( CAX6M) of Case 1.

Figure 1.3.2-9 Comparison of reaction force versus vertical displacement for the different analyses tested for Case 1.

Sample listings

1-402

Static Stress/Displacement Analyses

Listing 1.3.2-1 *HEADING AXISYMMETRIC UPSETTING PROBLEM -- COARSE MESH (WITH RIGID SURFACE) SECTION CONTROLS USED (HOURGLASS=STIFFNESS) *RESTART,WRITE,NUM=30 *NODE 1, 13,.01 1201,0.,.015 1213,.01,.015 *NGEN,NSET=MIDDLE 1,13 *NGEN,NSET=TOP 1201,1213 *NFILL MIDDLE,TOP,12,100 *NSET,NSET=AXIS,GEN 1,1201,100 *ELEMENT,TYPE=CAX4R,ELSET=BILLET 1,1,2,102,101 *ELGEN,ELSET=BILLET 1,12,1,1,12,100,100 *NODE, NSET=NRIGID 2003,0.01,.02 *SOLID SECTION,ELSET=BILLET,MATERIAL=METAL, CONTROL=B *SECTION CONTROLS, HOURGLASS=STIFFNESS, NAME=B *MATERIAL,NAME=METAL *ELASTIC 200.E9,.3 *PLASTIC 7.E8,0.00 3.7E9,10.0 *DENSITY 7833., *BOUNDARY MIDDLE,2 AXIS,1 2003,1 2003,3,6 *AMPLITUDE,NAME=RAMP

1-403

Static Stress/Displacement Analyses

0.,0., 2.E-4,1., 5.5E-4,1. *SURFACE,TYPE=ELEMENT,NAME=BILLET TOP,S3 SIDE,S2 *SURFACE,NAME=RIGID,TYPE=SEGMENTS START, 0.02,.015 LINE, 0.00,.015 *RIGID BODY, REF NODE=2003, ANALYTICAL SURFACE =RIGID *STEP *DYNAMIC,EXPLICIT ,5.5E-4 *BOUNDARY,TYPE=VELOCITY,AMPLITUDE=RAMP 2003,2,,-20. *ELSET,ELSET=TOP,GEN 1101,1112,1 *ELSET,ELSET=SIDE,GEN 12,1112,100 *SURFACE INTERACTION,NAME=RIG_BILL *FRICTION 1.0, *CONTACT PAIR,INTERACTION=RIG_BILL RIGID,BILLET *MONITOR,NODE=2003,DOF=2 *FILE OUTPUT,NUM=2,TIMEMARKS=YES *EL FILE PEEQ,MISES *HISTORY OUTPUT, TIME=4.E-7 *NODE HISTORY, NSET=NRIGID U2,RF2 *NODE FILE, NSET=NRIGID U,RF *END STEP

1.3.3 Superplastic forming of a rectangular box Product: ABAQUS/Standard In this example we consider the superplastic forming of a rectangular box. The example illustrates the use of rigid elements to create a smooth three-dimensional rigid surface. Superplastic metals exhibit high ductility and very low resistance to deformation and are, thus, suitable for forming processes that require very large deformations. Superplastic forming has a number of advantages over conventional forming methods. Forming is usually accomplished in one step rather than several, and intermediate annealing steps are usually unnecessary. This process allows the

1-404

Static Stress/Displacement Analyses

production of relatively complex, deep-shaped parts with quite uniform thickness. Moreover, tooling costs are lower since only a single die is usually required. Drawbacks associated with this method include the need for tight control of temperature and deformation rate. Very long forming times make this method impractical for high volume production of parts. A superplastic forming process usually consists of clamping a sheet against a die whose surface forms a cavity of the shape required. Gas pressure is then applied to the opposite surface of the sheet, forcing it to acquire the die shape.

Rigid surface The *SURFACE option allows the creation of a rigid faceted surface created from an arbitrary mesh of three-dimensional rigid elements (either triangular R3D3 or quadrilateral R3D4 elements). See ``Defining analytical rigid surfaces,'' Section 2.3.4 of the ABAQUS/Standard User's Manual, for a discussion of smoothing of master surfaces. ABAQUS automatically smoothes any discontinuous surface normal transitions between the surface facets.

Solution-dependent amplitude One of the main difficulties in superplastically forming a part is the control of the processing parameters. The temperature and the strain rates that the material experiences must remain within a certain range for superplasticity to be maintained. The former is relatively easy to achieve. The latter is more difficult because of the unknown distribution of strain rates in the part. The manufacturing process must be designed to be as rapid as possible without exceeding a maximum allowable strain rate at any material point. For this purpose ABAQUS has a feature that allows the loading (usually the gas pressure) to be controlled by means of a solution-dependent amplitude. The options invoked are *AMPLITUDE, DEFINITION=SOLUTION DEPENDENT and a target maximum *CREEP STRAIN RATE CONTROL. In the loading options the user specifies a reference value. The amplitude definition requires an initial, a minimum, and a maximum load multiplier. During a *VISCO procedure ABAQUS will then monitor the maximum creep strain rate and compare it with the target value. The load amplitude is adjusted based on this comparison. This controlling algorithm is simple and relatively crude. The purpose is not to follow the target values exactly but to obtain a practical loading schedule.

Geometry and model The example treated here corresponds to superplastic forming of a rectangular box whose final dimensions are 1524 mm (60 in) long by 1016 mm (40 in) wide by 508 mm (20 in) deep with a 50.8 mm (2 in) flange around it. All fillet radii are 101.6 mm (4 in). The box is formed by means of a uniform fluid pressure. A quarter of the blank is modeled using 704 membrane elements of type M3D4R. These are bilinear membrane elements with fully reduced integration and hourglass control. The initial dimensions of the blank are 1625.6 mm (64 in) by 1117.6 mm (44 in), and the thickness is 3.175 mm (0.125 in). The blank is clamped at all its edges. The flat initial configuration of the membrane model is entirely singular in the normal direction unless it is stressed in biaxial tension. This difficulty is prevented by applying a small biaxial initial stress of 6.89 kPa (1 lb/in 2) by means of the *INITIAL CONDITIONS,

1-405

Static Stress/Displacement Analyses

TYPE=STRESS option. The female die is modeled as a rigid body and is meshed with rigid R3D3 elements. The rigid surface is defined with the *SURFACE option by grouping together those faces of the 231 R3D3 elements used to model the die that face the contact direction. See Figure 1.3.3-1 for an illustration of the rigid element mesh. To avoid having points "fall off" the rigid surface during the course of the analysis, more than a quarter of the die has been modeled, as shown in Figure 1.3.3-2. It is always a good idea to extend the rigid surface far enough so that contacting nodes will not slide off the master surface. By default, ABAQUS generates a unique normal to the rigid surface at each node point, based on the average of the normals to the elements sharing each node. There are times, however, when the normal to the surface should be specified directly. This is discussed in ``Node definition,'' Section 2.1.1 of the ABAQUS/Standard User's Manual. In this example the flange around the box must be flat to ensure compatibility between the originally flat blank and the die. Therefore, an outer normal (0, 1, 0) has been specified at the 10 nodes that make up the inner edge of the flange. This is done by entering the direction cosines after the node coordinates. The labels of these 10 vertices are 9043, 9046, 9049, 9052, 9089, 9090, 9091, 9121, 9124, and 9127; and their definitions can be found in superplasticbox_node.inp.

Material The material in the blank is assumed to be elastic-viscoplastic, and the properties roughly represent the 2004 (Al-6Cu-0.4Zr)-based commercial superplastic aluminum alloy Supral 100 at 470°C. It has a Young's modulus of 71 GPa (10.3 ´ 106 lb/in2) and a Poisson's ratio of 0.34. The flow stress is assumed to depend on the plastic strain rate according to ¾ f = A("_pl )1=2 ; where A is 179.2 MPa (26. ´ 103 lb/in2) and the time is in seconds.

Loading and controls We perform two analyses to compare constant pressure loading and a pressure schedule automatically adjusted to achieve a maximum strain rate of 0.02/sec. In the constant load case the prestressed blank is subjected to a rapidly applied external pressure of 68.8 kPa (10 lb/in 2), which is then held constant for 3000 sec until the box has been formed. In the second case the prestressed blank is subjected to a rapidly applied external pressure of 1.38 kPa (0.2 lb/in 2). The pressure schedule is then chosen by ABAQUS. The initial application of the pressures is assumed to occur so quickly that it involves purely elastic response. This is achieved by using the *STATIC procedure. The creep response is developed in a second step using the *VISCO procedure. During the *VISCO step the parameter CETOL controls the time increment and, hence, the accuracy of the transient creep solution. ABAQUS compares the equivalent creep strain rate at the beginning and

1-406

Static Stress/Displacement Analyses

the end of an increment. The difference should be less than CETOL divided by the time increment. Otherwise, the increment is reattempted with a smaller time increment. The usual guideline for setting CETOL is to decide on an acceptable error in stress and convert it to an error in strain by dividing by the elastic modulus. For this problem we assume that moderate accuracy is required and choose CETOL as 0.5%. In general, larger values of CETOL allow ABAQUS to use larger time increments, resulting in a less accurate and less expensive analysis. In the automatic scheduling analysis the pressure is referred to an amplitude that allows for a maximum pressure of 1.38 MPa (200 lb/in 2) and a minimum pressure of 0.138 kPa (0.02 lb/in 2). The target creep strain rate is a constant entered using the *CREEP STRAIN RATE CONTROL option.

Results and discussion Figure 1.3.3-3 through Figure 1.3.3-5show a sequence of deformed configurations during the automatically controlled forming process. The stages of deformation are very similar in the constant load process. However, the time necessary to obtain the deformation is much shorter with automatic loading--the maximum allowable pressure is reached after 83.3 seconds. The initial stages of the deformation correspond to inflation of the blank because there is no contact except at the edges of the box. Contact then occurs at the box's bottom, with the bottom corners finally filling. Although there is some localized thinning at the bottom corners, with strains on the order of 100%, these strains are not too much larger than the 80% strains seen on the midsides. Figure 1.3.3-6 shows the equivalent plastic strain at the end of the process. The constant load case provides similar results. Figure 1.3.3-7 shows the evolution in time of the ratio between the maximum creep strain rate found in the model and the target creep strain rate. The load applied initially produces a low maximum creep strain rate at the beginning of the analysis. At the end the maximum creep strain rate falls substantially as the die cavity fills up. Although the curve appears very jagged, it indicates that the maximum peak strain rate is always relatively close to the target value. This is quite acceptable in practice. Figure 1.3.3-8 shows the pressure schedule that ABAQUS calculates for this problem. For most of the time, while the sheet does not contact the bottom of the die, the pressure is low. Once the die starts restraining the deformation, the pressure can be increased substantially without producing high strain rates.

Input files superplasticbox_constpress.inp Constant pressure main analysis. superplasticbox_autopress.inp Automatic pressurization main analysis. superplasticbox_node.inp Node definitions for the rigid elements. superplasticbox_element.inp

1-407

Static Stress/Displacement Analyses

Element definitions for the rigid R3D3 elements.

Figures Figure 1.3.3-1 Rigid surface for die.

Figure 1.3.3-2 Initial position of blank with respect to die.

Figure 1.3.3-3 Automatic loading: deformed configuration after 34 sec in Step 2.

1-408

Static Stress/Displacement Analyses

Figure 1.3.3-4 Automatic loading: deformed configuration after 63 sec in Step 2.

Figure 1.3.3-5 Automatic loading: deformed configuration after 83 sec in Step 2.

1-409

Static Stress/Displacement Analyses

Figure 1.3.3-6 Automatic loading: inelastic strain in the formed box.

Figure 1.3.3-7 History of ratio between maximum creep strain rate and target creep strain rate.

Figure 1.3.3-8 History of pressure amplitude.

1-410

Static Stress/Displacement Analyses

Sample listings

1-411

Static Stress/Displacement Analyses

Listing 1.3.3-1 *HEADING SUPERPLASTIC FORMING OF BOX WITH MEMBRANES - CONSTANT LOADING *RESTART, WRITE, FREQUENCY=30 ** ** PLATE DEFINITION ** *NODE 1, 4.0, 20.0, -4.0 23, 26.0, 20.0, -4.0 3201, 4.0, 20.0, -36.0 3223, 26.0, 20.0, -36.0 *NGEN, NSET=EDGE3 1,3201,100 *NGEN, NSET=EDGE5 23,3223,100 *NFILL, NSET=PLATE EDGE3,EDGE5,22,1 *NSET, NSET=EDGE1, GENERATE 1,23,1 *NSET, NSET=EDGE7, GENERATE 3201,3223,1 *ELEMENT, TYPE=M3D4, ELSET=PLATE1 1,1,2,102,101 *ELGEN, ELSET=PLATE1 1,21,1,1,31,100,100 *NSET,ELSET=PLATE1, NSET=NCONT *ELEMENT, TYPE=M3D4, ELSET=PLATE2 22,22,23,123,122 3101,3101,3102,3202,3201 *ELGEN, ELSET=PLATE2 22,32,100,100 3101,21,1,1 *ELSET,ELSET=PLATE PLATE1,PLATE2 *MEMBRANE SECTION, ELSET=PLATE, MATERIAL=SUPRAL .125, ** ** MATERIAL IS CLOSE TO SUPRAL100 AT 470C ** *MATERIAL, NAME=SUPRAL

1-412

Static Stress/Displacement Analyses

*ELASTIC 10.3E6, .34 *CREEP, LAW=TIME 1.48E-9, 2., 0. ** ** CONTACT surface ** *NODE, NSET=DIE 10000, 0.0, 0.0, 0.0 *RIGID BODY, ELSET=ERIGID, REFNODE=10000 *NODE, INPUT=superplasticbox_node.inp *ELEMENT,TYPE=R3D3,ELSET=ERIGID, INPUT=superplasticbox_element.inp *SURFACE,NAME=DIE ERIGID,SPOS *SURFACE,TYPE=NODE,NAME=SLAVES NCONT, *CONTACT PAIR, INTERACTION=DIE_NODE, smooth=0.2 SLAVES,DIE *SURFACE INTERACTION,NAME=DIE_NODE ** ** BOUNDARY AND INITIAL CONDITIONS ** *BOUNDARY EDGE1,3 EDGE7,2,3 EDGE3,1 EDGE5,1,2 10000,1,6 *INITIAL CONDITIONS, TYPE=STRESS PLATE, 1.0, 1.0 *NSET,NSET=NSELECT 101,121,1001,1101,1507,2509 1,113,1211,1308,1408,1508,1509,1705 ** ** STEP 1 ** *STEP, INC=50, NLGEOM, unsymm=yes *STATIC 1.E-4,1.0, *DLOAD PLATE,P,-10. *CONTACT PRINT, FREQUENCY=100

1-413

Static Stress/Displacement Analyses

*CONTACT FILE, FREQUENCY=100, NSET=NSELECT *EL PRINT, ELSET=PLATE , FREQUENCY=100 S, E CE, SINV, *PRINT, CONTACT=YES *NODE PRINT, NSET=EDGE3, FREQUENCY=100 U, *NODE FILE, NSET=EDGE3, FREQUENCY=100 U, *END STEP ** ** STEP 2 ** *STEP, INC=500, NLGEOM, unsymm=yes *VISCO, CETOL=0.005 0.005, 3000.0 *DLOAD PLATE,P,-10. *END STEP

1-414

Static Stress/Displacement Analyses

Listing 1.3.3-2 *HEADING SUPERPLASTIC FORMING OF BOX WITH MEMBRANES - AUTOMATIC LOADING *RESTART, WRITE, FREQUENCY=30 ** ** PLATE DEFINITION ** *NODE 1, 4.0, 20.0, -4.0 23, 26.0, 20.0, -4.0 3201, 4.0, 20.0, -36.0 3223, 26.0, 20.0, -36.0 *NGEN, NSET=EDGE3 1,3201,100 *NGEN, NSET=EDGE5 23,3223,100 *NFILL, NSET=PLATE EDGE3,EDGE5,22,1 *NSET, NSET=EDGE1, GENERATE 1,23,1 *NSET, NSET=EDGE7, GENERATE 3201,3223,1 *NSET, NSET=CENTER 1, *ELEMENT, TYPE=M3D4, ELSET=PLATE1 1,1,2,102,101 *ELGEN, ELSET=PLATE1 1,21,1,1,31,100,100 *NSET,ELSET=PLATE1, NSET=NCONT *ELEMENT, TYPE=M3D4, ELSET=PLATE2 22,22,23,123,122 3101,3101,3102,3202,3201 *ELGEN, ELSET=PLATE2 22,32,100,100 3101,21,1,1 *ELSET,ELSET=PLATE PLATE1,PLATE2 *MEMBRANE SECTION, ELSET=PLATE, MATERIAL=SUPRAL .125, ** ** MATERIAL IS CLOSE TO SUPRAL100 AT 470C

1-415

Static Stress/Displacement Analyses

** *MATERIAL, NAME=SUPRAL *ELASTIC 10.3E6, .34 *CREEP, LAW=TIME 1.48E-9, 2., 0. ** ** CONTACT surface ** *NODE, NSET=DIE 10000, 0.0, 0.0, 0.0 *RIGID BODY, ELSET=ERIGID, REFNODE=10000 *NODE, INPUT=superplasticbox_node.inp *ELEMENT,TYPE=R3D3,ELSET=ERIGID, INPUT=superplasticbox_element.inp *SURFACE,NAME=DIE ERIGID,SPOS *SURFACE,type=node,NAME=SLAVES NCONT, *CONTACT PAIR, INTERACTION=DIE_NODE, smooth=0.2 SLAVES,DIE *SURFACE INTERACTION,NAME=DIE_NODE ** ** BOUNDARY AND INITIAL CONDITIONS ** *BOUNDARY EDGE1,3 EDGE7,2,3 EDGE3,1 EDGE5,1,2 10000,1,6 *INITIAL CONDITIONS, TYPE=STRESS PLATE, 1.0, 1.0 *AMPLITUDE,DEFINITION=SOLUTION DEPENDENT,NAME=AUTO 1.,0.1,1000. *NSET,NSET=NSELECT 101,121,1001,1101,1507,2509 1,113,1211,1308,1408,1508,1509,1705 ** ** STEP 1 ** *STEP, INC=30, NLGEOM, unsymm=yes *STATIC

1-416

Static Stress/Displacement Analyses

2.E-3,1.0, *DLOAD PLATE,P,-0.2 *CONTACT PRINT, FREQUENCY=100 *CONTACT FILE, FREQUENCY=100, NSET=NSELECT *EL PRINT, ELSET=PLATE , FREQUENCY=100 S, E CE, SINV, *PRINT, CONTACT=YES *NODE PRINT, NSET=EDGE3, FREQUENCY=100 U, *NODE FILE, NSET=EDGE3, FREQUENCY=100 U, *END STEP ** ** STEP 2 ** *STEP, INC=500, NLGEOM, unsymm=yes *VISCO, CETOL=0.005 0.2, 2000.0 *DLOAD,AMPLITUDE=AUTO PLATE,P,-0.2 *CREEP STRAIN RATE CONTROL, ELSET=PLATE, AMPLITUDE=AUTO 0.02 , ** TO WRITE THE AUTOMATIC SOLUTION CONTROL ** VARIABLES AMPCU AND RATIO TO THE RESULTS ** FILE EVERY INCREMENT SUCH FILE HAS TO BE ** ACTIVATED *NODE FILE, NSET=CENTER, FREQUENCY=1 U, *END STEP

1.3.4 Stretching of a thin sheet with a hemispherical punch Products: ABAQUS/Standard ABAQUS/Explicit Stamping of sheet metals by means of rigid punches and dies is a standard manufacturing process. In most bulk forming processes the loads required for the forming operation are often the primary concern. However, in sheet forming the prediction of strain distributions and limit strains (which define the onset of local necking) are most important. Such analysis is complicated in that it requires consideration of large plastic strains during deformation, an accurate description of material response including strain hardening, the treatment of a moving boundary that separates the region in contact

1-417

Static Stress/Displacement Analyses

with the punch head from the unsupported one, and the inclusion of friction between the sheet and the punch head. The stretching of a thin circular sheet with a hemispherical punch is considered in this example.

Geometry and model The geometry of this problem is shown in Figure 1.3.4-1. The sheet being stretched has a clamping radius, r0 , of 59.18 mm. The radius of the punch, rp , is 50.8 mm; the die radius, rd , is 6.35 mm; and the initial thickness of the sheet, t0 , is 0.85 mm. Such a sheet has been tested experimentally by Ghosh and Hecker (1975) and has been analyzed by Wang and Budiansky (1978) using an axisymmetric membrane shell finite element formulation. The analysis is conducted statically in ABAQUS/Standard and dynamically in ABAQUS/Explicit such that inertial forces are relatively small. The initial configuration for the ABAQUS/Explicit analysis is shown in Figure 1.3.4-2. The sheet, the punch, and the die are modeled as separate parts, each instanced once. As an axisymmetric problem in ABAQUS/Standard the sheet is modeled using 50 elements of type SAX1 (or MAX1) or 25 elements of type SAX2 (or MAX2). The ABAQUS/Explicit model uses 50 elements of type SAX1. Mesh convergence studies (not reported here) have been done and indicate that these meshes give acceptably accurate results for most of the values of interest. To test the three-dimensional membrane and shell elements in ABAQUS/Standard, a 10° sector is modeled using 100 elements of type S4R, S4, or M3D4R or 25 elements of type M3D9R. All these meshes are reasonably fine; they are used to obtain good resolution of the moving contact between the sheet and the dies. In the ABAQUS/Standard shell models nine integration points are used through the thickness of the sheet to ensure the development of yielding and elastic-plastic bending response; in ABAQUS/Explicit five integration points are used through the thickness of the sheet. The rigid punch and die are modeled in ABAQUS/Standard as analytical rigid surfaces with the *SURFACE option in conjunction with the *RIGID BODY option. The top and bottom surfaces of the sheet are defined with the *SURFACE option. In ABAQUS/Explicit the punch and die are modeled as rigid bodies using the *RIGID BODY option; the surface of the punch and die are modeled either by analytical rigid surfaces or RAX2 elements. The rigid surfaces are offset from the blank by half of the thickness of the blank because the contact algorithm in ABAQUS/Explicit takes the shell thickness into account.

Material properties The material (aluminum-killed steel) is assumed to satisfy the Ramberg-Osgood relation between true stress and logarithmic strain: " = ¾=E + (¾=K )n ; where Young's modulus, E, is 206.8 GPa; the reference stress value, K, is 0.510 GPa; and the work-hardening exponent, n, is 4.76. The material is assumed to be linear elastic below a 0.5% offset yield stress of 170.0 MPa and the stress-strain curve beyond that value is defined in piecewise linear segments using the *PLASTIC option. (The 0.5% offset yield stress is defined from the Ramberg-Osgood fit by taking (" ¡ ¾=E ) to be 0.5% and solving for the stress.) Poisson's ratio is 1-418

Static Stress/Displacement Analyses

0.3. The membrane element models in ABAQUS/Standard are inherently unstable in a static analysis unless some prestress is present in the elements prior to the application of external loading. Therefore, an equibiaxial initial stress condition equal to 5% of the initial yield stress is prescribed for the membrane elements in ABAQUS/Standard.

Contact interactions The contact between the sheet and the rigid punch and the rigid die is modeled with the *CONTACT PAIR option. The mechanical interaction between the contact surfaces is assumed to be frictional contact, with a coefficient of friction of 0.275 in ABAQUS/Standard and 0.265 in ABAQUS/Explicit.

Loading The ABAQUS/Standard analysis is carried out in six steps; the ABAQUS/Explicit analysis is carried out in four steps. In each of the first four steps of the ABAQUS/Standard analysis either the die or the punch head is moved using the *BOUNDARY option. In ABAQUS/Explicit the velocity of the punch head is prescribed using the *BOUNDARY option; the magnitude of the velocity is specified with the *AMPLITUDE option. It is ramped up to 30 m/s at 1.24 milliseconds during the first step and then kept constant until time reaches 1.57 milliseconds at the end of the second step. It is then ramped down to zero at a time of 1.97 milliseconds at the end of the third step. In the first step of the ABAQUS/Standard analysis the die is moved so that it just touches the sheet. In the next three steps (the first three steps of the ABAQUS/Explicit analysis) the punch head is moved toward the sheet through total distances of 18.6 mm, 28.5 mm, and 34.5 mm, respectively. The purpose of these three steps is to compare the results with those provided experimentally by Ghosh and Hecker for these punch displacements. More typically the punch would be moved through its entire travel in one step. Two final steps are included in the ABAQUS/Standard analysis. In the first step the metal sheet is held in place and the contact pairs are removed from the model with the *MODEL CHANGE, TYPE=CONTACT PAIR, REMOVE option. In the second step the original boundary conditions for the metal sheet are reintroduced for springback analysis. However, this springback step is not included for the analyses using membrane elements, since these elements do not have any bending stiffness and residual bending stress is often a key determinant of springback. In the final step of the ABAQUS/Explicit analysis the punch head is moved away from the sheet for springback analysis. A viscous pressure load is applied to the surface of the shell during this step to damp out transient wave effects so that quasi-static equilibrium can be reached quickly. This effect happens within approximately 2 milliseconds from the start of unloading. The coefficient of viscous pressure is chosen to be 0.35 MPa sec/m, approximately 1% of the value of ½cd , where ½ is the material density of the sheet and cd is the dilatational wave speed. A value of viscous pressure of ½cd would absorb all the energy in a pressure wave. For typical structural problems choosing a small percentage of this value provides an effective way of minimizing ongoing dynamic effects. Static equilibrium is reached when residual stresses in the sheet are reasonably constant over time.

Results and discussion

1-419

Static Stress/Displacement Analyses

Figure 1.3.4-2 shows the initial, undeformed profile of the blank, the die, and the punch. Figure 1.3.4-3 illustrates the deformed sheet and the punch and the die. Figure 1.3.4-4 shows a plot of the same system after the punch is lifted back, showing the springback of the sheet. Figure 1.3.4-5 and Figure 1.3.4-6 show the distribution of nominal values of radial and circumferential membrane strain in the sheet for 18.6 mm punch head displacement. Figure 1.3.4-7 and Figure 1.3.4-8 show the strain distributions at a punch head displacement of 28.5 mm, and Figure 1.3.4-9 and Figure 1.3.4-10 show the strain distributions at a punch head displacement of 34.5 mm. The strain distributions for the SAX1 models compare well with those obtained experimentally by Ghosh and Hecker (1975) and those obtained numerically by Wang and Budiansky (1978), who used a membrane shell finite element formulation. The important phenomenon of necking during stretching is reproduced at nearly the same location, although slightly different strain values are obtained. Draw beads are used to hold the edge of the sheet in the experiment, but in this analysis the sheet is simply clamped at its edge. Incorporation of the draw bead boundary conditions may further improve the correlation with the experimental data. A spike can be observed in the radial strain distribution toward the edge of the sheet in some of the ABAQUS/Standard shell models. This strain spike is the result of the sheet bending around the die. The spike is not present in the membrane element models since they possess no bending stiffness. The results obtained with the axisymmetric membrane models are compared with those obtained from the axisymmetric shell models and were found to be in good agreement. These analyses assume values of 0.265 or 0.275 for the coefficient of friction. Ghosh and Hecker do not give a value for their experiments, but Wang and Budiansky assume a value of 0.17. The coefficient of friction has a marked effect on the peak strain during necking and may be a factor contributing to the discrepancy of peak strain results during necking. The values used in these analyses have been chosen to provide good correlation with the experimental data. The distributions of the residual stresses on springback of the sheet in ABAQUS/Explicit are shown in Figure 1.3.4-11 and Figure 1.3.4-12.

Input files ABAQUS/Standard input files thinsheetstretching_m3d4r.inp Element type M3D4R. thinsheetstretching_m3d9r.inp Element type M3D9R. thinsheetstretching_max1.inp Element type MAX1. thinsheetstretching_max2.inp Element type MAX2.

1-420

Static Stress/Displacement Analyses

thinsheetstretching_s4.inp Element type S4. thinsheetstretching_s4r.inp Element type S4R. thinsheetstretching_sax1.inp Element type SAX1. thinsheetstretching_sax2.inp Element type SAX2. thinsheetstretching_restart.inp Restart of thinsheetstretching_sax2.inp. ABAQUS/Explicit input files hemipunch_anl.inp Model using analytical rigid surfaces to describe the rigid surface. hemipunch.inp Model using rigid elements to describe the rigid surface.

References · Ghosh, A. K., and S. S. Hecker, ``Failure in Thin Sheets Stretched Over Rigid Punches ,'' Metallurgical Transactions, vol. 6A, pp. 1065-1074, 1975. · Wang, N. M., and B. Budiansky, ``Analysis of Sheet Metal Stamping by a Finite Element Method,'' Journal of Applied Mechanics, vol. 45, pp. 73-82, 1978.

Figures Figure 1.3.4-1 Configuration and dimensions for hemispherical punch stretching.

1-421

Static Stress/Displacement Analyses

Figure 1.3.4-2 Initial ABAQUS/Explicit configuration.

Figure 1.3.4-3 Configuration for punch head displacement of 34.5 mm, ABAQUS/Explicit.

Figure 1.3.4-4 Final configuration after springback, ABAQUS/Explicit.

1-422

Static Stress/Displacement Analyses

Figure 1.3.4-5 Strain distribution for punch head displacement of 18.6 mm, ABAQUS/Standard.

Figure 1.3.4-6 Strain distribution for punch head displacement of 18.6 mm, ABAQUS/Explicit.

Figure 1.3.4-7 Strain distribution for punch head displacement of 28.5 mm, ABAQUS/Standard.

1-423

Static Stress/Displacement Analyses

Figure 1.3.4-8 Strain distribution for punch head displacement of 28.5 mm, ABAQUS/Explicit.

Figure 1.3.4-9 Strain distribution for punch head displacement of 34.5 mm, ABAQUS/Standard.

1-424

Static Stress/Displacement Analyses

Figure 1.3.4-10 Strain distribution for punch head displacement of 34.5 mm, ABAQUS/Explicit.

Figure 1.3.4-11 Residual stress on top surface after springback, ABAQUS/Explicit.

1-425

Static Stress/Displacement Analyses

Figure 1.3.4-12 Residual stress on bottom surface after springback, ABAQUS/Explicit.

Sample listings

1-426

Static Stress/Displacement Analyses

Listing 1.3.4-1 *HEADING WANG AND BUDIANSKY'S SPHERICAL PUNCH WITH SAX1 50 ELEMENTS, 9 LAYERS *RESTART,WRITE,FREQUENCY=250 *PREPRINT,ECHO=YES *PART,NAME=BLANK *NODE,NSET=MID 1,0.0,0.0 *NODE,NSET=REFD 401,50.59,0. *NFILL,BIAS=1.0,NSET=METND MID,REFD,40,10 *NODE,NSET=END 501,59.18,0. *NFILL,BIAS=1.0,NSET=METND REFD,END,10,10 *NSET,NSET=NODWR,GENERATE 1,501,10 *ELEMENT,TYPE=SAX1 1,1,11 *ELGEN,ELSET=METAL 1,50,10 *ELSET,ELSET=EDIE,GENERATE 42,49,1 *ELSET,ELSET=ECON,GENERATE 1,41,1 *SHELL SECTION,ELSET=METAL,MATERIAL=SAMP 0.85,9 *END PART *MATERIAL,NAME=SAMP *ELASTIC 206.8,0.3 *PLASTIC 0.1700000, 0.0000000E+00 0.1800000 , 1.7205942E-03 0.1900000 , 3.8296832E-03 0.2000000 , 6.3897874E-03 0.2100000, 9.4694765E-03 0.2200000, 1.3143660E-02 0.2300000, 1.7493792E-02 0.2400000, 2.2608092E-02

1-427

Static Stress/Displacement Analyses

0.2500000, 2.8581845E-02 0.2600000, 3.5517555E-02 0.2700000, 4.3525275E-02 0.2800000, 5.2722659E-02 0.2900000, 6.3235357E-02 0.3000000, 7.5197279E-02 0.3100000, 8.8750519E-02 0.3200000, 0.1040458 0.3300000, 0.1212430 0.3400000, 0.1405106 0.3500000, 0.1620263 0.3600000, 0.1859779 0.3700000, 0.2125620 0.3800000, 0.2419857 0.3900000, 0.2744660 0.4000000, 0.3102303 0.4100000, 0.3495160 0.4200000, 0.3925720 0.4300000, 0.4396578 0.4400000, 0.4910434 0.4500000, 0.5470111 0.4600000, 0.6078544 0.4700000, 0.6738777 0.4800000, 0.7453985 0.4900000, 0.8227461 0.5000000, 0.9062610 0.5100000 , 0.9962980 *PART,NAME=PUNCH *NODE,NSET=PUNCH 1000,0.,0. *RIGID BODY,ANALYTICAL SURFACE=BSURF,REF NODE=1000 *END PART *PART,NAME=DIE *NODE,NSET=DIE 2000,59.18,0.05 *RIGID BODY,ANALYTICAL SURFACE=DSURF,REF NODE=2000 *END PART *ASSEMBLY,NAME=FORM *INSTANCE,NAME=BLANK-1,PART=BLANK *SURFACE,NAME=ASURF ECON,SNEG *SURFACE,NAME=CSURF EDIE,SPOS

1-428

Static Stress/Displacement Analyses

*END INSTANCE *INSTANCE,NAME=PUNCH-1,PART=PUNCH *SURFACE,NAME=BSURF,TYPE=SEGMENTS START,0.0,0.0 CIRCL,50.8,-50.80,0.0,-50.80 *END INSTANCE *INSTANCE,NAME=DIE-1,PART=DIE *SURFACE,NAME=DSURF,TYPE=SEGMENTS START,61.00,0.05 LINE,59.18,0.05 CIRCL,52.83,6.4,59.18,6.4 LINE,52.83,8. *END INSTANCE *NSET,NSET=PUNK PUNCH-1.PUNCH,DIE-1.DIE *END ASSEMBLY *CONTACT PAIR,INTERACTION=ROUGH FORM.BLANK-1.ASURF,FORM.PUNCH-1.BSURF *CONTACT PAIR,INTERACTION=ROUGH FORM.BLANK-1.CSURF,FORM.DIE-1.DSURF *SURFACE INTERACTION,NAME=ROUGH *FRICTION 0.275, *BOUNDARY FORM.BLANK-1.1,1,1 FORM.BLANK-1.1,6,6 FORM.BLANK-1.501,1,1 FORM.BLANK-1.501,2,2 FORM.PUNCH-1.1000,6,6 FORM.PUNCH-1.1000,1,1 FORM.DIE-1.2000,1,1 FORM.DIE-1.2000,6,6 *STEP,INC=10,NLGEOM, UNSYMM=YES *STATIC 1.,1. *BOUNDARY FORM.DIE-1.2000,2,2,-0.05 *PRINT,RESIDUAL=NO,FREQUENCY=10 *EL PRINT,FREQUENCY=0 *NODE FILE,FREQUENCY=1000 U,RF COORD, *CONTACT FILE,SLAVE=FORM.BLANK-1.ASURF,FREQUENCY=1000

1-429

Static Stress/Displacement Analyses

*CONTACT FILE,SLAVE=FORM.BLANK-1.CSURF,FREQUENCY=1000 *END STEP *STEP,INC=2000,NLGEOM, UNSYMM=YES *STATIC 0.05,100.,1.E-5 *BOUNDARY FORM.PUNCH-1.1000,2,2,18.6 FORM.DIE-1.2000,2,2,-0.05 *MONITOR,NODE=FORM.PUNCH-1.1000,DOF=2 *NODE PRINT,NSET=FORM.PUNK,FREQUENCY=100 U,RF COORD, *END STEP *STEP,INC=2000,NLGEOM, UNSYMM=YES *STATIC 0.05,100.,1.E-5 *EL FILE,ELSET=FORM.BLANK-1.METAL,FREQUENCY=1000 5, S,E *BOUNDARY FORM.PUNCH-1.1000,2,2,28.5 FORM.DIE-1.2000,2,2,-0.05 *END STEP *STEP,INC=2000,NLGEOM, UNSYMM=YES *STATIC 0.05,100.,1.E-5 *BOUNDARY FORM.PUNCH-1.1000,2,2,34.5 FORM.DIE-1.2000,2,2,-0.05 *END STEP *STEP,INC=2000,NLGEOM, UNSYMM=YES *STATIC 100.,100. *BOUNDARY,FIXED FORM.BLANK-1.METND,1,2 FORM.BLANK-1.METND,6 *MODEL CHANGE,TYPE=CONTACT PAIR,REMOVE FORM.BLANK-1.ASURF,FORM.PUNCH-1.BSURF FORM.BLANK-1.CSURF,FORM.DIE-1.DSURF *EL FILE,ELSET=FORM.BLANK-1.METAL,FREQUENCY=1000 5, S, *END STEP

1-430

Static Stress/Displacement Analyses

*STEP,INC=2000,NLGEOM, UNSYMM=YES *STATIC 1.,100. *BOUNDARY,OP=NEW FORM.BLANK-1.1,1,1 FORM.BLANK-1.1,6,6 FORM.BLANK-1.501,1,1 FORM.BLANK-1.501,2,2 FORM.PUNCH-1.1000,6,6 FORM.PUNCH-1.1000,1,2 FORM.DIE-1.2000,1,2 FORM.DIE-1.2000,6,6 *MONITOR,NODE=FORM.BLANK-1.1,DOF=2 *EL FILE,ELSET=FORM.BLANK-1.METAL,FREQUENCY=1000 5, S, *END STEP

1-431

Static Stress/Displacement Analyses

Listing 1.3.4-2 *HEADING WANG AND BUDIANSKY'S SPHERICAL PUNCH WITH SAX1 ELEMENTS PUNCH AND DIE ARE ANALYTICAL RIGID SEGMENTS *PREPRINT,ECHO=YES *PART,NAME=BLANK *NODE 1,0.0,0.0 401,.05059,0. 501,.05918,0. *NGEN 1,401,10 401,501,10 *ELEMENT,TYPE=SAX1,ELSET=BLANK 1,1,11 *ELGEN,ELSET=BLANK 1,50,10 *ELSET,ELSET=CENTER,GEN 1,10,1 *SHELL SECTION,ELSET=BLANK,MATERIAL=SAMP 0.00085 *SURFACE, NAME=TOP BLANK,SPOS *SURFACE, NAME=BOTTOM BLANK,SNEG *END PART *MATERIAL,NAME=SAMP *DENSITY 7850. *ELASTIC 206.8E9,0.3 *PLASTIC 170.0E6, 0.0000000E+00 180.0E6, 1.7205942E-03 190.0E6, 3.8296832E-03 200.0E6, 6.3897874E-03 210.0E6, 9.4694765E-03 220.0E6, 1.3143660E-02 230.0E6, 1.7493792E-02 240.0E6, 2.2608092E-02 250.0E6, 2.8581845E-02

1-432

Static Stress/Displacement Analyses

260.0E6, 3.5517555E-02 270.0E6, 4.3525275E-02 280.0E6, 5.2722659E-02 290.0E6, 6.3235357E-02 300.0E6, 7.5197279E-02 310.0E6, 8.8750519E-02 320.0E6, 0.1040458 330.0E6, 0.1212430 340.0E6, 0.1405106 350.0E6, 0.1620263 360.0E6, 0.1859779 370.0E6, 0.2125620 380.0E6, 0.2419857 390.0E6, 0.2744660 400.0E6, 0.3102303 410.0E6, 0.3495160 420.0E6, 0.3925720 430.0E6, 0.4396578 440.0E6, 0.4910434 450.0E6, 0.5470111 460.0E6, 0.6078544 470.0E6, 0.6738777 480.0E6, 0.7453985 490.0E6, 0.8227461 500.0E6, 0.9062610 510.0E6, 0.9962980 ** *PART,NAME=PUNCH *NODE,NSET=REF_NODE 1000,0.,.051225 *RIGID BODY, REF NODE=REF_NODE, ANALYTICAL SURFACE=PUNCH_BOT *SURFACE, NAME=PUNCH_BOT, TYPE=SEGMENTS START, .0508,.051225 CIRCL, 0.,0.000425, 0.,.051225 *END PART *PART,NAME=DIE *NODE,NSET=REF_NODE 2000, .05918,-.006775 *RIGID BODY, REF NODE=REF_NODE, ANALYTICAL SURFACE=DIE_TOP *SURFACE, NAME=DIE_TOP, TYPE=SEGMENTS START, .05283,-.030425

1-433

Static Stress/Displacement Analyses

LINE, .05283,-.006775 CIRCL, .05918,-0.000425, .05918,-.006775 LINE, .05930,-0.000425 *END PART ** *ASSEMBLY,NAME=ASSEMBLY-1 *INSTANCE,NAME=BLANK-1,PART=BLANK *NSET,NSET=NOUT 1, *ELSET,ELSET=EOUT 22,23,24,25 *END INSTANCE *INSTANCE,NAME=PUNCH-1,PART=PUNCH *NSET,NSET=PUNCH 1000, *END INSTANCE *INSTANCE,NAME=DIE-1,PART=DIE *END INSTANCE *END ASSEMBLY *BOUNDARY ASSEMBLY-1.BLANK-1.1,1,1 ASSEMBLY-1.BLANK-1.1,6,6 ASSEMBLY-1.BLANK-1.501,1,2 ASSEMBLY-1.BLANK-1.501,6,6 ASSEMBLY-1.PUNCH-1.1000,1,1 ASSEMBLY-1.PUNCH-1.1000,1,6 ASSEMBLY-1.DIE-1.2000,1,2 ASSEMBLY-1.DIE-1.2000,6,6 *AMPLITUDE,NAME=LOAD,TIME=TOTAL 0.,0.,1.24E-3,1.,1.57E-3,1.,1.97E-3,0., 3.97E-3,-.25 *RESTART,WRITE,NUM=2,TIMEMARKS=NO *STEP *DYNAMIC,EXPLICIT ,1.24E-3 *BOUNDARY,TYPE=VELOCITY,AMP=LOAD ASSEMBLY-1.PUNCH-1.1000,2,2,-30. *SURFACE INTERACTION,NAME=PUNCH_TOP *FRICTION 0.265, *CONTACT PAIR, INTERACTION=PUNCH_TOP, CPSET=PUNCH_DIE ASSEMBLY-1.PUNCH-1.PUNCH_BOT,ASSEMBLY-1.BLANK-1.TOP

1-434

Static Stress/Displacement Analyses

ASSEMBLY-1.DIE-1.DIE_TOP,ASSEMBLY-1.BLANK-1.BOTTOM *FILE OUTPUT,NUMBER INTERVAL = 1 *EL FILE S,LE *ENERGY FILE *HISTORY OUTPUT,TIME=0. *NODE HISTORY,NSET=ASSEMBLY-1.PUNCH-1.PUNCH U2,RF2 *NODE HISTORY,NSET=ASSEMBLY-1.BLANK-1.NOUT U,V *EL HISTORY,ELSET=ASSEMBLY-1.BLANK-1.EOUT STH MISES,S,LE *ENERGY HISTORY ALLKE,ALLSE,ALLWK,ALLPD,ALLIE,ALLVD,ETOTAL,ALLAE, ALLCD,ALLFD,DT *OUTPUT, FIELD, NUMBER INTERVAL=4, TIMEMARKS=NO *CONTACT OUTPUT, CPSET=PUNCH_DIE, VARIABLE=PRESELECT *END STEP *STEP *DYNAMIC,EXPLICIT ,.33E-3 *END STEP *STEP *DYNAMIC,EXPLICIT ,.40E-3 *END STEP *STEP ** ** Unloading step ** *DYNAMIC,EXPLICIT ,2.E-3 *DLOAD,OP=NEW ASSEMBLY-1.BLANK-1.BLANK,VP,0.35E6 *END STEP

1.3.5 Deep drawing of a cylindrical cup Product: ABAQUS/Standard Deep drawing of sheet metal is an important manufacturing technique. In the deep drawing process a "blank" of sheet metal is clamped by a blank holder against a die. A punch is then moved against the

1-435

Static Stress/Displacement Analyses

blank, which is drawn into the die. Unlike the operation described in the hemispherical punch stretching example (``Stretching of a thin sheet with a hemispherical punch, '' Section 1.3.4), the blank is not assumed to be fixed between the die and the blank holder; rather, the blank is drawn from between these two tools. The ratio of drawing versus stretching is controlled by the force on the blank holder and the friction conditions at the interface between the blank and the blank holder and the die. Higher force or friction at the blank/die/blank holder interface limits the slip at the interface and increases the radial stretching of the blank. In certain cases drawbeads, shown in Figure 1.3.5-1, are used to restrain the slip at this interface even further. To obtain a successful deep drawing process, it is essential to control the slip between the blank and its holder and die. If the slip is restrained too much, the material will undergo severe stretching, thus potentially causing necking and rupture. If the blank can slide too easily, the material will be drawn in completely and high compressive circumferential stresses will develop, causing wrinkling in the product. For simple shapes like the cylindrical cup here, a wide range of interface conditions will give satisfactory results. But for more complex, three-dimensional shapes, the interface conditions need to be controlled within a narrow range to obtain a good product. During the drawing process the response is determined primarily by the membrane behavior of the sheet. For axisymmetric problems in particular, the bending stiffness of the metal yields only a small correction to the pure membrane solution, as discussed by Wang and Tang (1988). In contrast, the interaction between the die, the blank, and the blank holder is critical. Thus, thickness changes in the sheet material must be modeled accurately in a finite element simulation, since they will have a significant influence on the contact and friction stresses at the interface. In these circumstances the most suitable elements in ABAQUS are the 4-node reduced-integration axisymmetric quadrilateral, CAX4R; the first-order axisymmetric shell element, SAX1; the first-order axisymmetric membrane element, MAX1; the first-order finite-strain quadrilateral shell element, S4R; and the fully integrated general-purpose finite-membrane-strain shell element, S4. Membrane effects and thickness changes are modeled properly with CAX4R. However, the bending stiffness of the element is low. The element does not exhibit "locking" due to incompressibility or parasitic shear. It is also very cost-effective. In the shells and membranes the thickness change is calculated from the assumption of incompressible deformation of the material. This simplifying assumption does not allow for the development of stress in the thickness direction of the shell, thus making it difficult to model the contact pressure between the blank and the die and the blank holder. This situation is resolved in the shell and membrane models by using the *SURFACE BEHAVIOR, PRESSURE-OVERCLOSURE=EXPONENTIAL option (``Interaction normal to the surface,'' Section 21.3.3 of the ABAQUS/Standard User's Manual) to impose the proper clamping pressure in the thickness direction of the shell or membrane between the blank and the die and the blank holder.

Geometry and model The geometry of the problem is shown in Figure 1.3.5-2. The circular blank being drawn has an initial radius of 100 mm and an initial thickness of 0.82 mm. The punch has a radius of 50 mm and is rounded off at the corner with a radius of 13 mm. The die has an internal radius of 51.25 mm and is rounded off at the corner with a radius of 5 mm. The blank holder has an internal radius of 56.25 mm.

1-436

Static Stress/Displacement Analyses

The blank is modeled using 40 elements of type CAX4R or 31 elements of either type SAX1, MAX1, S4R, or S4. An 11.25° wedge of the circular blank is used in the three-dimensional S4R and S4 models. These meshes are rather coarse for this analysis. However, since the primary interest in this problem is to study the membrane effects, the analysis will still give a fair indication of the stresses and strains occurring in the process. The contact between the blank and the rigid punch, the rigid die, and the rigid blank holder is modeled with the *CONTACT PAIR option. The top and bottom surfaces of the blank are defined by means of the *SURFACE option. The rigid punch, the die, and the blank holder are modeled as analytical rigid surfaces with the *RIGID BODY option in conjunction with the *SURFACE option. The mechanical interaction between the contact surfaces is assumed to be frictional contact. Therefore, the *FRICTION option is used in conjunction with the various *SURFACE INTERACTION property options to specify coefficients of friction. For the shell models the interaction between the blank and the blank holder is also assumed to be "softened" contact, as discussed previously. At the start of the analysis for the CAX4R model, the blank is positioned precisely on top of the die and the blank holder is precisely in touch with the top surface of the blank. The punch is positioned 0.18 mm above the top surface of the blank. The shell and membrane models begin with the same state except that the blank holder is positioned a fixed distance above the blank. This fixed distance is the distance at which the contact pressure is set to zero by means of the *SURFACE BEHAVIOR, PRESSURE-OVERCLOSURE=EXPONENTIAL option.

Material properties The material (aluminum-killed steel) is assumed to satisfy the Ramberg-Osgood relation between true stress and logarithmic strain: ² = (¾=K )1=n : The reference stress value, K, is 513 MPa; and the work-hardening exponent, n, is 0.223. The Young's modulus is 211 GPa, and the Poisson's ratio is 0.3. An initial yield stress of 91.3 MPa is obtained with these data. The stress-strain curve is defined in piecewise linear segments in the *PLASTIC option, up to a total (logarithmic) strain level of 107%. The coefficient of friction between the interface and the punch is taken to be 0.25; and that between the die and the blank holder is taken as 0.1, the latter value simulating a certain degree of lubrication between the surfaces. The stiffness method of sticking friction is used in these analyses. The numerics of this method make it necessary to choose an acceptable measure of relative elastic slip between mating surfaces when sticking should actually be occurring. The basis for the choice is as follows. Small values of elastic slip best simulate the actual behavior but also result in a slower convergence of the solution. Permission of large relative elastic displacements between the contacting surfaces can cause higher strains at the center of the blank. In these runs we let ABAQUS choose the allowable elastic slip, which is done by determining a characteristic interface element length over the entire mesh and multiplying by a small fraction to get an allowable elastic slip measure. This method typically

1-437

Static Stress/Displacement Analyses

gives a fairly small amount of elastic slip. Although the material in this process is fully isotropic, the *ORIENTATION option is used with the CAX4R elements to define a local orientation that is coincident initially with the global directions. The reason for using this option is to obtain the stress and strain output in more natural coordinates: if the *ORIENTATION option is used in a geometrically nonlinear analysis, stress and strain components are given in a corotational framework. Hence, in our case throughout the motion, S11 will be the stress in the r-z plane in the direction of the middle surface of the cup. S22 will be the stress in the thickness direction, S33 will be the hoop stress, and S12 will be the transverse shear stress, which makes interpreting the results considerably easier. This orientation definition is not necessary with the SAX1 or MAX1 elements since the output for shell and membrane elements is already given in the local shell system. For the SAX1 and MAX1 model, S11 is the stress in the meridional direction and S22 is the circumferential (hoop) stress. An orientation definition would normally be needed for the S4R and S4 models but can be avoided by defining the wedge in such a manner that the single integration point of each element lies along the global x-axis. Such a model definition, along with appropriate kinematic boundary conditions, keeps the local stress output definitions for the shells as S11 being the stress in the meridional plane and S22 the hoop stress. There should be no in-plane shear, S12, in this problem. A transformation is used in the S4R and S4 models to impose boundary constraints in a cylindrical system.

Loading The entire analysis is carried out in five steps. In the first step the blank holder is pushed onto the blank with a prescribed displacement of -17.5 ´ 10-6 mm. This value is chosen to obtain a reaction force that is approximately equal to the applied force. In the shell models this displacement corresponds to zero clearance across the interface, thus resulting in the application of a predetermined clamping pressure across the shell thickness via the *SURFACE BEHAVIOR, PRESSURE-OVERCLOSURE=EXPONENTIAL option. In the second step the boundary condition is removed and replaced by the applied force of 100 kN on the blank holder. This force is kept constant during Steps 2 and 3. This technique of simulating the clamping process is used to avoid potential problems with rigid body modes of the blank holder, since there is no firm contact between the blank holder, the blank, and the die at the start of the process. The two-step procedure creates contact before the blank holder is allowed to move freely. In the third step the punch is moved toward the blank through a total distance of 60 mm. This step models the actual drawing process. During this step the option *CONTROLS, ANALYSIS=DISCONTINUOUS is included since contact with friction tends to create a severely discontinuous nonlinearity and we wish to avoid premature cutbacks of the automatic time incrementation scheme. The last two steps are used to simulate springback. In the fourth step all the nodes in the model are fixed in their current positions and the contact pairs are removed from the model with the *MODEL CHANGE, TYPE=CONTACT PAIR, REMOVE option. This is the most reliable method for releasing contact conditions. In the fifth, and final, step the regular set of boundary conditions is reinstated and the springback is allowed to take place. This part of the analysis with the CAX4R elements is included

1-438

Static Stress/Displacement Analyses

to demonstrate the feasibility of the unloading procedure only and is not expected to produce realistic results, since the reduced-integration elements have a purely elastic bending behavior. The springback is modeled with more accuracy in the shell element models.

Results and discussion Figure 1.3.5-3 shows deformed shapes that are predicted at various stages of the drawing process for the CAX4R model. The profiles show that the metal initially bends and stretches and is then drawn in over the surface of the die. The distributions of radial and circumferential strain for all three models and thickness strain for the CAX4R model are shown in Figure 1.3.5-4. The thickness for the shell or membrane models can be monitored with output variable STH (current shell or membrane thickness). The thickness does not change very much: the change ranges from approximately -12% in the cylindrical part to approximately +16% at the edge of the formed cup. Relatively small thickness changes are usually desired in deep drawing processes and are achieved because the radial tensile strain and the circumferential compressive strain balance each other. The drawing force as a function of punch displacement is shown in Figure 1.3.5-5. The curves for the three models compare closely. The oscillations in the force are a result of the rather coarse mesh--each oscillation represents an element being drawn over the corner of the die. Compared to the shell models, the membrane model predicts a smaller punch force for a given punch displacement. Thus, toward the end of the analysis the results for punch force versus displacement for the MAX1 model are closer to those for the CAX4R model. The deformed shape after complete unloading is shown in Figure 1.3.5-6, superimposed on the deformed shape under complete loading. The analysis shows the lip of the cup springing back strongly after the blank holder is removed for the CAX4R model. No springback is evident in the shell models. As was noted before, this springback in the CAX4R model is not physically realistic: in the first-order reduced-integration elements an elastic "hourglass control" stiffness is associated with the "bending" mode, since this mode is identical to the "hourglass" mode exhibited by this element in continuum situations. In reality the bending of the element is an elastic-plastic process, so that the springback is likely to be much less. A better simulation of this aspect would be achieved by using several elements through the thickness of the blank, which would also increase the cost of the analysis. The springback results for the shell models do not exhibit this problem and are clearly more representative of the actual elastic-plastic process.

Input files deepdrawcup_cax4r.inp CAX4R model. deepdrawcup_cax4i.inp Model using the incompatible mode element, CAX4I, as an alternative to the CAX4R element. In contrast to the reduced-integration, linear isoparametric elements such as the CAX4R element, the incompatible mode elements have excellent bending properties even with one layer of elements through the thickness (see ``Geometrically nonlinear analysis of a cantilever beam,'' Section 2.1.2 of the ABAQUS Benchmarks Manual) and have no hourglassing problems. However, they are

1-439

Static Stress/Displacement Analyses

computationally more expensive. deepdrawcup_s4.inp S4 model. deepdrawcup_s4r.inp S4R model. deepdrawcup_sax1.inp SAX1 model. deepdrawcup_postoutput.inp *POST OUTPUT analysis of deepdrawcup_sax1.inp. deepdrawcup_max1.inp MAX1 model. deepdrawcup_mgax1.inp MGAX1 model.

Reference · Wang, N. M., and S. C. Tang, "Analysis of Bending Effects in Sheet Forming Operations," International Journal for Numerical Methods in Engineering, vol. 25, pp. 253-267, January 1988.

Figures Figure 1.3.5-1 A typical drawbead used to limit slip between the blank and die.

Figure 1.3.5-2 Geometry and mesh for the deep drawing problem.

1-440

Static Stress/Displacement Analyses

Figure 1.3.5-3 Deformed shapes at various stages of the analysis.

1-441

Static Stress/Displacement Analyses

Figure 1.3.5-4 Strain distribution at the end of the deep drawing step.

1-442

Static Stress/Displacement Analyses

Figure 1.3.5-5 Punch force versus punch displacement.

1-443

Static Stress/Displacement Analyses

Figure 1.3.5-6 Deformed shape after unloading.

1-444

Static Stress/Displacement Analyses

Sample listings

1-445

Static Stress/Displacement Analyses

Listing 1.3.5-1 *HEADING DEEP DRAWING OF CYLINDRICAL CUP WITH CAX4R *RESTART,WRITE,FREQUENCY=25 *NODE 101, 181,0.1 301,0.0,0.00082 381,0.1,0.00082 *NGEN,NSET=BOT 101,181,2 *NGEN,NSET=TOP 301,381,2 *NSET,NSET=WRKPC BOT,TOP *NODE,NSET=DIE 100,0.1,-0.05 *NODE,NSET=PUNCH 200,0.,.05 *NODE,NSET=HOLDER 300,0.1,0.05 *NSET,NSET=TOOLS PUNCH,DIE,HOLDER *NSET,NSET=CENTER 101,301 *ELEMENT,TYPE=CAX4R,ELSET=BLANK 201,101,103,303,301 *ELGEN,ELSET=BLANK 201,40,2,2 *ELSET,ELSET=ALL BLANK, *SOLID SECTION,MATERIAL=STEEL,ORIENTATION=LOCAL, ELSET=BLANK *ORIENTATION,NAME=LOCAL 1.,0.,0.,0.,1.,0. 0,0., *MATERIAL,NAME=STEEL *ELASTIC 2.1E11,0.3 *PLASTIC,HARDENING=ISOTROPIC 0.91294E+08, 0.00000E+00 0.10129E+09, 0.21052E-03

1-446

Static Stress/Displacement Analyses

0.11129E+09, 0.52686E-03 0.12129E+09, 0.97685E-03 0.13129E+09, 0.15923E-02 0.14129E+09, 0.24090E-02 0.15129E+09, 0.34674E-02 0.16129E+09, 0.48120E-02 0.17129E+09, 0.64921E-02 0.18129E+09, 0.85618E-02 0.19129E+09, 0.11080E-01 0.20129E+09, 0.14110E-01 0.21129E+09, 0.17723E-01 0.22129E+09, 0.21991E-01 0.23129E+09, 0.26994E-01 0.24129E+09, 0.32819E-01 0.25129E+09, 0.39556E-01 0.26129E+09, 0.47301E-01 0.27129E+09, 0.56159E-01 0.28129E+09, 0.66236E-01 0.29129E+09, 0.77648E-01 0.30129E+09, 0.90516E-01 0.31129E+09, 0.10497E+00 0.32129E+09, 0.12114E+00 0.33129E+09, 0.13916E+00 0.34129E+09, 0.15919E+00 0.35129E+09, 0.18138E+00 0.36129E+09, 0.20588E+00 0.37129E+09, 0.23287E+00 0.38129E+09, 0.26252E+00 0.39129E+09, 0.29502E+00 0.40129E+09, 0.33054E+00 0.41129E+09, 0.36929E+00 0.42129E+09, 0.41147E+00 0.43129E+09, 0.45729E+00 0.44129E+09, 0.50696E+00 0.45129E+09, 0.56073E+00 0.46129E+09, 0.61881E+00 0.47129E+09, 0.68145E+00 0.48129E+09, 0.74890E+00 0.49129E+09, 0.82142E+00 0.50129E+09, 0.89928E+00 0.51129E+09, 0.98274E+00 0.52129E+09, 0.10721E+01 *ELSET,ELSET=EDIE,GENERATE

1-447

Static Stress/Displacement Analyses

231,279,2 *ELSET,ELSET=EHOLDER,GENERATE 241,279,2 *ELSET,ELSET=EPUNCH,GENERATE 201,249,2 *RIGID BODY,ANALYTICAL SURFACE=BSURF,REF NODE=100 *SURFACE,TYPE=SEGMENTS,NAME=BSURF START,0.05125,-0.060 LINE,0.05125,-0.005 CIRCL,0.05625,0.0,0.05625,-0.005 LINE,0.1,0.0 *RIGID BODY,ANALYTICAL SURFACE=DSURF,REF NODE=300 *SURFACE,TYPE=SEGMENTS,NAME=DSURF START,0.1,0.00082 LINE,0.05630,0.00082 CIRCL,0.05625,.00087,.05630,.00087 LINE,0.05625,.06 *RIGID BODY,ANALYTICAL SURFACE=FSURF,REF NODE=200 *SURFACE,TYPE=SEGMENTS,FILLET RADIUS=.013, NAME=FSURF START,0.05,0.060 LINE,0.05,2.250782E-3 CIRCL,0.0,0.001,0.0,1.001 LINE,-0.001,0.001 *SURFACE,NAME=ASURF EDIE,S1 *SURFACE,NAME=CSURF EHOLDER,S3 *SURFACE,NAME=ESURF EPUNCH,S3 *CONTACT PAIR,INTERACTION=ROUGH1 ASURF,BSURF *CONTACT PAIR,INTERACTION=ROUGH2 CSURF,DSURF *CONTACT PAIR,INTERACTION=ROUGH3 ESURF,FSURF *SURFACE INTERACTION,NAME=ROUGH1 *FRICTION 0.1, *SURFACE INTERACTION,NAME=ROUGH2 *FRICTION 0.1, *SURFACE INTERACTION,NAME=ROUGH3

1-448

Static Stress/Displacement Analyses

*FRICTION 0.25, *STEP,INC=10,NLGEOM, UNSYMM=YES PUSH THE BLANKHOLDER DOWN BY A PRESCRIBED DISPLACEMENT *STATIC 1.,1. *BOUNDARY CENTER,1,1 DIE,1,1 DIE,2,2 DIE,6,6 PUNCH,1,1 PUNCH,2,2 PUNCH,6,6 HOLDER,1,1 HOLDER,2,2,-1.75E-8 HOLDER,6,6 *MONITOR,NODE=200,DOF=2 *CONTACT CONTROLS,FRICTION ONSET=DELAY *PRINT,CONTACT=YES *NODE PRINT,NSET=TOOLS,FREQUENCY=100 COORD,U,RF *EL PRINT,ELSET=ALL,FREQUENCY=500 S,E *NODE FILE,NSET=TOOLS,FREQUENCY=10 U,RF *CONTACT FILE,SLAVE=ASURF,FREQUENCY=10 *CONTACT FILE,SLAVE=CSURF,FREQUENCY=10 *CONTACT FILE,SLAVE=ESURF,FREQUENCY=10 *END STEP *STEP,INC=10,NLGEOM APPLY PRESCRIBED FORCE ON BLANKHOLDER AND RELEASE DISPLACEMENT *STATIC 1.,1. *BOUNDARY,OP=NEW CENTER,1,1 DIE,1,1 DIE,2,2 DIE,6,6 PUNCH,1,1 PUNCH,2,2

1-449

Static Stress/Displacement Analyses

PUNCH,6,6 HOLDER,1,1 HOLDER,6,6 *CLOAD HOLDER,2,-100000. *END STEP *STEP,INC=500,NLGEOM MOVE THE PUNCH DOWN *STATIC .01,1.,1.E-6 *CONTROLS,ANALYSIS=DISCONTINUOUS *BOUNDARY,OP=NEW CENTER,1,1 DIE,1,1 DIE,2,2 DIE,6,6 PUNCH,1,1 PUNCH,2,2,-.06 PUNCH,6,6 HOLDER,1,1 HOLDER,6,6 *CLOAD HOLDER,2,-100000. *END STEP *STEP,INC=100,NLGEOM FIX ALL NODES AND REMOVE THE CONTACT SURFACES *STATIC 1.,1.,1.,1. *BOUNDARY,FIXED WRKPC,1,2 *MODEL CHANGE,TYPE=CONTACT PAIR,REMOVE ASURF,BSURF CSURF,DSURF ESURF,FSURF *CLOAD,OP=NEW HOLDER,2,0. *END STEP *STEP,INC=50,NLGEOM, UNSYMM=NO REPLACE THE BOUNDARY CONDITIONS BY THE REGULAR SET *STATIC .1,1.,1.E-6 *BOUNDARY,OP=NEW 181,2

1-450

Static Stress/Displacement Analyses

CENTER,1,1 *END STEP

1-451

Static Stress/Displacement Analyses

Listing 1.3.5-2 *HEADING DEEP DRAWING OF CYLINDRICAL CUP WITH SAX1 *RESTART,WRITE,FREQUENCY=25 *NODE 101, 181,0.1 *NGEN,NSET=BOT 101,181,2 *NSET,NSET=WRKPC,GENERATE 121,181,2 *NODE,NSET=DIE 100,0.,-0.05 *NODE,NSET=PUNCH 200,0.,.05 *NODE,NSET=HOLDER 300,0.,0.05 *NSET,NSET=TOOLS PUNCH,DIE,HOLDER *NSET,NSET=CENTER 101, *ELEMENT,TYPE=SAX1,ELSET=BLANK 201,101,121 202,121,123 *ELGEN,ELSET=BLANK 202,30,2,2 *SHELL SECTION,MATERIAL=STEEL,ELSET=BLANK .00082,5 *MATERIAL,NAME=STEEL *ELASTIC 2.1E11,0.3 *PLASTIC,HARDENING=ISOTROPIC 0.91294E+08, 0.00000E+00 0.10129E+09, 0.21052E-03 0.11129E+09, 0.52686E-03 0.12129E+09, 0.97685E-03 0.13129E+09, 0.15923E-02 0.14129E+09, 0.24090E-02 0.15129E+09, 0.34674E-02 0.16129E+09, 0.48120E-02 0.17129E+09, 0.64921E-02 0.18129E+09, 0.85618E-02

1-452

Static Stress/Displacement Analyses

0.19129E+09, 0.11080E-01 0.20129E+09, 0.14110E-01 0.21129E+09, 0.17723E-01 0.22129E+09, 0.21991E-01 0.23129E+09, 0.26994E-01 0.24129E+09, 0.32819E-01 0.25129E+09, 0.39556E-01 0.26129E+09, 0.47301E-01 0.27129E+09, 0.56159E-01 0.28129E+09, 0.66236E-01 0.29129E+09, 0.77648E-01 0.30129E+09, 0.90516E-01 0.31129E+09, 0.10497E+00 0.32129E+09, 0.12114E+00 0.33129E+09, 0.13916E+00 0.34129E+09, 0.15919E+00 0.35129E+09, 0.18138E+00 0.36129E+09, 0.20588E+00 0.37129E+09, 0.23287E+00 0.38129E+09, 0.26252E+00 0.39129E+09, 0.29502E+00 0.40129E+09, 0.33054E+00 0.41129E+09, 0.36929E+00 0.42129E+09, 0.41147E+00 0.43129E+09, 0.45729E+00 0.44129E+09, 0.50696E+00 0.45129E+09, 0.56073E+00 0.46129E+09, 0.61881E+00 0.47129E+09, 0.68145E+00 0.48129E+09, 0.74890E+00 0.49129E+09, 0.82142E+00 0.50129E+09, 0.89928E+00 0.51129E+09, 0.98274E+00 0.52129E+09, 0.10721E+01 *RIGID BODY,ANALYTICAL SURFACE=HOLDER,REF NODE=300 *SURFACE,TYPE=SEGMENTS,NAME=HOLDER, FILLET RADIUS=0.001 START,0.12,1.75E-8 LINE,0.05625,1.75E-8 LINE,0.05625,.06 *RIGID BODY,ANALYTICAL SURFACE=DIE,REF NODE=100 *SURFACE,TYPE=SEGMENTS,NAME=DIE, FILLET RADIUS=0.00541

1-453

Static Stress/Displacement Analyses

START,0.05125,-0.060 LINE,0.05125,0.0 LINE,0.12,0.0 *RIGID BODY,ANALYTICAL SURFACE=PUNCH,REF NODE=200 *SURFACE,TYPE=SEGMENTS,NAME=PUNCH, FILLET RADIUS=.01341 START,0.05,0.060 LINE,0.05,2.250782E-3 CIRCL,0.0,.0001,0.0,1.0001 LINE,-0.001,0.0001 ** ** Contact with holder ** *ELSET,ELSET=HOLD_CON,GENERATE 222,260,2 *SURFACE,NAME=HLD_SURF HOLD_CON,SPOS *CONTACT PAIR,INTERACTION=FRIC1 HLD_SURF,HOLDER *SURFACE INTERACTION,NAME=FRIC1 *SURFACE BEHAVIOR, PRESSURE-OVERCLOSURE=EXPONENTIAL 1.75E-8,4.5E6 *FRICTION 0.0, ** ** Contact with die ** *ELSET,ELSET=DIE_CON,GENERATE 212,260,2 *SURFACE,NAME=DIE_SURF DIE_CON,SNEG *CONTACT PAIR,INTERACTION=FRIC2 DIE_SURF,DIE *SURFACE INTERACTION,NAME=FRIC2 *FRICTION 0.0, ** ** Contact with punch ** *ELSET,ELSET=PUN_CON2,GENERATE 202,230,2 *SURFACE,NAME=PCH_SURF

1-454

Static Stress/Displacement Analyses

PUN_CON2,SPOS *CONTACT PAIR,INTERACTION=FRIC3 PCH_SURF,PUNCH *SURFACE INTERACTION,NAME=FRIC3 *FRICTION 0.0, *SURFACE,TYPE=NODE,NAME=PCH_PNT 101, *CONTACT PAIR,INTERACTION=FRIC4 PCH_PNT,PUNCH *SURFACE INTERACTION,NAME=FRIC4 *FRICTION 0.0, ** ** *STEP,INC=10, UNSYMM=YES PUSH THE BLANKHOLDER DOWN BY A PRESCRIBED DISPLACEMENT *STATIC 1.,1. *BOUNDARY CENTER,1,1 CENTER,6,6 DIE,1,1 DIE,2,2 DIE,6,6 PUNCH,1,1 PUNCH,2,2 PUNCH,6,6 HOLDER,1,1 HOLDER,2,2,-1.75E-8 HOLDER,6,6 *MONITOR,NODE=200,DOF=2 *PRINT,CONTACT=YES *NODE PRINT,NSET=TOOLS,FREQUENCY=100 COORD,U,RF *EL PRINT,ELSET=BLANK,FREQUENCY=500 S,E STH, *CONTACT PRINT,FREQUENCY=500 *CONTACT FILE,FREQUENCY=500 *NODE FILE,NSET=TOOLS,FREQUENCY=10 U,RF

1-455

Static Stress/Displacement Analyses

*END STEP *STEP,INC=10,NLGEOM, UNSYMM=YES APPLY PRESCRIBED FORCE ON BLANKHOLDER AND RELEASE DISPLACEMENT *STATIC 1.,1. *BOUNDARY,OP=NEW CENTER,1,1 CENTER,6,6 DIE,1,1 DIE,2,2 DIE,6,6 PUNCH,1,1 PUNCH,2,2 PUNCH,6,6 HOLDER,1,1 HOLDER,6,6 *CLOAD HOLDER,2,-100000. *CHANGE FRICTION,INTERACTION=FRIC2 *FRICTION 0.1, *CHANGE FRICTION,INTERACTION=FRIC1 *FRICTION 0.1, *CHANGE FRICTION,INTERACTION=FRIC3 *FRICTION 0.25, *END STEP *STEP,INC=500,NLGEOM,UNSYMM=YES MOVE THE PUNCH DOWN *STATIC .01,1.,1.E-6 *CONTROLS,ANALYSIS=DISCONTINUOUS *BOUNDARY,OP=NEW CENTER,1,1 CENTER,6,6 DIE,1,1 DIE,2,2 DIE,6,6 PUNCH,1,1 PUNCH,2,2,-.06 PUNCH,6,6

1-456

Static Stress/Displacement Analyses

HOLDER,1,1 HOLDER,6,6 *CLOAD HOLDER,2,-100000. *END STEP *STEP,INC=1,NLGEOM, UNSYMM=YES FIX ALL NODES AND REMOVE THE CONTACT SURFACES *STATIC 1.,1.,1.,1. *BOUNDARY,FIXED WRKPC,1,6 *BOUNDARY,FIXED CENTER,1,6 *MODEL CHANGE,TYPE=CONTACT PAIR,REMOVE HLD_SURF,HOLDER PCH_PNT,PUNCH PCH_SURF,PUNCH DIE_SURF,DIE *CLOAD,OP=NEW HOLDER,2,0. *END STEP *STEP,INC=50,NLGEOM, UNSYMM=YES REPLACE THE BOUNDARY CONDITIONS BY THE REGULAR SET *STATIC .1,1.,1.E-6 *BOUNDARY,OP=NEW CENTER,1,1 CENTER,6,6 181,2,2 *END STEP

1.3.6 Extrusion of a cylindrical metal bar with frictional heat generation Products: ABAQUS/Standard ABAQUS/Explicit This analysis illustrates how extrusion problems can be simulated with ABAQUS. In this particular problem the radius of an aluminum cylindrical bar is reduced 33% by an extrusion process. The generation of heat due to plastic dissipation inside the bar and the frictional heat generation at the workpiece/die interface are considered.

Geometry and model The bar has an initial radius of 100 mm and is 300 mm long. Figure 1.3.6-1 shows half of the cross-section of the bar, modeled with first-order axisymmetric elements ( CAX4T elements in

1-457

Static Stress/Displacement Analyses

ABAQUS/Standard and CAX4RT elements in ABAQUS/Explicit). The die is assumed to be rigid. In ABAQUS/Standard the die is modeled with CAX4T elements, which are made into an isothermal rigid body with the *RIGID BODY, ISOTHERMAL option. The *SURFACE option is used to define the slave surface on the outside of the bar and the master surface on the inside of the die. To model a die that has no sharp corners and is smooth in the transition region, the SMOOTH parameter on the *CONTACT PAIR option is set to 0.48. In ABAQUS/Explicit the die is modeled with either an analytical rigid surface or discrete rigid elements (RAX2). The analytical rigid surface is defined using the *RIGID BODY option in conjunction with the *SURFACE option. The FILLET RADIUS parameter on the *SURFACE option is set to 0.075 to remove sharp corners in the transition region of the die. For simplicity we do not model any heat transfer in the die--we simply fix the temperature of the rigid body reference node and assume that no heat is transmitted between the bar and the die. Half the heat dissipated as a result of friction is assumed to be conducted into the workpiece; the other half is conducted into the die. 90% of the nonrecoverable work because of plasticity is assumed to heat the work material. More realistic analysis would include thermal modeling of the die. The ABAQUS/Explicit simulations are performed both with and without adaptive meshing.

Material model and interface behavior The material model is chosen to reflect the response of a typical commercial purity aluminum alloy. The material is assumed to harden isotropically. The dependence of the flow stress on the temperature is included, but strain rate dependence is ignored. Instead, representative material data at a strain rate of 0.1 sec-1 are selected to characterize the flow strength. The interface is assumed to have no conductive properties. Coulomb friction is assumed for the mechanical behavior, with a friction coefficient of 0.1. The *GAP HEAT GENERATION option is used to specify the fraction, fg , of total heat generated by frictional dissipation that is transferred to the two bodies in contact. Half of this heat is conducted into the workpiece, and the other half is conducted into the die.

Boundary conditions, loading, and solution control In the first step the bar is moved to a position where contact is established and slipping of the workpiece against the die begins. In the second step the bar is extruded through the die to realize the extrusion process. This is accomplished by prescribing displacements to the nodes at the top of the bar. In the third step the contact elements are removed in preparation for the cool down portion of the simulation. In ABAQUS/Standard this is performed in a single step: the bar is allowed to cool down using film conditions, and deformation is driven by thermal contraction during the fourth step. In ABAQUS/Explicit the cool down simulation is broken into two steps: the first introduces viscous pressure to damp out dynamic effects and, thus, allow the bar to reach static equilibrium quickly; the balance of the cool down simulation is performed in a fifth step. The relief of residual stresses through creep is not analyzed in this example. In ABAQUS/Explicit mass scaling is used to reduce the computational cost of the analysis; nondefault

1-458

Static Stress/Displacement Analyses

hourglass control is used to control the hourglassing in the model. The default integral viscoelastic approach to hourglass control generally works best for problems where sudden dynamic loading occurs; a stiffness-based hourglass control is recommended for problems where the response is quasi-static. A combination of stiffness and viscous hourglass control is used in this problem. For purposes of comparison a second problem is also analyzed, in which the first two steps of the previous analysis are repeated in a static analysis with the adiabatic heat generation capability. The adiabatic analysis neglects heat conduction in the bar. Frictional heat generation must also be ignored in this case. This problem is analyzed only in ABAQUS/Standard.

Results and discussion The following discussion centers around the results obtained with ABAQUS/Standard. The results of the ABAQUS/Explicit simulation are in close agreement with those obtained with ABAQUS/Standard. Figure 1.3.6-2 shows the deformed configuration after Step 2 of the analysis. Figure 1.3.6-3 and Figure 1.3.6-4 show contour plots of plastic strain and temperature at the end of Step 2 for the fully coupled analysis. The plastic deformation is most severe near the surface of the workpiece, where plastic strains exceed 100%. The peak temperature also occurs at the surface of the workpiece because of plastic deformation and frictional heating. The peak temperature occurs immediately after the radial reduction zone of the die. This is expected for two reasons. First, the material that is heated by dissipative processes in the reduction zone will cool by conduction as the material progresses through the postreduction zone. Second, frictional heating is largest in the reduction zone because of the larger values of shear stress in that zone. The peak surface temperature is approximately 106°C (i.e., ¢T ¼ 86°C). If we ignore the zone of extreme distortion at the end of the bar, the temperature increase on the surface is not as large for the adiabatic analysis (Figure 1.3.6-5) because of the absence of frictional heating. The surface temperatures in this analysis are approximately 80°C. As expected, the temperature field contours for the adiabatic heating analysis, Figure 1.3.6-5, are very similar to the contours of plastic strain, Figure 1.3.6-3, from the thermally coupled analysis. As noted earlier, excellent agreement is observed between the results obtained with ABAQUS/Explicit and ABAQUS/Standard. Figure 1.3.6-6 compares the effects of adaptive meshing on the element quality. The results obtained with adaptive meshing show significantly reduced mesh distortion. The material point in the bar that experiences the largest temperature rise during the course of the simulation is indicated (node 2029 in the model without adaptivity). Figure 1.3.6-7 compares the results obtained with ABAQUS/Explicit for the temperature history of this material point against the same results obtained with ABAQUS/Standard.

Input files ABAQUS/Standard input files metalbarextrusion_coupled_fric.inp Thermally coupled extrusion with frictional heat generation.

1-459

Static Stress/Displacement Analyses

metalbarextrusion_adiab.inp Extrusion with adiabatic heat generation and without frictional heat generation. metalbarextrusion_stabil.inp Thermally coupled extrusion with frictional heat generation and automatic stabilization. ABAQUS/Explicit input files metalbarextrusion_x_cax4rt.inp Thermally coupled extrusion with frictional heat generation and without adaptive meshing; die modeled with an analytical rigid surface; kinematic mechanical contact. metalbarextrusion_xad_cax4rt.inp Thermally coupled extrusion with frictional heat generation and adaptive meshing; die modeled with an analytical rigid surface; kinematic mechanical contact. metalbarextrusion_xd_cax4rt.inp Thermally coupled extrusion with frictional heat generation and without adaptive meshing; die modeled with RAX2 elements; kinematic mechanical contact. metalbarextrusion_xp_cax4rt.inp Thermally coupled extrusion with frictional heat generation and without adaptive meshing; die modeled with an analytical rigid surface; penalty mechanical contact.

Figures Figure 1.3.6-1 Mesh and geometry: axisymmetric extrusion, ABAQUS/Standard.

Figure 1.3.6-2 Deformed configuration, Step 2, ABAQUS/Standard.

1-460

Static Stress/Displacement Analyses

Figure 1.3.6-3 Plastic strain contours, Step 2, thermally coupled analysis (frictional heat generation), ABAQUS/Standard.

Figure 1.3.6-4 Temperature contours, Step 2, thermally coupled analysis (frictional heat generation),

1-461

Static Stress/Displacement Analyses

ABAQUS/Standard.

Figure 1.3.6-5 Temperature contours, Step 2, adiabatic heat generation (without heat generation due to friction), ABAQUS/Standard.

1-462

Static Stress/Displacement Analyses

Figure 1.3.6-6 Deformed shape of the workpiece: without adaptive remeshing, left; with adaptive remeshing, right; ABAQUS/Explicit.

1-463

Static Stress/Displacement Analyses

Figure 1.3.6-7 Temperature history of node 2029 (nonadaptive result), ABAQUS/Explicit.

Sample listings

1-464

Static Stress/Displacement Analyses

Listing 1.3.6-1 *HEADING Extrusion *RESTART,WRITE,FREQUENCY=50 *NODE 1,0.,0. 61,0.,.3 2001,.1,0. 2061,.1,.3 *NODE, NSET=NREF 99999, 0.5 , 0.0 *NGEN,NSET=AXIS 1,61,1 *NGEN,NSET=OUTSIDE 2001,2061,1 *NFILL,NSET=ALL AXIS,OUTSIDE,20,100 *ELEMENT,TYPE=CAX4T,ELSET=WORK 1,1,201,203,3 *ELGEN,ELSET=WORK 1,30,2,1,10,200,100 *ELSET,ELSET=BOT,GENERATE 1,901,100 *ELSET,ELSET=SIDE,GENERATE 901,930,1 *ELSET,ELSET=TOP,GENERATE 30,930,100 ** *** Node & element definitions for die ** *NODE, NSET=CONTACT 10001, 0.250000000, -0.180000000 10002, 0.250000000, -0.114444000 10003, 0.250000000, -0.048888900 10004, 0.250000000, 0.016666700 10005, 0.250000000, 0.082222200 10006, 0.250000000, 0.147778000 10007, 0.250000000, 0.213333000 10008, 0.250000000, 0.278889000 10009, 0.250000000, 0.344444000 10010, 0.250000000, 0.410000000 10011, 0.188867000, -0.180000000

1-465

Static Stress/Displacement Analyses

10012, 0.189030000, -0.106122000 10013, 0.199098000, -0.041751700 10014, 0.199227000, 0.022784300 10015, 0.199356000, 0.087320200 10016, 0.199484000, 0.151856000 10017, 0.199613000, 0.216392000 10018, 0.199742000, 0.280928000 10019, 0.199871000, 0.345464000 10020, 0.200000000, 0.410000000 10021, 0.127733000, -0.180000000 10022, 0.127815000, -0.103061000 10023, 0.149548000, -0.045875800 10024, 0.149613000, 0.012106400 10025, 0.149677000, 0.070088700 10026, 0.149742000, 0.128071000 10027, 0.149806000, 0.186053000 10028, 0.149871000, 0.244035000 10029, 0.149935000, 0.302018000 10030, 0.149999000, 0.360000000 10031, 0.066600000, -0.180000000 10032, 0.066600000, -0.100000000 10033, 0.099999000, -0.050000000 10034, 0.099999000, 0.001428570 10035, 0.099999000, 0.052857100 10036, 0.099999000, 0.104286000 10037, 0.099999000, 0.155714000 10038, 0.099999000, 0.207143000 10039, 0.099999000, 0.258571000 10040, 0.099999000, 0.310000000 *ELEMENT, TYPE=CAX4T, ELSET=CONTACT 10001, 10001, 10002, 10012, 10011 10002, 10002, 10003, 10013, 10012 10003, 10003, 10004, 10014, 10013 10004, 10004, 10005, 10015, 10014 10005, 10005, 10006, 10016, 10015 10006, 10006, 10007, 10017, 10016 10007, 10007, 10008, 10018, 10017 10008, 10008, 10009, 10019, 10018 10009, 10009, 10010, 10020, 10019 10010, 10011, 10012, 10022, 10021 10011, 10012, 10013, 10023, 10022 10012, 10013, 10014, 10024, 10023 10013, 10014, 10015, 10025, 10024

1-466

Static Stress/Displacement Analyses

10014, 10015, 10016, 10026, 10025 10015, 10016, 10017, 10027, 10026 10016, 10017, 10018, 10028, 10027 10017, 10018, 10019, 10029, 10028 10018, 10019, 10020, 10030, 10029 10019, 10021, 10022, 10032, 10031 10020, 10022, 10023, 10033, 10032 10021, 10023, 10024, 10034, 10033 10022, 10024, 10025, 10035, 10034 10023, 10025, 10026, 10036, 10035 10024, 10026, 10027, 10037, 10036 10025, 10027, 10028, 10038, 10037 10026, 10028, 10029, 10039, 10038 10027, 10029, 10030, 10040, 10039 *SOLID SECTION, ELSET=CONTACT, MATERIAL=RIG *RIGID BODY, ELSET=CONTACT, ISOTHERMAL=YES, REF NODE=99999 *SOLID SECTION,ELSET=WORK,MATERIAL=METAL *MATERIAL,NAME=METAL *ELASTIC 6.9E10,.33 *PLASTIC ** STRAIN RATE APPX .1 ** 60.E6,0.0 ,20. 90.E6,.125 ,20. 113.E6,.25 ,20. 124.E6,.375 ,20. 133.E6,0.5 ,20. 165.E6,1.0 ,20. 166.E6,2.0 ,20. 60.E6,0. ,50. 80.E6,.125 ,50. 97.E6,.25 ,50. 110.E6,.375 ,50. 120.E6,0.5 ,50. 150.E6,1.0 ,50. 151.E6,2.0 ,50. 50.E6,0.0 ,100. 65.E6,.125 ,100, 81.5E6,.25 ,100. 91.E6,.375 ,100. 100.E6,0.5 ,100. 125.E6,1.0 ,100.

1-467

Static Stress/Displacement Analyses

126.E6,2.0 ,100. 45.E6,0.0 ,150. 63.E6,.125 ,150. 75.E6,.25 ,150. 89.E6,.5 ,150. 110.E6,1. ,150. 111.E6,2. ,150. *SPECIFIC HEAT 880., *DENSITY 2700., *CONDUCTIVITY 204.,0. 225.,300. *EXPANSION,ZERO=20.0 8.42E-5, *INELASTIC HEAT FRACTION .9, ** *** material properties are inconsequential *** for rigid elements *** *MATERIAL, NAME=RIG *ELASTIC 1.0E10,0.3 *SPECIFIC HEAT 880., *DENSITY 2700., *CONDUCTIVITY 204.,0. 225.,300. *EXPANSION,ZERO=20.0 8.42E-5, ** ** ** *NSET,NSET=TOP,GENERATE 61,2061,100 *NSET,NSET=ALL 1,2061,1 *INITIAL CONDITIONS,TYPE=TEMPERATURE ALL,20.

1-468

Static Stress/Displacement Analyses

** *** surface definitions *** ** *ELSET, ELSET=INDIE, GEN 10019,10027,1 *ELSET, ELSET=BOTDIE, GEN 10001,10019,9 *SURFACE, NAME=RIGID, TYPE=ELEMENT INDIE, S3 BOTDIE,S4 *SURFACE, NAME=DEF1, TYPE=ELEMENT SIDE, S2 *SURFACE, NAME=DEF2, TYPE=ELEMENT BOT, S1 ** *** Interaction definitions ** *SURFACE INTERACTION, NAME=INTER *FRICTION 0.1 *GAP HEAT GENERATION 1.0, ** *** Contact pair definitions ** *CONTACT PAIR, INTERACTION=INTER, SMOOTH=0.48 DEF1, RIGID DEF2, RIGID ** *** elset for output purposes ** *ELSET,ELSET=EFILEOUT BOT,SIDE,TOP ** *** step 1 ** *STEP,INC=100,AMPLITUDE=RAMP,NLGEOM, UNSYMM=YES STABILIZE WORKPIECE INSIDE DIE *COUPLED TEMPERATURE-DISPLACEMENT,DELTMX=100. .1,1. *BOUNDARY NREF, 1, 2, 0.0 NREF, 6, 6, 0.0

1-469

Static Stress/Displacement Analyses

NREF,11,11,20.0 AXIS,1,1,0.0 TOP,2,2,-.000125 ALL,11,11,20.0 **2061,1,1,0.0 *PRINT,CONTACT=YES *NODE PRINT,FREQUENCY=10 U RF NT RFL *ENERGY PRINT,FREQUENCY=1 *END STEP ** *** step 2 ** *STEP,INC=800,AMPLITUDE=RAMP,NLGEOM, UNSYMM=YES EXTRUSION *COUPLED TEMPERATURE-DISPLACEMENT,DELTMX=100. .1,10. *BOUNDARY,OP=NEW NREF, 1, 2, 0.0 NREF, 6, 6, 0.0 NREF, 11,11,20.0 AXIS,1,1,0.0 TOP,2,2,-.25 **2061,1,1,0.0 *PRINT,CONTACT=YES *EL PRINT,ELSET=CONTACT,FREQUENCY=10 S E *EL FILE,FREQUENCY=999,ELSET=EFILEOUT S,E PE, *NSET,NSET=NFILEOUT AXIS,OUTSIDE,TOP *NODE FILE,FREQUENCY=999,NSET=NFILEOUT NT, *NODE PRINT,FREQUENCY=10 U RF NT RFL

1-470

Static Stress/Displacement Analyses

*ENERGY PRINT,FREQUENCY=1 *END STEP ** *** step 3 ** *STEP,INC=200,AMPLITUDE=RAMP,NLGEOM, UNSYMM=YES REMOVE CONTACT PAIRS *COUPLED TEMPERATURE-DISPLACEMENT,DELTMX=100. .1,.1, *MODEL CHANGE,REMOVE, TYPE=CONTACT PAIR DEF1, RIGID DEF2, RIGID *PRINT,CONTACT=YES *NODE PRINT,FREQUENCY=10 U RF NT RFL *EL FILE,FREQUENCY=0 *NODE FILE,FREQUENCY=0 *ENERGY PRINT,FREQUENCY=1 *END STEP ** *** step 4 ** *STEP,INC=200,AMPLITUDE=RAMP,NLGEOM, UNSYMM=YES LET WORKPIECE COOL DOWN *COUPLED TEMPERATURE-DISPLACEMENT,DELTMX=100. 100.,10000., *FILM BOT,F1,20.,10. TOP,F3,20.,10. SIDE,F2,20.,10. *PRINT,CONTACT=YES *NODE PRINT,FREQUENCY=10 U RF NT RFL *ENERGY PRINT,FREQUENCY=1 *EL FILE,FREQUENCY=999,ELSET=EFILEOUT S,E PE,

1-471

Static Stress/Displacement Analyses

*NODE FILE,FREQUENCY=999,NSET=NFILEOUT NT, *END STEP

1-472

Static Stress/Displacement Analyses

Listing 1.3.6-2 *HEADING Extrusion - adiabatic analysis *RESTART,WRITE,FREQUENCY=50 *NODE 1,0.,0. 61,0.,.3 2001,.1,0. 2061,.1,.3 *NODE, NSET=NREF 99999, 0.5, 0.0 ** *NGEN,NSET=AXIS 1,61,1 *NGEN,NSET=OUTSIDE 2001,2061,1 *NFILL,NSET=ALL AXIS,OUTSIDE,20,100 *ELEMENT,TYPE=CAX4,ELSET=WORK 1,1,201,203,3 *ELGEN,ELSET=WORK 1,30,2,1,10,200,100 *ELSET,ELSET=BOT,GENERATE 1,901,100 *ELSET,ELSET=SIDE,GENERATE 901,930,1 *ELSET,ELSET=TOP,GENERATE 30,930,100 ** *** Node & element definitions for die ** *NODE, NSET=CONTACT 10001, 0.250000000, -0.180000000 10002, 0.250000000, -0.114444000 10003, 0.250000000, -0.048888900 10004, 0.250000000, 0.016666700 10005, 0.250000000, 0.082222200 10006, 0.250000000, 0.147778000 10007, 0.250000000, 0.213333000 10008, 0.250000000, 0.278889000 10009, 0.250000000, 0.344444000 10010, 0.250000000, 0.410000000

1-473

Static Stress/Displacement Analyses

10011, 0.188867000, -0.180000000 10012, 0.189030000, -0.106122000 10013, 0.199098000, -0.041751700 10014, 0.199227000, 0.022784300 10015, 0.199356000, 0.087320200 10016, 0.199484000, 0.151856000 10017, 0.199613000, 0.216392000 10018, 0.199742000, 0.280928000 10019, 0.199871000, 0.345464000 10020, 0.200000000, 0.410000000 10021, 0.127733000, -0.180000000 10022, 0.127815000, -0.103061000 10023, 0.149548000, -0.045875800 10024, 0.149613000, 0.012106400 10025, 0.149677000, 0.070088700 10026, 0.149742000, 0.128071000 10027, 0.149806000, 0.186053000 10028, 0.149871000, 0.244035000 10029, 0.149935000, 0.302018000 10030, 0.149999000, 0.360000000 10031, 0.066600000, -0.180000000 10032, 0.066600000, -0.100000000 10033, 0.099999000, -0.050000000 10034, 0.099999000, 0.001428570 10035, 0.099999000, 0.052857100 10036, 0.099999000, 0.104286000 10037, 0.099999000, 0.155714000 10038, 0.099999000, 0.207143000 10039, 0.099999000, 0.258571000 10040, 0.099999000, 0.310000000 *ELEMENT, TYPE=CAX4, ELSET=CONTACT 10001, 10001, 10002, 10012, 10011 10002, 10002, 10003, 10013, 10012 10003, 10003, 10004, 10014, 10013 10004, 10004, 10005, 10015, 10014 10005, 10005, 10006, 10016, 10015 10006, 10006, 10007, 10017, 10016 10007, 10007, 10008, 10018, 10017 10008, 10008, 10009, 10019, 10018 10009, 10009, 10010, 10020, 10019 10010, 10011, 10012, 10022, 10021 10011, 10012, 10013, 10023, 10022 10012, 10013, 10014, 10024, 10023

1-474

Static Stress/Displacement Analyses

10013, 10014, 10015, 10025, 10024 10014, 10015, 10016, 10026, 10025 10015, 10016, 10017, 10027, 10026 10016, 10017, 10018, 10028, 10027 10017, 10018, 10019, 10029, 10028 10018, 10019, 10020, 10030, 10029 10019, 10021, 10022, 10032, 10031 10020, 10022, 10023, 10033, 10032 10021, 10023, 10024, 10034, 10033 10022, 10024, 10025, 10035, 10034 10023, 10025, 10026, 10036, 10035 10024, 10026, 10027, 10037, 10036 10025, 10027, 10028, 10038, 10037 10026, 10028, 10029, 10039, 10038 10027, 10029, 10030, 10040, 10039 *SOLID SECTION, ELSET=CONTACT, MATERIAL=RIG *RIGID BODY, ELSET=CONTACT, REF NODE=99999 *SOLID SECTION,ELSET=WORK,MATERIAL=METAL *MATERIAL,NAME=METAL *ELASTIC 6.9E10,.33 *PLASTIC ** STRAIN RATE APPX .1 ** 60.E6,0.0 ,20. 90.E6,.125 ,20. 113.E6,.25 ,20. 124.E6,.375 ,20. 133.E6,0.5 ,20. 165.E6,1.0 ,20. 166.E6,2.0 ,20. 60.E6,0. ,50. 80.E6,.125 ,50. 97.E6,.25 ,50. 110.E6,.375 ,50. 120.E6,0.5 ,50. 150.E6,1.0 ,50. 151.E6,2.0 ,50. 50.E6,0.0 ,100. 65.E6,.125 ,100, 81.5E6,.25 ,100. 91.E6,.375 ,100. 100.E6,0.5 ,100. 125.E6,1.0 ,100.

1-475

Static Stress/Displacement Analyses

126.E6,2.0 ,100. 45.E6,0.0 ,150. 63.E6,.125 ,150. 75.E6,.25 ,150. 89.E6,.5 ,150. 110.E6,1. ,150. 111.E6,2. ,150. *SPECIFIC HEAT 880., *DENSITY 2700., *CONDUCTIVITY 204.,0. 225.,300. *EXPANSION,ZERO=20.0 8.42E-5, *INELASTIC HEAT FRACTION .9, *NSET,NSET=TOP,GENERATE 61,2061,100 *NSET,NSET=ALL 1,2061,1 ** *** material properties are inconsequential *** for rigid elements *** *MATERIAL, NAME=RIG *ELASTIC 1.0E10,0.3 *PLASTIC ** STRAIN RATE APPX .1 ** 60.E6,0.0 ,20. 90.E6,.125 ,20. 113.E6,.25 ,20. 124.E6,.375 ,20. 133.E6,0.5 ,20. 165.E6,1.0 ,20. 166.E6,2.0 ,20. 60.E6,0. ,50. 80.E6,.125 ,50. 97.E6,.25 ,50. 110.E6,.375 ,50. 120.E6,0.5 ,50.

1-476

Static Stress/Displacement Analyses

150.E6,1.0 ,50. 151.E6,2.0 ,50. 50.E6,0.0 ,100. 65.E6,.125 ,100, 81.5E6,.25 ,100. 91.E6,.375 ,100. 100.E6,0.5 ,100. 125.E6,1.0 ,100. 126.E6,2.0 ,100. 45.E6,0.0 ,150. 63.E6,.125 ,150. 75.E6,.25 ,150. 89.E6,.5 ,150. 110.E6,1. ,150. 111.E6,2. ,150. *SPECIFIC HEAT 880., *DENSITY 2700., *CONDUCTIVITY 204.,0. 225.,300. *EXPANSION,ZERO=20.0 8.42E-5, ** *** surface definitions *** ** *ELSET, ELSET=INDIE, GEN 10019,10027,1 *ELSET, ELSET=BOTDIE, GEN 10001,10019,9 *SURFACE, NAME=RIGID, TYPE=ELEMENT INDIE, S3 BOTDIE,S4 *SURFACE, NAME=DEF1, TYPE=ELEMENT SIDE, S2 *SURFACE, NAME=DEF2, TYPE=ELEMENT BOT, S1 ** *** Interaction definitions ** *SURFACE INTERACTION, NAME=INTER *FRICTION

1-477

Static Stress/Displacement Analyses

0.1 *GAP HEAT GENERATION 1.0, ** *** Contact pair definitions ** *CONTACT PAIR, INTERACTION=INTER, SMOOTH=0.48 DEF1, RIGID DEF2, RIGID *INITIAL CONDITIONS,TYPE=TEMPERATURE ALL,20. *NSET, NSET=NALL CONTACT,ALL ** ** step 1 ** *STEP,INC=100,AMPLITUDE=RAMP,NLGEOM, UNSYMM=YES STABILIZE WORKPIECE INSIDE DIE *STATIC,ADIABATIC .1,1. *BOUNDARY NREF,1,2,0.0 NREF,6,6,0.0 AXIS,1,1,0.0 TOP,2,2,-.000125 *PRINT,CONTACT=YES *EL PRINT,ELSET=CONTACT,FREQUENCY=10 S E MISES PE *NODE PRINT,FREQUENCY=10 U RF *ENERGY PRINT,FREQUENCY=1 *OUTPUT, FIELD, FREQ=10 *ELEMENT OUTPUT, ELSET=WORK TEMP S E PE PEEQ *NODE OUTPUT, NSET=ALL

1-478

Static Stress/Displacement Analyses

U *END STEP ** *** step 2 ** *STEP,INC=800,AMPLITUDE=RAMP,NLGEOM, UNSYMM=YES EXTRUSION *STATIC,ADIABATIC .1,10. *BOUNDARY,OP=NEW NREF,1,2,0.0 NREF,6,6,0.0 AXIS,1,1,0.0 TOP,2,2,-.25 *PRINT,CONTACT=YES *EL PRINT,ELSET=CONTACT,FREQUENCY=10 S,E *NODE PRINT,FREQUENCY=10 U RF *EL FILE,FREQUENCY=999 S E PE TEMP *OUTPUT, FIELD, FREQ=10 *ELEMENT OUTPUT, ELSET=WORK TEMP S E PE PEEQ *NODE OUTPUT, NSET=ALL U *ENERGY PRINT,FREQUENCY=1 *END STEP

1-479

Static Stress/Displacement Analyses

Listing 1.3.6-3 *HEADING EXTRUSION OF A BAR WITH FRICTIONAL HEAT GENERATION EXPLICIT [CAX4RT] *NODE 1,0.,0. 61,0.,.3 2001,.1,0. 2061,.1,.3 *NGEN,NSET=AXIS 1,61,1 *NGEN,NSET=OUTSIDE 2001,2061,1 *NFILL,NSET=ALL AXIS,OUTSIDE,20,100 *NSET, NSET=TEMP 2025, 2027, 2029, 2031 *ELEMENT, TYPE=CAX4RT, ELSET=WORK 1,1,201,203,3 *ELGEN,ELSET=WORK 1,30,2,1,10,200,100 *ELSET,ELSET=BOT,GENERATE 1,901,100 *ELSET,ELSET=SIDE,GENERATE 901,930,1 *ELSET,ELSET=TOP,GENERATE 30,930,100 *SOLID SECTION,ELSET=WORK,MATERIAL=METAL, CONTROLS=HGLASS *SECTION CONTROLS,NAME=HGLASS,HOURGLASS=COMBINED *MATERIAL,NAME=METAL *ELASTIC 6.9E10,.33 *PLASTIC ** STRAIN RATE APPX .1 ** 60.E6,0.0 ,20. 90.E6,.125 ,20. 113.E6,.25 ,20. 124.E6,.375 ,20. 133.E6,0.5 ,20. 165.E6,1.0 ,20. 166.E6,2.0 ,20.

1-480

Static Stress/Displacement Analyses

60.E6,0. ,50. 80.E6,.125 ,50. 97.E6,.25 ,50. 110.E6,.375 ,50. 120.E6,0.5 ,50. 150.E6,1.0 ,50. 151.E6,2.0 ,50. 50.E6,0.0 ,100. 65.E6,.125 ,100, 81.5E6,.25 ,100. 91.E6,.375 ,100. 100.E6,0.5 ,100. 125.E6,1.0 ,100. 126.E6,2.0 ,100. 45.E6,0.0 ,150. 63.E6,.125 ,150. 75.E6,.25 ,150. 89.E6,.5 ,150. 110.E6,1. ,150. 111.E6,2. ,150. *SPECIFIC HEAT 880., *DENSITY 2700., *CONDUCTIVITY 204.,0. 225.,300. *EXPANSION,ZERO=20.0 8.42E-5, *INELASTIC HEAT FRACTION .9, *NODE, NSET=REFNODE 9999, 0.2, 0.0, 0.0 *ELEMENT, TYPE=HEATCAP, ELSET=CAP 99001,9999 *HEATCAP, ELSET=CAP 1., ** *NSET,NSET=TOP,GENERATE 61,2061,100 *NSET,NSET=ALL 1,2061,1 *INITIAL CONDITIONS,TYPE=TEMPERATURE

1-481

Static Stress/Displacement Analyses

ALL,20. *NSET,NSET=NFILEOUT AXIS,OUTSIDE,TOP *ELSET,ELSET=EFILEOUT BOT,SIDE,TOP *SURFACE, TYPE=S, NAME=DIE, FILLET=0.075 START,.25,-.18 LINE,.0866,-.18 LINE,.0666,-.18 LINE,.0666,-.17 LINE,.0666,-.15 LINE,.0666,-.1 LINE,.099999,-.05 LINE,.099999,0.0 LINE,.099999,.3 LINE,.099999,.31 LINE,.2,.41 *SURFACE,TYPE=ELEMENT, NAME=BAR BOT, S1 SIDE, S2 *RIGID BODY, REFNODE=9999, ISOTHERMAL=YES, ANALYTICAL SURFACE =DIE *STEP STABILIZE WORKPIECE INSIDE DIE *DYNAMIC TEMPERATURE-DISPLACEMENT, EXPLICIT ,1. *FIXED MASS SCALING, ELSET=WORK, FACTOR=1.E5 *CONTACT PAIR, INTERACTION=CONTACT BAR, DIE *SURFACE INTERACTION, NAME=CONTACT *FRICTION 0.1 , *GAP HEAT GENERATION 1.0,0.5 *BOUNDARY, TYPE=VELOCITY REFNODE,1,6,0.0 AXIS,1,1,0.0 TOP,2,2,-.000125 2061,1,1,0.0 *BOUNDARY ALL,11,11,20.0 REFNODE,11,11,20.0 *OUTPUT,FIELD,NUM=1,VAR=PRESELECT

1-482

Static Stress/Displacement Analyses

*OUTPUT,HISTORY,FREQ=50 *NODE OUTPUT, NSET=TEMP NT, *END STEP ** *STEP EXTRUSION *DYNAMIC TEMPERATURE-DISPLACEMENT, EXPLICIT ,10. *FIXED MASS SCALING, ELSET=WORK, FACTOR=1.E5 *BOUNDARY,OP=NEW, TYPE=VELOCITY REFNODE,1,6,0.0 AXIS,1,1,0.0 TOP,2,2,-.0249875 2061,1,1,0.0 *BOUNDARY,OP=NEW REFNODE,11,11,20.0 *FILE OUTPUT, NUM=1 *EL FILE,,ELSET=EFILEOUT S,E PE, *NODE FILE,NSET=NFILEOUT NT, *EL FILE,ELSET=EFILEOUT S,E PE, *NODE FILE,NSET=NFILEOUT NT, *OUTPUT, HISTORY, TIME INTERVAL=35.0 *NODE OUTPUT, NSET=TEMP NT, *OUTPUT, FIELD,NUM=4 *ELEMENT OUTPUT,ELSET=WORK S,PEEQ, TEMP, HFL *NODE OUTPUT NT, U *END STEP ** *STEP REMOVE CONTACT *DYNAMIC TEMPERATURE-DISPLACEMENT, EXPLICIT ,.1 *FIXED MASS SCALING, ELSET=WORK, FACTOR=1.E5

1-483

Static Stress/Displacement Analyses

*CONTACT PAIR, OP=DELETE BAR,DIE *BOUNDARY,OP=NEW, TYPE=VELOCITY REFNODE,1,6,0.0 AXIS,1,1,0.0 TOP,2,2,0.0 *END STEP ** *STEP LET WORKPIECE COOL DOWN--I (ADD VISCOUS PRESSURE) *DYNAMIC TEMPERATURE-DISPLACEMENT, EXPLICIT ,10. *FIXED MASS SCALING,ELSET=WORK,FACTOR=1.E6 *AMPLITUDE, NAME=RAMP,TIME=TOTAL TIME 0.0,0.0,11.1,0.0,10011.1,1.0 *FILM, AMP=RAMP BOT,F1,20.,10. TOP,F3,20.,10. SIDE,F2,20.,10. ** *DLOAD WORK,VP1,1.E8 WORK,VP2,1.E8 WORK,VP3,1.E8 WORK,VP4,1.E8 ** *FILE OUTPUT, NUM=2 *EL FILE,ELSET=EFILEOUT S,E PE, *NODE FILE,NSET=NFILEOUT NT, *OUTPUT, HISTORY, TIME INTERVAL=35.0 *NODE OUTPUT, NSET=TEMP NT, *OUTPUT, FIELD,NUM=2 *ELEMENT OUTPUT,ELSET=WORK S,PEEQ, TEMP, HFL *NODE OUTPUT NT, U *END STEP *STEP LET WORKPIECE COOL DOWN--II

1-484

Static Stress/Displacement Analyses

*DYNAMIC TEMPERATURE-DISPLACEMENT, EXPLICIT ,9990. *FIXED MASS SCALING,ELSET=WORK,FACTOR=4.E9 ** *DLOAD,OP=NEW ** *END STEP

1.3.7 Rolling of thick plates Product: ABAQUS/Explicit Hot rolling is a basic manufacturing technique used to transform preformed shapes into a form suitable for further processing. Rolling processes can be divided into different categories, depending on the complexity of metal flow and on the geometry of the rolled product. Finite element computations are used increasingly to analyze the elongation and spread of the material during rolling (Kobayashi, 1989). Although the forming process is often carried out at low roll speed, this example shows that a considerable amount of engineering information can be obtained by using the explicit dynamics procedure in ABAQUS/Explicit to model the process. The rolling process is first investigated using plane strain computations. These results are used to choose the modeling parameters associated with the more computationally expensive three-dimensional analysis. Since rolling is normally performed at relatively low speeds, it is natural to assume that static analysis is the proper modeling approach. Typical rolling speeds (surface speed of the roller) are on the order of 1 m/sec. At these speeds inertia effects are not significant, so the response--except for rate effects in the material behavior--is quasi-static. Representative rolling geometries generally require three-dimensional modeling, resulting in very large models, and include nonlinear material behavior and discontinuous effects--contact and friction. Because the problem size is large and the discontinuous effects dominate the solution, the explicit dynamics approach is often less expensive computationally and more reliable than an implicit quasi-static solution technique. The computer time involved in running a simulation using explicit time integration with a given mesh is directly proportional to the time period of the event. This is because numerical stability considerations restrict the time increment to µ

¢t ∙ min L

el

r

½ ¸ + 2¹

¶

;

where the minimum is taken over all elements in the mesh, Lel is a characteristic length associated with an element, ½ is the density of the material in the element, and ¸ and ¹ are the effective Lamé's constants for the material in the element. Since this condition effectively means that the time increment can be no larger than the time required to propagate a stress wave across an element, the computer time involved in running a quasi-static analysis can be very large. The cost of the simulation is directly proportional to the number of time increments required, n = T =¢t if ¢t remains constant, where T is

1-485

Static Stress/Displacement Analyses

the time period of the event being simulated. ( ¢t will not remain constant in general, since element distortion will change Lel and nonlinear material response will change the effective Lamé constants and density. But the assumption is acceptable for the purposes of this discussion.) Thus,

n = T max

Ã

1 Lel

s

¸ + 2¹ ½

!

:

To reduce n, we can speed up the simulation compared to the time of the actual process; that is, we can artificially reduce the time period of the event, T . This will introduce two possible errors. If the simulation speed is increased too much, the inertia forces will be larger and will change the predicted response (in an extreme case the problem will exhibit wave propagation response). The only way to avoid this error is to find a speed-up that is not too large. The other error is that some aspects of the problem other than inertia forces--for example, material behavior--may also be rate dependent. This implies that we cannot change the actual time period of the event being modeled. But we can see a simple equivalent--artificially increasing the material density, ½, by a factor f 2 reduces n to n=f , just as decreasing T to T =f . This concept, which is called "mass scaling," reduces the ratio of the event time to the time for wave propagation across an element while leaving the event time fixed, thus allowing treatment of rate-dependent material and other behaviors, while having exactly the same effect on inertia forces as speeding up the time of simulation. Mass scaling is attractive because it allows us to treat rate-dependent quasi-static problems efficiently. But we cannot take it too far or we allow the inertia forces to dominate and, thus, change the solution. This example illustrates the use of mass scaling and shows how far we can take it for a practical case.

Problem description A steel plate of an original square cross-section of 40 mm by 40 mm and a length of 92 mm is reduced to a 30 mm height by rolling through one roll stand. The radius of the rollers is 170 mm. The single roller in the model (taking advantage of symmetry) is assumed to be rigid and is modeled as an analytical rigid surface. The isotropic hardening yield curve of the steel is taken from Kopp and Dohmen (1990). Isotropic elasticity is assumed, with Young's modulus of 150 GPa and Poisson's ratio of 0.3. The strain hardening is described using 11 points on the yield stress versus plastic strain curve, with an initial yield stress of 168.2 MPa and a maximum yield stress of 448.45 MPa. No rate dependence or temperature dependence is taken into account. Coulomb friction is assumed between the roller and the plate, with a friction coefficient of 0.3. Friction plays an important role in this process, as it is the only mechanism by which the plate is pulled through the roll stand. If the friction coefficient is too low, the plate cannot be drawn through the roll stand. Initially, when a point on the surface of the plate has just made contact with the roller, the roller surface is moving faster than the point on the surface of the plate and there is a relative slip between the two surfaces. As the point on the plate is drawn into the process zone under the roller, it moves faster and, after a certain distance, sticks to the roller. As the point on the surface of the plate is pushed out of the process zone, it picks up speed and begins to move faster than the roller. This causes slip in the opposite direction before the point on the surface of the sheet finally loses contact with the roller.

1-486

Static Stress/Displacement Analyses

For plane strain computations a half-symmetry model with CPE4R elements is used. For the three-dimensional computations a one-quarter symmetry model with C3D8R elements is used. The roller is modeled with analytical rigid surfaces for both the two-dimensional and three-dimensional cases. For quasi-static rolling problems perfectly round analytical surfaces can provide a more accurate representation of the revolved roller geometry, improve computational efficiency, and reduce noise when compared to element-based rigid surfaces. The roller is rotated through 32° at a constant angular velocity of 1 revolution per second (6.28 rad/sec), which corresponds to a roller surface speed of 1.07 m/sec. The plate is given an initial velocity in the global x-direction. The initial velocity is chosen to match the x-component of velocity of the roller at the point of first contact. This choice of initial velocity results in a net acceleration of zero in the x-direction at the point of contact and minimizes the initial impact between the plate and the roller. This minimizes the initial transient disturbance. In each analysis performed in this example, the *FIXED MASS SCALING option is used to scale the masses of all the elements in the model by factors of either 110, 2758, or 68962. These scaling factors translate into effective roller surface speeds of 11.2 m/sec, 56.1 m/sec, and 280.5 m/sec. An alternative, but equivalent, means of mass scaling could be achieved by scaling the actual density (entered on the *DENSITY option) by the aforementioned factors. The element formulation for the two-dimensional (using CPE4R elements) and three-dimensional (using C3D8R elements) analyses uses the pure stiffness form of hourglass control (HOURGLASS=STIFFNESS). The element formulation is selected using the *SECTION CONTROLS option. In addition, the three-dimensional model (using C3D8R elements) uses the centroidal (KINEMATIC SPLIT=CENTROID) kinematic formulation. These options are economical yet provide the necessary level of accuracy for this class of problems. Other cases using more computationally intensive element formulations are included for comparison: analyses that use the default section control options and a mass scaling factor of 2758 and two- and three-dimensional analyses that use an element formulation intermediate in computational cost between the two previous formulations. For the sole purpose of testing the performances of the modified triangular and tetrahedral elements, the problem is also analyzed in two dimensions using CPE6M elements and in three dimensions using C3D10M elements.

Results and discussion Table 1.3.7-1 shows the effective rolling speeds and the relative CPU cost of the cases using the element formulations recommended for this problem. The relative costs are normalized with respect to the CPU time for the two-dimensional model (using CPE4R elements) with the intermediate mass scaling value. In addition, Table 1.3.7-2 compares the relative CPU cost and accuracy between the different element formulations of the solid elements using the intermediate mass scaling value.

Plane strain rolling (CPE4R elements) A plane strain calculation allows the user to resolve a number of modeling questions in two dimensions before attempting a more expensive three-dimensional calculation. In particular, an acceptable effective mass scaling factor for running the transient dynamics procedure can be

1-487

Static Stress/Displacement Analyses

determined. Figure 1.3.7-1 through Figure 1.3.7-3 show contours of equivalent plastic strain for the three mass scaling factors using the STIFFNESS hourglass control. Figure 1.3.7-4 through Figure 1.3.7-6 show contours of shear stress for the same cases. These results show that there is very little difference between the lowest and the intermediate mass scaling cases. All the results are in good agreement with the quasi-static analysis results obtained with ABAQUS. The results of the largest mass scaling case show pronounced dynamic effects. Table 1.3.7-1 shows the relative run time of the quasi-static calculation, and Table 1.3.7-2 compares the different element formulations at the same level of mass scaling. The intermediate mass scaling case gives essentially the same results as the quasi-static calculation, using about one-seventh of the CPU time. In addition to the savings provided by the mass scaling option, more computational savings are achieved using the chosen element formulation of STIFFNESS hourglass control; the results for this formulation compare well to the results for the computationally more expensive element formulations.

Three-dimensional rolling (C3D8R elements) We have ascertained with the two-dimensional calculations that mass scaling by a factor of 2758 gives results that are essentially the same as a quasi-static solution. Figure 1.3.7-7 shows the distribution of the equivalent plastic strain of the deformed sheet for the three-dimensional case using the CENTROID kinematic and STIFFNESS hourglass section control options. Figure 1.3.7-8 shows the distribution of the equivalent plastic strain of the deformed sheet for the three-dimensional case using the default section control options ( AVERAGE STRAIN kinematic and RELAX STIFFNESS hourglass). Table 1.3.7-1 compares this three-dimensional case with the plane strain and quasi-static cases, and Table 1.3.7-2 compares the three different three-dimensional element formulations included here with the two-dimensional cases at the same level of mass scaling. The accuracy for all three element formulations tested is very similar for this problem, but significant savings are realized in the three-dimensional analyses when using more economical element formulations.

Analyses using CPE6M and C3D10M elements The total number of nodes in the CPE6M model is identical to the number in the CPE4R model. The number of nodes in the C3D10M model is 3440 (compared to 3808 in the C3D8R model). The analyses using the CPE6M and C3D10M elements use a mass scaling factor of 2758. Figure 1.3.7-9 and Figure 1.3.7-10 show the distribution of the equivalent plastic strain of the plate for the two-dimensional and three-dimensional cases, respectively. The results are in reasonably good agreement with other element formulations. However, the CPU costs are higher since the modified triangular and tetrahedral elements use more than one integration point in each element and the stable time increment size is somewhat smaller than in analyses that use reduced integration elements with the same node count. For the mesh refinements used in this problem, the CPE6M model takes about twice the CPU time as the CPE4R model, while the C3D10M model takes about 5.75 times the CPU time as the C3D8R model.

Input files roll2d330_anl_ss.inp

1-488

Static Stress/Displacement Analyses

Two-dimensional case (using CPE4R elements) with a mass scaling factor of 2758 and the STIFFNESS hourglass control. roll3d330_rev_anl_css.inp Three-dimensional case (using C3D8R elements) with a mass scaling factor of 2758; an analytical rigid surface of TYPE=REVOLUTION; and the CENTROID kinematic and STIFFNESS hourglass section control options. roll2d66_anl_ss.inp Two-dimensional case (using CPE4R elements) with a mass scaling factor of 110 using the STIFFNESS hourglass control. roll2d330_anl_cs.inp Two-dimensional case (using CPE4R elements) with a mass scaling factor of 2758 using the COMBINED hourglass control. roll2d330_cs.inp Two-dimensional case (using CPE4R elements) with a mass scaling factor of 2758 using the COMBINED hourglass control and rigid elements. roll3d330_css.inp Three-dimensional case (using C3D8R elements) with a mass scaling factor of 2758, rigid elements, and the CENTROID kinematic and STIFFNESS hourglass section control options. roll3d330_ocs.inp Three-dimensional case (using C3D8R elements) with a mass scaling factor of 2758, rigid elements, and the ORTHOGONAL kinematic and COMBINED hourglass section control options. roll2d1650_anl_ss.inp Two-dimensional case (using CPE4R elements) with a mass scaling factor of 68962 using the STIFFNESS hourglass control. roll3d330_rev_anl_ocs.inp Three-dimensional model (using C3D8R elements) with a mass scaling factor of 2758; an analytical rigid surface of TYPE=REVOLUTION; and the ORTHOGONAL kinematic and COMBINED hourglass section control options. roll3d330_rev_anl.inp Three-dimensional model (using C3D8R elements) with a mass scaling factor of 2758, an analytical rigid surface of TYPE=REVOLUTION, and the default section control options. roll3d330_cyl_anl.inp Three-dimensional model (using C3D8R elements) with a mass scaling factor of 2758, an analytical rigid surface of TYPE=CYLINDER, and the default section control options. roll2d66.inp

1-489

Static Stress/Displacement Analyses

Two-dimensional model (using CPE4R elements) with a mass scaling factor of 110 and default section controls. roll2d330.inp Two-dimensional model (using CPE4R elements) with a mass scaling factor of 2758 and default section controls. roll2d1650.inp Two-dimensional model (using CPE4R elements) with a mass scaling factor of 68962 and default section controls. roll3d330.inp Three-dimensional model using rigid elements and default section controls. roll2d66_anl.inp Two-dimensional model (using CPE4R elements) with a mass scaling factor of 110 using analytical rigid surfaces and default section controls. roll2d330_anl.inp Two-dimensional model (using CPE4R elements) with a mass scaling factor of 2758 using analytical rigid surfaces and default section controls. roll2d1650_anl.inp Two-dimensional model (using CPE4R elements) with a mass scaling factor of 68962 using analytical rigid surfaces and default section controls. roll2d330_anl_cpe6m.inp Two-dimensional case (using CPE6M elements) with a mass scaling factor of 2758. roll3d330_anl_c3d10m.inp Three-dimensional case (using C3D10M elements) with a mass scaling factor of 2758. roll3d_medium.inp Additional mesh refinement case (using C3D8R elements) included for the sole purpose of testing the performance of the code.

References · Kobayashi, S., S. I. Oh, and T. Altan, Metal Forming and the Finite Element Method , Oxford University Press, 1989. · Kopp, R., and P. M. Dohmen, "Simulation und Planung von Walzprozessen mit Hilfe der Finite-Elemente-Methode (FEM)," Stahl U. Eisen, no. 7, pp. 131-136, 1990.

Tables

1-490

Static Stress/Displacement Analyses

Table 1.3.7-1 Analysis cases and relative CPU costs. (The two-dimensional explicit analyses all use CPE4R elements and the STIFFNESS hourglass control. The three-dimensional explicit analysis uses C3D8R elements and the CENTROID kinematic, STIFFNESS hourglass section control options.) Analysis Type Mass Scaling Effective Roll Surface Relative CPU Factor Speed (m/sec) Time Explicit, plane strain 110.3 11.2 4.99 Explicit, plane strain 2758.5 56.1 1.00 Explicit, plane strain 68961.8 280.5 0.21 Implicit, plane strain quasi-static 6.90 Explicit, 3-D 2758.5 56.1 16.0

Table 1.3.7-2 Explicit section control options tested (mass scaling factor=2758.5). CPE4R and C3D8R elements are employed for the two-dimensional and three-dimensional cases, respectively. Spread values are reported for the half-model at node 24015. Analysis Type Section Controls Relative Kinematic Hourglass CPU Time Explicit, plane strain n/a STIFFNES 1.00 S Explicit, plane strain n/a RELAX 1.11 Explicit, plane strain n/a COMBINE 1.04 D 30.7 Explicit, 3-D AVERAGE RELAX STRAIN STIFFNES S Explicit, 3-D ORTHOGON COMBINE 21.2 AL D Explicit, 3-D CENTROID STIFFNES 16.0 S

Sprea d (mm) n/a n/a n/a 2.06

2.07 2.10

Figures Figure 1.3.7-1 Equivalent plastic strain for the plane strain case ( CPE4R) with STIFFNESS hourglass control (mass scaling factor=110.3).

1-491

Static Stress/Displacement Analyses

Figure 1.3.7-2 Equivalent plastic strain for the plane strain case ( CPE4R) with STIFFNESS hourglass control (mass scaling factor=2758.5).

Figure 1.3.7-3 Equivalent plastic strain for the plane strain case ( CPE4R) with STIFFNESS hourglass control (mass scaling factor=68961.8).

Figure 1.3.7-4 Shear stress for the plane strain case (CPE4R) with STIFFNESS hourglass control (mass scaling factor=110.3).

1-492

Static Stress/Displacement Analyses

Figure 1.3.7-5 Shear stress for the plane strain case (CPE4R) with STIFFNESS hourglass control (mass scaling factor=2758.5).

Figure 1.3.7-6 Shear stress for the plane strain case (CPE4R) with STIFFNESS hourglass control (mass scaling factor=68961.8).

Figure 1.3.7-7 Equivalent plastic strain for the three-dimensional case ( C3D8R) using the CENTROID kinematic and STIFFNESS hourglass section control options (mass scaling 1-493

Static Stress/Displacement Analyses

factor=2758.5).

Figure 1.3.7-8 Equivalent plastic strain for the three-dimensional case ( C3D8R) using the AVERAGE STRAIN kinematic and RELAX STIFFNESS hourglass section control options (mass scaling factor=2758.5).

Figure 1.3.7-9 Equivalent plastic strain for the plane strain case ( CPE6M) (mass scaling factor=2758.5).

1-494

Static Stress/Displacement Analyses

Figure 1.3.7-10 Equivalent plastic strain for the three-dimensional case ( C3D10M) (mass scaling factor=2758.5).

Sample listings

1-495

Static Stress/Displacement Analyses

Listing 1.3.7-1 *HEADING Thick plate rolling: Plane Strain, ABAQUS/Explicit (Analytical rigid surfaces) SECTION CONTROLS USED (HOURGLASS=STIFFNESS) *RESTART,WRITE,NUM=10 ** *NODE ** Bar 1, 0., 0. 401, 0., 0.020 47, -00.092, 0. 447, -00.092, 0.020 ** *NGEN,NSET=BOTTOM 1,47,1 *NGEN,NSET=TOP 401,447,1 ** *NFILL,NSET=BAR BOTTOM,TOP,8,50 ** ***** Bar ** *ELEMENT,TYPE=CPE4R,ELSET=METAL 1,1,51,52,2 *ELGEN,ELSET=METAL 1,8,50,50,46,1,1 ** *ELSET,ELSET=TOP,GEN 351,396,1 *ELSET,ELSET=BACK,GEN 46,396,50 ** *SOLID SECTION,ELSET=METAL,MAT=C15,CONTROL=B 1., *SECTION CONTROLS, HOURGLASS=STIFFNESS, NAME=B ** *MATERIAL,NAME=C15 *ELASTIC 1.5E11,.3

1-496

Static Stress/Displacement Analyses

*PLASTIC 168.72E06,0 219.33E06,0.1 272.02E06,0.2 308.53E06,0.3 337.37E06,0.4 361.58E06,0.5 382.65E06,0.6 401.42E06,0.7 418.42E06,0.8 434.01E06,0.9 448.45E06,1.0 *DENSITY 7.85E3, ** ** Node for rigid surface *NODE 10000, 0.0409 , 0.185 *INITIAL CONDITIONS,TYPE=VELOCITY BAR,1,1.0367 ** ** *SURFACE, TYPE=SEGMENTS,NAME=ROLLER START, 0.040900, 0.015000 CIRCL, -.129100, 0.185000 , 0.0409 , 0.185 *SURFACE,TYPE=ELEMENT, NAME=SURF1 TOP,S2 *RIGID BODY, REF NODE=10000, ANALYTICAL SURFACE=ROLLER *STEP *DYNAMIC,EXPLICIT ,0.089286 *FIXED MASS SCALING,FACTOR=2758.5,ELSET=METAL ** ** Roller, Radius = .170 m ** *BOUNDARY BOTTOM,2,2 10000,1,2 ** *BOUNDARY,TYPE=VELOCITY 10000,6,6,6.2832 **

1-497

Static Stress/Displacement Analyses

*SURFACE INTERACTION,NAME=FRICT *FRICTION 0.3, *CONTACT PAIR,INTERACTION=FRICT SURF1,ROLLER ** ** *FILE OUTPUT,TIMEMARKS=YES,NUM=1 *EL FILE PEEQ,MISES,PE,LE *NODE FILE U, *ENERGY FILE *END STEP **

1-498

Static Stress/Displacement Analyses

Listing 1.3.7-2 *HEADING Thick plate rolling: 3-Dimensional, ABAQUS/Explicit SECTION CONTROLS USED (KINEMATIC=CENTROID, HOURGLASS=STIFFNESS) *RESTART,WRITE,NUM=4 *NODE ** Bar 1, 0., 0. 801, 0., 0.020 47, -00.092, 0. 847, -00.092, 0.020 24001, 0., 0. , -0.020 24801, 0., 0.020, -0.020 24047, -00.092, 0. , -0.020 24847, -00.092, 0.020, -0.020 *NGEN,NSET=BOT1 1,47,1 *NGEN,NSET=TOP1 801,847,1 *NGEN,NSET=BOT2 24001,24047,1 *NGEN,NSET=TOP2 24801,24847,1 *NFILL,NSET=ZSYMM BOT1,TOP1,8,100 *NFILL,NSET=SIDE BOT2,TOP2,8,100 *NFILL,NSET=BAR ZSYMM,SIDE,8,3000 *NSET,NSET=BOTTOM,GEN 1,47,1 3001,3047,1 6001,6047,1 9001,9047,1 12001,12047,1 15001,15047,1 18001,18047,1 21001,21047,1 24001,24047,1 **

1-499

Static Stress/Displacement Analyses

***** Bar ** *ELEMENT,TYPE=C3D8R,ELSET=METAL 1,2,1,3001,3002,102,101,3101,3102 *ELGEN,ELSET=METAL 1,8,100,100,46,1,1,8,3000,1000 ** *ELSET,ELSET=TOP,GEN 701,746,1 1701,1746,1 2701,2746,1 3701,3746,1 4701,4746,1 5701,5746,1 6701,6746,1 7701,7746,1 *ELSET,ELSET=BACK,GEN 46,746,100 1046,1746,100 2046,2746,100 3046,3746,100 4046,4746,100 5046,5746,100 6046,6746,100 7046,7746,100 *ELSET,ELSET=SIDE,GEN 7001,7046,1 7101,7146,1 7201,7246,1 7301,7346,1 7401,7446,1 7501,7546,1 7601,7646,1 7701,7746,1 ** *SOLID SECTION,ELSET=METAL,MAT=C15,CONTROL=C 1., *SECTION CONTROLS,KINEMATIC=CENTROID, HOURGLASS=STIFFNESS, NAME=C ** *MATERIAL,NAME=C15 *ELASTIC 1.5E11,.3

1-500

Static Stress/Displacement Analyses

*PLASTIC 168.72E06,0 219.33E06,0.1 272.02E06,0.2 308.53E06,0.3 337.37E06,0.4 361.58E06,0.5 382.65E06,0.6 401.42E06,0.7 418.42E06,0.8 434.01E06,0.9 448.45E06,1.0 *DENSITY 7.85E3, ** *NODE ** Reference node 30000, 0.0409 , 0.185 , -0.010 *INITIAL CONDITIONS,TYPE=VELOCITY BAR,1,1.0367 ** ***************** Step 1 *SURFACE, NAME=ROLLER, TYPE=REVOL 0.0409,0.185,-0.025,0.0409,0.185,0.005 START, 0.170,0.03 LINE, 0.170,0.0 *SURFACE,TYPE=ELEMENT, NAME=SURF1 TOP,S2 SIDE,S5 *RIGID BODY, REF NODE=30000, ANALYTICAL SURFACE=ROLLER *STEP *DYNAMIC,EXPLICIT ,0.089286 *FIXED MASS SCALING,FACTOR=2758.5,ELSET=METAL ** Roller, Radius = .170 m *BOUNDARY BOTTOM,2,2 ZSYMM,ZSYMM 30000,1,5 ** *BOUNDARY,TYPE=VELOCITY **30000,6,6,330.0

1-501

Static Stress/Displacement Analyses

30000,6,6,6.2832 ** *SURFACE INTERACTION,NAME=FRICT *FRICTION 0.3, *CONTACT PAIR,INTERACTION=FRICT SURF1,ROLLER ** *FILE OUTPUT,TIMEMARKS=YES,NUM=1 *EL FILE PEEQ,MISES,PE,LE *NODE FILE U, *ENERGY FILE *END STEP

1.3.8 Axisymmetric forming of a circular cup Products: ABAQUS/Standard ABAQUS/Explicit This example illustrates the hydroforming of a circular cup using an axisymmetric model. In this case a two-stage forming sequence is used, with annealing between the stages. Two analysis methods are used: in one the entire process is analyzed using ABAQUS/Explicit; in the other the forming sequences are analyzed with ABAQUS/Explicit, while the springback analyses are run in ABAQUS/Standard. Here, the import capability is used to transfer results between ABAQUS/Explicit and ABAQUS/Standard and vice versa.

Problem description The model consists of a deformable blank and three rigid dies. The blank has a radius of 150.0 mm, is 1.0 mm thick, and is modeled using axisymmetric shell elements, SAX1. The coefficient of friction between the blank and the dies is taken to be 0.1. Dies 1 and 2 are offset from the blank by half of the thickness of the blank, because the contact algorithm takes into account the shell thickness. To avoid pinching of the blank while die 3 is put into position for the second forming stage, the radial gap between dies 2 and 3 is set to be 20% bigger than the initial shell thickness. Figure 1.3.8-1 and Figure 1.3.8-2 show the initial geometry of the model. The three dies are modeled with either two-dimensional analytical rigid surfaces or RAX2 rigid elements. An analytical rigid surface can yield a more accurate representation of two-dimensional curved punch geometries and result in computational savings. Contact pressure can be viewed on the specimen surface, and the reaction force is available at the rigid body reference node. In addition, both the kinematic (default) and penalty contact formulations are tested. Results for the kinematic contact formulation using rigid elements are presented here. The blank is made of aluminum-killed steel, which is assumed to satisfy the Ramberg-Osgood relation between true stress and logarithmic strain,

1-502

Static Stress/Displacement Analyses

² = (¾=K )1=n ; with a reference stress value (K) of 513 MPa and work-hardening exponent (n) of 0.223. Isotropic elasticity is assumed, with Young's modulus of 211 GPa and Poisson's ratio of 0.3. With these data an initial yield stress of 91.3 MPa is obtained. The stress-strain behavior is defined by piecewise linear segments matching the Ramberg-Osgood curve up to a total (logarithmic) strain level of 107%, with Mises yield, isotropic hardening, and no rate dependence. The analysis that is performed entirely within ABAQUS/Explicit consists of six steps. In the first step contact is defined between the blank and dies 1 and 2. Both dies remain fixed while a distributed load of 10 MPa in the negative z-direction is ramped onto the blank. This load is then ramped off in the second step, allowing the blank to spring back to an equilibrium state. The third step is an annealing step. The annealing procedure in ABAQUS/Explicit sets all appropriate state variables to zero. These variables include stresses, strains (excluding the thinning strain for shells, membranes, and plane stress elements), plastic strains, and velocities. There is no time associated with an annealing step. The process occurs instantaneously. In the fourth step contact is defined between the blank and die 3 and contact is removed between the blank and die 1. Die 3 moves down vertically in preparation for the next pressure loading. In the fifth step another distributed load is applied to the blank in the positive z-direction, forcing the blank into die 3. This load is then ramped off in the sixth step to monitor the springback of the blank. To obtain a quasi-static response, an investigation was conducted to determine the optimum rate for applying the pressure loads and removing them. The optimum rate balances the computational time against the accuracy of the results; increasing the loading rate will reduce the computer time but lead to less accurate quasi-static results. The analysis that uses the import capability consists of four runs. The first run is identical to Step 1 of the ABAQUS/Explicit analysis described earlier. In the second run the ABAQUS/Explicit results for the first forming stage are imported into ABAQUS/Standard (using UPDATE=NO and STATE=YES on the *IMPORT option) for the first springback analysis. The third run imports the results of the first springback analysis into ABAQUS/Explicit for the subsequent annealing process and the second forming stage. By setting UPDATE=YES and STATE=NO on the *IMPORT option, this run begins with no initial stresses or strains, effectively simulating the annealing process. The final run imports the results of the second forming stage into ABAQUS/Standard for the second springback analysis.

Results and discussion Figure 1.3.8-3 to Figure 1.3.8-5show the results of the analysis conducted entirely within ABAQUS/Explicit using the rigid element approach and the kinematic contact formulation. Figure 1.3.8-3shows the deformed shape at the end of Step 2, after the elastic springback. Figure 1.3.8-4 shows the deformed shape at the end of the analysis, after the second elastic springback. Although it is not shown here, the amount of springback observed during the unloading steps is negligible. Figure 1.3.8-5 shows a contour plot of the shell thickness ( STH) at the end of the analysis. The thickness of

1-503

Static Stress/Displacement Analyses

the material at the center of the cup has been reduced by about 20%, while the thickness at the edges of the cup has been increased by about 10%. The results obtained using the import capability to perform the springback analyses in ABAQUS/Standard are nearly identical, as are those obtained using analytical rigid surfaces and/or penalty contact formulations.

Input files axiform.inp ABAQUS/Explicit analysis that uses rigid elements and kinematic contact. This file is also used for the first step of the analysis that uses the import capability. axiform_anl.inp Model using analytical rigid surfaces and kinematic contact. axiform_pen.inp Model using rigid elements and penalty contact. axiform_anl_pen.inp Model using analytical rigid surfaces and penalty contact. axiform_sprbk1.inp First springback analysis using the import capability. axiform_form2.inp Second forming analysis using the import capability. axiform_sprbk2.inp Second springback analysis using the import capability. axiform_restart.inp Restart of axiform.inp included for the purpose of testing the restart capability. axiform_rest_anl.inp Restart of axiform_anl.inp included for the purpose of testing the restart capability.

Figures Figure 1.3.8-1 Configuration at the beginning of stage 1.

1-504

Static Stress/Displacement Analyses

Figure 1.3.8-2 Configuration of dies in forming stage 2. (The dotted line shows the initial position of die 3.)

Figure 1.3.8-3 Deformed configuration after the first forming stage.

1-505

Static Stress/Displacement Analyses

Figure 1.3.8-4 Final configuration.

Figure 1.3.8-5 Contour plot of shell thickness.

Sample listings

1-506

Static Stress/Displacement Analyses

Listing 1.3.8-1 *HEADING SHEET METAL FORMING WITH ANNEALING DIE3 SLIDES DOWN FROM ABOVE TO AVOID INITIAL OVERCLOSURE *NODE,NSET=BLANK 1,0.,0.0005 41,.150,0.0005 *NGEN,NSET=BLANK 1,41,1 *ELEMENT,TYPE=SAX1,ELSET=BLANK 1, 1,2 *ELGEN,ELSET=BLANK 1, 40,1,1 *SHELL SECTION,ELSET=BLANK,MATERIAL=STEEL, SECTION INTEGRATION=GAUSS .001,5 *MATERIAL,NAME=STEEL *DENSITY 7800., *ELASTIC 2.1E11,0.3 *PLASTIC 0.91294E+08, 0.00000E+00 0.10129E+09, 0.21052E-03 0.11129E+09, 0.52686E-03 0.12129E+09, 0.97685E-03 0.13129E+09, 0.15923E-02 0.14129E+09, 0.24090E-02 0.15129E+09, 0.34674E-02 0.16129E+09, 0.48120E-02 0.17129E+09, 0.64921E-02 0.18129E+09, 0.85618E-02 0.19129E+09, 0.11080E-01 0.20129E+09, 0.14110E-01 0.21129E+09, 0.17723E-01 0.22129E+09, 0.21991E-01 0.23129E+09, 0.26994E-01 0.24129E+09, 0.32819E-01 0.25129E+09, 0.39556E-01 0.26129E+09, 0.47301E-01 0.27129E+09, 0.56159E-01

1-507

Static Stress/Displacement Analyses

0.28129E+09, 0.66236E-01 0.29129E+09, 0.77648E-01 0.30129E+09, 0.90516E-01 0.31129E+09, 0.10497E+00 0.32129E+09, 0.12114E+00 0.33129E+09, 0.13916E+00 0.34129E+09, 0.15919E+00 0.35129E+09, 0.18138E+00 0.36129E+09, 0.20588E+00 0.37129E+09, 0.23287E+00 0.38129E+09, 0.26252E+00 0.39129E+09, 0.29502E+00 0.40129E+09, 0.33054E+00 0.41129E+09, 0.36929E+00 0.42129E+09, 0.41147E+00 0.43129E+09, 0.45729E+00 0.44129E+09, 0.50696E+00 0.45129E+09, 0.56073E+00 0.46129E+09, 0.61881E+00 0.47129E+09, 0.68145E+00 0.48129E+09, 0.74890E+00 0.49129E+09, 0.82142E+00 0.50129E+09, 0.89928E+00 0.51129E+09, 0.98274E+00 0.52129E+09, 0.10721E+01 *NODE,NSET=DIE1 1001, 0.,-0.05 1002,.090,-0.05 1011,.100,-.040 199991, 0., -0.05 *NGEN,NSET=DIE1,LINE=C 1002,1011,1,,.090,-.040,0. *ELEMENT,TYPE=RAX2,ELSET=DIE1 1001, 1001,1002 *ELGEN,ELSET=DIE1 1001, 10,1,1 *NODE,NSET=DIE2 2001,.100,-.060 2002,.100,-.010 2011,.110, 0. 2012,.160, 0. 299991, .100, -.060 *NGEN,NSET=DIE2,LINE=C

1-508

Static Stress/Displacement Analyses

2002,2011,1,,.110,-.010,0.,0.,0.,-1. *ELEMENT,TYPE=RAX2,ELSET=DIE2 2001, 2001,2002 *ELGEN,ELSET=DIE2 2001, 11,1,1 *NODE,NSET=DIE3 ** raised by 0.05 from original shift outer ** surface inward by then lower by 0.005 ** (half the radius of curvature) ** further lower by 0.005 3001,.0 ,0.0044 3014,.050,-0.009 3015,.0888,-0.009 3024,.0988,0.001 3025,.0988,0.0405 399991,.0,0.0044 *NGEN,NSET=DIE3,LINE=C 3001,3014,1,, 0.0,-0.0956,0.,0.,0.,-1. 3015,3024,1,,.0888, 0.001, 0. *ELEMENT,TYPE=RAX2,ELSET=DIE3 3001, 3001,3002 *ELGEN,ELSET=DIE3 3001, 24,1,1 *BOUNDARY 1,XSYMM 199991,1,6 299991,1,6 399991,1,2 399991,6,6 *AMPLITUDE,NAME=R1,TIME=STEP TIME 0.,0., .8E-3,1.5E6, 1.7E-3,1.5E6, 3.E-3,1.E7, 3.5E-3,1.E7 *AMPLITUDE,NAME=R2,TIME=STEP TIME 0.,1.E7, 1.E-3,0. *AMPLITUDE,NAME=R3A,TIME=STEP TIME, DEFINITION=SMOOTH STEP 0.,0., 1.E-3, 1.0 *AMPLITUDE,NAME=R4,TIME=STEP TIME 0.,0., 1.E-3,.6E7 *AMPLITUDE,NAME=R5,TIME=STEP TIME 0.,.6E7, 1.E-3,0. *RESTART,WRITE,NUM=1 **

1-509

Static Stress/Displacement Analyses

** First downward pressure loading *SURFACE,TYPE=ELEMENT,NAME=TOP BLANK,SPOS *SURFACE,TYPE=ELEMENT,NAME=DIE1 DIE1,SPOS *SURFACE,TYPE=ELEMENT,NAME=DIE2 DIE2,SPOS *SURFACE,TYPE=ELEMENT,NAME=DIE3 DIE3,SNEG *SURFACE,TYPE=ELEMENT,NAME=BOTTOM BLANK,SNEG *RIGID BODY,ELSET=DIE3,REF NODE=399991 *RIGID BODY,ELSET=DIE1,REF NODE=199991 *RIGID BODY,ELSET=DIE2,REF NODE=299991 *STEP *DYNAMIC,EXPLICIT ,3.5E-3 *DLOAD,AMP=R1 BLANK,P,-1.0 *SURFACE INTERACTION,NAME=FRICT *FRICTION 0.1, *CONTACT PAIR,INTERACTION=FRICT DIE2,BOTTOM DIE1,BOTTOM *FILE OUTPUT,NUM=2, TIMEMARKS=YES *EL FILE STH, *OUTPUT,FIELD *ELEMENT OUTPUT STH, *NODE FILE U, *OUTPUT,FIELD *NODE OUTPUT U, *HISTORY OUTPUT,TIME=3.5E-6 *NSET,NSET=NOUT 1, *NODE HISTORY,NSET=NOUT U,V *ELSET,ELSET=EOUT 24,25,26

1-510

Static Stress/Displacement Analyses

*EL HISTORY,ELSET=EOUT STH, PEEQ,MISES,S,LE,PE *ENERGY HISTORY ALLKE,ALLSE,ALLWK,ALLPD,ALLAE,ALLCD,ALLFD,ALLIE, ALLVD,ETOTAL,DT *END STEP ** ** First springback *STEP *DYNAMIC,EXPLICIT ,1.E-3 *DLOAD,AMP=R2,OP=NEW BLANK,P,-1.0 *END STEP ** ** anneal *STEP *ANNEAL *END STEP ** ** gradually slide die 3 into position *STEP *DYNAMIC,EXPLICIT ,1.0E-3 *BOUNDARY, AMP=R3A 399991,2,2,-0.04 ***DLOAD,OP=NEW **BLANK, VP, 100.0 *CONTACT PAIR,INTERACTION=FRICT,OP=ADD DIE3,TOP *CONTACT PAIR,OP=DELETE DIE1,BOTTOM *END STEP ** ** Second upward pressure loading *STEP *DYNAMIC,EXPLICIT ,1.0E-3 *ELSET,ELSET=LOAD,GEN 1,26,1 *DLOAD,AMP=R4,OP=NEW LOAD,P,1.0

1-511

Static Stress/Displacement Analyses

*END STEP ** ** Second springback *STEP *DYNAMIC,EXPLICIT ,1.E-3 *DLOAD,AMP=R5,OP=NEW LOAD,P,1.0 *END STEP

1.3.9 Cup/trough forming Product: ABAQUS/Explicit This example illustrates the use of adaptive meshing in forging problems that include large amounts of shearing at the tool-blank interface; a cup and a trough are formed.

Problem description Three different geometric models are considered, as shown in Figure 1.3.9-1. Each model consists of a rigid punch, a rigid die, and a deformable blank. The outer top and bottom edges of the blank are cambered, which facilitates the flow of material against the tools. The punch and die have semicircular cross-sections; the punch has a radius of 68.4 mm, and the die has a radius of 67.9 mm. The blank is modeled as a von Mises elastic, perfectly plastic material with a Young's modulus of 4000 MPa and a yield stress of 5 MPa. The Poisson's ratio is 0.21; the density is 1.E-4 kg/mm 3. In each case the punch is moved 61 mm, while the die is fully constrained. The SMOOTH STEP parameter on the *AMPLITUDE option is used to ramp the punch velocity to a maximum, at which it remains constant. The SMOOTH STEP specification of the velocity promotes a quasi-static response to the loading.

Case 1: Axisymmetric model for cup forming The blank is meshed with CAX4R elements and measures 50 ´ 64.77 mm. The punch and the die are modeled as TYPE=SEGMENTS analytical rigid surfaces. Symmetry boundary conditions are prescribed at r=0. The finite element model is shown in Figure 1.3.9-2.

Case 2: Three-dimensional model for trough forming The blank is meshed with C3D8R elements and measures 50 ´ 64.7 ´ 64.7 mm. The punch and the die are modeled as TYPE=CYLINDER analytical rigid surfaces. Symmetry boundary conditions are applied at the x=0 and z=0 planes. The finite element model of the blank is shown in Figure 1.3.9-3.

Case 3: Three-dimensional model for cup forming The blank is meshed with C3D8R elements. A 90° wedge of the blank with a radius of 50 mm and a height of 64.7 mm is analyzed. The punch and the die are modeled as TYPE=REVOLUTION analytical rigid surfaces. Symmetry boundary conditions are applied at the x=0 and y=0 planes. The

1-512

Static Stress/Displacement Analyses

finite element model of the blank is shown in Figure 1.3.9-4.

Adaptive meshing A single adaptive mesh domain that incorporates the entire blank is used for each model. Symmetry planes are defined as Lagrangian boundary regions (the default), and contact surfaces are defined as sliding boundary regions (the default). Since this problem is quasi-static with relatively small amounts of deformation per increment, the default values for frequency, mesh sweeps, and other adaptive mesh parameters and controls are sufficient.

Results and discussion Figure 1.3.9-5 through Figure 1.3.9-7show the mesh configuration at the end of the forging simulation for Cases 1-3. In each case a quality mesh is maintained throughout the simulation. As the blank flattens out, geometric edges and corners that exist at the beginning of the analysis are broken and adaptive meshing is allowed across them. The eventual breaking of geometric edges and corners is essential for this type of problem to minimize element distortion and optimize element aspect ratios. For comparison purposes Figure 1.3.9-8 shows the deformed mesh for a pure Lagrangian simulation of Case 1 (the axisymmetric model). The mesh is clearly better when continuous adaptive meshing is used. Several diamond-shaped elements with extremely poor aspect ratios are formed in the pure Lagrangian simulation. Adaptive meshing improves the element quality significantly, especially along the top surface of the cup where solution gradients are highest. Figure 1.3.9-9 and Figure 1.3.9-10show contours of equivalent plastic strain at the completion of the forging for the adaptive meshing and pure Lagrangian analyses of Case 1, respectively. Overall plastic strains compare quite closely. Slight differences exist only along the upper surface, where the pure Lagrangian mesh becomes very distorted at the end of the simulation. The time histories of the vertical punch force for the adaptive and pure Lagrangian analyses agree closely for the duration of the forging, as shown in Figure 1.3.9-11.

Input files ale_cupforming_axi.inp Case 1. ale_cupforming_axinodes.inp External file referenced by Case 1. ale_cupforming_axielements.inp External file referenced by Case 1. ale_cupforming_cyl.inp Case 2. ale_cupforming_sph.inp Case 3. lag_cupforming_axi.inp

1-513

Static Stress/Displacement Analyses

Lagrangian solution of Case 1.

Figures Figure 1.3.9-1 Model geometries for each case.

Figure 1.3.9-2 Undeformed mesh for Case 1.

Figure 1.3.9-3 Undeformed mesh for Case 2.

1-514

Static Stress/Displacement Analyses

Figure 1.3.9-4 Undeformed mesh for Case 3.

Figure 1.3.9-5 Deformed mesh for Case 1.

1-515

Static Stress/Displacement Analyses

Figure 1.3.9-6 Deformed mesh for Case 2.

Figure 1.3.9-7 Deformed mesh for Case 3.

1-516

Static Stress/Displacement Analyses

Figure 1.3.9-8 Deformed mesh for Case 1 using a pure Lagrangian formulation.

Figure 1.3.9-9 Contours of equivalent plastic strain for Case 1 using adaptive meshing.

1-517

Static Stress/Displacement Analyses

Figure 1.3.9-10 Contours of equivalent plastic strain for Case 1 using a pure Lagrangian fomulation.

Figure 1.3.9-11 Comparison of time histories for the vertical punch force for Case 1.

1-518

Static Stress/Displacement Analyses

Sample listings

1-519

Static Stress/Displacement Analyses

Listing 1.3.9-1 *HEADING ADAPTIVE MESHING EXAMPLE BULK FORMING OF A CUP. Units - N, mm, sec *NODE, INPUT=ale_cupforming_axinodes.inp ** *ELEMENT, TYPE=CAX4R, ELSET=BLANK, INPUT=ale_cupforming_axielements.inp ** *SOLID SECTION, ELSET=BLANK, MATERIAL=AL1 ** *MATERIAL,NAME=AL1 *ELASTIC,TYPE=ISOTROPIC 4000,0.21 *PLASTIC,HARDENING=ISOTROPIC 5,0 5,0.22 *DENSITY 1.E-4, *ELSET, ELSET=BLANK_T, GEN 441, 450, 1 461, 470, 1 480, 480, 1 *ELSET, ELSET=BLANK_B, GEN 350, 440, 10 150, 240, 10 30, 40, 10 31, 39, 1 11, 20, 1 *NODE 900001,5,90,0 900003,0,-25,0 *NSET, NSET=XSYM, GEN 309,408, 11 67, 166, 11 1, 23, 11 551, 562, 11 *BOUNDARY 900003, 1, 6 900001, 1, 6 XSYM, XSYMM

1-520

Static Stress/Displacement Analyses

*NSET, NSET=REFN 900001, 900003 *AMPLITUDE,NAME=AMP,DEFINITION=SMOOTH STEP 0.0, 0.0, .5, 81.333, 1.,81.333 *RESTART, WRITE, NUMBER=30 *SURFACE,TYPE=ELEMENT,NAME=BLANK_B, REGION TYPE=SLIDING BLANK_B, *SURFACE, TYPE=SEGMENTS, NAME=DIE START, 0.0000000E+00, -0.1300000E+02 CIRCL, 0.7500000E+02 , 0.5200001E+02, 7.06897, 54.612727 *SURFACE,TYPE=ELEMENT,NAME=BLANK_T, REGION TYPE=SLIDING BLANK_T, *SURFACE, TYPE=SEGMENTS, NAME=PUNCH START, 80,144 LINE, 64,144 LINE, 64,134 CIRCL, 0,65.7,-4.44445,134 LINE, -1, 65.7 *RIGID BODY, REF NODE=900001, ANALYTICAL SURFACE =PUNCH *RIGID BODY, REF NODE=900003, ANALYTICAL SURFACE =DIE *STEP *DYNAMIC,EXPLICIT , 1. *BOUNDARY,TYPE=VELOCITY,AMPLITUDE=AMP 900001, 2,2, -1.00 *CONTACT PAIR, INTERACTION=TOP BLANK_T, PUNCH *SURFACE INTERACTION, NAME=TOP *FRICTION, TAUMAX=4. 0.1, *CONTACT PAIR, INTERACTION=BOTTOM BLANK_B, DIE *SURFACE INTERACTION, NAME=BOTTOM *FRICTION, TAUMAX=4. 0.1, *HISTORY OUTPUT, TIME INTERVAL=2.E-3 *NODE HISTORY, NSET=REFN U,RF *FILE OUTPUT,NUMBER INTERVAL=6, TIMEMARKS=YES *EL FILE, ELSET=BLANK_T MISES,PEEQ, *NODE FILE,NSET=REFN U,RF

1-521

Static Stress/Displacement Analyses

*ENERGY FILE *ADAPTIVE MESH, ELSET=BLANK *END STEP

1.3.10 Forging with sinusoidal dies Product: ABAQUS/Explicit This example illustrates the use of adaptive meshing in forging problems that incorporate geometrically complex dies and involve substantial material flow.

Problem description Three different geometric models are considered, as shown in Figure 1.3.10-1. Each model consists of a rigid die and a deformable blank. The cross-sectional shape of the die is sinusoidal with an amplitude and a period of 5 and 10 mm, respectively. The blank is steel and is modeled as a von Mises elastic-plastic material with a Young's modulus of 200 GPa, an initial yield stress of 100 MPa, and a constant hardening slope of 300 MPa. Poisson's ratio is 0.3; the density is 7800 kg/m 3. In all cases the die is moved downward vertically at a velocity of 2000 mm/sec and is constrained in all other degrees of freedom. The total die displacement is 7.6 mm for Cases 1 and 2 and 5.6 mm for Case 3. These displacements represent the maximum possible given the refinement and topology of the initial mesh (if the quality of the mesh is retained for the duration of the analysis). Although each analysis uses a sinusoidal die, the geometries and flow characteristics of the blank material are quite different for each problem.

Case 1: Axisymmetric model The blank is meshed with CAX4R elements and measures 20 ´ 10 mm. The dies are modeled as TYPE=SEGMENTS analytical rigid surfaces. The bottom of the blank is constrained in the z-direction, and symmetry boundary conditions are prescribed at r=0. The initial configuration of the blank and the die is shown in Figure 1.3.10-2.

Case 2: Three-dimensional model The blank is meshed with C3D8R elements and measures 20 ´ 10 ´ 10 mm.The dies are modeled as TYPE=CYLINDER analytical rigid surfaces. The bottom of the blank is constrained in the y-direction, and symmetry boundary conditions are applied at the x=0 and z=10 planes. The finite element model of the blank and the die is shown in Figure 1.3.10-3.

Case 3: Three-dimensional model The blank is meshed with C3D8R elements and measures 20 ´ 10 ´ 20 mm.The dies are modeled as TYPE=REVOLUTION analytical rigid surfaces. The bottom of the blank is constrained in the y-direction, and symmetry boundary conditions are applied at the x=0 and z=10 planes. The finite element model of the blank and the die is shown in Figure 1.3.10-4. The revolved die is displaced 1-522

Static Stress/Displacement Analyses

upward in the figure from its initial position for clarity.

Adaptive meshing A single adaptive mesh domain that incorporates the entire blank is used for each model. Symmetry planes are defined as Lagrangian boundary regions (the default), and contact surfaces are defined as sliding boundary regions (the default). Because the material flow for each of the geometries is substantial, the frequency and the intensity of adaptive meshing must be increased to provide an accurate solution. The value of the FREQUENCY parameter on the *ADAPTIVE MESH option is reduced from the default of 10 to 5 for all cases. The value of the MESH SWEEPS parameter is increased from the default of 1 to 3 for all cases.

Results and discussion Figure 1.3.10-5 and Figure 1.3.10-6show the deformed mesh and contours of equivalent plastic strain at the completion of the forming step for Case 1. Adaptive meshing maintains reasonable element shapes and aspect ratios. This type of forging problem cannot typically be solved using a pure Lagrangian formulation. Figure 1.3.10-7shows the deformed mesh for Case 2. A complex, doubly curved deformation pattern is formed on the free surface as the material spreads under the die. Element distortion appears to be reasonable. Figure 1.3.10-8and Figure 1.3.10-9 show the deformed mesh and contours of equivalent plastic strain for Case 3. Although the die is a revolved geometry, the three-dimensional nature of the blank gives rise to fairly complex strain patterns that are symmetric with respect to the planes of quarter symmetry.

Input files ale_sinusoid_forgingaxi.inp Case 1. ale_sinusoid_forgingaxisurf.inp External file referenced by Case 1. ale_sinusoid_forgingcyl.inp Case 2. ale_sinusoid_forgingrev.inp Case 3.

Figures Figure 1.3.10-1 Model geometries for each of the three cases.

1-523

Static Stress/Displacement Analyses

Figure 1.3.10-2 Initial configuration for Case 1.

1-524

Static Stress/Displacement Analyses

Figure 1.3.10-3 Initial configuration for Case 2.

Figure 1.3.10-4 Initial configuration for Case 3.

Figure 1.3.10-5 Deformed mesh for Case 1.

1-525

Static Stress/Displacement Analyses

Figure 1.3.10-6 Contours of equivalent plastic strain for Case 1.

Figure 1.3.10-7 Deformed mesh for Case 2.

Figure 1.3.10-8 Deformed mesh for Case 3.

1-526

Static Stress/Displacement Analyses

Figure 1.3.10-9 Contours of equivalent plastic strain for Case 3.

Sample listings

1-527

Static Stress/Displacement Analyses

Listing 1.3.10-1 *HEADING ADAPTIVE MESHING EXAMPLE 2D AXISYMMETRIC FORGING EXAMPLE Units - N, m, sec *RESTART, WRITE, NUMBER=10 *NODE 1, 0.00, 0.00 97, 0.02, 0.00 1165, 0.00, 0.01 1261, 0.02, 0.01 10000, 0.01, 0.02 *NGEN, NSET=BOT 1,97,1 *NGEN, NSET=TOP 1165,1261,1 *NFILL,NSET=NALL BOT, TOP, 12, 97 *NGEN, NSET=CENTER 1,1165,97 *ELEMENT, TYPE=CAX4R 1,1,2,99,98 *ELGEN, ELSET=METAL0 1,95,1,1,12,97,96, *ELEMENT, TYPE=CAX4R 96, 96,97,194,193 *ELGEN, ELSET=METAL1 96,12,97,96 *ELSET,ELSET=METAL METAL0,METAL1 *ELEMENT, TYPE=MASS, ELSET=PMASS 10000, 10000 *MASS, ELSET=PMASS 0.2, *ELSET, ELSET=UPPER, GEN 1057,1152,1 *ELSET, ELSET=SIDE, GEN 96,1152,96 *SOLID SECTION, ELSET=METAL, MATERIAL=STEEL *MATERIAL, NAME=STEEL *ELASTIC 200.E+9, .3

1-528

Static Stress/Displacement Analyses

*PLASTIC 1.E+8, 0.0 3.1E+9, 10.0 *DENSITY 7800.E+1, *BOUNDARY BOT, 2,2 CENTER, 1,1 10000,1,1 10000,6,6 *SURFACE, TYPE=SEGMENTS, NAME=RSURF, FILLET RADIUS=.001 *INCLUDE, INPUT=ale_sinusoid_forgingaxisurf.inp *SURFACE,TYPE=ELEMENT, NAME=TARGET, REGION TYPE=SLIDING UPPER, S3 SIDE, S2 *RIGID BODY, REF NODE=10000, ANALYTICAL SURFACE =RSURF *STEP *DYNAMIC, EXPLICIT ,.00038 *SURFACE INTERACTION, NAME=INTER *CONTACT PAIR, INTERACTION=INTER RSURF, TARGET *BOUNDARY, TYPE=VELOCITY 10000, 2, 2, -20. *HISTORY OUTPUT,TIME=0.0 *EL HISTORY,ELSET=UPPER S,LE,LEP,NE,NEP,PEEQ *ENERGY HISTORY ALLKE,ALLIE,ALLAE,ALLVD,ALLWK,ETOTAL, DT, *FILE OUTPUT,NUMBER INTERVAL=6, TIMEMARKS=YES *EL FILE S,LE,LEP,NE,NEP *NODE FILE U,RF *ENERGY FILE *ADAPTIVE MESH,ELSET=METAL,FREQUENCY=5, MESH SWEEPS=3 *END STEP

1-529

Static Stress/Displacement Analyses

1.3.11 Forging with multiple complex dies Product: ABAQUS/Explicit This example illustrates the use of adaptive meshing in forging problems that use multiple geometrically complex dies. The problem is based on a benchmark presented at the " FEM-Material Flow Simulation in the Forging Industry" workshop.

Problem description The benchmark problem is an axisymmetric forging, but in this example both axisymmetric and three-dimensional geometric models are considered. Each model is shown in Figure 1.3.11-1. Both models consist of two rigid dies and a deformable blank. The blank's maximum radial dimension is 895.2 mm, and its thickness is 211.4 mm. The outer edge of the blank is rounded to facilitate the flow of material through the dies. The blank is modeled as a von Mises elastic-plastic material with a Young's modulus of 200 GPa, an initial yield stress of 360 MPa, and a constant hardening slope of 30 MPa. The Poisson's ratio is 0.3; the density is 7340 kg/m 3. Both dies are fully constrained, with the exception of the top die, which is moved 183.4 mm downward at a constant velocity of 166.65 mm/s.

Case 1: Axisymmetric model The blank is meshed with CAX4R elements. A fine discretization is required in the radial direction because of the geometric complexity of the dies and the large amount of material flow that occurs in that direction. Symmetry boundary conditions are prescribed at r=0. The dies are modeled as TYPE=SEGMENTS analytical rigid surfaces. The initial configuration is shown in Figure 1.3.11-2.

Case 2: Three-dimensional model The blank is meshed with C3D8R elements. A 90° wedge of the blank is analyzed. The level of mesh refinement is the same as that used in the axisymmetric model. Symmetry boundary conditions are applied at the x=0 and z=0 planes. The dies are modeled as TYPE=REVOLUTION analytical rigid surfaces. The initial configuration of the blank only is shown in Figure 1.3.11-3. Although the tools are not shown in the figure, they are originally in contact with the blank.

Adaptive meshing A single adaptive mesh domain that incorporates the entire blank is used for each model. Symmetry planes are defined as Lagrangian boundary regions (the default), and contact surfaces are defined as sliding boundary regions (the default). Since this problem is quasi-static with relatively small amounts of deformation per increment, the defaults for frequency, mesh sweeps, and other adaptive mesh parameters and controls are sufficient.

Results and discussion Figure 1.3.11-4 and Figure 1.3.11-5show the deformed mesh for the axisymmetric case at an intermediate stage (t = 0.209 s) and in the final configuration ( t = 0.35 s), respectively. The elements

1-530

Static Stress/Displacement Analyses

remain well shaped throughout the entire simulation, with the exception of the elements at the extreme radius of the blank, which become very coarse as material flows radially during the last 5% of the top die's travel. Figure 1.3.11-6 shows contours of equivalent plastic strain at the completion of forming. Figure 1.3.11-7and Figure 1.3.11-8 show the deformed mesh for the three-dimensional case at t = 0.209 and t = 0.35, respectively. Although the axisymmetric and three-dimensional mesh smoothing algorithms are not identical, the elements in the three-dimensional model also remain well shaped until the end of the analysis, when the same behavior that is seen in the two-dimensional model occurs. Contours of equivalent plastic strain for the three-dimensional model (not shown) are virtually identical to those shown in Figure 1.3.11-6.

Input files ale_duckshape_forgingaxi.inp Case 1. ale_duckshape_forg_axind.inp External file referenced by the Case 1 analysis. ale_duckshape_forg_axiel.inp External file referenced by the Case 1 analysis. ale_duckshape_forg_axiset.inp External file referenced by the Case 1 analysis. ale_duckshape_forg_axirs.inp External file referenced by the Case 1 analysis. ale_duckshape_forgingrev.inp Case 2.

Reference · Industrieverband Deutscher Schmieden e.V.(IDS), "Forging of an Axisymmetric Disk," FEM-Material Flow Simulation in the Forging Industry, Hagen, Germany, October 1997.

Figures Figure 1.3.11-1 Axisymmetric and three-dimensional model geometries.

1-531

Static Stress/Displacement Analyses

Figure 1.3.11-2 Initial configuration for the axisymmetric model.

Figure 1.3.11-3 Initial configuration mesh for the three-dimensional model.

1-532

Static Stress/Displacement Analyses

Figure 1.3.11-4 The deformed mesh for the axisymmetric model at an intermediate stage.

Figure 1.3.11-5 The deformed mesh for the axisymmetric model at the end of forming.

Figure 1.3.11-6 Contours of equivalent plastic strain for the axisymmetric model at the end of forming.

1-533

Static Stress/Displacement Analyses

Figure 1.3.11-7 The deformed mesh for the three-dimensional model at an intermediate stage.

Figure 1.3.11-8 The deformed mesh for the three-dimensional model at the end of forming.

Sample listings 1-534

Static Stress/Displacement Analyses

Listing 1.3.11-1 *HEADING ADAPTIVE MESHING EXAMPLE FORGING WITH DUCK-SHAPED DIE (AXISYMMETRIC) Units - N, mm, sec *RESTART,WRITE,NUMBER INTERVAL=50 *NODE,INPUT=ale_duckshape_forg_axind.inp *ELEMENT, TYPE=CAX4R , ELSET=BLANK, INPUT=ale_duckshape_forg_axiel.inp *INCLUDE, INPUT=ale_duckshape_forg_axiset.inp *NSET,NSET=SIDE 1,83,164,245,326,407,488,569,650,731,812 *MATERIAL,NAME=BLANK *DENSITY 7340.e-9, *ELASTIC 2.E5, 0.3 *PLASTIC 360., 0. 390., 1. *SOLID SECTION,ELSET=BLANK,MATERIAL=BLANK *ELSET,ELSET=OUT,GEN 1,10,1 *NSET,NSET=REF 2000,2001 *SURFACE,TYPE=ELEMENT,NAME=BLANK, REGION TYPE=SLIDING BLANK, *SURFACE, NAME=TOP, TYPE=SEGMENTS *INCLUDE,INPUT=ale_duckshape_forg_axirs.inp *RIGID BODY,REF NODE=2000, ANALYTICAL SURFACE =BOT_1 *RIGID BODY,REF NODE=2001, ANALYTICAL SURFACE =TOP *STEP *DYNAMIC,EXPLICIT ,0.105 *BOUNDARY 2000,1 2000,3,6 2001,1,6 SIDE,1,1

1-535

Static Stress/Displacement Analyses

*BOUNDARY,TYPE=VELOCITY 2000,2,2,-166.652 *CONTACT PAIR,INTERACTION=SMOOTH BLANK,TOP BLANK,BOT_1 *SURFACE INTERACTION,NAME=SMOOTH *FILE OUTPUT,TIMEMARKS=YES,NUM=4 *EL FILE,ELSET=OUT PEEQ,MISES *NODE FILE,NSET=REF U, *ADAPTIVE MESH,ELSET=BLANK *END STEP

1.3.12 Flat rolling: transient and steady-state Product: ABAQUS/Explicit This example illustrates the use of adaptive meshing to simulate a rolling process using both transient and steady-state approaches, as shown in Figure 1.3.12-1. A transient flat rolling simulation is performed using three different methods: a "pure" Lagrangian approach, an adaptive meshing approach using a Lagrangian domain, and a mixed Eulerian-Lagrangian adaptive meshing approach in which material upstream from the roller is drawn from an Eulerian inflow boundary but the downstream end of the blank is handled in a Lagrangian manner. In addition, a steady-state flat rolling simulation is performed using an Eulerian adaptive mesh domain as a control volume and defining inflow and outflow Eulerian boundaries. Solutions using each approach are compared.

Problem description For each analysis case quarter symmetry is assumed; the model consists of a rigid roller and a deformable blank. The blank is meshed with C3D8R elements. The roller is modeled as an analytical rigid surface using the *SURFACE, TYPE=CYLINDER and *RIGID BODY options. The radius of the cylinder is 175 mm. Symmetry boundary conditions are prescribed on the right (z=0 plane) and bottom (y=0 plane) faces of the blank. Coulomb friction with a friction coefficient of 0.3 is assumed between the roller and the plate. All degrees of freedom are constrained on the roller except rotation about the z-axis, where a constant angular velocity of 6.28 rad/sec is defined. For each analysis case the blank is given an initial velocity of 0.3 m/s in the x-direction to initiate contact. The blank is steel and is modeled as a von Mises elastic-plastic material with isotropic hardening. The Young's modulus is 150 GPa, and the initial yield stress is 168.2 MPa. The Poisson's ratio is 0.3; the density is 7800 kg/m3. The *FIXED MASS SCALING option is used to scale the masses of all the blank elements by a factor of 2750 so that the analysis can be performed more economically. This scaling factor represents an approximate upper bound on the mass scaling possible for this problem, above which significant inertial effects would be generated.

1-536

Static Stress/Displacement Analyses

The *STEADY STATE DETECTION option is used to define the criteria for stopping the rolling analyses based on the achievement of a steady-state condition. The criteria used require the satisfaction of the steady-state detection norms of equivalent plastic strain, spread, force, and torque within the default tolerances. The exit plane for each norm is defined as the plane passing through the center of the roller with the normal to the plane coincident with the rolling direction. The SAMPLING parameter is set to PLANE BY PLANE for Case 1 through Case 3 for the steady-state detection norms to be evaluated as each plane of elements passes the exit plane. Case 4 requires that the SAMPLING parameter is set to UNIFORM since the initial mesh is roughly stationary due to the initial geometry and the inflow and outflow Eulerian boundaries. The finite element models used for each analysis case are shown in Figure 1.3.12-2. A description of each model and the adaptive meshing techniques used follows:

Case 1: Transient simulation--pure Lagrangian approach The blank is initially rectangular and measures 224 ´ 20 ´ 50 mm. No adaptive meshing is performed. The analysis is run until steady-state conditions are achieved.

Case 2: Transient simulation--Lagrangian adaptive mesh domain The finite element model for this case is identical to that used for Case 1, with the exception that a single adaptive mesh domain that incorporates the entire blank is defined to allow continuous adaptive meshing. Symmetry planes are defined as Lagrangian surfaces (the default), and the contact surface on the blank is defined as a sliding surface (the default). The analysis is run until steady-state conditions are achieved.

Case 3: Transient simulation--mixed Eulerian-Lagrangian approach This analysis is performed on a relatively short initial blank measuring 65 ´ 20 ´ 50 mm. Material is continuously drawn by the action of the roller on the blank through an inflow Eulerian boundary defined on the upstream end. The blank is meshed with the same number of elements as in Cases 1 and 2 so that similar aspect ratios are obtained as the blank lengthens and steady-state conditions are achieved. An adaptive mesh domain is defined that incorporates the entire blank. Because it contains at least one Eulerian surface, this domain is considered Eulerian for the purpose of setting parameter defaults. However, the analysis model has both Lagrangian and Eulerian aspects. The amount of material flow with respect to the mesh will be large at the inflow end and small at the downstream end of the domain. To account for the Lagrangian motion of the downstream end, the MESHING PREDICTOR option on the *ADAPTIVE MESH CONTROLS option is changed from the default of PREVIOUS to CURRENT for this problem. To mesh the inflow end accurately and to perform the analysis economically, the FREQUENCY parameter is set to 5 and the MESH SWEEPS parameter is set to 5. As in Case 2, symmetry planes are defined as Lagrangian boundary regions (the default), and the contact surface on the blank is defined as a sliding boundary region (the default). In addition, an Eulerian boundary region is defined on the upstream end using the *SURFACE, REGION

1-537

Static Stress/Displacement Analyses

TYPE=EULERIAN option. Adaptive mesh constraints are defined on the Eulerian surface using the *ADAPTIVE MESH CONSTRAINT option to hold the inflow surface mesh completely fixed while material is allowed to enter the domain normal to the surface. The *EQUATION option is used to ensure that the velocity normal to the inflow boundary is uniform across the surface. The velocity of nodes in the direction tangential to the inflow boundary surface is constrained.

Case 4: Steady-state simulation--Eulerian adaptive mesh domain This analysis employs a control volume approach in which material is drawn from an inflow Eulerian boundary and is pushed out through an outflow boundary by the action of the roller. The blank geometry for this analysis case is defined such that it approximates the shape corresponding to the steady-state solution: this geometry can be thought of as an "initial guess" to the solution. The blank initially measures 224 mm in length and 50 mm in width and has a variable thickness such that it conforms to the shape of the roller. The surface of the blank transverse to the rolling direction is not adjusted to account for the eventual spreading that will occur in the steady-state solution. Actually, any reasonable initial geometry will reach a steady state, but geometries that are closer to the steady-state geometry often allow a solution to be obtained in a shorter period of time. As in the previous two cases an adaptive mesh domain is defined on the blank, symmetry planes are defined as Lagrangian surfaces (the default), and the contact surface is defined as a sliding surface (the default). Inflow and outflow Eulerian surfaces are defined on the ends of the blank using the same techniques as in Case 3, except that for the outflow boundary adaptive mesh constraints are applied only normal to the boundary surface and no material constraints are applied tangential to the boundary surface. To improve the computational efficiency of the analysis, the frequency of adaptive meshing is increased to every fifth increment because the Eulerian domain undergoes very little overall deformation and the material flow speed is much less than the material wave speed. This frequency will cause the mesh at Eulerian boundaries to drift slightly. However, the amount of drift is extremely small and does not accumulate. There is no need to increase the mesh sweeps because this domain is relatively stationary and the default MESHING PREDICTOR setting for Eulerian domains is PREVIOUS. Very little mesh smoothing is required.

Results and discussion The final deformed configurations of the blank for each of the three transient cases are shown in Figure 1.3.12-3. The transient cases have reached a steady-state solution and have been terminated based on the criteria defined using the *STEADY STATE DETECTION option. Steady-state conditions are determined to have been reached when the reaction forces and moments on the roller have stabilized and the cross-sectional shape and distribution of equivalent plastic strain under the roller become constant over time. When using the *STEADY STATE DETECTION option, these conditions imply that the force, moment, spread, and equivalent plastic strain norms have stabilized such that the changes in the norms over three consecutive sampling intervals have fallen below the user-prescribed tolerances. See ``Steady-state detection,'' Section 7.7.1 of the ABAQUS/Explicit User's Manual, for a detailed discussion on the definition of the norms. Contours of equivalent plastic strain for each of the three transient cases are in good agreement and are shown in the final configuration of each blank in

1-538

Static Stress/Displacement Analyses

Figure 1.3.12-4. Figure 1.3.12-5 shows the initial and final mesh configurations at steady state. With the exception of Case 3 all analyses were terminated using the default steady-state norm tolerances. Case 3 required that the force and torque norm tolerances be increased from .005 to .01 due to the force and torque at the roller being rather noisy. To compare the results from the transient and steady-state approaches, the steady-state detection norms are summarized for each case in Table 1.3.12-1. The table shows a comparison of the values of the steady-state detection norms after the analyses have been terminated. The only significant difference is in the value of the spread norm for Case 4, which is higher than the others. The spread norm is defined as the largest of the second principle moments of inertia of the workpiece's cross-section. Since the spread norm is a cubic function of the lateral deformation of the workpiece, rather small differences in displacements between the test cases can lead to significant differences in the spread norms. Time history plots of the steady-state detection norms are also shown. Figure 1.3.12-9 and Figure 1.3.12-10 show time history plots of the steady-state force and torque norms, respectively, for all cases. The force and torque norms are essentially running averages of the force and moment on the roller and show good agreement for all four test cases. Figure 1.3.12-7 and Figure 1.3.12-8 show time history plots of the steady-state equivalent plastic strain and spread norms, respectively, for all cases. The equivalent plastic strains norms are in good agreement for all cases.

Input files lag_flatrolling.inp Case 1. ale_flatrolling_noeuler.inp Case 2. ale_flatrolling_inlet.inp Case 3. ale_flatrolling_inletoutlet.inp Case 4.

Table Table 1.3.12-1 Comparison of steady-state detection norms. Force norm Formulatio Spread norm Effective n plastic strain norm Case 1 1.349 E-7 .8037 -1.43 E6 Case 2 1.369 E-7 .8034 -1.43 E6 Case 3 1.365 E-7 .8018 -1.43 E6 Case 4 1.485 E-7 .8086 -1.40 E6

1-539

Torque norm

3.59 E4 3.55 E4 3.61 E4 3.65 E4

Static Stress/Displacement Analyses

Figures Figure 1.3.12-1 Diagram illustrating the four analysis approaches used in this problem.

Figure 1.3.12-2 Initial configurations for each case.

1-540

Static Stress/Displacement Analyses

Figure 1.3.12-3 Deformed mesh for Cases 1-3.

1-541

Static Stress/Displacement Analyses

Figure 1.3.12-4 Contours of equivalent plastic strain for Cases 1-3.

1-542

Static Stress/Displacement Analyses

Figure 1.3.12-5 Deformed mesh for Case 4 (shown with initial mesh for comparison).

1-543

Static Stress/Displacement Analyses

Figure 1.3.12-6 Contours of equivalent plastic strain for Case 4.

Figure 1.3.12-7 Comparison of equivalent plastic strain norm versus time for all cases.

Figure 1.3.12-8 Comparison of spread norm versus time for all cases.

1-544

Static Stress/Displacement Analyses

Figure 1.3.12-9 Comparison of force norm versus time for all cases.

Figure 1.3.12-10 Comparison of torque norm versus time for all cases.

1-545

Static Stress/Displacement Analyses

Sample listings

1-546

Static Stress/Displacement Analyses

Listing 1.3.12-1 *HEADING ADAPTIVE MESHING EXAMPLE FLAT ROLLING - ADAPTIVE MESH, EULERIAN INLET NODES Units - N, m, second ** *RESTART,W,N=20 *NODE 1, -.0851, 0.00000, 0.00000 253, -.0851, 0.02000, 0.00000 42, -.0200, 0.00000, 0.00000 294, -.0200, 0.02000, 0.00000 2059,-.0851, 0.00000, 0.05000 2100,-.0200, 0.00000, 0.05000 2311,-.0851, 0.02000, 0.05000 2352,-.0200, 0.02000, 0.05000 *NGEN, NSET=BOT1 1,42,1 *NGEN, NSET=TOP1 253,294,1 *NFILL,NSET=FRONT BOT1, TOP1, 6, 42 *NGEN, NSET=BOT2 2059,2100,1 *NGEN, NSET=TOP2 2311,2352, 1 *NFILL,NSET=BACK BOT2,TOP2, 6, 42 *NFILL, NSET=BAR FRONT,BACK, 7, 294 *ELEMENT, TYPE=C3D8R 1, 1, 2, 295, 296, 338, *ELGEN, ELSET=BAR 1,41,1,1,6,42,41,7,294,246 *NSET,NSET=BOT,GEN 1,42,1 295,336,1 589,630,1 883,924,1 1177,1218,1

44, 337

1-547

43,

Static Stress/Displacement Analyses

1471,1512,1 1765,1806,1 2059,2100,1 *SOLID SECTION,ELSET=BAR,MAT=C15,CONTROLS=SECT 1., *SECTION CONTROLS, NAME=SECT,HOURGLASS=STIFFNESS ** *MATERIAL,NAME=C15 *ELASTIC 1.5E11,.3 *PLASTIC 168.72E06,0 219.33E06,0.1 272.02E06,0.2 308.53E06,0.3 337.37E06,0.4 361.58E06,0.5 382.65E06,0.6 401.42E06,0.7 418.42E06,0.8 434.01E06,0.9 448.45E06,1.0 *DENSITY 7.85E3, *********************************************** **** ROLL *NODE,NSET=REF 10000, 0.0409 , 0.185 *INITIAL CONDITIONS,TYPE=VELOCITY BAR,1,.30 *NSET,NSET=LEFT,GEN 1,294,1 *BOUNDARY LEFT,ZSYMM BOT,YSYMM *ELSET,ELSET=SIDE,GEN 1477,1722,1 *ELSET,ELSET=TOP,GEN 206,246,1 452,492,1 698,738,1 944,984,1 1190,1230,1

1-548

Static Stress/Displacement Analyses

1436,1476,1 1682,1722,1 *NSET,NSET=EULER,GEN 1,253,42 295,547,42 589,841,42 883,1135,42 1177,1429,42 1471,1723,42 1765,2017,42 2059,2311,42 *NSET,NSET=EULERINT,GEN 337,505,42 631,799,42 925,1093,42 1219,1387,42 1513,1681,42 1807,1975,42 *NSET, NSET=EULERSMALL1, GEN 295,547,42 589,841,42 883,1135,42 1177,1429,42 1471,1723,42 1765,2017,42 2059,2311,42 *NSET, NSET=EULERSMALL2, GEN 43,253,42 337,547,42 631,841,42 925,1135,42 1219,1429,42 1513,1723,42 1807,2017,42 2101,2311,42 *NSET,NSET=EQN,GEN 43,253,42 295,547,42 589,841,42 883,1135,42 1177,1429,42 1471,1723,42 1765,2017,42

1-549

Static Stress/Displacement Analyses

2059,2311,42 *EQUATION 2, EQN,1,1.,1,1,-1. *ELSET, ELSET=EULER, GEN 1,1477,246 42,1518,246 83,1559,246 124,1600,246 165,1641,246 206,1682,246 *SURFACE, NAME=SURF1, REGION TYPE=SLIDING TOP,S5 SIDE,S2 *SURFACE, REGION TYPE=EULERIAN, NAME=EULER1 EULER,S6 *SURFACE,TYPE=CYLINDER,NAME=RIGID, FILLET RADIUS=.001 0.0409 , 0.185, 0.0, 0.05, 0.185,0.0 0.0409 , 0.185, -0.05 START,0.0,-0.175 CIRCL,-0.175,0.0,0.0,0.0 CIRCL,0.0,0.175,0.0,0.0 *RIGID BODY, REFNODE=10000, ANALYTICAL SURFACE = RIGID *STEP *DYNAMIC,EXPLICIT ,0.50 *STEADY STATE DETECTION,ELSET=BAR, SAMPLING=PLANE BY PLANE 1.0, 0., 0., .1, 0.0, 0.0 *STEADY STATE CRITERIA SSPEEQ, , .0409, 0., 0. SSSPRD, , .0409, 0., 0. SSTORQ, .01, .0409, 0., 0., 10000, 0., 0., 1. SSFORC, .01, .0409, 0., 0., 10000, 0., 1., 0. *BOUNDARY 10000,1,5 *BOUNDARY,TYPE=VELOCITY 10000,6,6,6.2832 *BOUNDARY,TYPE=VELOCITY,REGION TYPE=EULERIAN EULERSMALL1,3,3,0.0 EULERSMALL2,2,2,0.0

1-550

Static Stress/Displacement Analyses

*FIXED MASS SCALING, FACTOR=2750. *SURFACE INTERACTION,NAME=FRICT *FRICTION 0.3, *CONTACT PAIR,INTERACTION=FRICT SURF1,RIGID *FILE OUTPUT, NUMBER INTERVAL=10, TIMEMARKS=YES *EL FILE, ELSET=TOP MISES,PEEQ, *NODE FILE,NSET=REF U,RF *OUTPUT, FIELD,NUMBER INTERVAL=10 *ELEMENT OUTPUT MISES, PEEQ *NODE OUTPUT U, *OUTPUT,HISTORY,TIME INTERVAL=1.E-4 *NODE OUTPUT,NSET=REF RF2,RM3 *INCREMENTATION OUTPUT SSPEEQ,SSSPRD,SSTORQ,SSFORC *ADAPTIVE MESH, ELSET=BAR,FREQUENCY=5, MESH SWEEPS=5,CONTROLS=ALE *ADAPTIVE MESH CONSTRAINT EULER,1,3,0.0 *ADAPTIVE MESH CONTROLS,NAME=ALE,MESHING =CURRENT *ENDSTEP

1.3.13 Section rolling Product: ABAQUS/Explicit This example illustrates the use of adaptive meshing in a transient simulation of section rolling. Results are compared to a pure Lagrangian simulation.

Problem description This analysis shows a stage in the rolling of a symmetric I-section. Because of the cross-sectional shape of the I-section, two planes of symmetry exist and only a quarter of the section needs to be modeled. The quarter-symmetry model, shown in Figure 1.3.13-1, consists of two rigid rollers and a blank. Roller 1 has a radius of 747 mm, and roller 2 has a radius of 452 mm. The blank has a length of 775 mm, a web half-width of 176.5 mm, a web half-thickness of 24 mm, and a variable flange thickness. The finite element model is shown in Figure 1.3.13-2. The blank is meshed with C3D8R elements.

1-551

Static Stress/Displacement Analyses

Symmetry boundary conditions are applied on the y and z symmetry planes of the blank. The rollers are modeled as TYPE=REVOLUTION analytical rigid surfaces. Roller 1 has all degrees of freedom constrained except rotation about the z-axis, where a constant angular velocity of 5 rad/sec is specified. Roller 2 has all degrees of freedom constrained except rotation about the y-axis. An initial velocity of 5602.5 mm/sec in the negative x-direction is applied to the blank to initiate contact between the blank and the rollers. This velocity corresponds to the velocity of the rollers at the point of initial contact. The *VARIABLE MASS SCALING, TYPE=BELOW MIN option is used to scale the masses of all the blank elements so that a desired minimum stable time increment is achieved initially and the stable time increment does not fall below this minimum throughout the analysis. The loading rates and mass scaling definitions are such that a quasi-static solution is generated. The blank is steel and is modeled as a von Mises elastic-plastic material with a Young's modulus of 212 GPa, an initial yield stress of 80 MPa, and a constant hardening slope of 258 MPa. Poisson's ratio is 0.3; the density is 7833 kg/m 3. Coulomb friction with a friction coefficient of 0.3 is assumed between the rollers and the blank.

Adaptive meshing Adaptive meshing can improve the solution and mesh quality for section rolling problems that involve large deformations. A single adaptive mesh domain that incorporates the entire blank is defined. Symmetry planes are defined as Lagrangian boundary regions (the default), and the contact surface on the blank is defined as a sliding boundary region (the default). The default values are used for all adaptive mesh parameters and controls.

Results and discussion Figure 1.3.13-3 shows the deformed configuration of the blank when continuous adaptive meshing is used. For comparison purposes Figure 1.3.13-4 shows the deformed configuration for a pure Lagrangian simulation. The mesh at the flange-web interface is distorted in the Lagrangian simulation, but the mesh remains nicely proportioned in the adaptive mesh analysis. A close-up view of the deformed configuration of the blank is shown for each analysis in Figure 1.3.13-5 and Figure 1.3.13-6 to highlight the differences in mesh quality. Contours of equivalent plastic strain for each analysis are shown in Figure 1.3.13-5 and Figure 1.3.13-6. The plastic strain distributions are very similar. Figure 1.3.13-7 and Figure 1.3.13-8show time history plots for the y-component of reaction force and the reaction moment about the z-axis, respectively, for roller 1. The results for the adaptive mesh simulation compare closely to those for the pure Lagrangian simulation.

Input files ale_rolling_section.inp Analysis that uses adaptive meshing. ale_rolling_sectionnode.inp External file referenced by the adaptive mesh analysis.

1-552

Static Stress/Displacement Analyses

ale_rolling_sectionelem.inp External file referenced by the adaptive mesh analysis. ale_rolling_sectionnelset.inp External file referenced by the adaptive mesh analysis. ale_rolling_sectionsurf.inp External file referenced by the adaptive mesh analysis. lag_rolling_section.inp Lagrangian analysis.

Figures Figure 1.3.13-1 Geometry of the quarter-symmetry blank and the rollers.

1-553

Static Stress/Displacement Analyses

Figure 1.3.13-2 Quarter-symmetry finite element model.

Figure 1.3.13-3 Deformed blank for the adaptive mesh simulation.

Figure 1.3.13-4 Deformed blank for the pure Lagrangian simulation.

1-554

Static Stress/Displacement Analyses

Figure 1.3.13-5 Close-up of the deformed blank for the adaptive mesh simulation.

Figure 1.3.13-6 Close-up of the deformed blank for the pure Lagrangian simulation.

1-555

Static Stress/Displacement Analyses

Figure 1.3.13-7 Contours of equivalent plastic strain for the adaptive mesh simulation.

Figure 1.3.13-8 Contours of equivalent plastic strain for the pure Lagrangian simulation.

1-556

Static Stress/Displacement Analyses

Figure 1.3.13-9 Time history of the reaction force in the y-direction at the reference node of Roller 1.

Figure 1.3.13-10 Time history of the reaction moment about the z-axis at the reference node of Roller 1.

1-557

Static Stress/Displacement Analyses

Sample listings

1-558

Static Stress/Displacement Analyses

Listing 1.3.13-1 *HEADING ADAPTIVE MESHING EXAMPLE SECTION ROLLING Units - N, m, seconds *RESTART, WRITE,NUMBER=10 *SYSTEM -0.0949794,0.,0., -0.0949794,1.,0. -0.0949794,0.,1. *INCLUDE, INPUT=ale_rolling_sectionnode.inp *INCLUDE, INPUT=ale_rolling_sectionelem.inp *INCLUDE, INPUT=ale_rolling_sectionnelset.inp ** SECTION: METAL *SOLID SECTION, ELSET=METAL, MATERIAL=STEEL 1., *MATERIAL, NAME=STEEL *DENSITY 7833., *ELASTIC 2.12E+11, 0.281 *PLASTIC 8e+07, 0., 2.35e+08, 0.6 *ELEMENT, TYPE=ROTARYI, ELSET=ROTI 50000,10117 *ROTARY INERTIA, ELSET=ROTI 1.E-4,11.05,1.E-4 ** INITIAL CONDITION: VELOCITY *INITIAL CONDITIONS, TYPE=VELOCITY ROLNODES, 1, -4.187 ROLNODES, 2, 0. ROLNODES, 3, 0. ** STEP: STEP-1 ** *SURFACE, TYPE=REVOLUTION, NAME=VROLSURF -0.1800, 0., 0.6221, -0.1800, 100., 0.6221 START, 0.2, 0.2 LINE, 0.4354, 0.2 LINE, 0.45182, 0.035821 CIRCL, 0.45182,-0.035821, 0.093604, 6.9389E-18 LINE, 0.4354, -0.2 LINE, 0.2, -0.2

1-559

Static Stress/Displacement Analyses

*SURFACE, TYPE=REVOLUTION, NAME=HROLSURF -0.1800, 0.760, 0., -0.180, 0.760, 100. START, 0.547, 0.137 LINE, 0.71051, 0.12261 CIRCL, 0.747, 0.082765, 0.707, 0.082765 LINE, 0.747, -0.082765 CIRCL, 0.71051, -0.12261, 0.707, -0.082765 LINE, 0.547, -0.137 *RIGID BODY, REF NODE=10116, ANALYTICAL SURFACE =HROLSURF *RIGID BODY, REF NODE=10117, ANALYTICAL SURFACE =VROLSURF *INCLUDE, INPUT=ale_rolling_sectionsurf.inp *STEP *DYNAMIC, EXPLICIT , 0.227 *BOUNDARY, OP=NEW HROLREF, 1, 1 HROLREF, 2, 2 HROLREF, 3, 3 HROLREF, 4, 4 HROLREF, 5, 5 *BOUNDARY, OP=NEW, TYPE=VELOCITY HROLREF, 6, 6,-5. *BOUNDARY, OP=NEW VROLREF, 1, 1 VROLREF, 2, 2 VROLREF, 3, 3 VROLREF, 4, 4 VROLREF, 6, 6 *BOUNDARY, OP=NEW YSYM, YSYMM *BOUNDARY, OP=NEW ZSYM, ZSYMM *SURFACE INTERACTION, NAME=PRO-1 *FRICTION 0.3, ** INTERACTION: HOR_ROLL *CONTACT PAIR, INTERACTION=PRO-1 FLANGSURF, HROLSURF ** INTERACTION: VER_ROLL *CONTACT PAIR, INTERACTION=PRO-1 WEBSURF, VROLSURF

1-560

Static Stress/Displacement Analyses

*FILE OUTPUT, NUMBER INTERVAL=10, TIME MARKS=NO *NODE FILE, NSET=HROLREF RF, *HISTORY OUTPUT, TIME INTERVAL=0.0026 *ENERGY HISTORY ALLAE, ALLCD, ALLFD, ALLIE, ALLKE, ALLPD, ALLSE ALLVD, ALLWK, ETOTAL *NODE HISTORY, NSET=HROLREF RF2, RF3, RM2, RM3 *NODE HISTORY, NSET=VROLREF RF2, RF3, RM3, RM2 ** MASS SCALING: WHOLEMODEL 1 ** ROLLING *VARIABLE MASS SCALING,TYPE=BELOW MIN, FREQUENCY =50, ELSET=METAL,DT=2.E-5 *ADAPTIVE MESH,ELSET=METAL *END STEP

1.3.14 Ring rolling Product: ABAQUS/Explicit This example illustrates the use of adaptive meshing in a two-dimensional rolling simulation. Results are compared to those obtained using a pure Lagrangian approach.

Problem description Ring rolling is a specialized process typically used to manufacture parts with revolved geometries such as bearings. The three-dimensional rolling setup usually includes a freely mounted, idle roll; a continuously rotating driver roll; and guide rolls in the rolling plane. Transverse to the rolling plane, conical rolls are used to stabilize the ring and provide a forming surface in the out-of-plane direction. In this example a two-dimensional, plane stress idealization is used that ignores the effect of the conical rolls. A schematic diagram of the ring and the surrounding tools is shown in Figure 1.3.14-1. The driver roll has a diameter of 680 mm, and the idle and guide rolls have diameters of 102 mm. The ring has an initial inner diameter of 127.5 mm and a thickness of 178.5 mm. The idle and driver rolls are arranged vertically and are in contact with the inner and outer surfaces of the ring, respectively. The driver roll is rotated around its stationary axis, while the idle roll is moved vertically downward at a specified feed rate. For this simulation the x-y motion of the guide rolls is determined a priori and is prescribed so that the rolls remain in contact with the ring throughout the analysis but do not exert appreciable force on it. In practice the guide rolls are usually connected through linkage systems, and their motion is a function of both force and displacement. The ring is meshed with CPS4R elements, as shown in Figure 1.3.14-2. The ring is steel and is

1-561

Static Stress/Displacement Analyses

modeled as a von Mises elastic-plastic material with a Young's modulus of 150 GPa, an initial yield stress of 168.7 MPa, and a constant hardening slope of 884 MPa. The Poisson's ratio is 0.3; the density is 7800 kg/m3. The analysis is run so that the ring completes approximately 20 revolutions (16.5 seconds). The rigid rolls are modeled as TYPE=SEGMENTS analytical rigid surfaces. The driver roll is rotated at a constant angular velocity of 3.7888 rad/sec about the z-axis, while the idle roll has a constant feed rate of 4.9334 mm/sec and is free to rotate about the z-axis. All other degrees of freedom for the driver and idle rolls are constrained. A friction coefficient of 0.5 is defined at the blank-idle roll and blank-drive roll interfaces. Frictionless contact is used between the ring and guide rolls, and the rotation of the guide rolls is constrained since the actual guide rolls are free to rotate and exert negligible torque on the ring. To obtain an economical solution, the *FIXED MASS SCALING option is used to scale the masses of all elements in the ring by a factor of 2500. This scaling factor represents a reasonable upper limit on the mass scaling possible for this problem, above which significant inertial effects would be generated. Furthermore, since the two-dimensional model does not contain the conical rolls, the ring oscillates from side to side even under the action of the guide rolls. An artificial viscous pressure of 300 MPa sec/m is applied on the inner and outer surfaces of the ring to assist the guide rolls in preserving the circular shape of the ring. The pressure value was chosen by trial and error.

Adaptive meshing A single adaptive mesh domain that incorporates the ring is defined. Contact surfaces on the ring are defined as sliding boundary regions (the default). Because of the large number of increments required to simulate 20 revolutions, the deformation per increment is very small. Therefore, the frequency of adaptive meshing is changed from the default of 10 to every 50 increments. The cost of adaptive meshing at this frequency is negligible compared to the underlying analysis cost.

Results and discussion Figure 1.3.14-3 shows the deformed configuration of the ring after completing 20 revolutions with continuous adaptive meshing. High-quality element shapes and aspect ratios are maintained throughout the simulation. Figure 1.3.14-4 shows the deformed configuration of the ring when a pure Lagrangian simulation is performed. The pure Lagrangian mesh is distorted, especially at the inner radius where elements become skewed and very small in the radial direction. Figure 1.3.14-5 and Figure 1.3.14-6show time history plots for the y-component of reaction force on the idle roll and the reaction moment about the z-axis for the driver roll, respectively, for both the adaptive mesh and pure Lagrangian approaches. Although the final meshes are substantially different, the roll force and torque match reasonably well. For both the adaptive and pure Lagrangian solutions the plane stress idealization used here results in very localized through-thickness straining at the inner and outer radii of the ring. This specific type of localized straining is unique to plane stress modeling and does not occur in ring rolling processes. It is also not predicted by a three-dimensional finite element model. If adaptivity is used and refined meshing is desired to capture strong gradients at the inner and outer extremities, the initially uniform

1-562

Static Stress/Displacement Analyses

mesh can be replaced with a graded mesh. Although not shown here, a graded mesh concentrates element refinement in areas of strong gradients. The adaptive meshing technique preserves the initial grading when the SMOOTHING OBJECTIVE=GRADED parameter is used on the *ADAPTIVE MESH CONTROLS option.

Input files ale_ringroll_2d.inp Analysis that uses adaptive meshing. ale_ringroll_2dnode.inp External file referenced by the adaptive mesh analysis. ale_ringroll_2delem.inp External file referenced by the adaptive mesh analysis. guideamp.inp External file referenced by the adaptive mesh analysis. lag_ringroll_2d.inp Lagrangian analysis.

Figures Figure 1.3.14-1 Model geometry for the two-dimensional ring rolling analysis.

1-563

Static Stress/Displacement Analyses

Figure 1.3.14-2 Initial mesh configuration.

Figure 1.3.14-3 Deformed configuration after 20 revolutions using adaptive meshing.

1-564

Static Stress/Displacement Analyses

Figure 1.3.14-4 Deformed configuration after 20 revolutions using a pure Lagrangian approach.

Figure 1.3.14-5 Time history of the reaction force in the y-direction for the idle roll.

1-565

Static Stress/Displacement Analyses

Figure 1.3.14-6 Time history of the reaction moment about the z-axis for the driver roll.

Sample listings

1-566

Static Stress/Displacement Analyses

Listing 1.3.14-1 *HEADING ADAPTIVE MESHING EXAMPLE ROLLING OF A RING IN 2D (PLANE STRESS) WITH SMALL VISCOUS PRESSURE TO STABILIZE THE RING. Units - N, m, sec ** *NODE, INPUT=ale_ringroll_2dnode.inp *ELEMENT, TYPE=CPS4R, ELSET=RING, INPUT=ale_ringroll_2delem.inp *SOLID SECTION, ELSET=RING, MAT=C15, CONTROLS=SECT 0.119, *SECTION CONTROLS, NAME=SECT,HOURGLASS=STIFFNESS *MATERIAL,NAME=C15 *ELASTIC 1.5E11,.3 *PLASTIC 168.72E6,0.0 1053.00E6,1.0 *DENSITY 7.85E3, ***************** rigid bodies *** Driver roll *BOUNDARY, OP=NEW 1660, 1,, 0. 1660, 2,, 0. 1660, 3,, 0. ** *BOUNDARY, OP=NEW 1660, 4,, 0. 1660, 5,, 0. ** *** Idle roll *BOUNDARY, OP=NEW 1648, 1,, 0. 1648, 3,, 0. ** *BOUNDARY, OP=NEW 1648, 4,, 0. 1648, 5,, 0. *ELEMENT, TYPE=ROTARYI, ELSET=IDLEI 9000, 1648

1-567

Static Stress/Displacement Analyses

*ROTARY INERTIA, ELSET=IDLEI **0., 0., 0.3176634 0., 0., 0.3176634E4 *** *** Left guide roll *BOUNDARY, OP=NEW 1651, 3,, 0. 1651, 4,, 0. 1651, 6,, 0. *ELEMENT, TYPE=MASS, ELSET=MASSGUIDE 8001, 1651 *** Right guide roll *BOUNDARY, OP=NEW 1649, 3,, 0. 1649, 4,, 0. 1649, 6,, 0. ** *ELEMENT, TYPE=MASS, ELSET=MASSGUIDE 8002, 1649 *** *MASS, ELSET=MASSGUIDE **61.06563 61.06563E4, ************** *AMPLITUDE, NAME=IDLEVEL, DEFINITION=SMOOTH STEP 0., 1., 16.3, 1.0, 16.5, 0.0 *AMPLITUDE, NAME=DRVRVEL, DEFINITION=SMOOTH STEP 0., 0., 0.2, 1.0, 16.5, 1.0 *INCLUDE, INPUT=guideamp.inp *SURFACE,TYPE=ELEMENT, NAME=EXTERIOR, REGION TYPE=SLIDING EXTERIOR, *SURFACE, TYPE=SEGMENTS, NAME=LFTGUIDE START,-.39192431,.77060147,-.39192431,.87260147 CIRCL,-.49392431,.87260147,-.39192431,.87260147 CIRCL,-.39192431,.97460147,-.39192431,.87260147 CIRCL,-.28992431,.87260147,-.39192431,.87260147 CIRCL,-.39192431,.77060147,-.39192431,.87260147 *SURFACE,TYPE=ELEMENT, NAME=INTERIOR, REGION TYPE=SLIDING INTERIOR, *SURFACE, TYPE=SEGMENTS, NAME=RHTGUIDE START,.39192431,.77060147,.39192431,.87260147

1-568

Static Stress/Displacement Analyses

CIRCL,.28992431,.87260147,.39192431,.87260147 CIRCL,.39192431,.97460147,.39192431,.87260147 CIRCL,.49392431,.87260147,.39192431,.87260147 CIRCL,.39192431,.77060147,.39192431,.87260147 *SURFACE, TYPE=SEGMENTS, NAME=DRIVER START, 0., -.680 CIRCL,-0.680, 0., 0., 0. CIRCL, 0., 0.680, 0., 0. CIRCL, 0.680, 0., 0., 0. CIRCL, 0., -0.680, 0.,0. *SURFACE, TYPE=SEGMENTS, NAME=IDLE START, 0., 0.8585 CIRCL,-0.102, 0.9605, 0., 0.9605 CIRCL, 0., 1.0625, 0., 0.9605 CIRCL, 0.102, 0.9605, 0., 0.9605 CIRCL, 0., 0.8585, 0., 0.9605 *RIGID BODY, REF NODE=1648, ANALYTICAL SURFACE =IDLE *RIGID BODY, REF NODE=1649, ANALYTICAL SURFACE =RHTGUIDE *RIGID BODY, REF NODE=1651, ANALYTICAL SURFACE =LFTGUIDE *RIGID BODY, REF NODE=1660, ANALYTICAL SURFACE =DRIVER *STEP Ring Rolling process in Plane Strain. Reduce the thickness of the ring by 55.0% *DYNAMIC, EXPLICIT , 16.5, *FIXED MASS SCALING, ELSET=RING,FACTOR=2500. *********************** rigid surfaces: ********* driver roll *BOUNDARY, TYPE=VELOCITY, AMP=DRVRVEL 1660, 6, 6, -3.78884 ********* idle roll *BOUNDARY, TYPE=VELOCITY, AMP=IDLEVEL 1648, 2, 2, -4.933417E-3 ********* left guide roll *BOUNDARY,TYPE=DISPLACEMENT,AMP=X1651 1651,1,1,-1.0 *BOUNDARY,TYPE=DISPLACEMENT,AMP=Y1651 1651,2,2,1.0 ********* right guide roll

1-569

Static Stress/Displacement Analyses

*BOUNDARY,TYPE=DISPLACEMENT,AMP=X1649 1649,1,1,1.0 *BOUNDARY,TYPE=DISPLACEMENT,AMP=Y1649 1649,2,2,1.0 ******** define the contact pairs *ELSET, ELSET=INTERIOR, GEN 1, 1433, 8 *ELSET, ELSET=EXTERIOR, GEN 8, 1440, 8 *CONTACT PAIR, INTERACTION=FRIC EXTERIOR, DRIVER INTERIOR, IDLE *SURFACE INTERACTION, NAME=FRIC *FRICTION 0.5, *CONTACT PAIR EXTERIOR, LFTGUIDE EXTERIOR, RHTGUIDE *DLOAD INTERIOR, VP4, 3.0e8 EXTERIOR, VP2, 3.0e8 ****** *RESTART, WRITE, NUM=10 *NSET, NSET=QRTRPNTS 1, 406, 820, 1234, 9, 414, 828, 1242 *ELSET, ELSET=THRURING, GEN 1, 8, 1 *MONITOR, NODE=1660, DOF=6 *HISTORY OUTPUT, TIME INTERVAL=0.1 *NSET, NSET=REFNODES 1660, 1648, 1651, 1649 *NODE HISTORY, NSET=REFNODES U, UR3, RF, RM3 *NODE HISTORY, NSET=QRTRPNTS U, *EL HISTORY, ELSET=THRURING MISES, PEEQ, PRESS, ERV *ENERGY HISTORY *FILE OUTPUT, NUMBER INTER=5, TIME MARKS=YES *NODE FILE, NSET=REFNODES U, RF *NODE FILE, NSET=QRTRPNTS U,

1-570

Static Stress/Displacement Analyses

*EL FILE, ELSET=THRURING MISES, PEEQ, PRESS, ERV *ADAPTIVE MESH, ELSET=RING,FREQUENCY=50 *END STEP

1.3.15 Axisymmetric extrusion: transient and steady-state Product: ABAQUS/Explicit This example illustrates the use of adaptive meshing in simulations of extrusion processes with three axisymmetric analysis cases. First, a transient simulation is performed for a backward, flat-nosed die, extrusion geometry using adaptivity on a Lagrangian mesh domain. Second, a transient simulation is performed on the analogous forward, square die, extrusion geometry, also using adaptivity on a Lagrangian mesh domain. Finally, a steady-state simulation is performed for the forward extrusion geometry using adaptivity on an Eulerian mesh domain.

Problem description The model configurations for the three analysis cases are shown in Figure 1.3.15-1. Each of the models is axisymmetric and consists of one or more rigid tools and a deformable blank. The rigid tools are modeled as TYPE=SEGMENTS analytical rigid surfaces. All contact surfaces are assumed to be well-lubricated and, thus, are treated as frictionless. The blank is made of aluminum and is modeled as a von Mises elastic-plastic material with isotropic hardening. The Young's modulus is 38 GPa, and the initial yield stress is 27 MPa. The Poisson's ratio is 0.33; the density is 2672 kg/m 3.

Case 1: Transient analysis of a backward extrusion The model geometry consists of a rigid die, a rigid punch, and a blank. The blank is meshed with CAX4R elements and measures 28 ´ 89 mm. The blank is constrained along its base in the z-direction and at the axis of symmetry in the r-direction. Radial expansion is prevented by contact between the blank and the die. The punch and the die are fully constrained, with the exception of the prescribed vertical motion of the punch. The punch is moved downward 82 mm to form a tube with wall and endcap thicknesses of 7 mm each. The punch velocity is specified using the SMOOTH STEP parameter on the *AMPLITUDE option so that the response is essentially quasi-static. The deformation that occurs in extrusion problems, especially in those that involve flat-nosed die geometries, is extreme and requires adaptive meshing. Since adaptive meshing in ABAQUS/Explicit works with the same mesh topology throughout the step, the initial mesh must be chosen such that the mesh topology will be suitable for the duration of the simulation. A simple meshing technique has been developed for extrusion problems such as this. In two dimensions it uses a four-sided, mapped mesh domain that can be created with nearly all finite element mesh preprocessors. The vertices for the four-sided, mapped mesh are shown in Figure 1.3.15-1 and are denoted A, B, C, and D. Two vertices are located on either side of the extrusion opening, the third is in the corner of the dead material zone (the upper right corner of the blank), and the fourth vertex is located in the diagonally opposite corner. A 10 ´ 60 element mesh using this meshing technique is created for this analysis case and is shown in Figure 1.3.15-2. The mesh refinement is oriented such that the fine mesh along sides BC and DA will

1-571

Static Stress/Displacement Analyses

move up along the extruded walls as the punch is moved downward. An adaptive mesh domain is defined that incorporates the entire blank. Because of the extremely large distortions expected in the backward extrusion simulation, three mesh sweeps, instead of the default value of one, are specified using the MESH SWEEPS parameter on the *ADAPTIVE MESH option. The default adaptive meshing frequency of 10 is used. Alternatively, a higher frequency could be specified to perform one mesh sweep per adaptive mesh increment. However, this method would result in a higher computational cost because of the increased number of advection sweeps it would require. A substantial amount of initial mesh smoothing is performed by increasing the value of the INITIAL MESH SWEEPS parameter on the *ADAPTIVE MESH option to 100. The initially smoothed mesh is shown in Figure 1.3.15-2. Initial smoothing reduces the distortion of the mapped mesh by rounding out corners and easing sharp transitions before the analysis is performed; therefore, it allows the best mesh to be used throughout the analysis.

Case 2: Transient analysis of a forward extrusion The model geometry consists of a rigid die and a blank. The blank geometry and the mesh are identical to those described for Case 1, except that the mapped mesh is reversed with respect to the vertical plane so that the mesh lines are oriented toward the forward extrusion opening. The blank is constrained at the axis of symmetry in the r-direction. Radial expansion is prevented by contact between the blank and the die. The die is fully constrained. The blank is pushed up 19 mm by prescribing a constant velocity of 5 m/sec for the nodes along the bottom of the blank. As the blank is pushed up, material flows through the die opening to form a solid rod with a 7 mm radius. Adaptive meshing for Case 2 is defined in a similar manner as for Case 1. The undeformed mesh configurations, before and after initial mesh smoothing, are shown in Figure 1.3.15-3.

Case 3: Steady-state analysis of a forward extrusion The model geometry consists of a rigid die, identical to the die used for Case 2, and a blank. The blank geometry is defined such that it closely approximates the shape corresponding to the steady-state solution: this geometry can be thought of as an "initial guess" to the solution. As shown in Figure 1.3.15-4, the blank is discretized with a simple graded pattern that is most refined near the die fillet. No special mesh is required for the steady-state case since minimal mesh motion is expected during the simulation. The blank is constrained at the axis of symmetry in the r-direction. Radial expansion of the blank is prevented by contact between it and the die. An adaptive mesh domain is defined that incorporates the entire blank. Because the Eulerian domain undergoes very little overall deformation and the material flow speed is much less than the material wave speed, the frequency of adaptive meshing is changed to 5 from the default value of 1 to improve the computational efficiency of the analysis. The outflow boundary is assumed to be traction-free and is located far enough downstream to ensure that a steady-state solution can be obtained. This boundary is defined using the *SURFACE, REGION TYPE=EULERIAN option. A multi-point constraint is defined on the outflow boundary to keep the velocity normal to the boundary uniform. The inflow boundary is defined using the *BOUNDARY, REGION TYPE=EULERIAN option to prescribe a velocity of 5 m/sec in the vertical direction.

1-572

Static Stress/Displacement Analyses

Adaptive mesh constraints are defined on both the inflow and outflow boundaries to fix the mesh in the vertical direction using the *ADAPTIVE MESH CONSTRAINT option. This effectively creates a stationary control volume with respect to the inflow and outflow boundaries through which material can pass.

Results and discussion The results for each analysis case are described below.

Case 1 The use of the mapped meshing technique along with adaptive meshing allows the backward extrusion analysis to run to completion, creating the long tube with an endcap. Three plots of the deformed mesh at various times are shown in Figure 1.3.15-5. These plots clearly show how the quality of the mesh is preserved for the majority of the simulation. Despite the large amount of deformation involved, the mesh remains smooth and concentrated in the areas of high strain gradients. Extreme deformation and thinning at the punch fillet occurs near the end of the analysis. This thinning can be reduced by increasing the fillet radius of the punch. Corresponding contours of equivalent plastic strain are plotted in Figure 1.3.15-6. The plastic strains are highest along the inner surface of the tube.

Case 2 Adaptive meshing enables the transient forward extrusion simulation to proceed much further than would be possible using a pure Lagrangian approach. After pushing the billet 19 mm through the die, the analysis cannot be continued because the elements become too distorted. Since the billet material is essentially incompressible and the cross-sectional area of the die opening at the top is 1/16 of the original cross-sectional area of the billet, a rod measuring approximately 304 mm (three times the length of the original billet) is formed. Three plots of the deformed mesh at various times in the transient forward extrusion are shown in Figure 1.3.15-7. As in the backward extrusion case, the plots show that the quality of the mesh is preserved for a majority of the simulation. The last deformed shape has been truncated for clarity because the extruded column becomes very long and thin. Contours of equivalent plastic strain at similar times are shown in Figure 1.3.15-8. The plastic strain distribution developing in the vertical column does not reach a steady-state value, even at a height of 304 mm. The steady-state results reported in the discussion for Case 3 show that a steady-state solution based on the equivalent plastic strain distribution is not reached until much later. An absolute steady-state solution cannot be reached until the material on the upstream side of the dead material zone first passes along that zone and through the die opening. The dead material zone is roughly the shape of a triangle and is located in the upper right-hand corner of the die.

Case 3 The steady-state solution to the forward extrusion analysis is obtained at an extruded column height of 800 mm, which corresponds to pushing the billet 50 mm through the die. Thus, this analysis runs 2.5 times longer than Case 2.

1-573

Static Stress/Displacement Analyses

Contours of equivalent plastic strain in the middle and at the end of the simulation are shown in Figure 1.3.15-9. Time histories of the equivalent plastic strains on the outer edge of the extruded column at the outflow boundary and 27.5 mm below the outflow boundary are shown in Figure 1.3.15-10. The plastic strains at both locations converge to the same value by the end of the simulation, which indicates that the solution has reached a steady state. The final mesh configuration is shown in Figure 1.3.15-11. The mesh undergoes very little change from the beginning to the end of the analysis because of the accurate initial guess made for the steady-state domain shape and the ability of the adaptive meshing capability in ABAQUS/Explicit to retain the original mesh gradation. As a further check on the accuracy of the steady-state simulation and the conservation properties of adaptive meshing, a time history of the velocity at the outflow boundary is shown in Figure 1.3.15-12. The velocity reaches a steady value of approximately 80 m/s, which is consistent with the incompressible material assumption and the 1/16 ratio of the die opening to the billet size.

Input files ale_extrusion_back.inp Case 1. ale_extrusion_backnode.inp Node data for Case 1. ale_extrusion_backelem.inp Element data for Case 1. ale_extrusion_forward.inp Case 2. ale_extrusion_forwardnode.inp Node data for Case 2. ale_extrusion_forwardelem.inp Element data for Case 2. ale_extrusion_eulerian.inp Case 3. ale_extrusion_euleriannode.inp Node data for Case 3. ale_extrusion_eulerianelem.inp Element data for Case 3.

Figures

1-574

Static Stress/Displacement Analyses

Figure 1.3.15-1 Axisymmetric model geometries used in the extrusion analysis.

Figure 1.3.15-2 Undeformed configuration for Case 1, before and after initial smoothing.

1-575

Static Stress/Displacement Analyses

Figure 1.3.15-3 Undeformed configuration for Case 2, before and after initial smoothing.

1-576

Static Stress/Displacement Analyses

Figure 1.3.15-4 Undeformed configuration for Case 3.

1-577

Static Stress/Displacement Analyses

Figure 1.3.15-5 Deformed mesh at various times for Case 1.

1-578

Static Stress/Displacement Analyses

Figure 1.3.15-6 Contours of equivalent plastic strain at various times for Case 1.

1-579

Static Stress/Displacement Analyses

Figure 1.3.15-7 Deformed mesh at various times for Case 2.

1-580

Static Stress/Displacement Analyses

Figure 1.3.15-8 Contours of equivalent plastic strain at various times for Case 2.

1-581

Static Stress/Displacement Analyses

Figure 1.3.15-9 Contours of equivalent plastic strain at an intermediate stage and at the end of the analysis for Case 3.

1-582

Static Stress/Displacement Analyses

Figure 1.3.15-10 Time history of equivalent plastic strain along the outer edge of the extruded column for Case 3.

Figure 1.3.15-11 Final deformed mesh for Case 3.

1-583

Static Stress/Displacement Analyses

Figure 1.3.15-12 Time history of material velocity at the outflow boundary for Case 3.

Sample listings

1-584

Static Stress/Displacement Analyses

Listing 1.3.15-1 *HEADING ADAPTIVE MESHING EXAMPLE BACKWARD EXTRUSION,MATERIAL: ALUMINIUM Units: N, m, second *RESTART,W,N=10 *NODE, INPUT=ale_extrusion_backnode.inp ** *ELEMENT, TYPE=CAX4R,ELSET=BLANK, INPUT=ale_extrusion_backelem.inp *NSET, NSET=BOT, GENERATE 979, 1001, 1 *NSET, NSET=RIGHT,GENERATE 911, 979, 1 *NSET, NSET=TOP, GENERATE 1, 92, 1 183, 183, 1 274, 274, 1 365, 365, 1 456, 456, 1 547, 547, 1 638, 638, 1 729, 729, 1 820, 820, 1 911, 911, 1 *NSET, NSET=LEFT 91, 182, 273, 364, 455, 546, 637, 728, 819, 910, 1001 ** *SOLID SECTION, ELSET=BLANK, MATERIAL=ALUMINIUM *MATERIAL, NAME=ALUMINIUM *ELASTIC 38E9,0.33 *PLASTIC 27E6,0 31E6,0.25 32.5E6,0.5 *DENSITY 2672, *BOUNDARY 9999,1,1

1-585

Static Stress/Displacement Analyses

9999,6,6 LEFT,XSYMM BOT,YSYMM 9998,1,6 *NSET,NSET=REF 9999,9998 *ELSET, ELSET=OUT 1,2,3 *SURFACE,NAME=RIGHTS,TYPE=SEGMENTS START,0.028,-0.001 LINE,0.028,0.2 *SURFACE,TYPE=NODE,NAME=NSURF NCON, *SURFACE,NAME=TOPS,TYPE=SEGMENTS,FILLET =0.002 START,0.021,0.2 LINE,0.021,0.089 LINE,-0.0001,0.089 *RIGID BODY,REF NODE= 9998, ANALYTICAL SURFACE =RIGHTS *RIGID BODY,REF NODE= 9999, ANALYTICAL SURFACE =TOPS *STEP *DYNAMIC, EXPLICIT ,1.50337E-3 *BOUNDARY,TYPE=VELOCITY, AMP=STEP 9999,2,2,-60.0 *AMPLITUDE, DEFINITION=SMOOTH STEP, NAME=STEP 0.,0.,1.36667e-4,1.,1.36667e-3,1.,1.50337E-3, 0. *NSET,NSET=NCON TOP,RIGHT *CONTACT PAIR,INTERACTION=I1 NSURF,TOPS NSURF,RIGHTS *SURFACE INTERACTION,NAME=I1 *FILE OUTPUT, NUMBER=4, TIME MARKS=YES *NODE FILE, NSET=REF U,RF *EL FILE,ELSET=OUT MISES,PEEQ *ADAPTIVE MESH,ELSET=BLANK,FREQUENCY=10, MESH SWEEPS=3, INITIAL MESH SWEEPS=100 *ENDSTEP

1-586

Static Stress/Displacement Analyses

1.3.16 Two-step forming simulation Product: ABAQUS/Explicit This example illustrates the use of adaptive meshing in simulations of a two-step, bulk metal forming process. The problem is based on a benchmark problem presented at the Metal Forming Process Simulation in Industry conference.

Problem description The model consists of two sets of rigid forming tools (one set for each forming step) and a deformable blank. The blank and forming die geometries used in the simulation are shown in Figure 1.3.16-1. The initial configurations of the blank and the tools for each step are shown in Figure 1.3.16-2 and Figure 1.3.16-4. All forming tools are modeled as discrete rigid bodies and meshed with R3D4 and R3D3 elements. The blank, which is meshed with C3D8R elements, is cylindrical and measures 14.5 ´ 21 mm. A half model is constructed, so symmetry boundary conditions are prescribed at the y=0 plane. The blank is made of a steel alloy that is assumed to satisfy the Ramberg-Osgood relation for true stress and logarithmic strain, ² = (¾=K )1=n ; with a reference stress value (K) of 763 MPa and a work-hardening exponent (n) of 0.245. Isotropic elasticity is assumed, with a Young's modulus of 211 GPa and a Poisson's ratio of 0.3. An initial yield stress of 200 MPa is obtained with these data. The stress-strain behavior is defined by piecewise linear segments matching the Ramberg-Osgood curve up to a total (logarithmic) strain level of 140%, with von Mises yield and isotropic hardening. The analysis is conducted in two steps. For the first step the rigid tools consist of a planar punch, a planar base, and a forming die. The initial configuration for this step is shown in Figure 1.3.16-2. The base, which is not shown, is placed at the opening of the forming die to prevent material from passing through the die. The motion of the tools is fully constrained, with the exception of the prescribed displacement in the z-direction for the punch, which is moved 12.69 mm toward the blank at a constant velocity of 30 m/sec consistent with a quasi-static response. The deformed configuration of the blank at the completion of the first step is shown in Figure 1.3.16-3. In the second step the original punch and die are removed from the model and replaced with a new punch and die, as shown in Figure 1.3.16-4. The removal of the tools is accomplished by deleting the contact pairs between them and the blank with the *CONTACT PAIR, OP=DELETE option. Although not shown in the figure, the base is retained; both it and the new die are fully constrained. The punch is moved 10.5 mm toward the blank at a constant velocity of 30 m/sec consistent with a quasi-static response. The deformed configuration of the blank at the completion of the second step is shown in Figure 1.3.16-5.

Adaptive meshing 1-587

Static Stress/Displacement Analyses

A single adaptive mesh domain that incorporates the entire blank is used for both steps. A Lagrangian boundary region type (the default) is used to define the constraints on the symmetry plane, and a sliding boundary region type (the default) is used to define all contact surfaces. The frequency of adaptive meshing is increased to 5 for this problem since material flows quickly near the end of the step.

Results and discussion Figure 1.3.16-6 shows the deformed mesh at the completion of forming for an analysis in which a pure Lagrangian mesh is used. Comparing Figure 1.3.16-5 and Figure 1.3.16-6, the resultant mesh for the simulation in which adaptive meshing is used is clearly better than that obtained with a pure Lagrangian mesh. In Figure 1.3.16-7 through Figure 1.3.16-9path plots of equivalent plastic strain in the blank are shown using the pure Lagrangian and adaptive mesh domains for locations in the y=0 symmetry plane at an elevation of z=10 mm. The paths are defined in the positive x-direction (from left to right in Figure 1.3.16-4 to Figure 1.3.16-6). As shown in Figure 1.3.16-7, the results are in good agreement at the end of the first step. At the end of the second step the path is discontinuous. Two paths are considered: one that spans the left-hand side and another that spans the right-hand side of the U-shaped cross-section along the symmetry plane. The left- and right-hand paths are shown in Figure 1.3.16-8and Figure 1.3.16-9, respectively. The solutions from the second step compare qualitatively. Small differences can be attributed to the increased mesh resolution and reduced mesh distortion for the adaptive mesh domain.

Input files ale_forging_steelpart.inp Analysis with adaptive meshing. ale_forging_steelpartnode1.inp External file referenced by the adaptive mesh analysis. ale_forging_steelpartnode2.inp External file referenced by the adaptive mesh analysis. ale_forging_steelpartnode3.inp External file referenced by the adaptive mesh analysis. ale_forging_steelpartnode4.inp External file referenced by the adaptive mesh analysis. ale_forging_steelpartelem1.inp External file referenced by the adaptive mesh analysis. ale_forging_steelpartelem2.inp

1-588

Static Stress/Displacement Analyses

External file referenced by the adaptive mesh analysis. ale_forging_steelpartelem3.inp External file referenced by the adaptive mesh analysis. ale_forging_steelpartelem4.inp External file referenced by the adaptive mesh analysis. ale_forging_steelpartelem5.inp External file referenced by the adaptive mesh analysis. ale_forging_steelpartsets.inp External file referenced by the adaptive mesh analysis. lag_forging_steelpart.inp Pure Lagrangian analysis.

Reference · Hermann, M. and A. Ruf, "Forming of a Steel Part," Metal Forming Process Simulation in Industry, Stuttgart, Germany, September 1994.

Figures Figure 1.3.16-1 Two-step forging process.

1-589

Static Stress/Displacement Analyses

Figure 1.3.16-2 Initial configuration for the first step.

1-590

Static Stress/Displacement Analyses

Figure 1.3.16-3 Deformed blank at the end of the first step.

Figure 1.3.16-4 Configuration at the beginning of the second step.

Figure 1.3.16-5 Deformed blank at the end of the second step for the adaptive mesh analysis.

1-591

Static Stress/Displacement Analyses

Figure 1.3.16-6 Deformed blank at the end of the second step for the pure Lagrangian analysis.

Figure 1.3.16-7 Path plot of equivalent plastic strain at the end of the first step.

Figure 1.3.16-8 Path plot of equivalent plastic strain along the left side at the end of the second step.

1-592

Static Stress/Displacement Analyses

Figure 1.3.16-9 Path plot of equivalent plastic strain along the right side at the end of the second step.

Sample listings

1-593

Static Stress/Displacement Analyses

Listing 1.3.16-1 *HEADING ADAPTIVE MESHING EXAMPLE TWO-STAGE FORGING OF A STEEL PART Units: N, mm, seconds *NODE,NSET=MOLD, INPUT=ale_forging_steelpartnode1.inp *NODE,NSET=DIE1, INPUT=ale_forging_steelpartnode2.inp *ELEMENT, TYPE=C3D8R, ELSET=MOLD, INPUT=ale_forging_steelpartelem1.inp *NODE,NSET=PUNCH1 2000001,-1.,-1.,29. 200000,-1.,-1.,29. 200001,44.,-1.,29. 200002,44.,20.,29. 200003,-1.,20.,29. *ELEMENT, TYPE=R3D4, ELSET=PUNCH1 200000,200000,200003,200002,200001 *NODE,NSET=BASE 3000001,-1.,-1.,.000001 300000,-1.,-1.,.000001 300001,44.,-1.,.000001 300002,44.,20.,.000001 300003,-1.,20.,.000001 *ELEMENT, TYPE=R3D4, ELSET=BASE 300000,300000,300001,300002,300003 *ELEMENT, TYPE=R3D4, ELSET=DIE1, INPUT=ale_forging_steelpartelem2.inp *NODE,NSET=PUNCH2, INPUT=ale_forging_steelpartnode3.inp *ELEMENT, TYPE=R3D4, ELSET=PUNCH2, INPUT=ale_forging_steelpartelem3.inp *ELEMENT, TYPE=R3D3, ELSET=PUNCH2, INPUT=ale_forging_steelpartelem4.inp *NODE,NSET=DIE2, INPUT=ale_forging_steelpartnode4.inp *ELEMENT, TYPE=R3D4, ELSET=DIE2, INPUT=ale_forging_steelpartelem5.inp *INCLUDE,INPUT=ale_forging_steelpartsets.inp *BOUNDARY 1000001,1,6

1-594

Static Stress/Displacement Analyses

2000001,1,2 2000001,4,6 3000001,1,6 4000001,1,6 5000001,1,6 YSYMM,YSYMM RIG1,YSYMM RIG2,YSYMM RIG3,YSYMM RIG4,YSYMM *SOLID SECTION,ELSET=MOLD,MATERIAL=C15, CONTROLS=SECT *SECTION CONTROLS,NAME=SECT,HOURGLASS=STIFFNESS, KINEMATICS=ORTHOGONAL ** *MATERIAL,NAME=C15 *ELASTIC 210000.,0.3 *PLASTIC 200.000, 0.000 246.934, 0.010 434.092, 0.100 514.439, 0.200 568.167, 0.300 609.658, 0.400 643.916, 0.500 673.331, 0.600 699.247, 0.700 722.501, 0.800 743.654, 0.900 763.100, 1.000 781.129, 1.100 797.960, 1.200 813.762, 1.300 828.672, 1.400 *DENSITY 7.85E-9, *RESTART,WRITE,NUM=2 *NSET,NSET=P1 2000001, *NSET,NSET=P2 4000001, *SURFACE,TYPE=ELEMENT,NAME=PUNCH2

1-595

Static Stress/Displacement Analyses

PUNCH2,SPOS *SURFACE,TYPE=ELEMENT,NAME=TOP,REGION TYPE=SLIDING TOP,S2 *SURFACE,TYPE=ELEMENT,NAME=DIE1 DIE1,SPOS *SURFACE,TYPE=ELEMENT,NAME=DIE2 DIE2,SPOS *SURFACE,TYPE=ELEMENT,NAME=SIDE, REGION TYPE=SLIDING SIDE2,S5 SIDE4,S4 *SURFACE,TYPE=ELEMENT,NAME=BOTTOM, REGION TYPE=SLIDING BOTTOM,S1 *SURFACE,TYPE=ELEMENT,NAME=BASE BASE,SPOS *SURFACE,TYPE=ELEMENT,NAME=PUNCH1 PUNCH1,SPOS *RIGID BODY,ELSET=DIE1,REF NODE=1000001 *RIGID BODY,ELSET=PUNCH1,REF NODE=2000001 *RIGID BODY,ELSET=BASE,REF NODE=3000001 *RIGID BODY,ELSET=PUNCH2,REF NODE=4000001 *RIGID BODY,ELSET=DIE2,REF NODE=5000001 *STEP *DYNAMIC,EXPLICIT ,.000423333 *BOUNDARY,TYPE=VELOCITY 2000001,3,3,-30000. *CONTACT PAIR,INTERACTION=FRIC BOTTOM,BASE BOTTOM,DIE1 SIDE,DIE1 TOP,PUNCH1 ** *SURFACE INTERACTION, NAME=FRIC *FRICTION 0.1, ** *HISTORY OUTPUT,TIMEINTERVAL=0.0000042 *NODE HISTORY,NSET=P1 U,RF *ADAPTIVE MESH,ELSET=MOLD,FREQUENCY=5, CONTROLS=TEST

1-596

Static Stress/Displacement Analyses

*ADAPTIVE MESH CONTROLS, NAME=TEST, TRANSITION FEATURE ANGLE=0.0 *OUTPUT,FIELD,number=2 *ELEMENT OUTPUT peeq,mises *node output u, *END STEP *STEP *DYNAMIC,EXPLICIT ,.00035 *BOUNDARY,TYPE=VELOCITY 4000001,3,3,-30000. *CONTACT PAIR,INTERACTION=FRIC,OP=DELETE BOTTOM,DIE1 SIDE,DIE1 TOP,PUNCH1 ** *CONTACT PAIR,INTERACTION=FRIC BOTTOM,DIE2 SIDE,DIE2 TOP,PUNCH2 ** *SURFACE INTERACTION, NAME=FRIC *FRICTION 0.1, ** *HISTORY OUTPUT,TIMEINTERVAL=0.0000035 *NODE HISTORY,NSET=P2 U,RF *EL HISTORY,ELSET=TOP PEEQ, EDT, *ENERGY HISTORY ALLKE,ALLIE,ALLAE,ALLVD,ALLWK,ETOTAL, DT, *ADAPTIVE MESH,ELSET=MOLD,FREQUENCY=5 *OUTPUT,FIELD,number=2 *ELEMENT OUTPUT peeq,mises *node output u, *END STEP

1-597

Static Stress/Displacement Analyses

1.3.17 Upsetting of a cylindrical billet: coupled temperature-displacement and adiabatic analysis Products: ABAQUS/Standard ABAQUS/Explicit This example illustrates coupled temperature-displacement analysis in a metal forming application. The case studied is an extension of the standard test case that is defined in Lippmann (1979); thus, some verification of the results is available by comparison with the numerical results presented in that reference. The example is that of a small, circular billet of metal that is reduced in length by 60%. Here the problem is analyzed as a viscoplastic case, including heating of the billet by plastic work. Such analysis is often important in manufacturing processes, especially when significant temperature rises degrade the material. The problem is also analyzed in ABAQUS/Standard using a porous metal material model. The same problem is used to illustrate mesh rezoning in ABAQUS/Standard in ``Upsetting of a cylindrical billet in ABAQUS/Standard: quasi-static analysis with rezoning,'' Section 1.3.1; the same test case is also used in ``Upsetting of a cylindrical billet in ABAQUS/Explicit,'' Section 1.3.2.

Geometry and model The specimen is shown in Figure 1.3.17-1: a circular billet, 30 mm long, with a radius of 10 mm, compressed between flat, rough, rigid dies. All surfaces of the billet are assumed to be fully insulated: this thermal boundary condition is chosen to maximize the temperature rise. The finite element model is axisymmetric and includes the top half of the billet only since the middle surface of the billet is a plane of symmetry. In ABAQUS/Standard elements of type CAX8RT, 8-node quadrilaterals with reduced integration that allow for fully coupled temperature-displacement analysis, are used. A regular mesh with six elements in each direction is used, as shown in Figure 1.3.17-1. In ABAQUS/Explicit the billet is modeled with CAX4RT elements in a 12 ´ 12 mesh. The contact between the top and the lateral exterior surfaces of the billet and the rigid die is modeled with the *CONTACT PAIR option. The billet surface is defined by means of the *SURFACE option. The rigid die is modeled as an analytical rigid surface or as an element-based rigid surface, using the *RIGID BODY option in conjunction with the *SURFACE option. The mechanical interaction between the contact surfaces is assumed to be nonintermittent, rough frictional contact in ABAQUS/Standard. Therefore, two options are used in conjunction with the *SURFACE INTERACTION property option: the *FRICTION, ROUGH option to enforce a no-slip constraint between the two surfaces and the *SURFACE BEHAVIOR, NO SEPARATION option to ensure that separation does not occur once contact has been established. In ABAQUS/Explicit the friction coefficient between the billet and the rigid die is 1.0. The problem is also solved in ABAQUS/Standard with the first-order fully coupled temperature-displacement CAX4T elements in a 12 ´ 12 mesh. Similarly, the problem is solved using CAX8RT elements and user subroutines UMAT and UMATHT to illustrate the use of these subroutines. No mesh convergence studies have been performed, but the comparison with results given in

1-598

Static Stress/Displacement Analyses

Lippmann (1979) suggests that these meshes provide accuracy similar to the best of those analyses. The ABAQUS/Explicit simulations are performed both with and without adaptive meshing.

Material The material definition is basically that given in Lippmann (1979), except that the metal is assumed to be rate dependent. The thermal properties are added, with values that correspond to a typical steel, as well as the data for the porous metal plasticity model. The material properties are then Young's modulus: 200 GPa Poisson's ratio: 0.3 Thermal expansion coefficient: 1.2´10-5 per °C Initial static yield stress: 700 MPa Work hardening rate: 300 MPa¡ ¢p "_pl = D (¾=¾ ± ) ¡ 1 ; D = 40/s, p = 5 Strain rate dependence: Specific heat: 586 J/(kg°C) Density: 7833 kg/m3 Conductivity: 52 J/(m-s-°C) q Porous material parameters: 1 = q2 = q3 = 1:0 Initial relative density: 0.95 (f0 = 0.05) Since the problem definition in ABAQUS/Standard assumes that the dies are completely rough, no tangential slipping is allowed wherever the metal contacts the die.

Boundary conditions and loading The kinematic boundary conditions are symmetry on the axis (nodes at r =0, in node set AXIS, have ur =0 prescribed), symmetry about z =0 (all nodes at z =0, in node set MIDDLE, have uz =0 prescribed). To avoid overconstraint, the node on the top surface of the billet that lies on the symmetry axis is not part of the node set AXIS: the radial motion of this node is already constrained by a no-slip frictional constraint (see ``Common difficulties associated with contact modeling,'' Section 21.10.1 of the ABAQUS/Standard User's Manual). The rigid body reference node for the rigid surface that defines the die is constrained to have no rotation or ur -displacement, and its uz -displacement is prescribed to move 9 mm down the axis at constant velocity. The reaction force at the rigid reference node corresponds to the total force applied by the die. The thermal boundary conditions are that all external surfaces are insulated (no heat flux allowed). This condition is chosen because it is the most extreme case: it must provide the largest temperature rises possible, since no heat can be removed from the specimen. DELTMX is the limit on the maximum temperature change allowed to occur in any increment and is one of the controls for the automatic time incrementation scheme in ABAQUS/Standard. It is set to 100°C, which is a large value and indicates that we are not restricting the time increments because of accuracy considerations in integrating the heat transfer equations. In fact, the automatic time incrementation scheme will choose fairly small increments because of the severe nonlinearity present in the problem and the resultant need for several iterations per increment even with a relatively large number of increments. The large value is used for DELTMX to obtain a reasonable solution at low cost.

1-599

Static Stress/Displacement Analyses

In ABAQUS/Explicit the automatic time incrementation scheme is used to ensure numerical stability and to advance the solution in time. Mass scaling is used to reduce the computational cost of the analysis. The AMPLITUDE=RAMP parameter is included because the default amplitude variation for a transient, coupled temperature-displacement analysis is a step function, but here we want the die to move down at a constant velocity. Two versions of the analysis are run: a slow upsetting, where the upsetting occurs in 100 seconds, and a fast upsetting, where the event takes 0.1 second. Both versions are analyzed with the coupled temperature-displacement procedure. The fast upsetting is also run in ABAQUS/Standard as an adiabatic static stress analysis. The time period values are specified on the data line associated with the *COUPLED TEMPERATURE-DISPLACEMENT procedure, *DYNAMIC TEMPERATURE-DISPLACEMENT procedure, and the *STATIC procedure options. The adiabatic stress analysis is performed in the same time frame as the fast upsetting case. In all cases analyzed with ABAQUS/Standard an initial time increment of 1.5% of the time period is used; that is, 1.5 seconds in the slow case and 0.0015 second in the fast case. This value is chosen because it will result in a nominal axial strain of about 1% per increment, and experience suggests that such increment sizes are generally suitable for cases like this.

Results and discussion The results of the ABAQUS/Standard simulations are discussed first, beginning with the results for the viscoplastic fully dense material. The results of the slow upsetting are illustrated in Figure 1.3.17-2 to Figure 1.3.17-4. The results for the fast upsetting coupled temperature-displacement analysis are illustrated in Figure 1.3.17-5 to Figure 1.3.17-7; those for the adiabatic static stress analysis are shown in Figure 1.3.17-8 and Figure 1.3.17-9. Figure 1.3.17-2 and Figure 1.3.17-5 show the configuration that is predicted at 60% upsetting. The configuration for the adiabatic analysis is not shown since it is almost identical to the fast upsetting coupled case. Both the slow and the fast upsetting cases show the folding of the top outside surface of the billet onto the die, as well as the severe straining of the middle of the specimen. The second figure in each series (Figure 1.3.17-3 for the slow case, Figure 1.3.17-6 for the fast case, and Figure 1.3.17-8 for the adiabatic case) shows the equivalent plastic strain in the billet. Peak strains of around 180% occur in the center of the specimen. The third figure in each series (Figure 1.3.17-4 for the slow case, Figure 1.3.17-7 for the fast case, and Figure 1.3.17-9 for the adiabatic case) shows the temperature distributions, which are noticeably different between the slow and fast upsetting cases. In the slow case there is time for the heat to diffuse (the 60% upsetting takes place in 100 sec, on a specimen where a typical length is 10 mm), so the temperature distribution at 100 sec is quite uniform, varying only between 180°C and 185°C through the billet. In contrast, the fast upsetting occurs too quickly for the heat to diffuse. In this case the middle of the top surface of the specimen remains at 0°C at the end of the event, while the center of the specimen heats up to almost 600°C. There is no significant difference in temperatures between the fast coupled case and the adiabatic case. In the outer top section of the billet there are differences that are a result of the severe distortion of the elements in that region and the lack of dissipation of generated heat. The temperature in the rest of the billet compares well. This example illustrates the advantage of an adiabatic analysis, since a good representation of the results is obtained in about 60% of the computer time required for

1-600

Static Stress/Displacement Analyses

the fully coupled analysis. The results of the slow and fast upsetting of the billet modeled with the porous metal plasticity model are shown in Figure 1.3.17-10 to Figure 1.3.17-15. The deformed configuration is identical to that of Figure 1.3.17-2 and Figure 1.3.17-5. The extent of growth/closure of the voids in the specimen at the end of the analysis is shown in Figure 1.3.17-10 and Figure 1.3.17-13. The porous material is almost fully compacted near the center of the billet because of the compressive nature of the stress field in that region; on the other hand, the corner element is folded up and stretched out near the outer top portion of the billet, increasing the void volume fraction to almost 0.1 (or 10%) and indicating that tearing of the material is likely. The equivalent plastic strain is shown in Figure 1.3.17-11 (slow upsetting) and Figure 1.3.17-14 (fast upsetting) for the porous material; Figure 1.3.17-12 and Figure 1.3.17-15 show the temperature distribution for the slow and the fast upsetting of the porous metal. The porous metal needs less external work to achieve the same deformation compared to a fully dense metal. Consequently, there is less plastic work being dissipated as heat; hence, the temperature increase is not as much as that of fully dense metal. This effect is more pronounced in the fast upsetting problem, where the specimen heats up to only 510°C, compared to about 600°C for fully dense metal. Figure 1.3.17-16 to Figure 1.3.17-18 show predictions of total upsetting force versus displacement of the die. In Figure 1.3.17-16 the slow upsetting viscoplastic and porous plasticity results are compared with several elastic-plastic and rigid-plastic results that were collected by Lippmann (1979) and slow viscoplastic results obtained by Taylor (1981). There is general agreement between all the rate independent results, and these correspond to the slow viscoplastic results of the present example and of those found by Taylor (1981). In Figure 1.3.17-17 rate dependence of the yield stress is investigated. The fast viscoplastic and porous plasticity results show significantly higher force values throughout the event than the slow results. This effect can be estimated easily. A nominal strain rate of 6 sec is maintained throughout the event. With the viscoplastic model that is used, this effect increases the yield stress by 68%. This factor is very close to the load amplification factor that appears in Figure 1.3.17-17. Figure 1.3.17-18 shows that the force versus displacement prediction of the fast viscoplastic adiabatic analysis agrees well with the fully coupled results. Two cases using an element-based rigid surface to model the die are also considered in ABAQUS/Standard. To define the element-based rigid surface, the elements are assigned to rigid bodies using *RIGID BODY, ISOTHERMAL=YES. The results agree very well with the case when the analytical rigid surface is used. The automatic load incrementation results suggest that overall nominal strain increments of about 2% per increment were obtained, which is slightly better than what was anticipated in the initial time increment suggestion. These values are typical for problems of this class and are useful guidelines for estimating the computational effort required for such cases. The results obtained with ABAQUS/Explicit compare well with those obtained with ABAQUS/Standard, as illustrated in Figure 1.3.17-19, which compares the results obtained with ABAQUS/Explicit (without adaptive meshing) for the total upsetting force versus the displacement of the die against the same result obtained with ABAQUS/Standard. The agreement between the two solutions is excellent. Similar agreement is obtained with the results obtained from the ABAQUS/Explicit simulation using adaptive meshing. The mesh distortion is significantly reduced in

1-601

Static Stress/Displacement Analyses

this case, as illustrated in Figure 1.3.17-20.

Input files ABAQUS/Standard input files cylbillet_cax4t_slow_dense.inp Slow upsetting case with 144 CAX4T elements, using the fully dense material. cylbillet_cax4t_fast_dense.inp Fast upsetting case with 144 CAX4T elements, using the fully dense material. cylbillet_cax8rt_slow_dense.inp Slow upsetting case with CAX8RT elements, using the fully dense material. cylbillet_cax8rt_rb_s_dense.inp Slow upsetting case with CAX8RT elements, using the fully dense material and an element-based rigid surface for the die. cylbillet_cax8rt_fast_dense.inp Fast upsetting case with CAX8RT elements, using the fully dense material. cylbillet_cax8rt_slow_por.inp Slow upsetting case with CAX8RT elements, using the porous material. cylbillet_cax8rt_fast_por.inp Fast upsetting case with CAX8RT elements, using the porous material. cylbillet_cgax4t_slow_dense.inp Slow upsetting case with 144 CGAX4T elements, using the fully dense material. cylbillet_cgax4t_fast_dense.inp Fast upsetting case with 144 CGAX4T elements, using the fully dense material. cylbillet_cgax4t_rb_f_dense.inp Fast upsetting case with 144 CGAX4T elements, using the fully dense material and an element-based rigid surface for the die. cylbillet_cgax8rt_slow_dense.inp Slow upsetting case with CGAX8RT elements, using the fully dense material. cylbillet_cgax8rt_fast_dense.inp Fast upsetting case with CGAX8RT elements, using the fully dense material. cylbillet_c3d10m_adiab_dense.inp Adiabatic static analysis with fully dense material modeled with C3D10M elements.

1-602

Static Stress/Displacement Analyses

cylbillet_cax6m_adiab_dense.inp Adiabatic static analysis with fully dense material modeled with CAX6M elements. cylbillet_cax8r_adiab_dense.inp Adiabatic static analysis with fully dense material modeled with CAX8R elements. cylbillet_postoutput.inp *POST OUTPUT analysis, using the fully dense material. cylbillet_slow_usr_umat_umatht.inp Slow upsetting case with the material behavior defined in user subroutines UMAT and UMATHT. cylbillet_slow_usr_umat_umatht.f User subroutines UMAT and UMATHT used in cylbillet_slow_usr_umat_umatht.inp. ABAQUS/Explicit input files cylbillet_x_cax4rt_slow.inp Slow upsetting case with fully dense material modeled with CAX4RT elements and without adaptive meshing; kinematic mechanical contact. cylbillet_x_cax4rt_fast.inp Fast upsetting case with fully dense material modeled with CAX4RT elements and without adaptive meshing; kinematic mechanical contact. cylbillet_x_cax4rt_slow_adap.inp Slow upsetting case with fully dense material modeled with CAX4RT elements and with adaptive meshing; kinematic mechanical contact. cylbillet_x_cax4rt_fast_adap.inp Fast upsetting case with fully dense material modeled with CAX4RT elements and with adaptive meshing; kinematic mechanical contact. cylbillet_xp_cax4rt_fast.inp Fast upsetting case with fully dense material modeled with CAX4RT elements and without adaptive meshing; penalty mechanical contact.

References · Lippmann, H., Metal Forming Plasticity, Springer-Verlag, Berlin, 1979. · Taylor, L. M., "A Finite Element Analysis for Large Deformation Metal Forming Problems Involving Contact and Friction," Ph.D. Thesis, U. of Texas at Austin, 1981.

Figures

1-603

Static Stress/Displacement Analyses

Figure 1.3.17-1 Axisymmetric upsetting example: geometry and mesh (element type CAX8RT).

Figure 1.3.17-2 Deformed configuration at 60% upsetting: slow case, coupled temperature-displacement analysis, ABAQUS/Standard.

Figure 1.3.17-3 Plastic strain at 60% upsetting: slow case, coupled temperature-displacement analysis, ABAQUS/Standard.

1-604

Static Stress/Displacement Analyses

Figure 1.3.17-4 Temperature at 60% upsetting: slow case, coupled temperature-displacement analysis, ABAQUS/Standard.

Figure 1.3.17-5 Deformed configuration at 60% upsetting: fast case, coupled temperature-displacement analysis, ABAQUS/Standard.

Figure 1.3.17-6 Plastic strain at 60% upsetting: fast case, coupled temperature-displacement analysis, ABAQUS/Standard.

1-605

Static Stress/Displacement Analyses

Figure 1.3.17-7 Temperature at 60% upsetting: fast case, coupled temperature-displacement analysis, ABAQUS/Standard.

Figure 1.3.17-8 Plastic strain at 60% upsetting: fast case, adiabatic stress analysis, ABAQUS/Standard.

Figure 1.3.17-9 Temperature at 60% upsetting: fast case, adiabatic stress analysis, ABAQUS/Standard.

1-606

Static Stress/Displacement Analyses

Figure 1.3.17-10 Void volume fraction at 60% upsetting: porous material, slow coupled temperature-displacement analysis, ABAQUS/Standard.

Figure 1.3.17-11 Plastic strain at 60% upsetting: porous material, slow coupled temperature-displacement analysis, ABAQUS/Standard.

Figure 1.3.17-12 Temperature at 60% upsetting: porous material, slow coupled temperature-displacement analysis, ABAQUS/Standard.

1-607

Static Stress/Displacement Analyses

Figure 1.3.17-13 Void volume fraction at 60% upsetting: porous material, fast coupled temperature-displacement analysis, ABAQUS/Standard.

Figure 1.3.17-14 Plastic strain at 60% upsetting: porous material, fast coupled temperature-displacement analysis, ABAQUS/Standard.

Figure 1.3.17-15 Temperature at 60% upsetting: porous material, fast coupled temperature-displacement analysis, ABAQUS/Standard.

Figure 1.3.17-16 Force-deflection response for slow cylinder upsetting, ABAQUS/Standard.

1-608

Static Stress/Displacement Analyses

Figure 1.3.17-17 Rate dependence of the force-deflection response, ABAQUS/Standard.

1-609

Static Stress/Displacement Analyses

Figure 1.3.17-18 Force-deflection response: adiabatic versus fully coupled analysis, ABAQUS/Standard.

1-610

Static Stress/Displacement Analyses

Figure 1.3.17-19 Force-deflection response: ABAQUS/Explicit versus ABAQUS/Standard.

1-611

Static Stress/Displacement Analyses

Figure 1.3.17-20 Deformed configuration of the at 60% upsetting: slow case; without adaptive meshing, left; with adaptive meshing, right (ABAQUS/Explicit).

Sample listings

1-612

Static Stress/Displacement Analyses

Listing 1.3.17-1 *HEADING - AXISYMMETRIC UPSETTING PROBLEM - SLOW CASE - COUPLED TEMPERATURE-DISPLACEMENT ANALYSIS - (SLOW UPSETTING) *RESTART,WRITE,FREQUENCY=30 *NODE,NSET=RSNODE 9999,0.,.015 *NODE 1, 13,.01 1201,0.,.015 1213,.01,.015 *NGEN,NSET=MIDDLE 1,13 *NGEN,NSET=TOP 1201,1213 *NSET,NSET=TOPBND,GENERATE 1201,1212,1 *NFILL MIDDLE,TOP,12,100 *NSET,NSET=AXIS,GENERATE 1,1101,100 *ELEMENT,TYPE=CAX8RT,ELSET=METAL 1,1,3,203,201,2,103,202,101 *ELGEN,ELSET=METAL 1,6,2,1,6,200,100 *ELSET,ELSET=ESID,GENERATE 6,506,100 *ELSET,ELSET=ETOP,GENERATE 501,506,1 *SURFACE,NAME=ASURF ESID,S2 ETOP,S3 *RIGID BODY,ANALYTICAL SURFACE=BSURF,REF NODE=9999 *SURFACE,TYPE=SEGMENTS,NAME=BSURF START,.020,.015 LINE,-.001,.015 *CONTACT PAIR,INTERACTION=SMOOTH ASURF,BSURF *SOLID SECTION,ELSET=METAL,MATERIAL=EL

1-613

Static Stress/Displacement Analyses

*MATERIAL,NAME=EL *ELASTIC 200.E9,.3 *PLASTIC 7.E8,0.00 3.7E9,10.0 *RATE DEPENDENT 40.,5. *SPECIFIC HEAT 586., *DENSITY 7833., *CONDUCTIVITY 52., *EXPANSION 1.2E-5, *INELASTIC HEAT FRACTION 0.9, *SURFACE INTERACTION,NAME=SMOOTH *SURFACE BEHAVIOR,NO SEPARATION *FRICTION,ROUGH *BOUNDARY MIDDLE,2 AXIS,1 *STEP,INC=200,AMPLITUDE=RAMP,NLGEOM *COUPLED TEMPERATURE-DISPLACEMENT,DELTMX=100. 1.5,100.,5.E-8,5.0 *BOUNDARY RSNODE,1 RSNODE,6 RSNODE,2,,-.009 *PRINT,CONTACT=YES *CONTACT PRINT,SLAVE=ASURF,FREQUENCY=100 *CONTACT FILE,SLAVE=ASURF,FREQUENCY=200 *OUTPUT,FIELD,FREQ=200 *CONTACT OUTPUT,VARIABLE=PRESELECT,SLAVE=ASURF *CONTACT CONTROLS,FRICTION ONSET=DELAY *MONITOR,NODE=9999,DOF=2 *EL PRINT, ELSET=METAL,FREQUENCY=100 S,MISES E,PEEQ *NODE PRINT,FREQUENCY=25 U,RF,NT,RFL

1-614

Static Stress/Displacement Analyses

*NODE FILE,NSET=RSNODE RF, *OUTPUT,FIELD *NODE OUTPUT,NSET=RSNODE RF, *NODE FILE,FREQUENCY=200 NT, *OUTPUT,FIELD,FREQ=200 *NODE OUTPUT NT, *END STEP

1-615

Static Stress/Displacement Analyses

Listing 1.3.17-2 *HEADING - AXISYMMETRIC UPSETTING PROBLEM - WITH RIGID SURFACE - SECTION CONTROLS USED (HOURGLASS=STIFFNESS) - SLOW UPSETTING *NODE 1, 13,.01 1201,0.,.015 1213,.01,.015 *NGEN,NSET=MIDDLE 1,13 *NGEN,NSET=TOP 1201,1213 *NFILL MIDDLE,TOP,12,100 *NSET,NSET=AXIS,GEN 1,1201,100 *ELEMENT,TYPE=cax4rt,ELSET=BILLET 1,1,2,102,101 *ELGEN,ELSET=BILLET 1,12,1,1,12,100,100 *NODE, NSET=NRIGID 2003,0.01,.02 *SOLID SECTION,ELSET=BILLET, MATERIAL=METAL,CONTROL=B *SECTION CONTROLS, HOURGLASS=STIFFNESS, NAME=B *MATERIAL,NAME=METAL *ELASTIC 200.E9,.3 *PLASTIC 7.E8,0.00 3.7E9,10.0 *RATE DEPENDENT 40.,5. *SPECIFIC HEAT 586., *DENSITY 7833., *CONDUCTIVITY 52.,

1-616

Static Stress/Displacement Analyses

*EXPANSION 1.2E-5, *INELASTIC HEAT FRACTION 0.9, *BOUNDARY MIDDLE,2 AXIS,1 2003,1 2003,3,6 *SURFACE,TYPE=ELEMENT,NAME=BILLET TOP,S3 SIDE,S2 *SURFACE,NAME=RIGID,TYPE=SEGMENTS START, 0.02,.015 LINE, 0.00,.015 *RIGID BODY, REF NODE=2003, ANALYTICAL SURFACE =RIGID *STEP *DYNAMIC TEMPERATURE-DISPLACEMENT, EXPLICIT ,100.0 *FIXED MASS SCALING, ELSET=BILLET,FACTOR=1.E+10 *BOUNDARY,TYPE=VELOCITY 2003,2,,-9.e-5 *ELSET,ELSET=TOP,GEN 1101,1112,1 *ELSET,ELSET=SIDE,GEN 12,1112,100 *SURFACE INTERACTION,NAME=RIG_BILL *FRICTION 1.0, *CONTACT PAIR,INTERACTION=RIG_BILL RIGID,BILLET *MONITOR,NODE=2003,DOF=2 *FILE OUTPUT,NUM=2 *EL FILE PEEQ,MISES *NODE FILE, NSET=NRIGID U,RF *NODE FILE NT, *OUTPUT,FIELD,VAR=PRESELECT,NUM=5 *OUTPUT,HISTORY *NODE OUTPUT,NSET=NRIGID

1-617

Static Stress/Displacement Analyses

U2,RF2 *ENERGY OUTPUT ALLIE,ALLKE,ALLAE,ALLPD *END STEP

1.3.18 Unstable static problem: thermal forming of a metal sheet Product: ABAQUS/Standard This example demonstrates the use of automatic techniques to stabilize unstable static problems. Geometrically nonlinear static problems can become unstable for a variety of reasons. Instability may occur in contact problems, either because of chattering or because contact intended to prevent rigid body motions is not established initially. Localized instabilities can also occur; they can be either geometrical, such as local buckling, or material, such as material softening. This problem models the thermal forming of a metal sheet; the shape of the die may make it difficult to place the undeformed sheet exactly in initial contact, in which case the initial rigid body motion prevention algorithm is useful. Metal forming problems are characterized by relatively simply shaped parts being deformed by relatively complex-shaped dies. The initial placement of the workpiece on a die or the initial placement of a second die may not be a trivial geometrical exercise for an engineer modeling the forming process. ABAQUS accepts initial penetrations in contact pairs and instantaneously tries to resolve them; as long as the geometry allows for this to happen without excessive deformation, the misplacement of the workpiece usually does not cause problems. On the other hand, if the workpiece is initially placed away from the dies, serious problems may arise. Unless there are enough boundary conditions applied, singular finite element systems of equations result because one or more of the bodies has free rigid body motions. This typically arises when the deformation is applied through loads instead of boundary conditions. It is possible to eliminate this problem by modifying the model, which can be cumbersome for the analyst. Alternatively, the *CONTACT CONTROLS, APPROACH option allows initial placement of a body apart from others with smooth load-controlled motion until contact gets established. This example looks at the thermal forming of an aluminum sheet. The deformation is produced by applying pressure and gravity loads to push the sheet against a sculptured die. The deformation is initially elastic. Through heating, the yield stress of the material is lowered until permanent plastic deformations are produced. Subsequently, the assembly is cooled and the pressure loads are removed, leaving a formed part with some springback. Although the sheet is initially flat, the geometrical nature of the die makes it difficult to determine the exact location of the sheet when it is placed on the die. Therefore, an initial gap between the two bodies is modeled, as shown in Figure 1.3.18-1.

Geometry and model The model consists of a trapezoidal sheet 10.0 m (394.0 in) long, tapering from 2.0 m (78.75 in) to 3.0 m (118.0 in) wide, and 10.0 mm (0.4 in) thick. The die is a ruled surface controlled by two circles of radii 13.0 m (517.0 in) and 6.0 m (242.0 in) and dimensions slightly larger than the sheet. The sheet is initially placed over 0.2 m (7.9 in) apart from the die. The sheet has a longitudinal symmetry boundary condition, and one node prevents the remaining nodes from experiencing in-plane rigid body motion.

1-618

Static Stress/Displacement Analyses

The die is fixed throughout the analysis. The sheet mesh consists of 640 S4R shell elements, while the die is represented by 640 R3D4 rigid elements. The material is an aluminum alloy with a flow stress of 1.0 ´ 108 Pa (14.5 ksi) at room temperature. A flow stress of 1.0 ´ 103 Pa (0.15 psi) at 400°C is also provided, essentially declaring that at the higher temperature the material will flow plastically at any stress. A Coulomb friction coefficient of 0.1 is used to model the interaction between the sheet and die.

Results and discussion The analysis consists of three steps. In the first step a gravity load and a pressure load of 1.0 ´ 105 Pa (14.5 psi) are applied, both pushing the sheet against the die. This step is aided by the automatic contact approach procedure to prevent unrestrained motion of the sheet. This procedure consists of the application of viscous pressure along the contact direction (normal to the die), opposing the relative motion between the sheet and the die. During the first increment of the step ABAQUS applies a very high amount of damping so that it can judge the magnitude of the external loads being applied, as well as determine the initial distances between the slave and master surfaces. Based on the results of this initial attempt a suitable damping coefficient is calculated and the increment is repeated, such that a smooth approach is produced during the initial part of the step. In this particular case five increments take place before the first contact point closes; from then on the sheet is pressed against the die. As soon as contact is established, the relative velocities between the sheet and the die decrease and become almost zero at the end of the step, which essentially eliminates the damping forces. In addition, ABAQUS ramps down the damping coefficient to zero from the middle of the step on. This guarantees that the viscous forces decrease to zero, thus avoiding any discontinuity in the forces at the start of the next step. The shape and relatively low curvatures of the die are such that the deformation at the end of the step is elastic (Figure 1.3.18-2). In the second step a two-hour heating (from room temperature to 360°C) and cooling (back to 50°C) cycle is applied to the loaded assembly. As a result of the decrease in flow stress permanent (plastic) deformation develops, as shown in Figure 1.3.18-3. Finally, in the third step the pressure load is removed and the springback of the deformed sheet is calculated, as depicted in Figure 1.3.18-4.

Acknowledgements HKS would like to thank British Aerospace Airbus, Ltd. for providing the basic data from which this example was derived.

Input file unstablestatic_forming.inp Thermal forming model.

Figures Figure 1.3.18-1 Initial placement of the sheet apart from the die.

1-619

Static Stress/Displacement Analyses

Figure 1.3.18-2 Elastic deformation after gravity and pressure loading.

Figure 1.3.18-3 Permanent deformation produced by heating.

1-620

Static Stress/Displacement Analyses

Figure 1.3.18-4 Springback.

Sample listings

1-621

Static Stress/Displacement Analyses

Listing 1.3.18-1 *HEADING THERMAL FORMING OF AN ALUMINUM SHEET S.I Units, Kg, M, s, N ** *RESTART, WRITE, FREQUENCY=20, OVERLAY ** ** Rigid body node definitions *NODE,NSET=RIGID 1, -1.800000, 0.000000, 0.000000 17, 1.800000, 0.000000, 0.000000 901, 0.000000, 0.000000, 13.000000 681, -1.300000, 10.300000, 0.000000 697, 1.300000, 10.300000, 0.000000 902, 0.000000, 10.300000, 6.000000 *NGEN,NSET=END1,LINE=C 1,17,1,901 *NGEN,NSET=END2,LINE=C 681,697,1,902 *NFILL,NSET=RIGID END1,END2,40,17 ** ** Plate node definitions *NODE,NSET=DEFORM 10001, -1.000000, 10.150000, 0.1725 10017, 1.000000, 10.150000, 0.1725 10681, -1.500000, 0.150000, 0.1725 10697, 1.500000, 0.150000, 0.1725 *NGEN,NSET=SHORT 10001,10017 *NGEN,NSET=LONG 10681,10697 *NFILL,NSET=DEFORM SHORT,LONG,40,17 ** ** Rigid body reference node *NODE,NSET=FIX 99999, 0., 0., 0. ** ** Plate element definitions *ELEMENT, TYPE=S4R, ELSET=SHEET 10001, 10001, 10002, 10019, 10018

1-622

Static Stress/Displacement Analyses

*ELGEN,ELSET=SHEET 10001, 16, 1, 1, 40, 17, 16 *ELSET,ELSET=SHORT,GENERATE 10001,10016,1 ** ** Rigid surface element definitions *ELEMENT, TYPE=R3D4, ELSET=CONTACT 1, 1, 2, 19, 18 *ELGEN,ELSET=CONTACT 1, 16, 1, 1, 40, 17, 16 ** ** Plate 10mm in thickness *SHELL SECTION, ELSET=SHEET, MATERIAL=ALUMINUM 0.01, 5 ** *MATERIAL, NAME=ALUMINUM ** *ELASTIC 7.919714E10, 0.3, 292. *DENSITY 2.9e3, *EXPANSION 8.367e-6, ** *PLASTIC 1.e8,0,293. 1.e3,0,673. ** *RIGID BODY, ELSET=CONTACT, REF NODE=99999 ** *SURFACE, NAME=M1 CONTACT, SPOS *SURFACE, NAME=S1 SHEET, SPOS ** *CONTACT PAIR, INTERACTION=I1 S1, M1 *SURFACE INTERACTION, NAME=I1 *FRICTION, SLIP TOLERANCE=0.02 0.1, ** ** Nodes down the middle of the model on which ** boundary conditions are placed.

1-623

Static Stress/Displacement Analyses

*NSET,NSET=MIDDLE 10009, 10026, 10043, 10060, 10077, 10094, 10111, 10128, 10145, 10162, 10179, 10196, 10213, 10230, 10247, 10264, 10281, 10298, 10315, 10332, 10349, 10366, 10383, 10400, 10417, 10434, 10451, 10468, 10485, 10502, 10519, 10536, 10553, 10570, 10587, 10604, 10621, 10638, 10655, 10672, 10689, ** ** *BOUNDARY 10009,2,2,0.0 MIDDLE,1,1,0.0 99999, 1,6,0.0 ** ** Temperature amplitude card for use ** during forming step ** *AMPLITUDE, NAME=TEMP_PROF, VALUE=ABSOLUTE 0,293., 3600,633. , 7200,323. ** ** Initial ambient temperature for the plate ** *INITIAL CONDITIONS, TYPE=TEMPERATURE DEFORM,293.,293.,293.,293.,293. ** ** --------------------------------------------** ** Step 1 - Apply gravity loading together with ** 1 Bar pressure loading on plate to force it ** into the die. *STEP, INC=10000, NLGEOM *STATIC 0.1, 1., 1.E-10 ** ** pressure + gravity ** *DLOAD, OP=NEW SHEET,GRAV,9.81, 0., 0., -1.

1-624

Static Stress/Displacement Analyses

SHEET, P, 1.e5 ** *CONTACT CONTROLS,MASTER=M1, SLAVE=S1,APPROACH ** *NODE PRINT, FREQ=0 *EL PRINT, FREQ=0 *CONTACT PRINT, FREQ=999 *NODE FILE,NSET=SHORT,FREQ=999 U, *EL FILE, ELSET=SHORT, FREQ=999 S,E,PE *OUTPUT,FIELD,FREQ=20 *NODE OUTPUT U, *ELEMENT OUTPUT S,E,PEEQ *END STEP ** ** --------------------------------------------** ** Step 2 - Now perform the forming step. ** The temperature follows the profile on the ** *AMPLITUDE card *STEP, INC=10000, NLGEOM *STATIC 100.,7200.,1e-1,5.e2 ** *TEMPERATURE, OP=NEW, AMPLITUDE=TEMP_PROF DEFORM,1.,1.,1.,1.,1. ** *END STEP ** ** -------------------------------------------** ** Step 3 - Now release 1 Bar pressure ** (but maintain gravity load) *STEP, INC=10000, NLGEOM *STATIC 0.1, 1. ** *DLOAD, OP=NEW SHEET,GRAV,9.81, 0., 0., -1. **

1-625

Static Stress/Displacement Analyses

*END STEP

1.4 Fracture mechanics 1.4.1 A plate with a part-through crack: elastic line spring modeling Product: ABAQUS/Standard The line spring elements in ABAQUS allow inexpensive evaluation of the effects of surface flaws in shell structures, with sufficient accuracy for use in design studies. The basic concept of these elements is that they introduce the local solution, dominated by the singularity at the crack tip, into a shell model of the uncracked geometry. The relative displacements and rotations across the cracked section, calculated in the line spring elements, are then used to determine the magnitude of the local strain field and hence the J -integral and stress intensity factor values, as functions of position along the crack front. This example illustrates the use of these elements and provides some verification of the results they provide by comparison with a published solution and also by making use of the shell-to-solid submodeling technique.

Problem description A large plate with a symmetric, centrally located, semi-elliptic, part-through crack is subjected to edge tension and bending. The objective is to estimate the Mode I stress intensity factor, KI , as a function of position along the crack front. Symmetry allows one quarter of the plate to be modeled, as shown in Figure 1.4.1-1. The 8-node shell element, S8R, and the corresponding 3-node (symmetry plane) line spring element LS3S are used in the model. A mesh using LS6 elements is also included. Only half-symmetry is used in this case. When LS6 elements are used, the shell elements on either side of an LS6 element must be numbered such that the normals to these shell elements point in approximately the same direction.

Geometry and model For each load case (tension and bending) two plate thicknesses are studied: a "thick" case, for which the plate thickness is 76.2 mm (3.0 in); and a "thin" case, for which the plate thickness is 19.05 mm (0.75 in). For both thicknesses the semi-elliptic crack has a maximum depth ( a0 in Figure 1.4.1-2) of 15.24 mm (0.6 in) and a half-length, c, of 76.2 mm (3.0 in). The plate is assumed to be square, with dimensions 609.6 ´ 609.6 mm (24 ´ 24 in). The material is assumed to be linear elastic, with Young's modulus 207 GPa (30 ´ 106 lb/in2) and Poisson's ratio 0.3. A quarter of the plate is modeled, with symmetry along the edges of the quarter-model at x =0 and y =0. On the edge containing the flaw (y =0), the symmetry boundary conditions are imposed only on the unflawed segment of the edge, since they are built into the symmetry plane of the line spring element being used (LS3S). The loading consists of a uniform edge tension (per unit length) of 52.44 kN/m (300 lb/in) or a uniform

1-626

Static Stress/Displacement Analyses

edge moment (per unit length) of 1335 N-m/m (300 lb-in/in).

Results and discussion The stress intensity factors for the thick and thin plates are compared with the detailed solutions of Raju and Newman (1979) and Newman and Raju (1979) in Figure 1.4.1-3 (tension load) and Figure 1.4.1-4 (bending load). These plots show that the present results agree reasonably well with those of Raju and Newman over the middle portion of the flaw (Á >30°), with better correlation being provided for the thick case, possibly because the crack is shallower in that geometry. The accuracy is probably adequate for basic assessment of the criticality of the flaw for design purposes. For values of Á less than about 30° (that is, at the ends of the flaw), the stress intensity values predicted by the line spring model lose accuracy. This accuracy loss arises from a combination of the relative coarseness of the mesh, (especially in this end region where the crack depth varies rapidly), as well as from theoretical considerations regarding the appropriateness of line spring modeling at the ends of the crack. These points are discussed in detail by Parks (1981) and Parks et al. (1981).

Shell-to-solid submodeling around the crack tip An input file for the case a0 =t= 0.2, which uses the shell-to-solid submodeling capability, is included. This C3D20R element mesh allows the user to study the local crack area using the energy domain integral formulation for the J -integral. The submodel uses a focused mesh with four rows of elements p around the crack tip. A 1= r singularity is utilized at the crack tip, the correct singularity for a linear elastic solution. Symmetry boundary conditions are imposed on two edges of the submodel mesh, while results from the global shell analysis are interpolated to two edges by using the submodeling technique. The global shell mesh gives satisfactory J -integral results; hence, we assume that the displacements at the submodel boundary are sufficiently accurate to drive the deformation in the submodel. No attempt has been made to study the effect of making the submodel region larger or smaller. The submodel is shown superimposed on the global shell model in Figure 1.4.1-5. The variations of the J -integral values along the crack in the submodeled analysis are compared to the line spring element analysis in Figure 1.4.1-3 (tension load) and Figure 1.4.1-4 (bending load). Excellent correlation is seen between the three solutions. A more refined mesh in the shell-to-solid submodel near the plate surface would be required to obtain J -integral values that more closely match the reference solution.

Input files crackplate_ls3s.inp LS3S elements. crackplate_surfaceflaw.f A small program used to create a data file containing the surface flaw depths. crackplate_ls6_nosym.inp LS6 elements without symmetry about y = 0.

1-627

Static Stress/Displacement Analyses

crackplate_postoutput.inp *POST OUTPUT analysis. crackplate_submodel.inp Shell-to-solid submodel.

References · Newman, J. C., Jr., and I. S. Raju, "Analysis of Surface Cracks in Finite Plates Under Tension or Bending Loads," NASA Technical Paper 1578, National Aeronautics and Space Administration, December 1979. · Parks, D. M., "The Inelastic Line Spring: Estimates of Elastic-Plastic Fracture Mechanics Parameters for Surface-Cracked Plates and Shells," Journal of Pressure Vessel Technology, vol. 13, pp. 246-254, 1981. · Parks, D. M., R. R. Lockett, and J. R. Brockenbrough, "Stress Intensity Factors for Surface-Cracked Plates and Cylindrical Shells Using Line Spring Finite Elements," Advances in Aerospace Structures and Materials , Edited by S. S. Wang and W. J. Renton, ASME, AD-01, pp. 279-286, 1981. · Raju, I. S. and J. C. Newman Jr., "Stress Intensity Factors for a Wide Range of Semi-Elliptic Surface Cracks in Finite Thickness Plates," Journal of Engineering Fracture Mechanics, vol. 11, pp. 817-829, 1979.

Figures Figure 1.4.1-1 Quarter model of large plate with center surface crack.

1-628

Static Stress/Displacement Analyses

Figure 1.4.1-2 Schematic surface crack geometry for a semi-elliptical crack.

Figure 1.4.1-3 Stress intensity factor dependence on crack front position: tension loading.

1-629

Static Stress/Displacement Analyses

Figure 1.4.1-4 Stress intensity factor dependence on crack front position: moment loading.

Figure 1.4.1-5 Solid submodel superimposed on shell global model.

1-630

Static Stress/Displacement Analyses

Sample listings

1-631

Static Stress/Displacement Analyses

Listing 1.4.1-1 *HEADING QUARTER MODEL OF LARGE PLATE WITH CENTER SURFACE CRACK [S8R] *NODE 1,0.,0. 97,12.,0. 4801,0.,12. 4897,12.,12. *NGEN,NSET=ONY 1,4801,100 *NGEN,NSET=FREE 97,4897,100 *NGEN 1,97 101,197 201,297 401,497 601,697 1001,1097 1401,1497,2 2201,2297,2 3001,3097,2 3901,3997,2 4801,4897,2 *NSET,NSET=ONX 27,29,33,37,41,45,49,53,57 61,69,77,87,97 *ELEMENT,TYPE=LS3S,ELSET=LS 1,25,24,23 5,17,15,13 *ELGEN,ELSET=LS 1,4,-2,1 5,4,-4,1 *ELEMENT,TYPE=S8R,ELSET=SHELL 9,1,5,205,201,3,105,203,101 13,17,19,219,217,18,119,218,117 17,25,29,229,225,27,129,227,125 18,29,37,237,229,33,137,233,129 22,61,77,277,261,69,177,269,161 23,77,97,297,277,87,197,287,177 24,201,209,609,601,205,409,605,401

1-632

Static Stress/Displacement Analyses

26,601,609,1409,1401,605,1009,1405,1001 28,217,221,621,617,219,421,619,417 31,617,621,1421,1417,619,1021,1419,1017 34,229,237,637,629,233,437,633,429 38,629,637,1437,1429,633,1037,1433,1029 42,261,277,677,661,269,477,669,461 43,661,677,1477,1461,669,1077,1469,1061 44,277,297,697,677,287,497,687,477 45,677,697,1497,1477,687,1097,1487,1077 46,1401,1417,3017,3001,1409,2217,3009,2201 48,1417,1421,3021,3017,1419,2221,3019,2217 50,1421,1429,3029,3021,1425,2229,3025,2221 58,1477,1497,3097,3077,1487,2297,3087,2277 47,3001,3017,4817,4801,3009,3917,4809,3901 49,3017,3021,4821,4817,3019,3921,4819,3917 51,3021,3029,4829,4821,3025,3929,4825,3921 59,3077,3097,4897,4877,3087,3997,4887,3977 *ELGEN,ELSET=SHELL 9,4,4,1 13,4,2,1 18,4,8,1 24,2,8,1 26,2,8,1 28,3,4,1 31,3,4,1 34,4,8,1 38,4,8,1 46,2,28,6 52,3,16,2 47,2,28,6 53,3,16,2 *ELSET,ELSET=PRINT 9,59,15,16,17 *MATERIAL,NAME=A1 *ELASTIC 30.E6,.3 *SHELL SECTION,ELSET=SHELL,MATERIAL=A1 3.0,3 *SHELL SECTION,ELSET=LS,MATERIAL=A1 3.0, *SURFACE FLAW,SIDE=POSITIVE,INPUT=CRACK.FLW ** DATA GENERATED FROM PROGRAM 7-1-1-2 *ELSET,ELSET=TOPL

1-633

Static Stress/Displacement Analyses

47,49,51,53,55,57,59 *MPC QUADRATIC,203,201,205,209 QUADRATIC,207,201,205,209 QUADRATIC,211,209,213,217 QUADRATIC,215,209,213,217 QUADRATIC,218,217,219,221 QUADRATIC,220,217,219,221 QUADRATIC,222,221,223,225 QUADRATIC,224,221,223,225 QUADRATIC,1405,1401,1409,1417 QUADRATIC,1413,1401,1409,1417 QUADRATIC,1423,1421,1425,1429 QUADRATIC,1427,1421,1425,1429 QUADRATIC,1433,1429,1437,1445 QUADRATIC,1441,1429,1437,1445 QUADRATIC,1449,1445,1453,1461 QUADRATIC,1457,1445,1453,1461 *BOUNDARY ONY,1 ONY,5,6 ONX,2 ONX,4 ONX,6 1,3 *RESTART,WRITE,FREQUENCY=999 *STEP *STATIC 0.1,1.0 *CLOAD 4801,2,100. 4809,2,400. 4817,2,125. 4819,2,100. 4821,2,75. 4825,2,200. 4829,2,150. 4837,2,400. 4845,2,200. 4853,2,400. 4861,2,200. 4869,2,400. 4877,2,225.

1-634

Static Stress/Displacement Analyses

4887,2,500. 4897,2,125. *EL PRINT,ELSET=LS JK, S, *EL PRINT,ELSET=PRINT COORD, S, E, *EL FILE,ELSET=LS JK, S, *EL FILE,ELSET=PRINT COORD, S, E, *NODE PRINT U, *NODE FILE U, *END STEP

1-635

Static Stress/Displacement Analyses

Listing 1.4.1-2 CC--- PROGRAM TO GENERATE CRACK DEPTH DATA C PROGRAM CRACK C SUBROUTINE HKSMAIN C IMPLICIT REAL*8(A-H,O-Z) OPEN(UNIT=16,STATUS='NEW',ACCESS='SEQUENTIAL', 1 FORM='FORMATTED',FILE='CRACK.FLW') C=3. CC=C*C N=24 NNODE=N+1 X0=C/DBLE(N) X=0. DO 100 I=1,NNODE IF(I.GE.17) GO TO 1 IF((I/2)*2.EQ.I) GO TO 10 1 CONTINUE XX=X*X TMP=.2 Z=TMP*SQRT(CC-XX) WRITE(6,99) I,Z WRITE(16,99)I,Z 99 FORMAT(I5,', ',F10.7) 10 CONTINUE X=X+X0 100 CONTINUE REWIND 16 STOP END

1-636

Static Stress/Displacement Analyses

Listing 1.4.1-3 *HEADING PLATE WITH A PART THROUGH CRACK: LS6 ELEMENTS *RESTART,WRITE *NODE 1,0.,0.,0.,0.,0.,1. 97,12.,0.,0.,0.,0.,1. 4801,0.,12.,0.,0.,0.,1. 4897,12.,12.,0.,0.,0.,1. *NGEN,NSET=ONY 1,4801,100 *NGEN,NSET=FREE 97,4897,100 *NGEN,NSET=TOP 1,97 101,197 201,297 401,497 601,697 1001,1097 1401,1497,2 2201,2297,2 3001,3097,2 3901,3997,2 4801,4897,2 *NSET,NSET=ONX 27,29,33,37,41,45,49,53,57 61,69,77,87,97 *NCOPY, OLD SET=TOP, NEW SET=BOTTOM, CHANGE NUMBER=10000, REFLECT=LINE 0.,0.,0.,12.,0.,0. *NSET,NSET=NALL TOP,BOTTOM *NSET,NSET=ONY,GENERATE 10001,14801,100 *NSET,NSET=ONX1 10027,10029,10033,10037,10041,10045,10049,10053, 10057,10061,10069,10077,10087,10097 *MPC TIE,ONX,ONX1 *ELEMENT,TYPE=S8R,ELSET=SHELLT 9,1,5,205,201,3,105,203,101

1-637

Static Stress/Displacement Analyses

13,17,19,219,217,18,119,218,117 17,25,29,229,225,27,129,227,125 18,29,37,237,229,33,137,233,129 22,61,77,277,261,69,177,269,161 23,77,97,297,277,87,197,287,177 24,201,209,609,601,205,409,605,401 26,601,609,1409,1401,605,1009,1405,1001 28,217,221,621,617,219,421,619,417 31,617,621,1421,1417,619,1021,1419,1017 34,229,237,637,629,233,437,633,429 38,629,637,1437,1429,633,1037,1433,1029 42,261,277,677,661,269,477,669,461 43,661,677,1477,1461,669,1077,1469,1061 44,277,297,697,677,287,497,687,477 45,677,697,1497,1477,687,1097,1487,1077 46,1401,1417,3017,3001,1409,2217,3009,2201 48,1417,1421,3021,3017,1419,2221,3019,2217 50,1421,1429,3029,3021,1425,2229,3025,2221 58,1477,1497,3097,3077,1487,2297,3087,2277 47,3001,3017,4817,4801,3009,3917,4809,3901 49,3017,3021,4821,4817,3019,3921,4819,3917 51,3021,3029,4829,4821,3025,3929,4825,3921 59,3077,3097,4897,4877,3087,3997,4887,3977 *ELGEN,ELSET=SHELLT 9,4,4,1 13,4,2,1 18,4,8,1 24,2,8,1 26,2,8,1 28,3,4,1 31,3,4,1 34,4,8,1 38,4,8,1 46,2,28,6 52,3,16,2 47,2,28,6 53,3,16,2 *ELCOPY, ELEMENT SHIFT=10000, OLD SET=SHELLT, NEW SET=SHELLB,SHIFT NODES=10000 *ELEMENT,TYPE=LS6,ELSET=LS 1,25,24,23,10025,10024,10023 5,17,15,13,10017,10015,10013 *ELGEN,ELSET=LS

1-638

Static Stress/Displacement Analyses

1,4,-2,1 5,4,-4,1 *ELSET,ELSET=SALL SHELLT,SHELLB,LS *ELSET,ELSET=SHELLS SHELLT,SHELLB *NORMAL SALL,NALL,0.,0.,1. *ELSET,ELSET=PRINT 9,59,15,16,17 *MATERIAL,NAME=A1 *ELASTIC 30.E6,.3 *SHELL SECTION,ELSET=SHELLS,MATERIAL=A1 .75,3 *SHELL SECTION,ELSET=LS,MATERIAL=A1 .75, *SURFACE FLAW,SIDE=POSITIVE 10001, 0.6000000 10003, 0.5979130 10005, 0.5916080 10007, 0.5809475 10009, 0.5656854 10011, 0.5454356 10013, 0.5196152 10015, 0.4873397 10017, 0.4472136 10018, 0.4235269 10019, 0.3968627 10020, 0.3665720 10021, 0.3316625 10022, 0.2904738 10023, 0.2397916 10024, 0.1713914 10025, 0.00 *ELSET,ELSET=TOPL 47,49,51,53,55,57,59 *ELSET,ELSET=BOTL 10047,10049,10051,10053,10055,10057,10059 *MPC QUADRATIC,203,201,205,209 QUADRATIC,207,201,205,209 QUADRATIC,211,209,213,217

1-639

Static Stress/Displacement Analyses

QUADRATIC,215,209,213,217 QUADRATIC,218,217,219,221 QUADRATIC,220,217,219,221 QUADRATIC,222,221,223,225 QUADRATIC,224,221,223,225 QUADRATIC,1405,1401,1409,1417 QUADRATIC,1413,1401,1409,1417 QUADRATIC,1423,1421,1425,1429 QUADRATIC,1427,1421,1425,1429 QUADRATIC,1433,1429,1437,1445 QUADRATIC,1441,1429,1437,1445 QUADRATIC,1449,1445,1453,1461 QUADRATIC,1457,1445,1453,1461 QUADRATIC,10203,10201,10205,10209 QUADRATIC,10207,10201,10205,10209 QUADRATIC,10211,10209,10213,10217 QUADRATIC,10215,10209,10213,10217 QUADRATIC,10218,10217,10219,10221 QUADRATIC,10220,10217,10219,10221 QUADRATIC,10222,10221,10223,10225 QUADRATIC,10224,10221,10223,10225 QUADRATIC,11405,11401,11409,11417 QUADRATIC,11413,11401,11409,11417 QUADRATIC,11423,11421,11425,11429 QUADRATIC,11427,11421,11425,11429 QUADRATIC,11433,11429,11437,11445 QUADRATIC,11441,11429,11437,11445 QUADRATIC,11449,11445,11453,11461 QUADRATIC,11457,11445,11453,11461 *BOUNDARY ONY,1 ONY,5,6 4897,3 14897,3 10097,2 10097,4 *STEP *STATIC *CLOAD 10025,1,0., 10025,2,0. 10025,3,0. 10025,4,0.

1-640

Static Stress/Displacement Analyses

10025,5,0. 10025,6,0. 4801,4,-100. 4809,4,-400. 4817,4,-125. 4819,4,-100. 4821,4,-75. 4825,4,-200. 4829,4,-150. 4837,4,-400. 4845,4,-200. 4853,4,-400. 4861,4,-200. 4869,4,-400. 4877,4,-225. 4887,4,-500. 4897,4,-125. 14801,4,100. 14809,4,400. 14817,4,125. 14819,4,100. 14821,4,75. 14825,4,200. 14829,4,150. 14837,4,400. 14845,4,200. 14853,4,400. 14861,4,200. 14869,4,400. 14877,4,225. 14887,4,500. 14897,4,125. *EL FILE JK, *END STEP

1.4.2 Conical crack in a half-space with and without submodeling Product: ABAQUS/Standard The purpose of this example is to verify that ABAQUS correctly evaluates contour integrals when the crack extension direction varies along the crack front. For the conical-shaped crack shown in Figure 1.4.2-1, the crack extension direction changes as the crack front is swept around the circle. The

1-641

Static Stress/Displacement Analyses

problem is axisymmetric and can, therefore, also be modeled using axisymmetric elements. The contour integrals for the three-dimensional model are verified by comparing them to results using axisymmetric elements.

Full modeling vs. submodeling The full three-dimensional crack model has an RMS wavefront of 2800. The submodeling capability is used to obtain accurate results by running two, much smaller, models: first, a global model to get the displacement solution with moderate accuracy away from the crack tip; and then a submodel to obtain a more accurate solution, and, hence, more accurate J -integrals, along the crack front. These models have RMS wavefronts of less than 1700, allowing them to be run on a smaller computer than is required to run the full three-dimensional model.

Geometry and model The geometry analyzed is a conical crack in a half-space, as shown in Figure 1.4.2-1. The crack intersects the free surface at 45° and extends 15 units into the half-space. Pressure loading is applied on the region of the half-space surface circumscribed by the crack. The full three-dimensional and axisymmetric meshes are shown in Figure 1.4.2-2 and Figure 1.4.2-3, respectively. The full three-dimensional model represents one-quarter of the problem, using symmetry about the x-y and y-z planes, and is composed of 10 sectors parallel to the y-axis. In the region up to a distance of approximately 10 times the crack length away from the crack, reduced-integration elements (C3D20R and CAX8R) are used. Beyond this region infinite elements (CIN3D12R and CINAX5R) are used. The focused mesh surrounding the crack tip in a plane parallel to the y-axis consists of 8 rings of 16 elements. It encompasses half of the crack length and extends the same distance ahead of the crack tip. p To obtain the desired 1/ r strain singularity, all the nodes in each crack front node set are tied together using multi-point constraints; and on element edges radial to the crack front, the midside nodes are moved to the 1/4 point position. This improves the modeling of the strain field near the crack tip, which results in more accurate contour integral values. There are three regions of degenerate elements. At the crack tip collapsed elements are necessary to provide the desired singularity. The elements at the crack opening and the elements along the y-axis are collapsed to simplify the meshing. Figure 1.4.2-4 shows the displaced shape of the mesh near the crack for the three-dimensional case.

Submodel Submodeling is also used to solve the problem with smaller meshes. The global model represents the same problem as the full model, but with a coarser mesh. Only one ring of elements is used in the focused part of the global model mesh compared to eight rings in the full model. For the three-dimensional global model only five sectors of elements parallel to the 2-axis are used, as opposed to 10 sectors in the full model. The axisymmetric global model is shown in Figure 1.4.2-5. The submodels consist of only the focused region of the mesh around the crack tip and contain eight rings and, in the three-dimensional case, 10 sectors. Quarter-symmetry boundary conditions are applied to the three-dimensional submodel as well as to the global model. The axisymmetric and three-dimensional submodels are shown in Figure 1.4.2-6 and Figure 1.4.2-7, respectively. It is

1-642

Static Stress/Displacement Analyses

assumed that the global model's coarse mesh is sufficiently accurate to drive the submodel: if the global model's displacement field far from the crack tip is accurate, the submodel can obtain accurate contour integral results. If two "driven" nodes on opposite faces of the crack share exactly the same location in the submodel, the submodeling capability is unable to assign the driven nodes to an element uniquely. The two nodes will behave as if they are tied together across the crack. In this example problem nodes 1033 and 65033 are defined to be approximately 0.01% of their typical element length away from their intended location along the crack. Moving the nodes this small amount does not affect the results but alleviates the assignment problem.

Results and discussion J -integral results are shown in Table 1.4.2-1. Neither the axisymmetric nor the three-dimensional global models used to drive submodels provide useful J values. The submodels driven by these global models, however, give J -integral results that differ from their related full models by only 2%. In the three-dimensional models the J -integrals on planes that include element corner nodes differ slightly from the J -integrals on planes that include only element midside nodes. The difference occurs because the strain singularity at the crack tip is reproduced on planes of nodes that include corner nodes, whereas on planes of nodes passing through midside nodes there is no singularity since we use 20-node elements. The use of 27-node elements adjacent to the crack line should eliminate this problem. In addition, the stress intensity factors and the T -stresses are calculated. The interaction integral method, in which the auxiliary plane strain crack-tip fields are employed, is used for their calculations. Since the crack front is very close to the symmetry axis, more refined meshes should be used to make the plane strain condition prevail locally around the crack front so that contour-independent results can be obtained. The calculated values of the stress intensity factors KI , KII , and KIII ; J -integral (estimated from both stress intensity factors and ABAQUS); and the T -stresses are shown in Table 1.4.2-2, Table 1.4.2-3, Table 1.4.2-4, Table 1.4.2-5, and Table 1.4.2-6, respectively. ABAQUS automatically outputs the J -integrals based on the stress intensity factors when the latter are evaluated. These J values are compared with the J values calculated directly by ABAQUS in Table 1.4.2-5, and good agreement is observed between them. The sign of KII is different in the three-dimensional model and in the axisymmetric model. This is not a problem since the sign of KII will depend on the order of the crack front node sets arranged for the contour integral computation.

Input files conicalcrack_3dglobal.inp Three-dimensional global model. conicalcrack_3dsubmodel.inp Three-dimensional submodel.

1-643

Static Stress/Displacement Analyses

conicalcrack_full3d.inp Full three-dimensional model. conicalcrack_node.inp Node definitions for conicalcrack_full3d.inp. conicalcrack_element.inp Element definitions for conicalcrack_full3d.inp. conicalcrack_axiglobal.inp Axisymmetric global model. conicalcrack_axisubmodel.inp Axisymmetric submodel. conicalcrack_fullaxi.inp Full axisymmetric model. conicalcrack_3dsubmodel_rms.inp Three-dimensional submodel with refined meshes. conicalcrack_full3d_rms.inp Full three-dimensional model with refined meshes. conicalcrack_node_rms.inp Node definitions for conicalcrack_full3d_rms.inp. conicalcrack_element_rms.inp Element definitions for conicalcrack_full3d_rms.inp. conicalcrack_axisubmodel_rms.inp Axisymmetric submodel with refined meshes. conicalcrack_fullaxi_rms.inp Full axisymmetric model with refined meshes.

Tables Table 1.4.2-1 J -integral estimates (´ 10-7) for conical crack. Contour 1 is omitted from the average value calculations. Solution

Full

Crack Front Location Crack tip

1 5 1.360

Contour 2 3 6 7 1.331

1.336

1-644

4 8 1.337

Average Value, Contours 2-8

Static Stress/Displacement Analyses

Axisymmetric

Corner nodes Full Three-dimensiona Midside l nodes

Submodel Axisymmetric

Crack tip

Corner nodes Submodel Three-dimensiona Midside l nodes

5 1.337 5 1.361 5 1.331 5 1.360 3 1.338 7 1.390 3 1.367 6 1.392 1 1.365 7 1.390 5 1.369 3

6 1.337 7 1.331 4 1.334 5 1.331 6 1.339 4 1.361 0 1.368 0 1.361 4 1.365 3 1.361 6 1.370 1

3 1.337 9 1.335 5 1.333 6 1.336 7 1.340 0 1.366 0 1.368 2 1.365 8 1.363 9 1.367 0 1.371 1

2 1.337 9 1.335 6 1.332 5 1.338 0 1.340 6 1.367 1 1.367 3 1.366 1 1.363 8 1.368 4 1.369 9

1.3364

1.3340

1.3379

1.3665

1.3646

1.3682

Table 1.4.2-2 Stress intensity factor KI estimates for conical crack using refined meshes. Contour 1 is omitted from the average value calculations. Solution Crack 1 Front

2

Contour 3

4

5

0.478 3 0.477 2 0.476 4 0.526 9 0.526 2 0.525 3

0.479 3 0.478 4 0.477 1 0.528 0 0.527 5 0.526 2

0.479 7 0.479 1 0.477 2 0.528 4 0.528 2 0.526 3

0.480 1 0.479 8 0.477 2 0.528 8 0.528 9 0.526 3

Location Full Axisymmetric

Crack tip

Corner Full nodes Three-dimensiona Midside l nodes Submodel Crack tip Axisymmetric Corner Submodel nodes Three-dimensiona Midside l nodes

0.487 7 0.472 4 0.492 8 0.537 3 0.521 0 0.543 5

Average Value, Contours 2-5 0.4794 0.4786 0.4770 0.5280 0.5277 0.5260

Table 1.4.2-3 Stress intensity factor KII estimates for conical crack using refined meshes. Contour 1

1-645

Static Stress/Displacement Analyses

is omitted from the average value calculations. Solution Crack 1 2 Front

Contour 3

4

5

Location Full Axisymmetric

Crack tip

Corner Full nodes Three-dimensiona Midside l nodes Submodel Crack tip Axisymmetric Corner Submodel nodes Three-dimensiona Midside l nodes

-2.078 -2.039

Average Value, Contours 2-5 -2.040

2.015

2.041

-2.04 1 2.045

2.108

2.037

2.041

2.041

2.041

2.040

-2.090 -2.050

-2.052 -2.051

-2.051

2.057

2.057

2.056

2.053

2.053

2.052

2.027

2.053

-2.05 3 2.057

2.121

2.049

2.052

-2.041 -2.039 2.045

2.045

2.044

Table 1.4.2-4 Stress intensity factor KIII estimates for conical crack using refined meshes. Contour 1 is omitted from the average value calculations. Solution Crack 1 2 Front Location Corner Full nodes Three-dimensiona Midside l nodes Corner Submodel nodes Three-dimensiona Midside l nodes

0.000 0 0.015 0 0.000 0 0.016

0.000 0 0.014 0 0.000 0 0.016

Contour 3

4

5

0.000 0 0.014 0 0.000 0 0.015

0.000 0 0.013 0 0.000 0 0.015

0.000 0 0.013 0 0.000 0 0.014

Average Value, Contours 2-5 0.0000 0.0140 0.0000 0.015

Table 1.4.2-5 J -integral estimates (´ 10-7) for conical crack using refined meshes. JK denotes the J estimated from stress intensity factors; JA denotes the J estimated directly by ABAQUS. Contour Average Solution Crack 1 2 3 4 5 Value, Front (JK) (JK) (JK) (JK) (JK) Contours Location 1 2 3 4 5 2-5 (JA) (JA) (JA) (JA) (JA) Full Crack tip 1.382 1.330 1.334 1.333 1.332 1.332 1.377 1.331 1.335 1.336 1.336 1.334 Axisymmetric Corner 1.300 1.333 1.337 1.338 1.338 1.337

1-646

Static Stress/Displacement Analyses

Full nodes Three-dimensiona Midside l nodes Submodel Crack tip Axisymmetric Corner Submodel nodes Three-dimensiona Midside l nodes

1.306 1.422 1.412 1.413 1.407 1.329 1.336 1.454 1.443

1.331 1.327 1.330 1.359 1.360 1.363 1.361 1.357 1.360

1.336 1.332 1.335 1.363 1.365 1.367 1.366 1.362 1.365

1.336 1.332 1.335 1.363 1.365 1.368 1.366 1.362 1.365

1.336 1.332 1.336 1.361 1.365 1.368 1.366 1.362 1.366

1.335 1.331 1.334 1.362 1.364 1.367 1.365 1.361 1.364

Table 1.4.2-6 T -stress estimates for conical crack using refined meshes. Contour 1-2 is omitted from the average value calculations. Solution Crack Front Location Full Crack tip Axisymmetric Corner Full nodes Three-dimensiona Midside l nodes Submodel Crack tip Axisymmetric Corner Submodel nodes Three-dimensiona Midside l nodes

1

Contour 3

2

-1.161 -0.981 -0.640 -0.971 -1.315 -0.973 -1.182 -0.983 -0.598 -0.974 -1.366 -0.976

-0.98 2 -0.97 6 -0.97 7 -0.98 5 -0.97 9 -0.98 0

Figures Figure 1.4.2-1 Conical crack in a half-space.

1-647

Average Value, Contours 3-5 -0.981 -0.981 -0.981 4

5

-0.976 -0.976

-0.976

-0.978 -0.979

-0.978

-0.984 -0.984

-0.984

-0.979 -0.979

-0.979

-0.981 -0.982

-0.981

Static Stress/Displacement Analyses

Figure 1.4.2-2 Full three-dimensional mesh.

Figure 1.4.2-3 Full axisymmetric mesh.

1-648

Static Stress/Displacement Analyses

Figure 1.4.2-4 Three-dimensional displaced shape.

Figure 1.4.2-5 Axisymmetric global model for use with submodeling.

1-649

Static Stress/Displacement Analyses

Figure 1.4.2-6 Three-dimensional global model with submodel overlaid.

Figure 1.4.2-7 Axisymmetric global model with submodel overlaid.

1-650

Static Stress/Displacement Analyses

Sample listings

1-651

Static Stress/Displacement Analyses

Listing 1.4.2-1 *HEADING FULL THREE-DIMENSIONAL CONICAL CRACK MODEL *WAVEFRONT MINIMIZATION,SUPPRESS ** INCLUDE NODE DATA *INCLUDE,INPUT=conicalcrack_node.inp ** INCLUDE ELEMENT DATA *INCLUDE,INPUT=conicalcrack_element.inp *MATERIAL,NAME=STEEL *ELASTIC 30.E6,0.3 *SOLID SECTION, MATERIAL=STEEL, ELSET=EALL *MPC TIE,TIP01,TIP02 TIE,TIP11,TIP12 TIE,TIP21,TIP22 TIE,TIP31,TIP32 TIE,TIP41,TIP42 TIE,TIP51,TIP52 TIE,TIP61,TIP62 TIE,TIP71,TIP72 TIE,TIP81,TIP82 TIE,TIP91,TIP92 TIE,TIP101,TIP102 TIE,TIP111,TIP112 TIE,TIP121,TIP122 TIE,TIP131,TIP132 TIE,TIP141,TIP142 TIE,TIP151,TIP152 TIE,TIP161,TIP162 TIE,TIP171,TIP172 TIE,TIP181,TIP182 TIE,TIP191,TIP192 TIE,TIP201,TIP202 *NSET,NSET=N571,GENERATE 57833,2057833,100000 *NSET,NSET=N572,GENERATE 57865,2057865,100000 *NSET,NSET=N65,GENERATE 65833,2065833,100000 *MPC

1-652

Static Stress/Displacement Analyses

TIE,N572,N571 TIE,N65,N571 *NSET,NSET=N18,GENERATE 1833,2001833,100000 *NSET,NSET=N98,GENERATE 9833,2009833,100000 *MPC TIE,N18,N98 *MPC TIE,Y1,Y0 TIE,Y2,Y0 TIE,Y3,Y0 TIE,Y4,Y0 TIE,Y5,Y0 TIE,Y6,Y0 TIE,Y7,Y0 TIE,Y8,Y0 TIE,Y9,Y0 TIE,Y10,Y0 TIE,Y11,Y0 TIE,Y12,Y0 TIE,Y13,Y0 TIE,Y14,Y0 TIE,Y15,Y0 TIE,Y16,Y0 TIE,Y17,Y0 TIE,Y18,Y0 TIE,Y19,Y0 TIE,Y20,Y0 *BOUNDARY N0,3,3 N20,1,1 Y0,1,1 Y0,3,3 *STEP APPLY PRESSURE LOAD *STATIC 1.0,1.0 *DLOAD TOP9,P4,10. *CONTOUR INTEGRAL,CONTOURS=8,OUTPUT=BOTH T0,0.70710678,-0.70710678,0. T1,0.70492701,-0.70710678,0.055478959

1-653

Static Stress/Displacement Analyses

T2,0.69840112,-0.70710678,0.11061587 T3,0.68756936,-0.70710678,0.1650708 T4,0.67249851,-0.70710678,0.21850801 T5,0.65328148,-0.70710678,0.27059805 T6,0.63003676,-0.70710678,0.32101976 T7,0.60290764,-0.70710678,0.36946228 T8,0.5720614,-0.70710678,0.41562694 T9,0.53768821,-0.70710678,0.45922912 T10,0.5,-0.70710678,0.5 T11,0.45922912,-0.70710678,0.53768821 T12,0.41562694,-0.70710678,0.5720614 T13,0.36946228,-0.70710678,0.60290764 T14,0.32101976,-0.70710678,0.63003676 T15,0.27059805,-0.70710678,0.65328148 T16,0.21850801,-0.70710678,0.67249851 T17,0.1650708,-0.70710678,0.68756936 T18,0.11061587,-0.70710678,0.69840112 T19,0.055478959,-0.70710678,0.70492701 T20,0.,-0.70710678,0.70710678 *CONTOUR INTEGRAL,CONTOURS=8,OUTPUT=BOTH, TYPE=K FACTORS T0,0.70710678,-0.70710678,0. T1,0.70492701,-0.70710678,0.055478959 T2,0.69840112,-0.70710678,0.11061587 T3,0.68756936,-0.70710678,0.1650708 T4,0.67249851,-0.70710678,0.21850801 T5,0.65328148,-0.70710678,0.27059805 T6,0.63003676,-0.70710678,0.32101976 T7,0.60290764,-0.70710678,0.36946228 T8,0.5720614,-0.70710678,0.41562694 T9,0.53768821,-0.70710678,0.45922912 T10,0.5,-0.70710678,0.5 T11,0.45922912,-0.70710678,0.53768821 T12,0.41562694,-0.70710678,0.5720614 T13,0.36946228,-0.70710678,0.60290764 T14,0.32101976,-0.70710678,0.63003676 T15,0.27059805,-0.70710678,0.65328148 T16,0.21850801,-0.70710678,0.67249851 T17,0.1650708,-0.70710678,0.68756936 T18,0.11061587,-0.70710678,0.69840112 T19,0.055478959,-0.70710678,0.70492701 T20,0.,-0.70710678,0.70710678 *CONTOUR INTEGRAL,CONTOURS=8,OUTPUT=BOTH,

1-654

Static Stress/Displacement Analyses

TYPE=T-STRESS T0,0.70710678,-0.70710678,0. T1,0.70492701,-0.70710678,0.055478959 T2,0.69840112,-0.70710678,0.11061587 T3,0.68756936,-0.70710678,0.1650708 T4,0.67249851,-0.70710678,0.21850801 T5,0.65328148,-0.70710678,0.27059805 T6,0.63003676,-0.70710678,0.32101976 T7,0.60290764,-0.70710678,0.36946228 T8,0.5720614,-0.70710678,0.41562694 T9,0.53768821,-0.70710678,0.45922912 T10,0.5,-0.70710678,0.5 T11,0.45922912,-0.70710678,0.53768821 T12,0.41562694,-0.70710678,0.5720614 T13,0.36946228,-0.70710678,0.60290764 T14,0.32101976,-0.70710678,0.63003676 T15,0.27059805,-0.70710678,0.65328148 T16,0.21850801,-0.70710678,0.67249851 T17,0.1650708,-0.70710678,0.68756936 T18,0.11061587,-0.70710678,0.69840112 T19,0.055478959,-0.70710678,0.70492701 T20,0.,-0.70710678,0.70710678 *EL PRINT S, *NODE PRINT U,RF *ENDSTEP

1-655

Static Stress/Displacement Analyses

Listing 1.4.2-2 *HEADING AXISYMMETRIC CONICAL CRACK MODEL--GLOBAL WITH 1 RING *WAVEFRONT MINIMIZATION,SUPPRESS *SYSTEM 10.,0.,0. *NODE,SYSTEM=C 1833,0.,0.,0. 9833,0.,0.,0. 57833,0.,0.,0. 57865,0.,0.,0. 65833,0.,0.,0. 1001,15.,-45.,0. 65001,15.,-45.,0. 1033,8.,-45.,0. 65033,8.,-45.,0. 33033,25.,-45.,0. 41033,25.,-18.,0. 57033,10.,-18.,0. 9033,10.,-72.,0. 25033,25.,-72.,0. 41065,25.,0.,0. 57065,10.,0.,0. *SYSTEM 0.,0.,0. *NODE,SYSTEM=C 9865,0.,0.,0. 9065,15.,-90.,0. 25065,30.,-90.,0. 25865,170.,-90.,0. 25965,340.,-90.,0. 25833,170.,-60.,0. 25933,340.,-60.,0. 33833,170.,-45.,0. 33933,340.,-45.,0. 41833,170.,-30.,0. 41933,340.,-30.,0. 41865,170.,0.,0. 41965,340.,0.,0. ** **CRACK TIP REGION *NGEN,NSET=TIP

1-656

Static Stress/Displacement Analyses

1001,65001,1000 *NGEN,NSET=OUTER1 1033,9033,1000 *NGEN,NSET=OUTER2 9033,25033,1000 *NGEN,NSET=OUTER3 25033,33033,1000 *NGEN,NSET=OUTER4 33033,41033,1000 *NGEN,NSET=OUTER5 41033,57033,1000 *NGEN,NSET=OUTER6 57033,65033,1000 *NSET,NSET=OUTER OUTER1,OUTER2,OUTER3,OUTER4,OUTER5,OUTER6 *NFILL,NSET=JREGION,SINGULAR=1 TIP,OUTER,2,16 ** **SECTION 9 *NGEN,NSET=BOT9 9033,9065,1 *NGEN,NSET=TOP9 9833,9865,1 *NFILL,NSET=ALL9 BOT9,TOP9,16,50 ** **SECTION 25 *NGEN,NSET=BOT25 25033,25065,1 *NGEN,NSET=TOP25,LINE=C 25833,25865,1,9865 *NFILL,NSET=ALL25,BIAS=0.8 BOT25,TOP25,16,50 ** **SECTION 41 *NGEN,NSET=BOT41 41033,41065,1 *NGEN,NSET=TOP41,LINE=C 41833,41865,1,9865 *NFILL,NSET=ALL41,BIAS=0.8 BOT41,TOP41,16,50 ** **SECTION 925

1-657

Static Stress/Displacement Analyses

*NFILL,NSET=ALL925 BOT9,BOT25,16,1000 ** **SECTION 2541 *NSET,NSET=BOT2533,GENERATE 25033,33033,1000 *NGEN,NSET=TOP2533,LINE=C 25833,33833,1000,9865 *NSET,NSET=BOT3341,GENERATE 33033,41033,1000 *NGEN,NSET=TOP3341,LINE=C 33833,41833,1000,9865 *NSET,NSET=BOT2541 BOT2533,BOT3341 *NSET,NSET=TOP2541 TOP2533,TOP3341 *NFILL,NSET=ALL2541,BIAS=0.8 BOT2541,TOP2541,16,50 ** **SECTION 4157 *NGEN,NSET=BOT57 57033,57065,1 *NFILL,NSET=ALL4157 BOT41,BOT57,16,1000 ** **SECTION 57 *NGEN,NSET=TOP57 57833,57865,1 *NFILL,NSET=ALL57,BIAS=1.0 BOT57,TOP57,16,50 ** **SECTION 5765 *NGEN,NSET=TOP5765 57833,65833,1000 *NFILL,NSET=ALL5765,BIAS=1.0 OUTER6,TOP5765,16,50 ** **SECTION 19 *NGEN,NSET=TOP19 1833,9833,1000 *NFILL,NSET=ALL19 OUTER1,TOP19,16,50 **

1-658

Static Stress/Displacement Analyses

**INFINITE ELEMENT REGION *NGEN,NSET=INF25,LINE=C 25933,25965,8,9865 *NGEN,NSET=INF2533,LINE=C 25933,33933,4000,9865 *NGEN,NSET=INF3341,LINE=C 33933,41933,4000,9865 *NGEN,NSET=INF41,LINE=C 41933,41965,8,9865 *NSET,NSET=INF INF25,INF2533,INF3341,INF41 ** **CRACK TIP REGION ELEMENTS *ELEMENT,TYPE=CAX8R 1001,1001,1033,5033,5001,1017,3033,5017,3001 *ELGEN,ELSET=RING 1001,16,4000,4000 ** **ELEMENTS SECTION 9 *ELEMENT,TYPE=CAX8R 9033,9033,9233,9241,9041,9133,9237,9141,9037 *ELGEN,ELSET=SECT9 9033,4,8,8,4,200,200 *ELSET,ELSET=TOP9,GENERATE 9633,9657,8 ** **ELEMENTS SECTION 25 *ELEMENT,TYPE=CAX8R 25233,25233,25033,25041,25241,25133,25037, 25141,25237 *ELGEN,ELSET=SECT25 25233,4,8,8,4,200,200 ** **ELEMENTS SECTION 19 *ELEMENT,TYPE=CAX8R 1033,1033,1233,5233,5033,1133,3233,5133,3033 *ELGEN,ELSET=SECT19 1033,2,4000,4000,4,200,200 ** **ELEMENT SECTION 925 *ELEMENT,TYPE=CAX8R 13033,13033,9033,9041,13041,11033,9037, 11041,13037

1-659

Static Stress/Displacement Analyses

*ELGEN,ELSET=SECT925 13033,4,8,8,4,4000,4000 ** **ELEMENT SECTION 2541 *ELEMENT,TYPE=CAX8R 29233,29233,29033,25033,25233,29133,27033, 25133,27233 *ELGEN,ELSET=SECT2541 29233,4,4000,4000,4,200,200 ** **ELEMENT SECTION 41 *ELEMENT, TYPE=CAX8R 41241,41241,41041,41033,41233,41141,41037, 41133,41237 *ELGEN,ELSET=SECT41 41241,4,8,8,4,200,200 ** **ELEMENT SECTION 4157 *ELEMENT,TYPE=CAX8R 41041,41041,45041,45033,41033,43041,45037, 43033,41037 *ELGEN,ELSET=SECT4157 41041,4,8,8,4,4000,4000 ** **ELEMENT SECTION 57 *ELEMENT, TYPE=CAX8R 57041,57041,57241,57233,57033,57141,57237, 57133,57037 *ELGEN,ELSET=SECT57 57041,4,8,8,4,200,200 ** **ELEMENT SECTION 5765 *ELEMENT,TYPE=CAX8R 57033,57033,57233,61233,61033,57133,59233, 61133,59033 *ELGEN,ELSET=SECT5765 57033,2,4000,4000,4,200,200 ** **INFINITE ELEMENTS *ELEMENT,TYPE=CINAX5R 41941,41841,41833,41933,41941,41837 *ELGEN,ELSET=INF41 41941,4,8,8

1-660

Static Stress/Displacement Analyses

*ELEMENT,TYPE=CINAX5R 29933,29833,25833,25933,29933,27833 *ELGEN,ELSET=INF2541 29933,4,4000,4000 *ELEMENT,TYPE=CINAX5R 25933,25833,25841,25941,25933,25837 *ELGEN,ELSET=INF25 25933,4,8,8 *ELSET,ELSET=INF INF41,INF2541,INF25 ** *ELSET,ELSET=E1 RING,SECT9,SECT25,SECT41,SECT57,SECT19,SECT925, SECT2541,SECT4157,SECT5765,INF *MATERIAL,NAME=STEEL *ELASTIC 30.E6,0.3 *SOLID SECTION, MATERIAL=STEEL, ELSET=E1 ** **ADD BOUNDARY CONDITIONS *NSET,NSET=R9,GENERATE 9065,9865,50 *NSET,NSET=R925,GENERATE 9065,25065,1000 *NSET,NSET=R25,GENERATE 25065,25865,50 *NSET,NSET=YAXIS R9,R925,R25 *NSET,NSET=L57,GENERATE 57065,57865,50 *NSET,NSET=L4157,GENERATE 41065,57065,1000 *NSET,NSET=L41,GENERATE 41065,41865,50 *NSET,NSET=XAXIS TOP9,L57,L4157,L41 *BOUNDARY YAXIS,XSYMM ** **MPC'S TO TIE REDUNDANT NODES *NSET,NSET=TIP1,GENERATE 1001,64001,1000 *NSET,NSET=TIP2,GENERATE

1-661

Static Stress/Displacement Analyses

2001,65001,1000 *MPC TIE,TIP1,TIP2 *MPC TIE,57865,57833 *MPC TIE,57833,65833 *MPC TIE,1833,9833 ** *STEP APPLY PRESSURE LOAD *STATIC 1.0,1.0 *DLOAD TOP9,P2,10. *CONTOUR INTEGRAL,CONTOURS=1,OUTPUT=BOTH TIP,0.707107,-0.707107 *CONTOUR INTEGRAL,CONTOURS=1,OUTPUT=BOTH, TYPE=K FACTORS TIP,0.707107,-0.707107 *CONTOUR INTEGRAL,CONTOURS=1,OUTPUT=BOTH, TYPE=T-STRESS TIP,0.707107,-0.707107 *EL PRINT S, *NODE PRINT U,RF *NODE FILE U, *OUTPUT,FIELD *NODE OUTPUT U, *ENDSTEP

1-662

Static Stress/Displacement Analyses

Listing 1.4.2-3 *HEADING AXISYMMETRIC CONICAL CRACK MODEL SUBMODEL WITH 8 RINGS *WAVEFRONT MINIMIZATION,SUPPRESS *SYSTEM 10.,0.,0. *NODE,SYSTEM=C 1833,0.,0.,0. 9833,0.,0.,0. 57833,0.,0.,0. 57865,0.,0.,0. 65833,0.,0.,0. 1001,15.,-45.,0. 65001,15.,-45.,0. 1033,8.,-45.,0. 65033,8.,-45.,0. 33033,25.,-45.,0. 41033,25.,-18.,0. 57033,10.,-18.,0. 9033,10.,-72.,0. 25033,25.,-72.,0. 41065,25.,0.,0. 57065,10.,0.,0. *SYSTEM 0.,0.,0. *NODE,SYSTEM=C 9865,0.,0.,0. 9065,15.,-90.,0. 25065,30.,-90.,0. 25865,170.,-90.,0. 25965,340.,-90.,0. 25833,170.,-60.,0. 25933,340.,-60.,0. 33833,170.,-45.,0. 33933,340.,-45.,0. 41833,170.,-30.,0. 41933,340.,-30.,0. 41865,170.,0.,0. 41965,340.,0.,0. *NODE,SYSTEM=R 1033,15.656,-5.6579

1-663

Static Stress/Displacement Analyses

65033,15.658,-5.6559 ** **CRACK TIP REGION *NGEN,NSET=TIP 1001,65001,2000 *NGEN,NSET=OUTER1 1033,9033,2000 *NGEN,NSET=OUTER2 9033,25033,2000 *NGEN,NSET=OUTER3 25033,33033,2000 *NGEN,NSET=OUTER4 33033,41033,2000 *NGEN,NSET=OUTER5 41033,57033,2000 *NGEN,NSET=OUTER6 57033,65033,2000 *NSET,NSET=OUTER OUTER1,OUTER2,OUTER3,OUTER4,OUTER5,OUTER6 *NFILL,NSET=JREGION,SINGULAR=1 TIP,OUTER,16,2 ** **CRACK TIP REGION ELEMENTS *ELEMENT,TYPE=CAX8R 1001,1001,1005,5005,5001,1003,3005,5003,3001 *ELGEN,ELSET=RINGS 1001,16,4000,4000,8,4,4 ** *MATERIAL,NAME=STEEL *ELASTIC 30.E6,0.3 *SOLID SECTION, MATERIAL=STEEL, ELSET=RINGS ** **MPC'S TO TIE REDUNDANT NODES *NSET,NSET=TIP1,GENERATE 1001,63001,2000 *NSET,NSET=TIP2,GENERATE 3001,65001,2000 *MPC TIE,TIP1,TIP2 *SUBMODEL OUTER, **

1-664

Static Stress/Displacement Analyses

*STEP *STATIC 1.,1. *BOUNDARY,SUBMODEL,STEP=1 OUTER,1,2 *CONTOUR INTEGRAL,CONTOURS=8,OUTPUT=BOTH TIP,0.707107,-0.707107 *CONTOUR INTEGRAL,CONTOURS=8,OUTPUT=BOTH, TYPE=K FACTORS TIP,0.707107,-0.707107 *CONTOUR INTEGRAL,CONTOURS=8,OUTPUT=BOTH, TYPE=T-STRESS TIP,0.707107,-0.707107 *EL PRINT S, *NODE PRINT U,RF *ENDSTEP

1.4.3 Elastic-plastic line spring modeling of a finite length cylinder with a part-through axial flaw Product: ABAQUS/Standard The elastic-plastic line spring elements in ABAQUS are intended to provide inexpensive solutions for problems involving part-through surface cracks in shell structures loaded predominantly in Mode I by combined membrane and bending action in cases where it is important to include the effects of inelastic deformation. This example illustrates the use of these elements. The case considered is a long cylinder with an axial flaw in its inside surface, subjected to internal pressure. It is taken from the paper by Parks and White (1982). When the line spring element model reaches theoretical limitations, the shell-to-solid submodeling technique is utilized to provide accurate J -integral results. The energy domain integral is used to evaluate the J -integral for this case.

Geometry and model The cylinder has an inside radius of 254 mm (10 in), wall thickness of 25.4 mm (1 in), and is assumed to be very long. The mesh is shown in Figure 1.4.3-1. It is refined around the crack by using multi-point constraints (MPCs). There are 70 shell elements of type S8R in the symmetric quarter-model and eight symmetric line spring elements (type LS3S) along the crack. The mesh is taken from Parks and White, who suggest that this mesh is adequately convergent with respect to the fracture parameters (J -integral values) that are the primary objective of the analysis. No independent mesh studies have been done. The use of MPCs to refine a mesh of reduced integration shell elements (such as S8R) is generally satisfactory in relatively thick shells as in this case. However, it is not

1-665

Static Stress/Displacement Analyses

recommended for thin shells because it introduces constraints that "lock" the response in the finer mesh regions. In a thin shell case the finer mesh would have to be carried out well away from the region of high strain gradients. Three different flaws are studied. All have the semi-elliptic geometry shown in Figure 1.4.3-2, with, in all cases, c = 3a0 : The three flaws have a0 =t ratios of 0.25 (a shallow crack), 0.5, and 0.8 (a deep crack). In all cases the axial length of the cylinder is taken as 14 times the crack half-length, c: this is assumed to be sufficient to approximate the infinite length. An input data file for the case a0 =t =.5 without making the symmetry assumption about z =0 is also included. This mesh uses the LS6 line spring elements and serves to check the elastic-plastic capability of the LS6 elements. The results are the same as for the corresponding mesh using LS3S elements and symmetry about z =0. The formulation of the LS6 elements assumes that the plasticity is predominately due to Mode I deformation around the flaw and neglects the effect of the Mode II and Mode III deformation around the flaw. In the global mesh the displacement in the z-direction is constrained to be zero at the node at the end of the flaw where the flaw depth goes to zero. To duplicate this constraint in the mesh using LS6 elements, the two nodes at the end of the flaw (flaw depth = 0) are constrained to have the same displacements.

Material The cylinder is assumed to be made of an elastic-plastic metal, with a Young's modulus of 206.8 GPa (30 ´ 106 lb/in2), a Poisson's ratio of 0.3, an initial yield stress of 482.5 MPa (70000 lb/in 2, and constant work hardening to an ultimate stress of 689.4 MPa (10 5 lb/in2) at 10% plastic strain, with perfectly plastic behavior at higher strains.

Loading The loading consists of uniform internal pressure applied to all of the shell elements, with edge loads applied to the far end of the cylinder to provide the axial stress corresponding to a closed-end condition. Even though the flaw is on the inside surface of the cylinder, the pressure is not applied on the exposed crack face. Since pressure loads on the flaw surface of line spring elements are implemented using linear superposition in ABAQUS, there is no theoretical basis for applying these loads when nonlinearities are present. We assume that this is not a large effect in this problem. For consistency with the line spring element models, pressure loading of the crack face is not applied to the shell-to-solid submodel.

Results and discussion The line spring elements provide J -integral values directly. Figure 1.4.3-3 shows the J -integral values at the center of the crack as functions of applied pressure for the three flaws. In the input data the maximum time increment size has been limited so that adequately smooth graphs can be obtained. Figure 1.4.3-4 shows the variations of the J -integral values along the crack for the half-thickness crack ¹ ¹ y t, is used, where R (a0 =t =0.5), at several different pressure levels (a normalized pressure, p^ = pR=¾ is the mean radius of the cylinder). These results all agree closely with those reported by Parks and White (1982), where the authors state that these results are also confirmed by other work. In the region

1-666

Static Stress/Displacement Analyses

Á <30° the results are inaccurate for two reasons. First, the depth of the flaw is changing very rapidly in this region, which makes the line spring approximation quite inaccurate. Second, J el is of the same order of magnitude as J pl , but the line spring plasticity model is only valid when J el << J pl : The results toward the center of the crack (Á >30°) are more accurate than those at the ends of the crack since the flaw depth changes less rapidly with position in this region and J pl is much larger than J el : For this reason only J values for Á >30° are shown in Figure 1.4.3-4.

Shell-to-solid submodeling around the crack tip An input file for the case a0 =t =0.25, which uses the shell-to-solid submodeling capability, is included. This C3D20R element mesh allows the user to study the local crack area using the energy domain integral formulation for the J -integral. The submodel uses a focused mesh with four rows of elements around the crack tip. A 1/r singularity is utilized at the crack tip, the correct singularity for a fully developed perfectly plastic solution. Symmetry boundary conditions are imposed on two edges of the submodel mesh, while results from the global shell analysis are interpolated to two surfaces via the submodeling technique. The global shell mesh gives satisfactory J -integral results; hence, we assume that the displacements at the submodel boundary are sufficiently accurate to drive the deformation in the submodel. No attempt has been made to study the effect of making the submodel region larger or smaller. The submodel is shown superimposed on the global shell model in Figure 1.4.3-5. In addition, an input file for the case a0 =t =0.25, which consists of a full three-dimensional C3D20R solid element model, is included for use as a reference solution. This model has the same general characteristics as the submodel mesh. See inelasticlinespring_c3d20r_ful.inp for further details about this mesh. One important difference exists in performing this analysis with shell elements as opposed to continuum elements. The pressure loading is applied to the midsurface of the shell elements as opposed to the continuum elements, where the pressure is accurately applied along the inside surface of the cylinder. For this analysis this discrepancy results in about 10% higher J -integral values for the line spring shell element analysis as compared to the full three-dimensional solid element model. Results from the submodeled analyses are compared to the LS3S line spring element analysis and full solid element mesh for variations of the J -integral values along the crack at the a normalized pressure ¹ is the mean radius of the cylinder. As seen in Figure 1.4.3-6, ¹ (¾y t) = 0.898, where R loading of pR= the line spring elements underestimate the J -integral values for Á <50° for reasons described previously. Note that at Á =0° the J -integral should be zero due to the lack of crack-tip constraint at the cylinder surface. A more refined mesh would be required to model this phenomenon properly. It is quite obvious that the use of shell-to-solid submodeling is required to augment a line spring element model analysis to obtain accurate J -integral values near the surface of the cylinder.

Input files inelasticlinespring_05.inp a0 =t = 0.5. inelasticlinespring_05_nosym.inp a0 =t = 0.5 without the symmetry assumption across z =0, using line spring element type LS6.

1-667

Static Stress/Displacement Analyses

inelasticlinespring_progcrack.f A program used to create a data file giving the flaw depths as a function of position along the crack. inelasticlinespring_025.inp Shallow crack case, a0 =t =0.25. inelasticlinespring_08.inp Deep crack case, a0 =t =0.8. inelasticlinespring_c3d20r_sub.inp C3D20R (a0 =t =0.25) submodel. inelasticlinespring_c3d20r_ful.inp C3D20R (a0 =t =0.25) full model.

Reference · Parks, D. M., and C. S. White, "Elastic-Plastic Line-Spring Finite Elements for Surface-Cracked Plates and Shells," Transactions of the ASME, Journal of Pressure Vessel Technology, vol. 104, pp. 287-292, November 1982.

Figures Figure 1.4.3-1 Finite element model for an axial flaw in a pressurized cylinder.

1-668

Static Stress/Displacement Analyses

Figure 1.4.3-2 Schematic of a semi-elliptical surface crack.

1-669

Static Stress/Displacement Analyses

Figure 1.4.3-3 Normalized J -integral values EJ =(¾y2 t) versus normalized applied pressure ¹ is the mean radius of the cylinder. ¹ (¾y t), where R pR=

Figure 1.4.3-4 Normalized J -integral values EJ =(¾y2 t) versus position along the flaw surface given ¹ is the ¹ (¾y t)= .574, 1.097, and 1.172. R by 2Á=¼, for a0 =t =0.5, and normalized applied pressures pR=

mean radius of the cylinder.

Figure 1.4.3-5 Solid submodel superimposed on shell global model.

1-670

Static Stress/Displacement Analyses

Figure 1.4.3-6 Normalized J -integral values EJ =(¾y2 t) versus position along the flaw surface given ¹ is the mean radius of the ¹ (¾y t) =0.898. R by 2Á=¼ for a0 =t =0.25 and at the normalized pressure. pR=

cylinder.

1-671

Static Stress/Displacement Analyses

Sample listings

1-672

Static Stress/Displacement Analyses

Listing 1.4.3-1 *HEADING FINITE LENGTH AXIAL FLAW IN PRESSURIZED CYLINDER *NODE,SYSTEM=C 1, 10.5,-90.,0. 97, 10.5,-90.,6. 99, 10.5,-90.,9. 103, 10.5,-90.,21. 9601, 10.5,234.,0. 9697, 10.5,234.,6. 9699, 10.5,234.,9. 9703, 10.5,234.,21. 11201, 10.5,90.,0. 11297, 10.5,90.,6. 11299, 10.5,90.,9. 11303, 10.5,90.,21. 99991, 0.,0.,0. 99992, 0.,0.,6. 99993, 0.,0.,9. 99994, 0.,0.,21. *NGEN,NSET=BOTTOM,LINE=C 1,9601,200,99991,,,,,,-1. 9601,11201,200,99991,,,,,,-1. *NGEN,NSET=MID1,LINE=C 97,9697,200,99992,,,,,,-1. 9697,11297,200,99992,,,,,,-1. *NGEN,NSET=MID2,LINE=C 99,9699,200,99993,,,,,,-1. 9699,11299,200,99993,,,,,,-1. *NGEN,NSET=TOP,LINE=C 103,9703,200,99994,,,,,,-1. 9703,11303,200,99994,,,,,,-1. *NGEN 1,97 97,99 99,103 *NSET,NSET=EDGE1,GENERATE 25,103 *NGEN,NSET=EDGE2 11201,11297 11297,11299 11299,11303

1-673

Static Stress/Displacement Analyses

*NFILL BOTTOM,MID1,96 MID1,MID2,2 MID2,TOP,4 *NSET,NSET=N1 103,11303 *NSET,NSET=N2 4903,9903,10303,10703,11103 *NSET,NSET=N3 9703,10103,10503,10903 *NSET,NSET=ND1 1, ** *ELEMENT,TYPE=S8R,ELSET=SHELL 9, 1,5,405,401,3,205,403,201 13, 17,19,419,417,18,219,418,217 17, 25,29,429,425,27,229,427,225 18, 29,37,437,429,33,237,433,229 22, 61,77,477,461,69,277,469,261 23, 77,97,497,477,87,297,487,277 24, 401,409,1209,1201,405,809,1205,801 26, 1201,1209,2809,2801,1205,2009,2805,2001 28, 417,421,1221,1217,419,821,1219,817 31, 1217,1221,2821,2817,1219,2021,2819,2017 34, 429,437,1237,1229,433,837,1233,829 38, 1229,1237,2837,2829,1233,2037,2833,2029 42, 461,477,1277,1261,469,877,1269,861 43, 1261,1277,2877,2861,1269,2077,2869,2061 44, 477,497,1297,1277,487,897,1287,877 45, 1277,1297,2897,2877,1287,2097,2887,2077 46, 2801,2817,6017,6001,2809,4417,6009,4401 48, 2817,2821,6021,6017,2819,4421,6019,4417 50, 2821,2829,6029,6021,2825,4429,6025,4421 58, 2877,2897,6097,6077,2887,4497,6087,4477 47, 6001,6017,9617,9601,6009,7817,9609,7801 49, 6017,6021,9621,9617,6019,7821,9619,7817 51, 6021,6029,9629,9621,6025,7829,9625,7821 59, 6077,6097,9697,9677,6087,7897,9687,7877 1002, 97,99,9699,9697,98,4899,9698,4897 1101, 9601,9697,10097,10001,9649,9897,10049,9801 1102, 9697,9699,10099,10097,9698,9899,10098,9897 *ELGEN,ELSET=SHELL 9,4,4,1

1-674

Static Stress/Displacement Analyses

13,4,2,1 18,4,8,1 24,2,8,1 26,2,8,1 28,3,4,1 31,3,4,1 34,4,8,1 38,4,8,1 46,2,28,6 52,3,16,2 47,2,28,6 53,3,16,2 1002,3,2,1 1102,3,2,1 1101,4,400,100 1102,4,400,100 1103,4,400,100 1104,4,400,100 *ELSET,ELSET=SHELL1,GENERATE 1,59 *MATERIAL,NAME=MSHELL *ELASTIC 30.E6,.3 *PLASTIC 7.E4,0. 1.E5,.0976 *SHELL SECTION,ELSET=SHELL,MATERIAL=MSHELL 1., *ELEMENT,TYPE=LS3S 1, 25,24,23 5, 17,15,13 *ELGEN,ELSET=CRACK 1, 4,-2,1 5, 4,-4,1 *SURFACE FLAW,SIDE=NEGATIVE 1, 0.5000000 3, 0.4982609 5, 0.4930066 7, 0.4841229 9, 0.4714045 11, 0.4545297 13, 0.4330127 15, 0.4061164

1-675

Static Stress/Displacement Analyses

17, 0.3726780 18, 0.3529390 19, 0.3307189 20, 0.3054766 21, 0.2763854 22, 0.2420615 23, 0.1998263 24, 0.1428261 25, 0.0000000 *SHELL SECTION,ELSET=CRACK,MATERIAL=MSHELL 1., *MPC QUADRATIC, 403,401,405,409 QUADRATIC, 407,401,405,409 QUADRATIC, 411,409,413,417 QUADRATIC, 415,409,413,417 QUADRATIC, 418,417,419,421 QUADRATIC, 420,417,419,421 QUADRATIC, 422,421,423,425 QUADRATIC, 424,421,423,425 QUADRATIC, 2805,2801,2809,2817 QUADRATIC, 2813,2801,2809,2817 QUADRATIC, 2823,2821,2825,2829 QUADRATIC, 2827,2821,2825,2829 QUADRATIC, 2833,2829,2837,2845 QUADRATIC, 2841,2829,2837,2845 QUADRATIC, 2849,2845,2853,2861 QUADRATIC, 2857,2845,2853,2861 QUADRATIC, 9609,9601,9649,9697 QUADRATIC, 9617,9601,9649,9697 QUADRATIC, 9619,9601,9649,9697 QUADRATIC, 9621,9601,9649,9697 QUADRATIC, 9625,9601,9649,9697 QUADRATIC, 9629,9601,9649,9697 QUADRATIC, 9637,9601,9649,9697 QUADRATIC, 9645,9601,9649,9697 QUADRATIC, 9653,9601,9649,9697 QUADRATIC, 9661,9601,9649,9697 QUADRATIC, 9669,9601,9649,9697 QUADRATIC, 9677,9601,9649,9697 QUADRATIC, 9687,9601,9649,9697 QUADRATIC, 7897,9697,4897,97 QUADRATIC, 6097,9697,4897,97

1-676

Static Stress/Displacement Analyses

QUADRATIC, 4497,9697,4897,97 QUADRATIC, 2897,9697,4897,97 QUADRATIC, 2097,9697,4897,97 QUADRATIC, 1297,9697,4897,97 QUADRATIC, 897,9697,4897,97 QUADRATIC, 497,9697,4897,97 QUADRATIC, 297,9697,4897,97 *RESTART,WRITE,FREQUENCY=5 ** *STEP,INC=10 *STATIC 1.,1. *CLOAD N1,3,1.15E4 N3,3,2.30E4 N2,3,4.60E4 *DLOAD SHELL,P,3325. *BOUNDARY EDGE1,XSYMM EDGE2,XSYMM BOTTOM,ZSYMM 11201,2 *NODE PRINT,NSET=ND1,SUMMARY=NO U, RF, *EL PRINT,ELSET=CRACK JK, *ENERGY PRINT *NODE FILE,NSET=ND1 U,RF *OUTPUT,FIELD *NODE OUTPUT,NSET=ND1 U,RF *EL FILE,ELSET=CRACK JK, *OUTPUT,FIELD *ELEMENT OUTPUT,ELSET=CRACK JK, *EL FILE,ELSET=SHELL LOADS, *OUTPUT,FIELD *ELEMENT OUTPUT,ELSET=SHELL

1-677

Static Stress/Displacement Analyses

LOADS, *ENERGY FILE *OUTPUT,HISTORY,FREQUENCY=1 *ENERGY OUTPUT,VARIABLE=PRESELECT *END STEP ** *STEP,INC=20 *STATIC .1,1.,,.1 *CLOAD N1,3,.2875E5 N3,3,.575E5 N2,3,1.15E5 *DLOAD SHELL,P,8312.5 *END STEP

1-678

Static Stress/Displacement Analyses

Listing 1.4.3-2 CC--- PROGRAM TO GENERATE CRACK DEPTH DATA C PROGRAM CRACK C SUBROUTINE HKSMAIN C IMPLICIT REAL*8(A-H,O-Z) C=1.5 CC=C*C N=24 NNODE=N+1 X0=C/DBLE(N) X=0. DO 100 I=1,NNODE IF(I.GE.17) GO TO 1 IF((I/2)*2.EQ.I) GO TO 10 1 CONTINUE XX=X*X TMP=3. Z=SQRT(CC-XX)/TMP WRITE(6,99) I,Z WRITE(16,99)I,Z 99 FORMAT(I5,F10.7) 10 CONTINUE X=X+X0 100 CONTINUE REWIND 16 STOP END

1.4.4 Crack growth in a three-point bend specimen Product: ABAQUS/Standard This example illustrates the modeling of crack length versus time to simulate crack propagation and the use of crack opening displacement as a crack propagation criterion. For stable crack growth in ductile materials, experimental evidence indicates that the value of the crack opening displacement (COD) at a specified distance behind the crack tip associated with ongoing crack extension is usually a constant. ABAQUS provides the critical crack opening displacement, at a specified distance behind the crack tip, as a crack propagation criterion. The other crack propagation model used in this example--prescribed crack length versus time--is usually used to verify the results obtained from experiments. ABAQUS also provides the critical stress criterion for crack propagation in brittle

1-679

Static Stress/Displacement Analyses

materials. In this example an edge crack in a three-point bend specimen is allowed to grow based on the crack opening displacement criterion. Crack propagation is first modeled by giving the crack length as a function of time. The data for the crack length are taken from Kunecke, Klingbeil, and Schicker (1993). The data for the crack propagation analysis using the COD criterion are taken from the first analysis. This example demonstrates how the COD criterion can be used in stable crack growth analysis.

Problem description An edge crack in a three-point bend specimen in plane strain, subjected to Mode I loading, is considered (see Figure 1.4.4-1). The crack length to specimen width ratio is 0.2. The length of the specimen is 55 mm, and its width is 10 mm. The specimen is subjected to bending loads such that initially a well-contained plastic zone develops for the stationary crack. Subsequently, the crack is allowed to grow.

Geometry and model Due to symmetry only one-half of the specimen is analyzed. The crack tip is modeled as initially blunted so that finite deformation effects near the crack tip can be taken into account (the NLGEOM parameter is used on the *STEP option). The mesh is composed of 1737 CPE4 elements (Figure 1.4.4-2). A reasonably fine mesh, necessary to obtain a smooth load versus crack length relation, is used to model the area in which the plastic zone grows and crack propagation occurs. The loading point and the support points for the specimen are simulated by analytical rigid surfaces, as shown in Figure 1.4.4-2.

Material The material is assumed to be elastic-plastic, with a Young's modulus of E = 200 GPa and Poisson's ratio of 0.3. The plastic work hardening data are given in Table 1.4.4-1.

Loading and solution control The analysis is carried out in two stages. The first stage consists of pushing the rigid surface 1.0 mm into the specimen. No crack growth is specified during this stage. In the second stage the crack is allowed to propagate while the rigid surface is moved an additional 1.951 mm. Once a crack-tip node debonds, the traction at the tip is initially carried as a reaction force at that node. This force is ramped down to zero according to the amplitude curve specified under the *DEBOND option. The manner in which the forces at the debonded nodes are ramped down greatly influences the convergence of the solution. The convergence of the solution is also affected by reversals in plastic flow due to crack propagation. In such circumstances, very small time increments are required to continue the analysis. In the present analysis the *CONTROLS, PARAMETER=FIELD, FIELD=DISPLACEMENT option is used to relax the tolerances so that more rapid convergence is achieved. Because of the localized nature of the nonlinearity in this problem, the resulting loss of

1-680

Static Stress/Displacement Analyses

accuracy is not significant. The *CONTROLS option is generally not recommended.

Crack length versus time In the case when the crack length is given as a function of time, the second step in the analysis consists of letting the crack grow according to a prescribed crack length versus time relationship, using the data taken from Kunecke, Klingbeil, and Schicker.

COD criterion The loading of the specimen and the specification of the COD criterion for crack growth demonstrates the flexibility of the COD criterion on the *DEBOND option. Frequently, the crack opening displacement is measured at the mouth of the crack tip: this is called the crack mouth opening displacement (CMOD). The crack opening displacement can also be measured at the position where the initial crack tip was located. Alternatively, the crack-tip opening angle ( CTOA), defined as the angle between the two surfaces at the tip of the crack, is measured. The crack-tip opening angle can be easily reinterpreted as the crack opening at a distance behind the crack tip. In this example the COD specification required to use both the CMOD and the CTOA criteria is demonstrated. For the purposes of demonstration the crack opening displacement at the mouth of the crack is used as the initial debond criterion. The first three nodes along the crack propagation surface are allowed to debond when the crack opening displacement at the mouth of the crack reaches a critical value. To achieve this, the following loading sequence is adopted: in Step 1, the specimen is loaded to a particular value (*DEBOND is not used), and in Step 2 the first crack-tip node is allowed to debond (*DEBOND is used). Steps 3 and 4 and Steps 5 and 6 follow the same sequence as Steps 1 and 2 so that the two successive nodes can debond. Since, the crack opening displacement is measured at the mouth of the crack, the value of the DISTANCE parameter on the *FRACTURE CRITERION option is different in Steps 2, 4, and 6. The loading sequence adopted above outlines a way in which the CMOD measurements can be simulated without encountering the situation in which the COD is measured beyond the bound of the specimen, which would lead to an error message. In this example, the loads at which the crack-tip nodes debonded were known a priori. In general, such information may not be available, and the restart capabilities in ABAQUS can be used to determine the load at which the fracture criterion is satisfied. The remaining bonded nodes along the crack propagation surface are allowed to debond based on averaged values of the crack-tip opening angles for different accumulated crack lengths. The data prescribed under the *FRACTURE CRITERION option in Step 7 are the crack opening displacement values that were computed from the crack-tip opening angles observed in the analysis that uses the prescribed crack length versus time criterion. These crack-tip opening angles are converted to critical crack opening displacements at a fixed distance of 0.04 mm behind the crack tip. Hence, the crack opening displacement is measured very close to the current crack tip.

Results and discussion Figure 1.4.4-3 shows a plot of the accumulated incremental crack length versus time. The

1-681

Static Stress/Displacement Analyses

user-specified data, as well as the results obtained from the finite element analysis based on the two criteria, are plotted. Good agreement is observed between the user input values and the results from the analysis. The curve based on the COD criterion does not correspond with the user-specified data toward the end of the analysis because an average crack opening displacement was assumed. Figure 1.4.4-4 shows the reaction force at the node where the displacements are applied as a function of the accumulated incremental crack length, obtained from the analysis in which the crack length was specified as a function of time. The curve obtained when the COD criterion is used is almost identical and is not shown in this figure. Figure 1.4.4-5 depicts the variation of the reaction force as a function of the displacement at the rigid body reference node. The contours of equivalent plastic strain in the near crack-tip region for two different crack advance positions are shown in Figure 1.4.4-6and Figure 1.4.4-7. Contours of the Mises equivalent stress at the final stage of the analysis are shown in Figure 1.4.4-8.

Input files crackgrowth_lengthvtime.inp Analysis with the crack length versus time criterion. crackgrowth_cod.inp Analysis with the COD criterion. crackgrowth_model.inp Model data for the two analysis files.

Reference · G. Kunecke, D. Klingbeil, and J. Schicker, "Rißfortschrittssimulation mit der ABAQUS-option DEBOND am Beispiel einer statisch belasteten Kerbschlagbiegeprobe," presented at the ABAQUS German Fracture Mechanics group meeting in Stuttgart, November 1993.

Table Table 1.4.4-1 Stress-strain data for isotropic plastic behavior. True Stress True Strain (MPa) 461.000 0.0 472.810 0.0187 521.390 0.0280 628.960 0.0590 736.306 0.1245 837.413 0.2970 905.831 0.5756 1208.000 1.9942 1-682

Static Stress/Displacement Analyses

Figures Figure 1.4.4-1 Schematic of the three-point bend specimen.

Figure 1.4.4-2 Finite element mesh for the three-point bend specimen.

Figure 1.4.4-3 Accumulated incremental crack length versus time.

1-683

Static Stress/Displacement Analyses

Figure 1.4.4-4 Variation of the reaction force as a function of the cumulative crack length.

Figure 1.4.4-5 Variation of the reaction force as a function of displacement.

Figure 1.4.4-6 Plastic zone for an accumulated crack length of 1.03 mm.

1-684

Static Stress/Displacement Analyses

Figure 1.4.4-7 Plastic zone for an accumulated crack length of 2.18 mm.

Figure 1.4.4-8 Contours of Mises stress for an accumulated crack length of 2.18 mm.

Sample listings 1-685

Static Stress/Displacement Analyses

Listing 1.4.4-1 *HEADING CRACK GROWTH IN A THREE POINT BEND SPECIMEN: CRACK LENGTH CRITERION. ** ** Input file defining the model data. ** *INCLUDE, INPUT=crackgrowth_model.inp ** ** step 1: Load the specimen ** *STEP,NLGEOM,INC=100 ** *STATIC 0.001, 1.0 ** *** load application ** *BOUNDARY 9997, 1, 1, 1.0 *CONTACT CONTROLS,FRICTION ONSET=DELAY *EL PRINT,FREQUENCY=0 *NODE PRINT,FREQUENCY=0 *CONTACT PRINT ,SLAVE=DBDSL,MASTER=DBDMS DBT, DBSF, DBS *CONTACT FILE,FREQUENCY=10 CSTRESS, CDISP *CONTACT FILE,FREQUENCY=10,SLAVE=DBDSL,MASTER=DBDMS DBT, DBSF, DBS *PRINT, CONTACT=YES *EL PRINT,FREQUENCY=0 *NODE PRINT,FREQUENCY=0 *END STEP ** *** Step 2: Debond the bonded nodes ** ** Use the following lines if the analysis ** is to be run through to completion. ** **STEP,NLGEOM,INC=500 **STATIC **0.005, 1.951, 0.00001, 0.05

1-686

Static Stress/Displacement Analyses

**BOUNDARY **9997, 1, 1, 2.951 ** *STEP,NLGEOM,INC=750 *STATIC 0.005, 0.4, 0.00001, 0.05 *BOUNDARY 9997, 1, 1, 1.4 ** *DEBOND,SLAVE=DBDSL,MASTER=DBDMS, TIME INCREMENT=.001,OUTPUT=BOTH,FREQUENCY=1 0.0 , 1.0 0.005, 0.0 *FRACTURE CRITERION, TYPE=CRACK LENGTH, NSET=REF, TOLERANCE=0.1 1.000001, 0.000000001, 1.256, 0.097, 1.416, 0.181, 1.577, 0.284, 1.737, 0.404, 1.898, 0.541, 2.058, 0.696, 2.114, 0.751, 2.190, 0.830, 2.263, 0.909, 2.332, 0.988, 2.398, 1.067, 2.461, 1.146, 2.521, 1.225, 2.577, 1.304, 2.631, 1.383, 2.681, 1.462, 2.727, 1.541, 2.771, 1.620, 2.811, 1.699, 2.848, 1.778, 2.881, 1.857, 2.912, 1.936, 2.939, 2.015, 2.951, 2.054 *CONTROLS, PARAMETERS=FIELD, FIELD=DISPLACEMENT , 0.1 *CONTACT FILE,FREQUENCY=10

1-687

Static Stress/Displacement Analyses

CSTRESS, CDISP *CONTACT FILE,FREQUENCY=10,SLAVE=DBDSL, MASTER=DBDMS DBT,DBSF, DBS *CONTACT PRINT CSTRESS, CDISP *CONTACT PRINT,SLAVE=DBDSL,MASTER=DBDMS DBT,DBSF,DBS *PRINT, CONTACT=YES *EL PRINT,FREQUENCY=0 *NODE PRINT,FREQUENCY=0 *END STEP

1-688

Static Stress/Displacement Analyses

Listing 1.4.4-2 *HEADING CRACK GROWTH IN A THREE POINT BEND SPECIMEN: COD CRITERION. ** ** Input file defining the model data. ** *INCLUDE, INPUT=crackgrowth_model.inp ** ** step 1: load the specimen ** *STEP,NLGEOM,INC=100 *STATIC 0.001, 1.0 ** *** load application ** *BOUNDARY 9997, 1, 1, 1.0 *EL PRINT,FREQUENCY=0 *NODE PRINT,FREQUENCY=0 *CONTACT PRINT,SLAVE=DBDSL,MASTER=DBDMS DBT, DBSF, DBS *CONTACT FILE,FREQUENCY=10,SLAVE=DBDSL, MASTER=DBDMS DBT, DBSF, DBS *PRINT, CONTACT=YES *END STEP ** *** step 2: Debond the first node. ** *STEP,NLGEOM,INC=1 *STATIC 0.005, 0.005, 0.00001 *BOUNDARY 9997, 1, 1, 1.005 *DEBOND,SLAVE=DBDSL,MASTER=DBDMS, TIME INCREMENT=.005,FREQUENCY=1,OUTPUT=BOTH 0.0 , 1.0 0.005, 0.0 *FRACTURE CRITERION,TYPE=COD,TOLERANCE=0.01, DISTANCE=2.36,SYMMETRY

1-689

Static Stress/Displacement Analyses

2.446, 0.028 *CONTROLS, PARAMETERS=FIELD, FIELD=DISPLACEMENT , 0.1 *CONTACT FILE,SLAVE=DBDSL,MASTER=DBDMS DBT,DBSF,DBS *CONTACT PRINT,SLAVE=DBDSL,MASTER=DBDMS DBT,DBSF,DBS *PRINT, CONTACT=YES *EL PRINT,FREQUENCY=0 *NODE PRINT,FREQUENCY=0 *END STEP ** ** step 3: Load to the point where the second ** node is about to debond. ** *STEP,NLGEOM,INC=20 *STATIC 0.001, 0.0644, 0.00001 *BOUNDARY 9997, 1, 1, 1.0694 *CONTACT FILE,FREQUENCY=10,SLAVE=DBDSL, MASTER=DBDMS DBT,DBSF,DBS *CONTACT PRINT,SLAVE=DBDSL,MASTER=DBDMS DBT,DBSF,DBS *PRINT, CONTACT=YES *EL PRINT,FREQUENCY=0 *NODE PRINT,FREQUENCY=0 *END STEP *** ***** step 4: Debond the second node. *** *STEP,NLGEOM,INC=20 *STATIC 1.0E-06, 1.E-06 *BOUNDARY 9997, 1, 1, 1.069401 *DEBOND,SLAVE=DBDSL,MASTER=DBDMS, TIME INCREMENT=.001,FREQUENCY=2,OUTPUT=BOTH 0.0 , 1.0 0.005, 0.0 *FRACTURE CRITERION,TYPE=COD,TOLERANCE=0.01, DISTANCE=2.389,SYMMETRY

1-690

Static Stress/Displacement Analyses

2.475, 0.06 *CONTACT FILE,SLAVE=DBDSL,MASTER=DBDMS DBT,DBSF,DBS *CONTACT PRINT,SLAVE=DBDSL,MASTER=DBDMS DBT,DBSF,DBS *PRINT, CONTACT=YES *EL PRINT,FREQUENCY=0 *NODE PRINT,FREQUENCY=0 *END STEP ** ** step 5: Load to the point where the third ** node is about to debond ** *STEP,NLGEOM,INC=50 *STATIC 0.001, 0.085, 0.00001 *BOUNDARY 9997, 1, 1, 1.1544 *CONTACT FILE,FREQUENCY=10,SLAVE=DBDSL, MASTER=DBDMS DBT,DBSF,DBS *CONTACT PRINT,SLAVE=DBDSL,MASTER=DBDMS DBT,DBSF,DBS *PRINT, CONTACT=YES *EL PRINT,FREQUENCY=0 *NODE PRINT,FREQUENCY=0 *END STEP *** ***** step 6: Debond the third node *** *STEP,NLGEOM,INC=20 *STATIC 1.0E-06, 1.E-06 *BOUNDARY 9997, 1, 1, 1.154401 *DEBOND,SLAVE=DBDSL,MASTER=DBDMS, TIME INCREMENT=.001,FREQUENCY=2,OUTPUT=BOTH 0.0 , 1.0 0.005, 0.0 *FRACTURE CRITERION,TYPE=COD,TOLERANCE=0.01, DISTANCE=2.426,SYMMETRY 2.518, 0.0934 *CONTACT FILE,SLAVE=DBDSL,MASTER=DBDMS

1-691

Static Stress/Displacement Analyses

DBT,DBSF,DBS *CONTACT PRINT,SLAVE=DBDSL,MASTER=DBDMS DBT,DBSF,DBS *PRINT, CONTACT=YES *EL PRINT,FREQUENCY=0 *NODE PRINT,FREQUENCY=0 *END STEP ** *** step 7: Debond the rest of the nodes. ** ** ** Use the following lines if the analysis is ** to run through to completion **STEP,NLGEOM,INC=500 **STATIC **0.001, 1.752, 0.00001 **BOUNDARY **9997, 1, 1, 2.951 ** *STEP,NLGEOM,INC=75 *STATIC 0.001, 0.40, 0.00001 *BOUNDARY 9997, 1, 1, 1.40 *DEBOND,SLAVE=DBDSL,MASTER=DBDMS, TIME INCREMENT=.001,FREQUENCY=2,OUTPUT=BOTH 0.0 , 1.0 0.005, 0.0 *FRACTURE CRITERION,TYPE=COD,TOLERANCE=0.01, DISTANCE=0.04,SYMMETRY 0.023, 0.262 0.021, 1.037 0.019, 1.66 0.012, 2.18 *CONTACT FILE,FREQUENCY=10,SLAVE=DBDSL, MASTER=DBDMS DBT,DBSF,DBS *CONTACT PRINT,SLAVE=DBDSL,MASTER=DBDMS DBT,DBSF,DBS *PRINT, CONTACT=YES *EL PRINT,FREQUENCY=0 *NODE PRINT,FREQUENCY=0 *END STEP

1-692

Static Stress/Displacement Analyses

1.5 Import analyses 1.5.1 Springback of two-dimensional draw bending Products: ABAQUS/Standard ABAQUS/Explicit This example illustrates the forming and springback analysis of a two-dimensional draw bending process. The forming analysis is performed using ABAQUS/Explicit, and the springback analysis is run with ABAQUS/Standard using the *IMPORT option.

Problem description The example described here is one of the benchmark tests reported at the Numisheet '93 Conference. The benchmark contains a series of six problems performed with three different materials and two different blank holder forces. One of the six problems is described here. The simulations for all the problems are described in the paper by Taylor et al. (1993). The blank initially measures 350 mm by 35 mm and is 0.78 mm thick. The problem is essentially a plane strain problem (the out-of-plane dimension for the blank is 35 mm). A cross-section of the geometry of the die, the punch, the blank holder, and the blank is shown in Figure 1.5.1-1. The total blank holder force is 2.45 kN, and a mass of 5 kg is attached to the blank holder. A coefficient of friction of 0.144 is used for all interacting surfaces. The blank is made of mild steel. The material is modeled as an elastic-plastic material with isotropic elasticity, using the Hill anisotropic yield criterion for the plasticity. The following material properties are used: Young's modulus = 206.0 GPa Poisson's ratio = 0.3 Density = 7800. Yield stress ¾0 = 167.0 MPa Anisotropic yield criterion: R11 =1.0, R22 =1.0402, R33 =1.24897, R12 =1.07895, R13 =1.0, R23 =1.0 The problem is symmetric about a plane through the center of the punch, and only half of the problem is modeled. The blank is modeled with a single row of 175 first-order shell elements. Symmetry boundary conditions are applied on the plane of symmetry, and boundary conditions are applied on all the nodes of the blank to simulate the plane strain conditions. The forming process is simulated in two steps with ABAQUS/Explicit. The blank holder force is applied in the first step of the analysis. The force is ramped on to minimize inertia effects. In the second step of the analysis the punch is moved down 70 mm by prescribing the velocity of the rigid body reference node for the punch. The velocity is applied with a triangular amplitude function, starting and ending with zero velocity, and with a peak velocity occurring at the middle of the time period. A significant amount of springback occurs in this case. Because the blank is very flexible and the fundamental mode of vibration is low, it would take a long simulation to obtain a quasi-static solution of the springback analysis in ABAQUS/Explicit.

1-693

Static Stress/Displacement Analyses

The springback analysis is performed with ABAQUS/Standard using the *IMPORT option. The results from the forming simulation in ABAQUS/Explicit are imported into ABAQUS/Standard, and a static analysis calculates the springback. During this step an artificial stress state that equilibrates the imported stress state is applied automatically by ABAQUS/Standard and gradually removed during the step. The displacement obtained at the end of the step is the springback, and the stresses give the residual stress state. The UPDATE parameter on the *IMPORT option determines the reference configuration. When the UPDATE parameter is set equal to YES on the *IMPORT option, the deformed sheet with its material state at the end of the ABAQUS/Explicit analysis is imported into ABAQUS/Standard and the deformed configuration becomes the reference configuration. This procedure is most convenient if, during postprocessing, the displacements due to springback need to be displayed. When the UPDATE parameter is set equal to NO on the *IMPORT option, the material state, displacements, and strains of the deformed sheet at the end of the ABAQUS/Explicit analysis are imported into ABAQUS/Standard, and the original configuration remains as the reference configuration. This procedure should be used if it is desirable to obtain a continuous displacement solution. In this two-dimensional draw bending problem significant springback occurs, and large-displacement effects are included in the calculations by including the NLGEOM parameter on the *STEP option. Further details of the import capability are discussed in ``Transferring results between ABAQUS/Explicit and ABAQUS/Standard,'' Section 7.6.1 of the ABAQUS/Standard User's Manual and Section 7.3.1 of the ABAQUS/Explicit User's Manual.

Results and discussion The optimum peak velocity for the punch (the value that gives quasi-static results at least cost) is determined by running the explicit analysis with peak velocities of 30 m/s, 15 m/s, and 5 m/s. The energy histories are shown in Figure 1.5.1-2, Figure 1.5.1-3, and Figure 1.5.1-4, respectively. From these results it is evident that the amount of kinetic energy in the model is too large at a peak velocity of 30 m/s for the analysis to simulate the quasi-static forming process, while at a peak velocity of 5 m/s the kinetic energy is virtually zero. A peak velocity for the punch of 15 m/s is chosen for the forming analysis, as the kinetic energy for this case is considered low enough not to affect the results significantly. For accurate springback analysis it is important that stresses are not influenced by inertia effects. The blank at the end of the ABAQUS/Explicit forming analysis is shown in Figure 1.5.1-5. The shape after springback is shown in Figure 1.5.1-6. The results compare well with the reported experimental data. In the numerical results the angle between the outside flange and the horizontal axis is 20.4°. The average angle measured in the experiments is 17.1°, with a range from 9° to 23° in the experimental results. The results of the springback analysis when the reference configuration is updated are nearly identical to that when the reference configuration is not updated.

Input files springback_exp_form.inp

1-694

Static Stress/Displacement Analyses

Forming analysis in ABAQUS/Explicit with a punch velocity of 15 m/s. springback_std_importyes.inp Springback analysis in ABAQUS/Standard with the *IMPORT, UPDATE=YES option. springback_std_importno.inp Springback analysis in ABAQUS/Standard with the *IMPORT, UPDATE=NO option. springback_std_both.inp Input data used with ABAQUS/Standard for both the forming and the springback analyses. springback_exp_punchv30.inp Forming analysis in ABAQUS/Explicit with a punch velocity of 30 m/s. springback_exp_punchv5.inp Forming analysis in ABAQUS/Explicit with a punch velocity of 5 m/s.

Reference · Taylor, L. M., J. Cao, A. P. Karafillis, and M. C. Boyce, "Numerical Simulations of Sheet Metal Forming," Proceedings of 2nd International Conference, NUMISHEET 93, Isehara, Japan, Ed. A. Makinovchi, et al.

Figures Figure 1.5.1-1 Cross-section showing the geometry of the die, the punch, the blank holder, and the blank.

1-695

Static Stress/Displacement Analyses

Figure 1.5.1-2 Energy history for forming analysis: 30 m/s peak velocity of punch.

Figure 1.5.1-3 Energy history for forming analysis: 15 m/s peak velocity of punch.

Figure 1.5.1-4 Energy history for forming analysis: 5 m/s peak velocity of punch.

1-696

Static Stress/Displacement Analyses

Figure 1.5.1-5 Blank at the end of the forming analysis in ABAQUS/Explicit.

Figure 1.5.1-6 Blank after springback in ABAQUS/Standard.

Sample listings

1-697

Static Stress/Displacement Analyses

Listing 1.5.1-1 *HEADING 2D Draw Bending problem for Numisheet'93 Mild steel, 2.45kN blankholder force Shell elements ; Explicit analysis ** **------------------------ blank *NODE 1, 351, 0.175 *NGEN, NSET=BLANK1 1,351,1 *NCOPY, OLD=BLANK1,NEW=BLANK2,CHANGE=1000,SHIFT 0., 0.005 *NSET, NSET=BLANK BLANK1,BLANK2 *ELEMENT, TYPE=S4R 1,1,3,1003,1001 *ELGEN, ELSET=BLANK 1,175,2,2 *SHELL SECTION, ELSET=BLANK, MATERIAL=STEEL 0.00078,5 *MATERIAL,NAME=STEEL *DENSITY 7800., *ELASTIC 206.E9,0.3 *PLASTIC .15403E+09,.00000E+00 .19410E+09,.10000E-01 .21913E+09,.20000E-01 .23803E+09,.30000E-01 .25348E+09,.40000E-01 .26668E+09,.50000E-01 .27826E+09,.60000E-01 .28864E+09,.70000E-01 .29807E+09,.80000E-01 .30674E+09,.90000E-01 .31477E+09,.10000E+00 .32226E+09,.11000E+00 .32930E+09,.12000E+00

1-698

Static Stress/Displacement Analyses

.33594E+09,.13000E+00 .34224E+09,.14000E+00 .34822E+09,.15000E+00 .35393E+09,.16000E+00 .35940E+09,.17000E+00 .36464E+09,.18000E+00 .36968E+09,.19000E+00 .37454E+09,.20000E+00 .37922E+09,.21000E+00 .38375E+09,.22000E+00 .38814E+09,.23000E+00 .39239E+09,.24000E+00 .39652E+09,.25000E+00 .40053E+09,.26000E+00 .40443E+09,.27000E+00 .40822E+09,.28000E+00 .41193E+09,.29000E+00 .41554E+09,.30000E+00 .41906E+09,.31000E+00 .42251E+09,.32000E+00 .42588E+09,.33000E+00 .42917E+09,.34000E+00 .43240E+09,.35000E+00 .43556E+09,.36000E+00 .43866E+09,.37000E+00 .44169E+09,.38000E+00 .44468E+09,.39000E+00 .44760E+09,.40000E+00 .45047E+09,.41000E+00 .45330E+09,.42000E+00 .45607E+09,.43000E+00 .45880E+09,.44000E+00 .46148E+09,.45000E+00 .46413E+09,.46000E+00 .46672E+09,.47000E+00 .46928E+09,.48000E+00 .47181E+09,.49000E+00 .47429E+09,.50000E+00 *POTENTIAL 1., 1.0402,1.24897,1.07895,1.,1. ** **---------------------------- die *NODE

1-699

Static Stress/Displacement Analyses

2000, 0.026, -0.001, -0.080 *NODE, NSET=DIE 2001, 0.026, -0.001, -0.080 2002, 0.026, -0.001, -0.00539 2008, 0.031, -0.001, -0.00039 2009, 0.180, -0.001, -0.00039 *NGEN, NSET=DIE, LINE=C 2002, 2008, 1,, 0.031, -0.001, -0.00539 *NCOPY, CHANGE=100, OLD=DIE, NEW=DIE, SHIFT 0., 0.007 *ELEMENT, TYPE=R3D4 2001, 2001, 2002, 2102, 2101 *ELGEN, ELSET=DIE 2001, 8, 1, 1 *RIGID BODY, ELSET=DIE, REF NODE=2000 ** **---------------------------- punch *NODE 3000, 0.000, -0.001, 0.001 *NODE, NSET=PUNCH 3001, 0.000, -0.001, 0.001 3002, 0.020, -0.001, 0.001 3008, 0.025, -0.001, 0.006 3009, 0.025, -0.001, 0.081 *NGEN, NSET=PUNCH, LINE=C 3002, 3008, 1, , 0.02, -0.001, 0.006 *NCOPY, CHANGE=100, OLD=PUNCH, NEW=PUNCH, SHIFT 0., 0.007 *ELEMENT, TYPE=R3D4 3001, 3001, 3002, 3102, 3101 *ELGEN, ELSET= PUNCH 3001, 8,1 *RIGID BODY, ELSET=PUNCH, REF NODE=3000 ** **---------------------------- holder *NODE, NSET=HOLDER 4001, 0.031, -0.001, 0.010 4002, 0.031, -0.001, 0.00039 4003, 0.081, -0.001, 0.00039 4004, 0.086, -0.001, 0.00539 *NODE

1-700

Static Stress/Displacement Analyses

4005, 0.0585, 0.0025, 0.010 *NCOPY, OLD=HOLDER, NEW=HOLDER, CHANGE=100, SHIFT 0, 0.007 *ELEMENT, TYPE=R3D4 4001, 4001, 4002, 4102, 4101 *ELGEN, ELSET=HOLDER 4001, 3, 1, *RIGID BODY, ELSET=HOLDER, REF NODE=4005 *ELEMENT, TYPE=MASS, ELSET=EM1 4100, 4005 *MASS, ELSET=EM1 2.5, ** **----------------------------- surfaces *SURFACE, NAME=PUNCH PUNCH,S2 *SURFACE, NAME=HOLDER HOLDER,S2 *SURFACE, NAME=DIE DIE,S1 *SURFACE, NAME=TOP BLANK,S1 *SURFACE, NAME=BOTTOM BLANK,S2 ** **----------------------- boundary conditions *BOUNDARY BLANK, 2,2 BLANK, 4,4 BLANK, 6,6 1, 1,1 1001, 1,1 2000, 1,6 3000, 1,3 3000, 4,6 4005, 1,2 4005, 4,6 ** *RESTART, WRITE, NUMBER INT=1 ** *AMPLITUDE,NAME=APUNCH 0.,0., 0.00466666667, 1., 0.00933333333, 0.

1-701

Static Stress/Displacement Analyses

*AMPLITUDE,NAME=RAMP 0.0, 0.0, 0.00001, 1.0 *ELSET,ELSET=CHECK 57,151 *NSET,NSET=CHECKN 1,20,57 ** **---------- apply blankholder force *STEP *DYNAMIC, EXPLICIT ,0.00001 *CLOAD,AMP=RAMP 4005, 3, -175.0 ** *SURFACE INTERACTION, NAME=ALLCONT *FRICTION 0.144, *CONTACT PAIR, INTERACTION=ALLCONT PUNCH,TOP *CONTACT PAIR, INTERACTION=ALLCONT HOLDER,TOP *CONTACT PAIR, INTERACTION=ALLCONT DIE,BOTTOM ** *FILE OUTPUT,NUM=1 *NODE FILE U,V *EL FILE S, PEEQ, MISES STH, *END STEP ** ** ------------------- move punch down *STEP *DYNAMIC,EXPLICIT , 0.00933333333 *BOUNDARY,AMP=APUNCH,TYPE=VELOCITY 3000,3,3,-15.0 ** *RESTART,WRITE, NUMBER INT=1 *HISTORY OUTPUT,TIME=0.0 *EL HISTORY, ELSET=CHECK, SECTION=1 S,

1-702

Static Stress/Displacement Analyses

*NODE HISTORY, NSET=CHECKN U3, V3, A3 *ENERGY HISTORY ALLKE,ALLSE,ALLPD,ALLIE,ALLWK,ETOTAL,ALLFD *END STEP

1-703

Static Stress/Displacement Analyses

Listing 1.5.1-2 *HEADING 2D Draw bending problem for Numisheet'93 Mild steel, 2.45kN blankholder force *IMPORT,STEP=2,INT=1,STATE=YES, UPDATE=YES BLANK, *IMPORT NSET BLANK, *BOUNDARY BLANK,2,2 BLANK, 4,4 BLANK, 6,6 1,1,6 1001,1,6 *RESTART,WRITE,FREQ=1 ** *STEP,NLGEOM,INC=50 *STATIC 0.1,1. *NODE FILE,FREQ=1 U, *PRINT,FREQ=1 *NODE PRINT,FREQ=50 U, RF, *EL PRINT,FREQ=0 *END STEP

1.5.2 Deep drawing of a square box Products: ABAQUS/Standard ABAQUS/Explicit This example illustrates the forming of a three-dimensional shape by a deep drawing process. The most efficient way to analyze this type of problem is to analyze the forming step with ABAQUS/Explicit and to import the results in ABAQUS/Standard to analyze the springback that occurs after the blank is removed from the tool with a static procedure. Since the forming process is essentially a quasi-static problem, the computations with ABAQUS/Explicit are performed over a sufficiently long time period to render inertial effects negligible. For verification purposes the complete analysis is also carried out with ABAQUS/Standard. However, this is computationally more expensive and will be prohibitively expensive for simulation of the forming of realistic, complex components.

Problem description

1-704

Static Stress/Displacement Analyses

The blank is initially square, 200 mm by 200 mm, and is 0.82 mm thick. The rigid die is a flat surface with a square hole 102.5 mm by 102.5 mm, rounded at the edges with a radius of 10 mm. The rigid square punch measures 100 mm by 100 mm and is rounded at the edges with the same 10 mm radius. The blank holder can be considered a flat plate, since the blank never comes close to its edges. The geometry of these parts is illustrated in Figure 1.5.2-1and Figure 1.5.2-2. The rigid surfaces are offset from the blank by half of the thickness of the blank. The contact algorithm in ABAQUS/Explicit takes into account the shell thickness. When the forming step is modeled with ABAQUS/Standard, the thickness is accounted for indirectly by shifting the pressure penetration curve defined with the *SURFACE BEHAVIOR option. A mass of 0.6396 kg is attached to the blank holder, and a concentrated load of 2.287 ´ 104 N is applied to the control node of the blank holder. The blank holder is then allowed to move only in the vertical direction to accommodate changes in blank thickness during deformation. The coefficient of friction between the sheet and the punch is taken to be 0.25, and that between the sheet and the die is 0.125. It is assumed that there is no friction between the blank and the blank holder. The blank is made of aluminum-killed steel, which is assumed to satisfy the Ramberg-Osgood relation between true stress and logarithmic strain: ² = (¾=K )1=n ; with a reference stress value (K) of 513 MPa and a work-hardening exponent (n) of 0.223. Isotropic elasticity is assumed, with a Young's modulus of 211 GPa and a Poisson's ratio of 0.3. An initial yield stress of 91.3 MPa is obtained from these data. The stress-strain behavior is defined by piecewise linear segments matching the Ramberg-Osgood curve up to a total (logarithmic) strain level of 107%, with Mises yield, isotropic hardening, and no rate dependence. Given the symmetry of the problem, it is sufficient to model only a one-eighth sector of the box. However, we have employed a full one-quarter model to make it easier to visualize. We use 4-node, three-dimensional rigid surface elements (type R3D4) to model the die, the punch, and the blank holder. The blank is modeled with 4-node, bilinear finite-strain shell elements (type S4R). This problem was used by Nagtegaal and Taylor (1991) to compare implicit and explicit finite element techniques for the analysis of sheet metal forming problems. The computer time involved in running the simulation using explicit time integration with a given mesh is directly proportional to the time period of the event, since the stable time increment size is a function of the mesh size (length) and the material stiffness. Thus, it is usually desirable to run the simulation at an artificially high speed compared to the physical process. If the speed in the simulation is increased too much, the solution does not correspond to the low-speed physical problem; i.e., inertial effects begin to dominate. In a typical forming process the punch may move at speeds on the order of 1 m/sec, which is extremely slow compared to typical wave speeds in the materials to be formed. (The wave speed in steel is approximately 5000 m/sec.) In general, inertia forces will not play a dominant role for forming rates that are considerably higher than the nominal 1 m/sec rates found in the physical problem. The explicit solutions obtained with punch speeds of 10, 30, and 100 m/sec are compared with the static solution obtained with ABAQUS/Standard. The results at 10 m/sec were virtually indistinguishable from the static results. Minor differences could be observed at the intermediate speed of 30 m/sec. The results at

1-705

Static Stress/Displacement Analyses

100 m/sec were considerably different from the static results. In the results presented here, the drawing process is simulated by moving the reference node for the punch downward through a total distance of 36 mm at a constant velocity of 30 m/sec. Comparison of analyses of various metal forming problems using explicit dynamic and static procedures is discussed in the paper by Nagtegaal and Taylor. Although this example does not contain rate-dependent material properties, it is common in sheet metal forming applications for this to be a consideration. If the material is rate-dependent, the velocities cannot be artificially increased without affecting the material response. Instead, the analyst can use the technique of mass scaling to adjust the effective punch velocity without altering the material properties. ``Rolling of thick plates,'' Section 1.3.7, contains an explanation and an example of the mass scaling technique. The results from the forming simulation obtained using ABAQUS/Explicit are made available to ABAQUS/Standard by using the *IMPORT option with the parameter UPDATE=YES. The springback that occurs and the residual stress state are then determined by performing a static analysis in ABAQUS/Standard. During this step an artificial stress state that equilibrates the imported stress state is applied automatically by ABAQUS/Standard and gradually removed during the step. The displacement obtained at the end of the step is the springback, and the stresses give the residual stress state. Only the deformed sheet with its material state at the end of the ABAQUS/Explicit analysis is imported into ABAQUS/Standard. Boundary conditions are imposed in the ABAQUS/Standard analysis to prevent rigid body motion and for symmetry. The node at the center of the box is fixed in the z-direction. The springback of the formed sheet is also analyzed in ABAQUS/Standard by setting UPDATE=NO on the *IMPORT option. In this case the displacements are the total values relative to the original reference configuration. This makes it easy to compare the results with the analysis in which both the forming and springback are analyzed with ABAQUS/Standard. Further details of the import capability are discussed in ``Transferring results between ABAQUS/Explicit and ABAQUS/Standard,'' Section 7.6.1 of the ABAQUS/Standard User's Manual and Section 7.3.1 of the ABAQUS/Explicit User's Manual.

Contact modeling in the forming step In ABAQUS/Explicit the contact constraints, which take the current shell thickness into account, are enforced with the default, kinematic contact method in the primary input file, although a model that uses penalty contact is also included. (Penalty contact is invoked if MECHANICAL CONSTRAINT=PENALTY is included on the *CONTACT PAIR option.) The results with these two methods are very similar. It would also be valid to use a combination of both methods in one analysis; for example, penalty contact between the blank holder and the blank and kinematic contact for the other contact pairs. If the penalty method is used to model contact between the punch and the blank, the blank will tend to bounce off the punch after an impact at the beginning of the analysis (the blank is initially at rest). This phenomenon does not occur with kinematic contact because impacts are perfectly plastic for kinematic contact. The significance of this phenomenon has been greatly reduced in the analysis that uses penalty contact by ramping up the velocity of the punch smoothly over the initial 1% of the step duration.

1-706

Static Stress/Displacement Analyses

Because contact occurs on both sides of the blank, a double-sided surface is used to model the blank in ABAQUS/Explicit. In ABAQUS/Explicit when a shell is pinched between two contact surfaces, such as between the blank holder and die in this problem, at least one of the constraints will not be enforced exactly, even if kinematic enforcement is used for both contact pairs. This aspect is discussed in ``Common difficulties associated with contact modeling,'' Section 20.5.1 of the ABAQUS/Explicit User's Manual. The slight noncompliance does not affect the predicted properties of the formed part significantly. Double-sided surfaces are not available in ABAQUS/Standard, so two single-sided surfaces are used to model the blank when the forming step is modeled in ABAQUS/Standard: one surface to model the top of the blank and one to model the bottom of the blank. When a shell in ABAQUS/Standard is pinched between two surfaces, at least one of the constraints must use "softened" contact. In the analysis in which the forming and the springback steps are carried out with ABAQUS/Standard, softened contact is used for all contact constraints. The contact stiffness is chosen sufficiently high so that the results are not affected significantly.

Results and discussion Figure 1.5.2-3 shows contours of shell thickness in the blank after forming. Figure 1.5.2-4 shows contours of equivalent plastic strain in the blank in the final deformed shape. Closer inspection of the results reveals that the corners of the box are formed by stretching, whereas the sides are formed by drawing action. This effect leads to the formation of shear bands that run diagonally across the sides of the box, resulting in a nonhomogeneous wall thickness. Note also the uneven draw of the material from the originally straight sides of the blank. Applying a more localized restraint near the midedges of the box (for example, by applying drawbeads) and relaxing the restraint near the corners of the box is expected to increase the quality of the formed product. Figure 1.5.2-5 shows the reaction force on the punch. Figure 1.5.2-6 shows the vertical displacement of the blank holder over time. The rise of the blank holder is attributable to the increased thickness of the blank, as well as to the tendency of the blank to lift up off of the die. Figure 1.5.2-7 shows the thinning of an element at the corner of the box. The springback analysis runs in 6 increments in ABAQUS/Standard. Most of the springback occurs in the z-direction, and the springback is not significant. The corner of the outside edge of the formed box drops approximately 0.45 mm, while the vertical side of the box rises by approximately 0.2 mm. Figure 1.5.2-8 shows a contour plot of the displacements in the z-direction obtained from the springback analysis. The analysis with UPDATE=NO on the *IMPORT option yields similar results. However, in this case the displacements are interpreted as total values relative to the original configuration.

Input files deepdrawbox_exp_form.inp Forming analysis with ABAQUS/Explicit. deepdrawbox_std_importyes.inp

1-707

Static Stress/Displacement Analyses

ABAQUS/Standard springback analysis with the UPDATE=YES parameter on the *IMPORT option. deepdrawbox_std_importno.inp ABAQUS/Standard springback analysis with the UPDATE=NO parameter on the *IMPORT option. deepdrawbox_std_both.inp Forming and springback analyses done in ABAQUS/Standard. deepdrawbox_exp_form_penalty.inp Original mesh using penalty contact in ABAQUS/Explicit. deepdrawbox_exp_finemesh.inp Forming analysis of a fine mesh case (included for the sole purpose of testing the performance of the ABAQUS/Explicit code). deepdrawbox_std_finesprngback.inp Springback analysis of a fine mesh case (included for the sole purpose of testing the performance of the ABAQUS/Explicit code).

Reference · Nagtegaal, J. C., and L. M. Taylor, "Comparison of Implicit and Explicit Finite Element Methods for Analysis of Sheet Forming Problems," VDI Berichte No. 894, 1991.

Figures Figure 1.5.2-1 Meshes for the die, punch, and blank holder.

1-708

Static Stress/Displacement Analyses

Figure 1.5.2-2 Undeformed mesh for the blank.

Figure 1.5.2-3 Contours of shell thickness.

Figure 1.5.2-4 Contours of equivalent plastic strain.

1-709

Static Stress/Displacement Analyses

Figure 1.5.2-5 Reaction force on the punch versus punch displacement.

Figure 1.5.2-6 Vertical holder displacement versus time.

Figure 1.5.2-7 Shell thickness of the thinnest part of the blank versus time.

1-710

Static Stress/Displacement Analyses

Figure 1.5.2-8 Contour plot showing the springback in the z-direction.

Sample listings

1-711

Static Stress/Displacement Analyses

Listing 1.5.2-1 *HEADING DEEP DRAWING OF A SQUARE BOX (1/4 SYMMETRY MODEL) ** ** Generate the mesh for the PUNCH ** *NODE 101,.0 ,.0,0.00041 107,.04,.0,0.00041 113,.05,.0 ,.01 119,.05,.0 ,.07 199,.04,.0 ,.01 701,.0 ,.04,0.00041 707,.04,.04,0.00041 713,.05,.04,.01 719,.05,.04,.07 799,.04,.04,.01 1307,.04,.04,.00041 1313,.04,.05,.01 1319,.04,.05,.07 1399,.04,.04,.01 1907,.0 ,.04,.00041 1913,.0 ,.05,.01 1919,.0 ,.05,.07 1999,.0 ,.04,.01 199991,0.,0.,0.00041 *NGEN,NSET=P1 101,107,1 113,119,1 *NGEN,NSET=P1,LINE=C 107,113,1,199 *NGEN,NSET=P2 701,707,1 713,719,1 *NGEN,NSET=P2,LINE=C 707,713,1,799 *NSET,NSET=P2C,GEN 707,719,1 *NGEN,NSET=P3 1313,1319,1 *NGEN,NSET=P3,LINE=C

1-712

Static Stress/Displacement Analyses

1307,1313,1,1399 *NGEN,NSET=P4 1913,1919,1 *NGEN,NSET=P4,LINE=C 1907,1913,1,1999 *NFILL P1,P2,6,100 P3,P4,6,100 *NCOPY,CHANGE NUMBER=100,OLD SET=P2C,SHIFT, MULTIPLE=6 0.,0.,0. .04,.04,0., .04,.04,1.,15. *NSET,NSET=P4,GEN 101,701,100 *ELEMENT,TYPE=R3D4,ELSET=PUNCH 1, 101,102,202,201 109, 708,709,809,808 241, 707, 708, 808,707 242, 707, 808, 908,707 243, 707, 908,1008,707 244, 707,1008,1108,707 245, 707,1108,1208,707 246, 707,1208,1308,707 247, 707,1308,1408,706 248, 706,1408,1508,705 249, 705,1508,1608,704 250, 704,1608,1708,703 251, 703,1708,1808,702 252, 702,1808,1908,701 *ELGEN,ELSET=PUNCH 1, 18,1,1, 6,100,18 109, 11,1,1, 12,100,11 *RIGID BODY,ELSET=PUNCH,REF NODE=199991 ** ** Generate the mesh for the HOLDER ** *NODE 20101,.06,.0,.01 20102,.06,.0,.00041 20108,.13,.0,.00041 20109,.13,.0,.01 20701,.06,.05,.01 20702,.06,.05,.00041

1-713

Static Stress/Displacement Analyses

20708,.13,.05,.00041 20709,.13,.05,.01 21301,.05,.06,.01 21302,.05,.06,.00041 21308,.05,.13,.00041 21309,.05,.13,.01 21901,.0,.06,.01 21902,.0,.06,.00041 21908,.0,.13,.00041 21909,.0,.13,.01 299991,0.06,0.,0.01 *NGEN,NSET=H1 20101,20102,1 20102,20108,1 20108,20109,1 *NGEN,NSET=H2 20701,20702,1 20702,20708,1 20708,20709,1 *NGEN,NSET=H3 21301,21302,1 21302,21308,1 21308,21309,1 *NGEN,NSET=H4 21901,21902,1 21902,21908,1 21908,21909,1 *NFILL H1,H2,6,100 H3,H4,6,100 *NCOPY,CHANGE NUMBER=100,OLD SET=H2,SHIFT, MULTIPLE=6 0.,0.,0. .05,.05,0., .05,.05,1.,15. *ELEMENT,TYPE=R3D4,ELSET=HOLDER 20001, 20101,20201,20202,20102 *ELGEN,ELSET=HOLDER 20001, 8,1,1, 18,100,8 *RIGID BODY,ELSET=HOLDER,REF NODE=299991 *ELEMENT,TYPE=MASS,ELSET=EMASS 20000,299991 *MASS,ELSET=EMASS 6.396E-1,

1-714

Static Stress/Displacement Analyses

** ** Generate the mesh for the DIE ** *NODE 599991, .05125, 0., -0.06 *NODE,NSET=DIE 50101, .05125,0.,-.06 50107, .05125,0.,-.01 50113, .06125,0.,-0.00041 50119, .13000,0.,-0.00041 50199, .06125,0.,-.01 ** 50701, .05125,.04125,-.06 50707, .05125,.04125,-.01 50713, .06125,.04125,-0.00041 50719, .13000,.04125,-0.00041 50799, .06125,.04125,-.01 ** 51301, .04125,.05125,-.06 51307, .04125,.05125,-.01 51313, .04125,.06125,-0.00041 51319, .04125,.13000,-0.00041 51399, .04125,.06125,-.01 ** 51901, 0.,.05125,-.06 51907, 0.,.05125,-.01 51913, 0.,.06125,-0.00041 51919, 0.,.13000,-0.00041 51999, 0.,.06125,-.01 *NGEN,NSET=D1 50101,50107,1 50113,50119,1 *NGEN,NSET=D1,LINE=C 50107,50113,1,50199 *NGEN,NSET=D2 50701,50707,1 50713,50719,1 *NGEN,NSET=D2,LINE=C 50707,50713,1,50799 *NGEN,NSET=D3 51301,51307,1 51313,51319,1 *NGEN,NSET=D3,LINE=C

1-715

Static Stress/Displacement Analyses

51307,51313,1,51399 *NGEN,NSET=D4 51901,51907,1 51913,51919,1 *NGEN,NSET=D4,LINE=C 51907,51913,1,51999 *NFILL D1,D2,6,100 D3,D4,6,100 *NCOPY,CHANGE NUMBER=100,OLD SET=D2,SHIFT, MULTIPLE=6 0.,0.,0. .04125,.04125,0., .04125,.04125,1., 15. *ELEMENT,TYPE=R3D4 50001, 50101,50102,50202,50201 *ELGEN,ELSET=DIE 50001, 18,1,1, 18, 100,18 *RIGID BODY,ELSET=DIE,REF NODE=599991 ** ** Generate the mesh for the BLANK ** *NODE 90001,.0,.0,0. 90036,.1,.0,0. 91261,.0,.1,0. 91296,.1,.1,0. *NGEN,NSET=B1 90001,90036,1 *NGEN,NSET=B2 91261,91296,1 *NFILL B1,B2,35,36 *NSET,NSET=B4,GEN 90001,91261,36 *ELEMENT,TYPE=S4R,ELSET=BLANK 3001, 90001,90002,90038,90037 *ELGEN,ELSET=BLANK 3001, 35,1,1, 35,36,35 *SHELL SECTION,MATERIAL=STEEL,ELSET=BLANK, SECTION INTEGRATION=GAUSS .00082,5 ** ** Define material properties for STEEL

1-716

Static Stress/Displacement Analyses

** *MATERIAL,NAME=STEEL *DENSITY 7800., *ELASTIC 2.1E11,0.3 *PLASTIC 0.91294E+08, 0.00000E+00 0.10129E+09, 0.21052E-03 0.11129E+09, 0.52686E-03 0.12129E+09, 0.97685E-03 0.13129E+09, 0.15923E-02 0.14129E+09, 0.24090E-02 0.15129E+09, 0.34674E-02 0.16129E+09, 0.48120E-02 0.17129E+09, 0.64921E-02 0.18129E+09, 0.85618E-02 0.19129E+09, 0.11080E-01 0.20129E+09, 0.14110E-01 0.21129E+09, 0.17723E-01 0.22129E+09, 0.21991E-01 0.23129E+09, 0.26994E-01 0.24129E+09, 0.32819E-01 0.25129E+09, 0.39556E-01 0.26129E+09, 0.47301E-01 0.27129E+09, 0.56159E-01 0.28129E+09, 0.66236E-01 0.29129E+09, 0.77648E-01 0.30129E+09, 0.90516E-01 0.31129E+09, 0.10497E+00 0.32129E+09, 0.12114E+00 0.33129E+09, 0.13916E+00 0.34129E+09, 0.15919E+00 0.35129E+09, 0.18138E+00 0.36129E+09, 0.20588E+00 0.37129E+09, 0.23287E+00 0.38129E+09, 0.26252E+00 0.39129E+09, 0.29502E+00 0.40129E+09, 0.33054E+00 0.41129E+09, 0.36929E+00 0.42129E+09, 0.41147E+00 0.43129E+09, 0.45729E+00 0.44129E+09, 0.50696E+00

1-717

Static Stress/Displacement Analyses

0.45129E+09, 0.46129E+09, 0.47129E+09, 0.48129E+09, 0.49129E+09, 0.50129E+09, 0.51129E+09, 0.52129E+09,

0.56073E+00 0.61881E+00 0.68145E+00 0.74890E+00 0.82142E+00 0.89928E+00 0.98274E+00 0.10721E+01

** ** Define surfaces ** *SURFACE, NAME=PUNCH PUNCH,SNEG *SURFACE, NAME=HOLDER HOLDER,SPOS *SURFACE, NAME=DIE DIE,SPOS *SURFACE, NAME=BLANK BLANK, ** ** Apply symmetry boundary conditions ** *BOUNDARY D1,2,2 P1,2,2 H1,2,2 D2,1,1 P2,1,1 H2,1,1 B1,YSYMM B4,XSYMM 199991, 1,2 199991, 4,6 299991,1,2 299991,4,6 599991,1,3 599991,4,6 ** ** Simulate the deep drawing operation ** *RESTART,WRITE,NUMBER INTERVAL=2, TIMEMARKS=NO ** *STEP

1-718

Static Stress/Displacement Analyses

*DYNAMIC,EXPLICIT ,.0012 *BOUNDARY,TYPE=VELOCITY 199991,3,3,-30. *CLOAD 299991, 3, -2.287E4 ** *SURFACE INTERACTION,NAME=PUNCH_TOP *FRICTION 0.25, *CONTACT PAIR,INTERACTION=PUNCH_TOP PUNCH,BLANK *CONTACT PAIR HOLDER,BLANK *SURFACE INTERACTION,NAME=DIE_BOTT *FRICTION 0.125, *CONTACT PAIR,INTERACTION=DIE_BOTT DIE,BLANK ** *FILE OUTPUT,TIMEMARKS=YES,NUM=1 *EL FILE PEEQ,MISES *NODE FILE U,V *ENERGY FILE ** ** history output ** *NSET,NSET=NPUNCH 199991, *NSET,NSET=HOLDER 299991, *ELSET,ELSET=ELHIST 3647, *HISTORY OUTPUT,TIME INTERVAL=.6E-4 *NODE HISTORY,NSET=NPUNCH U3,RF3 *NODE HISTORY,NSET=HOLDER U3,V3,A3, *EL HISTORY,ELSET=ELHIST STH, PEEQ,

1-719

Static Stress/Displacement Analyses

*ENERGY HISTORY ALLKE,ALLSE,ALLWK,ALLPD,ALLIE,ALLVD,ETOTAL, ALLFD,ALLCD,DT,ALLAE *OUTPUT,FIELD,OP=NEW,NUMBER INTERVAL=5, TIMEMARKS=NO *ELEMENT OUTPUT S, PEEQ *NODE OUTPUT U, *OUTPUT,HISTORY,OP=NEW,TIME INTERVAL=2.4E-6 *ENERGY OUTPUT ALLAE,ALLIE,ALLKE,ALLPD,ALLSE,ALLVD,ALLWK,ETOTAL *END STEP

1-720

Static Stress/Displacement Analyses

Listing 1.5.2-2 *HEADING SHEET METAL FORMING: import model spring back analysis *IMPORT,STEP=1,INT=2,STATE=YES, UPDATE=YES BLANK, *IMPORT NSET B1,B4 *BOUNDARY B1,YSYMM B4,XSYMM 90001,1,6 ** *RESTART,WRITE,FREQUENCY=100 ** *STEP,NLGEOM,INC=50 *STATIC 0.1,1. *NODE FILE,FREQ=1 U, *PRINT,FREQ=50 *NODE PRINT,FREQ=50 U, RF, *EL PRINT,FREQ=0 *END STEP

1-721

Dynamic Stress/Displacement Analyses

2. Dynamic Stress/Displacement Analyses 2.1 Dynamic stress analyses 2.1.1 Nonlinear dynamic analysis of a structure with local inelastic collapse Product: ABAQUS/Standard This example illustrates an inexpensive approach to the prediction of the overall response of a structure that exhibits complex local behavior. The case studied is an unrestrained pipe whip example, where an initially straight pipe undergoes so much motion that the pipe section collapses. A two-stage technique is used to predict the response. First, the collapse of the section is studied under static conditions using a generalized plane strain model. This analysis defines the moment-curvature relationship for the section under conditions of pure bending. It also shows how the section deforms as it collapses. This information can be used to judge whether the deformation is reasonable with respect to possible failure (fracture) of the section. In addition, this first stage analysis can be used to calculate the change in the cross-sectional area enclosed by the pipe as a function of the curvature of the pipe. In a pipe whip case the driving force is caused by fluid jetting from a break in the pipe; and, if the pipe does undergo such large motion, a section may be deformed sufficiently to choke the flow. The second stage of the analysis is to predict the overall dynamic response of the pipe, using the moment-curvature response of the section that has been obtained in the first analysis to define the inelastic bending behavior of the beam. This two-stage approach provides a straightforward, inexpensive method of evaluating the event. The method is approximate and may give rise to significant errors. That aspect of the approach is discussed in the last section below.

Modeling The problem is shown in Figure 2.1.1-1. To investigate the static collapse of the section, we consider a unit length of an initially straight pipe subjected to a pure bending moment and assume that plane sections remain plane. We can think of this unit length of pipe as being bounded at its ends by rigid walls and imagine the bending to be achieved by rotation of the walls relative to each other, the end sections being allowed to distort only in the plane of the walls (see Figure 2.1.1-2). With this idealization the pipe section can be modeled and discretized using generalized plane strain elements, as shown in Figure 2.1.1-2. Bending occurs about the x-axis, and symmetry conditions are prescribed along the y-axis. There will not be symmetry about the x-axis because of the Poisson's effect. To remove rigid body motion in the y-direction, point A is fixed in that direction. Symmetry implies no x-displacement at x =0 and that there is no rotation of the section about the y-axis. 8-node and 4-node generalized plane strain elements with reduced integration are used. In addition to the eight or four regular nodes used for interpolation, these elements require two extra nodes that are common to all elements in the model. Degree of freedom 1 at the first of these extra nodes is the relative displacement between the boundary planes, while the first two degrees of freedom at the second extra node are the relative rotation of these planes. Since the problem involves bending the pipe cross-section, fully integrated 4-node elements will not

2-722

Dynamic Stress/Displacement Analyses

provide accurate results, especially when the pipe is fairly thin, because they will suffer from "shear locking"--they will not provide the bending deformation because to do so requires that they shear at their integration points and this shearing requires an unrealistically large amount of strain energy. This problem is avoided by integrating the elements only at their centroids but the elements then exhibit singular modes--modes of deformation that do not cause strain. ABAQUS uses orthogonal hourglass generalized strains and associated stiffness to avoid such spurious singular mode behavior. Although these techniques are not always reliable, they can work well and do so in this example. A superior approach would be to use the fully integrated incompatiable mode element CGPE6I element. For additional discussion of these points see ``Performance of continuum and shell elements for linear analysis of bending problems,'' Section 2.3.5 of the ABAQUS Benchmarks Manual. For the dynamic analysis of the pipe whip event the pipeline is modeled with 10 beam elements of type B21. These are planar beam elements that use linear interpolation of displacement and rotation. The moment-curvature relation obtained from the static analysis (shown in Figure 2.1.1-7) is used in the *BEAM GENERAL SECTION, SECTION=NONLINEAR GENERAL option input data to define the bending behavior of the beams. A definition for the axial force versus strain behavior of the beams is also required and is provided by conversion of the uniaxial stress-strain relation given in Figure 2.1.1-1 into force versus strain by multiplying the stress by the current area, A, of the cross section. This current area is computed from the original cross-sectional area A0 by assuming that the material is incompressible, so A = A0 l0 =l, where l is the current length and l0 is the original length. This definition of the beam section behavior provides for no interaction between the bending and axial stretching, although in most real cases there will actually be some interaction. However, this approximation is probably reasonable in this particular problem since the response is predominantly bending and no appreciable error is introduced by the little stretching that does occur.

Loading and solution control In the large-displacement static analysis of the inelastic collapse of the section, rotation of the boundary planes about the x-axis is prescribed at the second extra node of the generalized plane strain model. The Riks procedure is used: this method usually provides rapid convergence in such cases, especially when unstable response occurs. In the large-displacement dynamic analysis the blowdown force is treated as a follower force. During the first 0.06 seconds of the event it has a constant magnitude of 30 kN (this is about three times the load required to produce maximum moment in the static response of the section). After that time the load is zero. The response is computed for a time period of 0.4 seconds, using automatic time incrementation. A half-step residual tolerance ( HAFTOL) of 30 kN (which is the magnitude of the applied load) is used. Since we expect considerable plastic deformation, high frequency response should be damped quickly in the actual event, so that this value of HAFTOL should be adequate to give reasonably accurate results.

Results and discussion Figure 2.1.1-3 shows a series of deformed configuration plots from the static analysis using element type CGPE10R, and Figure 2.1.1-4 shows the same plots for the analysis using element type CGPE6R.

2-723

Dynamic Stress/Displacement Analyses

Figure 2.1.1-5 and Figure 2.1.1-6are corresponding plots of equivalent plastic strain. Figure 2.1.1-3and Figure 2.1.1-5 clearly show that the discretization is too coarse or should be rezoned later in the deformation, but it is judged that this is not critical to the overall moment-rotation response prediction. Figure 2.1.1-7 shows the moment-curvature responses predicted by the analyses. The unstable nature of the response is clearly illustrated. Figure 2.1.1-8 shows a series of deformed configuration plots from the dynamic analysis. After the shutdown of the force at 0.06 seconds, the momentum of the pipe is enough to cause localization of the deformation at the root of the cantilever as the section collapses there: the pipe whips around this hinge in a full circle and beyond its initial configuration. As well as this major hinge at the root, permanent plastic deformation develops throughout most of the pipe, leaving it bent into an arc. Time history plots of the tip displacement are shown in Figure 2.1.1-9and of the curvature strain at the localized hinge in Figure 2.1.1-10. Figure 2.1.1-11 shows the moment-curvature response for the element at the support and shows the elastic unloading and reloading that takes place during and at the end of the event. Figure 2.1.1-12shows the history of the energy content during the dynamic analysis and clearly shows the initial build-up of kinetic energy, which is then converted almost entirely to plastic dissipation. This two-stage approach to the problem has the advantages of being simple and computationally inexpensive. It contains some obvious approximations. One is that interaction effects between bending, axial, and torsional behavior are neglected. This lack of interaction between the various modes of cross-sectional response is a basic approximation of the nonlinear beam general section option. In reality, axial or torsional strain will have the effect of reducing the strength of the section in bending. This effect is unlikely to be significant in a case that is dominated by bending, but it can be important if large axial or torsional loadings occur. The approach also neglects the effect of the axial gradient of the cross-sectional behavior on the response. This may be a significant error, but its evaluation would require a detailed, three-dimensional analysis for comparison; and that exercise is beyond the scope of this example. Another possibly significant error is the neglect of rate effects on the response. The cross-sectional collapse involves large strains, which occur in a very short time in the dynamic loadings, so high strain rates arise. It is likely that the material will exhibit strain rate dependence in its yield behavior and will, therefore, be rather stiffer than the static analysis predicts it to be. This should have the effect of spreading the hinge along the pipe and reducing the localization (because the strain rates increase at the section where most deformation is occurring, and that increased strain rate increases the resistance of the section). The magnitude of this effect can be estimated from the solution we have obtained. From Figure 2.1.1-5we see that typical strains in the section are about 10-20% when the section is far into collapse; and Figure 2.1.1-10shows that, in the dynamic event, it takes about 0.2 seconds for this to occur. This implies average gross strain rates of about 1.0 per second in that period of the response. In typical piping steels such a strain rate might raise the yield stress 5-10% above its static value. This is not a large effect, so the mitigation of localization by rate effects is probably not a major aspect of this event. Again, a more precise assessment of this error would require a fully three-dimensional analysis. Overall it seems likely that this simple and computationally inexpensive two-stage approach to the problem is providing results that are sufficiently realistic to be used in design, although it would be most desirable to compare these results with physical experimental data or data from a full, detailed, three-dimensional analysis to support that statement. Finally, it should be

2-724

Dynamic Stress/Displacement Analyses

noted that the section considered here is relatively thick ( R=t =3.5). In pipes with thin walls (R=t >20) it is to be expected that the behavior will be affected strongly by internal fluid pressure in the pipe and by the interaction between axial and bending forces. Such thin-walled pipes could be modeled at relatively low cost by using ELBOW elements directly in the dynamic analysis instead of this two-stage approach. An additional concern with very thin pipes is that they are more likely to tear and leak, rather than choke the flow.

Input files nonlindyncollapse_cge10r.inp Static analysis of the elastic-plastic collapse of the pipe section using CGPE10R elements. nonlindyncollapse_nonlingsect.inp Dynamic analysis of the inelastic pipe whip response using nonlinear beam general section definitions for the axial and bending behaviors of the pipe. nonlindyncollapse_cgpe6i.inp Static analysis using element type CGPE6I. nonlindyncollapse_cgpe6r.inp Static analysis using element type CGPE6R. nonlindyncollapse_postoutput1.inp *POST OUTPUT analysis. nonlindyncollapse_postoutput2.inp *POST OUTPUT analysis.

Figures Figure 2.1.1-1 Elastic-plastic pipe subjected to rupture force.

2-725

Dynamic Stress/Displacement Analyses

Figure 2.1.1-2 Initially straight pipe collapsing under pure bending; generalized plane strain model.

2-726

Dynamic Stress/Displacement Analyses

Figure 2.1.1-3 Deformed shapes of collapsing pipe section under pure bending, element type CGPE10R.

2-727

Dynamic Stress/Displacement Analyses

Figure 2.1.1-4 Deformed shapes of collapsing pipe section under pure bending, element type CGPE6R.

2-728

Dynamic Stress/Displacement Analyses

Figure 2.1.1-5 Equivalent plastic strain contours in collapsing pipe section, element type CGPE10R.

2-729

Dynamic Stress/Displacement Analyses

Figure 2.1.1-6 Equivalent plastic strain contours in collapsing pipe section, element type CGPE6R.

2-730

Dynamic Stress/Displacement Analyses

Figure 2.1.1-7 Moment-curvature response predicted for collapsing section under pure bending.

2-731

Dynamic Stress/Displacement Analyses

Figure 2.1.1-8 Displaced positions of pipe, every 20 increments. Initial increments in top figure, final increments in bottom figure.

2-732

Dynamic Stress/Displacement Analyses

Figure 2.1.1-9 Tip displacement history.

2-733

Dynamic Stress/Displacement Analyses

Figure 2.1.1-10 Curvature-time history for the element at the support.

Figure 2.1.1-11 Moment versus curvature in the element at the support.

2-734

Dynamic Stress/Displacement Analyses

Figure 2.1.1-12 Energy history for the beam.

Sample listings

2-735

Dynamic Stress/Displacement Analyses

Listing 2.1.1-1 *HEADING COLLAPSING PIPE SECTION *NODE 1, 2, *NODE,NSET=SYM 101,0.,-28.55 201,0.,-30.925 301,0.,-33.3 401,0.,-35.675 501,0.,-38.05 117,0.,28.55 217,0.,30.925 317,0.,33.3 417,0.,35.675 517,0.,38.05 *NGEN,LINE=C 101,117,1,1,,,,0.,0.,1. 201,217,2,1,,,,0.,0.,1. 301,317,1,1,,,,0.,0.,1. 401,417,2,1,,,,0.,0.,1. 501,517,1,1,,,,0.,0.,1. *NSET,NSET=MON 2, *ELEMENT,TYPE=CGPE10R 11, 101,301,303,103,201,302,203,102,1,2 *ELGEN,ELSET=ALL 11,2,200,1 11,8,2,10 12,8,2,10 *ELSET,ELSET=PRINT 11,12,41,42,51,52,81,82 *SOLID SECTION,MATERIAL=MAT,ELSET=ALL *MATERIAL,NAME=MAT *ELASTIC 2.08E5,.3 *PLASTIC 316.,0. 324.,.02 388.,.04 431.,.06

2-736

Dynamic Stress/Displacement Analyses

464.,.08 492.,.1 547.,.15 589.,.2 624.,.25 654.,.3 705.,.4 747.,.5 784.,.6 816.,.7 845.,.8 871.,.9 895.,1. *BOUNDARY SYM,XSYMM 2,2 509,2 *RESTART,WRITE,FREQUENCY=5 *STEP,NLGEOM,INC=100 *STATIC,RIKS .01,1.,.01, , ,2,1,.03 *BOUNDARY 2,1,1,.05 *MONITOR,NODE=2,DOF=1 *NODE PRINT,FREQUENCY=10 U,RF *NODE FILE,NSET=MON U,RF *EL PRINT,ELSET=PRINT,FREQUENCY=5 E, PE, *EL FILE,ELSET=PRINT,FREQUENCY=5 E,PE *END STEP

2-737

Dynamic Stress/Displacement Analyses

Listing 2.1.1-2 *HEADING INELASTIC NONLINEAR BEAM GENERAL SECTION DYNAMICS *NODE 1, *NODE,NSET=N11 11,3. *NGEN 1,11 *ELEMENT,TYPE=B21 1,1,2 *ELGEN,ELSET=EALL 1,10,1,1 *BEAM GENERAL SECTION,DENSITY=7827., SECTION=NONLINEAR GENERAL,ELSET=EALL 1.9877E-3,1.1245E-6,0.,1.1245E-6,2.2490E-6 0.,0.,-1. *AXIAL 0.,0. 6.48E5,.02 7.46E5,.04 8.12E5,.06 8.57E5,.08 8.90E5,.1 *M1 0.,0. 1.35E4,.4 1.43E4,1. 1.60E4,1.6 1.73E4,2.2 1.80E4,3. 1.90E4,4. 1.80E4,5. 1.15E4,10.2 .90E4,13. .75E4,16.2 .65E4,21. .58E4,30. *BOUNDARY 1,1,6 *AMPLITUDE,NAME=P,TIME=STEP TIME 0.,1.,.06,1.,.0601,0.

2-738

Dynamic Stress/Displacement Analyses

*RESTART,WRITE,FREQUENCY=20 *STEP,NLGEOM,INC=600 *DYNAMIC,HAFTOL=30.E3 .001,.4 *CLOAD,FOLLOWER,AMPLITUDE=P 11,2,-30000. *PRINT,RESIDUAL=NO *NODE PRINT,FREQUENCY=20 *EL PRINT,FREQUENCY=20 SF, SPE,SEPE *EL FILE,FREQUENCY=20 SF, SPE,SEPE *NODE FILE,NSET=N11 U,CF *ENERGY FILE *END STEP

2.1.2 Detroit Edison pipe whip experiment Product: ABAQUS/Standard This example is a model of a simple, small-displacement pipe whip experiment conducted by the Detroit Edison Company and reported by Esswein et al. (1978). The problem involves rather small displacements but provides an interesting case because some (limited) experimental results are available. It is a typical pipe whip restraint design case. It is a rather straightforward analysis because the restraint limits the motion and the geometry is so simple.

Geometry and model The geometry and loading are shown in Figure 2.1.2-1. The pipe has a straight run of length 2.286 m (90 in), a very stiff elbow, and a cantilever "stick" 482.6 mm (19 in) long. A bursting diaphragm is installed at the end of the "stick" to initiate the blowdown. The restraint is a set of three U-bolts coupled together. The blowdown force history measured in the experiment is also shown in Figure 2.1.2-1. All dimensions, material properties, and this force history are taken from Esswein et al. (1978). The horizontal pipe run is modeled with eight elements of type B23 (cubic interpolation beam with planar motion), and the stick is modeled with two elements of the same type. The elbow is treated as a fully rigid junction, so the node at the elbow is shared between the two branches. The bursting diaphragm structure is modeled as a lumped mass of 106.8 kg (0.61 lb s 2/in). The restraint is modeled as a single truss element. For the pipe the Young's modulus is 207 GPa (30 ´ 106 lb/in2), the initial yield stress is 214 MPa (31020 lb/in 2), and the work hardening modulus is 846 "0.2 MPa (122700"0.2 lb/in2) after yield. The restraint has an elastic stiffness of 131.35 MN/m (750000 lb/in), a yield force of

2-739

Dynamic Stress/Displacement Analyses

16681 N (3750 lb), and--when yielding--a force-displacement response F = 2.2716 ± 0.235 MN/m (12971± 0.235 lb/in). These values are taken from Esswein et al. (1978), where it is stated that they are based on measurements of static values with the stresses and forces increased by 50% in the plastic range to account for strain-rate effects. When it is known that strain-rate effects are important to the response it is preferable to model them directly, using the *RATE DEPENDENT suboption of the *PLASTIC option. This has not been done in this case because the actual material is not specified. Isotropic hardening is assumed for both the pipe and the restraint since the plastic flows are presumed to be in the large flow regime and not just incipient plasticity (where the Bauschinger effect can be important). The cross-section of the pipe is integrated with a seven-point Simpson rule: this should be of sufficient accuracy for this problem. Generally, in beam-like problems without repeated large magnitude excitation, a higher-order integration scheme would show only significantly different results at late times in the response, and then the differences are not too important in models of this rather unrefined level. Esswein et al. (1978) provide the blowdown force-time history shown in Figure 2.1.2-1. This is applied as a point load at the end of the stick. In reality the fluid force during blowdown occurs at the piping elbows; but, since the displacements remain small, this detail is not important.

Solution control Automatic time stepping is used, with an initial time increment of 100 ¹sec and the value of the half-step residual, HAFTOL on the *DYNAMIC option, set to 4448 N (1000 lb). This value is based on actual force values expected (in this case, the blowdown force): HAFTOL is chosen to be about 10% of peak real forces. This should give good accuracy in the dynamic integration.

Results and discussion The displacement of the node that hits the restraint is shown in Figure 2.1.2-2, and the force between the pipe and restraint is shown in Figure 2.1.2-3. Some experimental results from Esswein et al. (1978) are shown in Figure 2.1.2-3. The analysis appears to predict the closure time and the peak force between the pipe and restraint quite well. However, the numerical solution (like the numerical solution given by Esswein et al., 1978) shows a slower force rise time than the experiment. A possible explanation may be the material model, where viscoplastic (strain-rate-dependent yield) effects have been modeled as enhanced yield values, as discussed above: this means that, at the high strain rate that occurs just after impact, the actual material can carry higher stresses than the model, and so will respond more stiffly. The oscillation in the gap force in Figure 2.1.2-3after the initial loading of the restraint is presumably caused by the difference in the basic natural frequencies of the restraint and the pipe: this oscillation is sufficiently severe to cause two slight separations.

Input files detroitedison.inp Input data for this analysis.

2-740

Dynamic Stress/Displacement Analyses

detroitedison_postoutput.inp *POST OUTPUT analysis.

Reference · Esswein, G., S. Levy, M. Triplet, G. Chan, and N. Varadavajan, Pipe Whip Dynamics, ASME Special Publication, 1978.

Figures Figure 2.1.2-1 Detroit Edison experiment.

Figure 2.1.2-2 Displacement history at constrained end.

2-741

Dynamic Stress/Displacement Analyses

Figure 2.1.2-3 Gap force history.

2-742

Dynamic Stress/Displacement Analyses

Sample listings

2-743

Dynamic Stress/Displacement Analyses

Listing 2.1.2-1 *HEADING DECO EXAMPLE 10 *WAVEFRONT MINIMIZATION, SUPPRESS *NODE 1, 97.,19. 2,97.,9. 3,97. 4,90. 5,78. 6,66. 7,54. 8,42. 9,30. 10,15. 11,0. 12,90.,-3.18 13,90.,997. *NSET,NSET=NFIL 3,4 *ELEMENT,TYPE=B23 1,1,2 *ELGEN,ELSET=BEAM 1,10 *ELEMENT,TYPE=T3D2,ELSET=TRUS 11,12,13 *SOLID SECTION, ELSET=TRUS, MATERIAL=A2 1., *MATERIAL,NAME=A2 *DENSITY 1.174E-6, *ELASTIC 7.5E8, *PLASTIC,HARDENING=ISOTROPIC 3741.,0. 1.1046E4,4.85E-4 1.3E4,9.83E-4 1.53E4,1.98E-3 1.8E4,3.98E-3 *BEAM SECTION,SECTION=PIPE,ELSET=BEAM,MATERIAL=A1 2.25,.337 *MATERIAL,NAME=A1

2-744

Dynamic Stress/Displacement Analyses

*DENSITY 7.338E-4, *ELASTIC 30.E6, *PLASTIC,HARDENING=ISOTROPIC 3.102E4,0. 4.252E4,3.58E-3 6.74E4,4.775E-2 8.893E4,.197 1.227E5,.9959 *ELEMENT,TYPE=MASS,ELSET=MASS 21,1 *MASS,ELSET=MASS .61, *ELEMENT,TYPE=GAPUNI,ELSET=GAP1 31,4,12 *GAP,ELSET=GAP1 3.181,0.,-1.,0. *AMPLITUDE,NAME=P 0.,7200.,.00045,7200.,.00046,7272.,.0291,7272. .0292,7920.,.1,7920. *BOUNDARY 11,1,2 11,6 12,1 12,3 13,1,3 *RESTART,WRITE,FREQUENCY=100 *STEP,NLGEOM,INC=500 APPLY CONCENTRATED FORCE *DYNAMIC,HAFTOL=1000. 100.E-6,.1 *CLOAD,AMPLITUDE=P 1,2,-1. *MONITOR,NODE=1,DOF=2 *ENERGY PRINT,FREQUENCY=5 *NODE PRINT,NSET=NFIL,FREQUENCY=10 U, *EL PRINT,FREQUENCY=10,ELSET=MASS ELEN, *PRINT,RESIDUAL=NO,FREQUENCY=5 *EL PRINT,ELSET=TRUS,FREQUENCY=20 S,

2-745

Dynamic Stress/Displacement Analyses

E, PE,PEEQ *NODE PRINT,FREQUENCY=40 U, V, A, CF, RF, *EL PRINT,ELSET=BEAM,FREQUENCY=80 S, SF, E, PE,PEEQ *NODE FILE,NSET=NFIL U, *EL FILE,ELSET=GAP1 S,E *EL FILE,ELSET=MASS ELEN, *END STEP

2.1.3 Plate impact simulation Product: ABAQUS/Explicit This example simulates the oblique impact of a rigid spherical projectile onto a flat armor plate at a velocity of 1000 m/sec. A failure model is used for the plate, thus allowing the projectile to perforate the plate. The example illustrates impact, shear failure, and the use of infinite elements.

Problem description The armor plate has a thickness of 10 mm and is assumed to be semi-infinite in size compared to the projectile. This is accomplished by using CIN3D8 infinite elements around the perimeter of the plate. The plate is modeled using 4480 C3D8R elements. The armor plate material has Young's modulus of 206.8 GPa, Poisson's ratio of 0.3, density of 7800 kg/m 3, yield stress of 1220 MPa, and a constant hardening slope of 1220 MPa. The material definition also includes a shear failure model, which causes ABAQUS/Explicit to remove elements from the mesh as they fail. Failure is assumed to occur at an equivalent plastic strain of 100%, at which point the element is removed from the model instantaneously. (The value of the failure strain is chosen somewhat arbitrarily; it is not intended to model any particular material.) The sphere has a diameter of 20 mm and is assumed to be rigid, with a mass corresponding to a uniform material with a density of 37240 kg/m 3. The rotary inertia of the sphere is not needed in the model because we assume there is no friction between the sphere and the plate. Boundary conditions are applied to constrain the motion of the sphere in the y-direction. Two approaches for modeling the

2-746

Dynamic Stress/Displacement Analyses

surface of the sphere are tested: using an analytical rigid surface and using R3D4 rigid elements. Analytical rigid surfaces are the preferred means for representing simple rigid geometries such as this in terms of both accuracy and computational performance. However, more complex three-dimensional surface geometries that occur in practice must be modeled with surfaces formed by element faces. Results for the faceted representations are presented here. The element formulation for the C3D8R elements is modified with the *SECTION CONTROLS option. The advocated formulation for this problem uses the CENTROID kinematic formulation and the COMBINED hourglass control. Two other formulations are included for comparison: the default formulation using the AVERAGE STRAIN kinematic formulation and the RELAX STIFFNESS hourglass control and the formulation using the ORTHOGONAL kinematic formulation and the COMBINED hourglass control. Only half of the plate is modeled, using appropriate symmetry boundary conditions in the x-z plane. The model is shown in Figure 2.1.3-1. The complete sphere is modeled for visualization purposes. There are 17094 degrees of freedom in the model. Since elements in the plate will fail and be removed from the model, nodes in the interior of the plate will be exposed to contact with the surface of the rigid sphere. Thus, contact must be modeled between the surface of the sphere, defined as an element-based surface using the *SURFACE, TYPE=ELEMENT option, and a node-based surface that contains all of the nodes in the plate within a radius of 20 mm of the point of impact, defined with the *SURFACE, TYPE=NODE option. The *CONTACT PAIR option is used to define contact between the surface of the sphere and any of the nodes contained in the node set.

Results and discussion The spherical projectile impacts the plate at 1000 m/sec at an angle of 30° to the normal to the plate. Deformed shapes at different stages of the analysis are shown in Figure 2.1.3-2through Figure 2.1.3-4 for the CENTROID kinematic and COMBINED hourglass section control options (analysis case pl3d_erode_ccs). Early in the analysis, shown in Figure 2.1.3-2, a relatively small amount of material has been eroded from the surface of the plate and the plate is still deforming under the sphere. In Figure 2.1.3-3the plate has been perforated and the projectile is still in contact with the edge of the hole. In Figure 2.1.3-4 the projectile has exited the plate and is moving as a rigid body. Figure 2.1.3-5and Figure 2.1.3-6 show the history of the projectile's velocity (Table 2.1.3-1 shows the analysis options used to obtain these results for analyses using different section controls). The analysis pl3d_erode_ccs shows comparable accuracy to the other analyses at a much reduced computational cost; however, strain and stress values vary more than the primary variables (velocity, displacement, etc.). In Figure 2.1.3-2 through Figure 2.1.3-4the failed elements have been eliminated by creating a display group in ABAQUS/Viewer that contains only the active elements.

Input files pl3d_erode_ccs.inp Model using the CENTROID kinematic and COMBINED hourglass section control options.

2-747

Dynamic Stress/Displacement Analyses

sphere_n.inp External file referenced in this input. sphere_e.inp External file referenced in this input. pl3d_erode.inp Model using the default section controls. pl3d_erode_ale.inp Model using the default section controls and the *ADAPTIVE MESH option. pl3d_erode_ocs.inp Model using the ORTHOGONAL kinematic and COMBINED hourglass section control options. pl3d_erode_anl.inp Model using an analytical rigid surface and the default section controls.

Table Table 2.1.3-1 Analysis options tested. Analysis File Relative Section Controls Kinematic Hourglass CPU Time pl3d_erode 1.0 average relax pl3d_erode_oc 0.70 orthogonal combined s pl3d_erode_cc 0.57 centroid combined s

Figures Figure 2.1.3-1 Undeformed mesh.

2-748

Dynamic Stress/Displacement Analyses

Figure 2.1.3-2 Deformed shape at 10 microseconds (analysis using the following section control options: CENTROID kinematics and COMBINED hourglass control).

Figure 2.1.3-3 Deformed shape at 30 microseconds (analysis using the following section control options: CENTROID kinematics and COMBINED hourglass control).

Figure 2.1.3-4 Deformed shape at 40 microseconds (analysis using the following section control options: CENTROID kinematics and COMBINED hourglass control).

2-749

Dynamic Stress/Displacement Analyses

Figure 2.1.3-5 Vertical component of the projectile velocity.

Figure 2.1.3-6 Horizontal component of the projectile velocity.

2-750

Dynamic Stress/Displacement Analyses

Sample listings

2-751

Dynamic Stress/Displacement Analyses

Listing 2.1.3-1 *HEADING RIGID SPHERE IMPACTING ON THICK PLATE WITH PENETRATION AND ELEMENT EROSION SECTION CONTROLS USED (KINEMA=CENTROID, HOURGLASS=COMBINED) *PREPRINT,ECHO=NO,MODEL=NO,HISTORY=NO *NODE 1,-.0040, 0.0,0.0 9, .0040, 0.0,0.0 37,-.0031,.0031,0.0 41, 0.0,.0040,0.0 45, .0031,.0031,0.0 46, .0040, 0.0,0.0 50, .0031,.0031,0.0 54, 0.0,.0040,0.0 58,-.0031,.0031,0.0 62,-.0040, 0.0,0.0 318, .02,0.0,0.0 334,-.02,0.0,0.0 488, .04,0.0,0.0 504,-.04,0.0,0.0 505, .05,0.0,0.0 521,-.05,0.0,0.0 *NGEN,NSET=A 1,9,1 *NGEN,NSET=B 37,41,1 41,45,1 *NGEN,NSET=C 46,50,1 50,54,1 54,58,1 58,62,1 *NGEN,NSET=D,LINE=C 318,334,1,,0.,0.,0.,0.,0.,1. *NGEN,NSET=E,LINE=C 488,504,1,,0.,0.,0.,0.,0.,1. *NGEN,NSET=TOP,LINE=C 505,521,1,,0.,0.,0.,0.,0.,1. *NFILL,NSET=TOP A,B,4,9

2-752

Dynamic Stress/Displacement Analyses

C,D,16,17 *NFILL,BIAS=.9,NSET=TOP D,E,10,17 *NCOPY,OLD SET=TOP,SHIFT,CHANGE 0.,0.,-.001 0.,0.,0.,0.,0.,1.,0.0 *NCOPY,OLD SET=TOP,SHIFT,CHANGE 0.,0.,-.002 0.,0.,0.,0.,0.,1.,0.0 *NCOPY,OLD SET=TOP,SHIFT,CHANGE 0.,0.,-.003 0.,0.,0.,0.,0.,1.,0.0 *NCOPY,OLD SET=TOP,SHIFT,CHANGE 0.,0.,-.004 0.,0.,0.,0.,0.,1.,0.0 *NCOPY,OLD SET=TOP,SHIFT,CHANGE 0.,0.,-.005 0.,0.,0.,0.,0.,1.,0.0 *NCOPY,OLD SET=TOP,SHIFT,CHANGE 0.,0.,-.006 0.,0.,0.,0.,0.,1.,0.0 *NCOPY,OLD SET=TOP,SHIFT,CHANGE 0.,0.,-.007 0.,0.,0.,0.,0.,1.,0.0 *NCOPY,OLD SET=TOP,SHIFT,CHANGE 0.,0.,-.008 0.,0.,0.,0.,0.,1.,0.0 *NCOPY,OLD SET=TOP,SHIFT,CHANGE 0.,0.,-.009 0.,0.,0.,0.,0.,1.,0.0 *NCOPY,OLD SET=TOP,SHIFT,CHANGE 0.,0.,-.010 0.,0.,0.,0.,0.,1.,0.0 ** *NSET,NSET=YSYM,GEN 1, 9, 1 46, 488,17 62, 504,17 1001,1009,1 1046,1488,17 1062,1504,17 2001,2009,1 2046,2488,17

NUMBER=1000

NUMBER=2000

NUMBER=3000

NUMBER=4000

NUMBER=5000

NUMBER=6000

NUMBER=7000

NUMBER=8000

NUMBER=9000

NUMBER=10000

2-753

Dynamic Stress/Displacement Analyses

2062,2504,17 3001,3009,1 3046,3488,17 3062,3504,17 4001,4009,1 4046,4488,17 4062,4504,17 5001,5009,1 5046,5488,17 5062,5504,17 6001,6009,1 6046,6488,17 6062,6504,17 7001,7009,1 7046,7488,17 7062,7504,17 8001,8009,1 8046,8488,17 8062,8504,17 9001,9009,1 9046,9488,17 9062,9504,17 10001,10009,1 10046,10488,17 10062,10504,17 *NSET,NSET=FRONT,GEN 1, 385,1 ** *ELEMENT,TYPE=C3D8R,ELSET=TOP 1, 1002,1003,1012,1011, 2, 3,12,11 19, 1008,1046,1047,1017, 8,46,47,17 20, 1017,1047,1048,1026, 17,47,48,26 21, 1026,1048,1049,1035, 26,48,49,35 22, 1035,1049,1050,1051, 35,49,50,51 23, 1034,1035,1051,1052, 34,35,51,52 24, 1033,1034,1052,1053, 33,34,52,53 25, 1032,1033,1053,1054, 32,33,53,54 26, 1031,1032,1054,1055, 31,32,54,55 27, 1030,1031,1055,1056, 30,31,55,56 28, 1029,1030,1056,1057, 29,30,56,57 29, 1059,1029,1057,1058, 59,29,57,58 30, 1060,1020,1029,1059, 60,20,29,59 31, 1061,1011,1020,1060, 61,11,20,60

2-754

Dynamic Stress/Displacement Analyses

32, 1062,1002,1011,1061, 62, 2,11,61 33, 1046,1063,1064,1047, 46,63,64,47 *ELGEN,ELSET=TOP 1, 6,1,1, 3, 9, 6 33, 16,1,1, 26,17,16 *ELEMENT,TYPE=CIN3D8,ELSET=TINF 449, 489,488,1488,1489, 506,505,1505,1506 *ELGEN,ELSET=TINF 449, 16,1,1 ** *ELCOPY,OLD SET=TOP,NEW SET=PLATE,SHIFT NODES=1000, ELEMENT SHIFT=1000 *ELCOPY,OLD SET=TOP,NEW SET=PLATE,SHIFT NODES=2000, ELEMENT SHIFT=2000 *ELCOPY,OLD SET=TOP,NEW SET=PLATE,SHIFT NODES=3000, ELEMENT SHIFT=3000 *ELCOPY,OLD SET=TOP,NEW SET=PLATE,SHIFT NODES=4000, ELEMENT SHIFT=4000 *ELCOPY,OLD SET=TOP,NEW SET=PLATE,SHIFT NODES=5000, ELEMENT SHIFT=5000 *ELCOPY,OLD SET=TOP,NEW SET=PLATE,SHIFT NODES=6000, ELEMENT SHIFT=6000 *ELCOPY,OLD SET=TOP,NEW SET=PLATE,SHIFT NODES=7000, ELEMENT SHIFT=7000 *ELCOPY,OLD SET=TOP,NEW SET=PLATE,SHIFT NODES=8000, ELEMENT SHIFT=8000 *ELCOPY,OLD SET=TOP,NEW SET=PLATE,SHIFT NODES=9000, ELEMENT SHIFT=9000 *ELSET,ELSET=PLATE TOP, ** *ELCOPY,OLD SET=TINF,NEW SET=INF,SHIFT NODES=1000, ELEMENT SHIFT=1000 *ELCOPY,OLD SET=TINF,NEW SET=INF,SHIFT NODES=2000, ELEMENT SHIFT=2000 *ELCOPY,OLD SET=TINF,NEW SET=INF,SHIFT NODES=3000, ELEMENT SHIFT=3000 *ELCOPY,OLD SET=TINF,NEW SET=INF,SHIFT NODES=4000, ELEMENT SHIFT=4000 *ELCOPY,OLD SET=TINF,NEW SET=INF,SHIFT NODES=5000, ELEMENT SHIFT=5000 *ELCOPY,OLD SET=TINF,NEW SET=INF,SHIFT NODES=6000, ELEMENT SHIFT=6000

2-755

Dynamic Stress/Displacement Analyses

*ELCOPY,OLD SET=TINF,NEW SET=INF,SHIFT NODES=7000, ELEMENT SHIFT=7000 *ELCOPY,OLD SET=TINF,NEW SET=INF,SHIFT NODES=8000, ELEMENT SHIFT=8000 *ELCOPY,OLD SET=TINF,NEW SET=INF,SHIFT NODES=9000, ELEMENT SHIFT=9000 *ELSET,ELSET=INF TINF, ** *SOLID SECTION,ELSET=PLATE,MATERIAL=RHA,CONTROL=B *SOLID SECTION,ELSET=INF, MATERIAL=INF,CONTROL=B *SECTION CONTROLS, KINEMA=CENTROID, HOURGLASS=COMBINED, NAME=B ** ** Sphere with radius of .01 m. ** *NODE,NSET=SPHERE,INPUT=sphere_n.inp *ELEMENT,TYPE=R3D4,ELSET=SPHERE, INPUT=sphere_e.inp *ELEMENT,TYPE=MASS,ELSET=MASS 50000,599991 *MASS,ELSET=MASS ** Mass based on a density of 37240 Kg/m^3 ** and radius of .01 m. .078, ** *MATERIAL,NAME=RHA *DENSITY 7800., *ELASTIC 207.8E9,.3 *PLASTIC 1220.E6,0. 2440.E6,1. *SHEAR FAILURE 1.0, *MATERIAL,NAME=INF *DENSITY 7800., *ELASTIC 206.8E9,.3 *INITIAL CONDITIONS,TYPE=VELOCITY 599991,1, 500.

2-756

Dynamic Stress/Displacement Analyses

599991,3,-866.6 *BOUNDARY YSYM,2,2 599991, 2 599991, 4,6 *RESTART,WRITE,NUM=8 *SURFACE,TYPE=ELEMENT,NAME=SPHERE SPHERE,SPOS *NSET,NSET=ERODE_NSET,GEN 1, 385,1 1001,1385,1 2001,2385,1 3001,3385,1 4001,4385,1 5001,5385,1 6001,6385,1 7001,7385,1 8001,8385,1 9001,9385,1 10001,10385,1 *SURFACE,TYPE=NODE,NAME=ERODE ERODE_NSET, *RIGID BODY,ELSET=SPHERE,REF NODE=599991 *STEP *DYNAMIC,EXPLICIT ,40.E-6 *CONTACT PAIR SPHERE,ERODE *HISTORY OUTPUT, TIME INTERVAL=0.0 *NSET, NSET=N1 599991, *NODE HISTORY, NSET=N1 V, *FILE OUTPUT, NUM=2, TIMEMARKS=YES *NODE FILE U,V *EL FILE S,PEEQ STATUS, *EL FILE ELEN, *END STEP

2-757

Dynamic Stress/Displacement Analyses

2.1.4 Tennis racket and ball Product: ABAQUS/Explicit This example simulates the oblique impact of a tennis ball onto a racket at 6.706 m/sec (264 in/sec). The example illustrates contact between a deforming surface and a node set, the definition of initial stresses via the *INITIAL CONDITIONS option, and modeling of the compressible gas inside the ball with hydrostatic fluid cavity elements.

Problem description The strings on the tennis racket are modeled using T3D2 truss elements. They are assumed to be linear elastic, with Young's modulus of 6.895 GPa (1.0 ´ 106 psi), Poisson's ratio of 0.3, and density of 1143 kg/m3 (1.07 ´ 10-4 lb sec2in-4). The strings are under an initial tension of 44.48 N (10 lb), which is specified with the *INITIAL CONDITIONS option. The frame is assumed to be rigid and is modeled using R3D4 elements. The nodes of the strings (truss elements) around the perimeter are the same nodes as those used for the R3D4 elements. The reference node for the rigid frame has boundary conditions applied to constrain all six degrees of freedom on the rigid body so that the frame does not move. The tennis ball is modeled as a sphere, using 150 S4R shell elements. It is assumed to be made of rubber, modeled with the *HYPERELASTIC option as a Mooney-Rivlin material with the constants C10 = 0.690 MPa (100 lb/in 2) and C01 = 0.173 MPa (25 lb/in 2). ABAQUS/Explicit requires some compressibility for hyperelastic materials. In the results shown here, D1 = 0.0145 MPa -1 (10-4 psi-1). This gives an initial bulk modulus ( K0 = 2=D1 ) that is 80 times the initial shear modulus 2(C10 + C01 ). This ratio is lower than the ratio for typical rubbers, but the results are not particularly sensitive to this value in this case because the rubber is unconfined. A more accurate representation of the material's compressibility would be needed if the rubber were confined by stiffer adjacent components or reinforcement. Decreasing D1 by an order of magnitude (thus increasing the initial bulk modulus by a factor of 10) has little effect on the overall results but causes a reduction in the stable p time increment by a factor of 10 due to the increase in the bulk modulus. The density of the tennis ball is 1068 kg/m 3 (1.07 ´ 10-4 lb sec2in-4). The tennis ball is under an initial internal pressure of 41 kPa (6 psi) in addition to the ambient atmospheric pressure of 100 kPa (14.7 psi). Hydrostatic fluid elements of type F3D4 are used to model the gas in the tennis ball. Since the ball is impermeable to gas, the pressure of the gas will rise when the volume of the ball decreases, and vice versa. The fluid density is arbitrarily chosen to be one-tenth of that of rubber under an ambient pressure of 100 kPa (14.7 psi). Static equilibrium gives the value of the initial biaxial membrane stresses in the shell elements of the sphere as pr=2t = 155 kPa (22.5 psi) to balance the internal pressure (here p is the internal gas pressure, r is the radius of the sphere, and t is the tennis ball thickness). This initial state of stress in the ball is defined with the *INITIAL CONDITIONS option. A coefficient of friction of 0.1 is specified between the ball and the strings. The ball impacts on the strings at 6.706 m/sec (264 in/sec) at an angle of 15°.

2-758

Dynamic Stress/Displacement Analyses

No attempt has been made to generate an accurate model of the ball and strings: the model parameters are chosen simply to provide a "soft" ball relative to the strings to illustrate contact effects. The complete model is shown in Figure 2.1.4-1. There are 2241 degrees of freedom in the model. An element-based surface is defined on the tennis ball using the *SURFACE, TYPE=ELEMENT option. Since the truss elements are line elements, they do not form a planar surface. A node-based surface is defined that contains all the nodes of the strings using the *SURFACE, TYPE=NODE option. The *CONTACT PAIR option is then used to define contact between the element-based surface of the ball and any of the nodes defined in the node-based surface.

Results and discussion Figure 2.1.4-2 shows the position of the ball with respect to the strings in the undeformed configuration. The deformed shapes at different stages of the analysis are shown in Figure 2.1.4-3through Figure 2.1.4-7. Figure 2.1.4-8shows a time history of the energies for the model. These include the total internal energy (ALLIE), the kinetic energy (ALLKE), the viscous dissipation (ALLVD), the energy dissipated by friction (ALLFD), the external work (ALLWK), and the total energy balance for the model (ETOTAL). The total energy is seen to remain almost constant during the analysis, as it should. Figure 2.1.4-9and Figure 2.1.4-10 give the history of pressure inside the ball and the history of the actual volume of the ball. It can be seen that both the gas pressure inside the ball and the ball volume stabilize after 10 msec.

Input files tennis.inp Input data used in this analysis. tennis_ef1.inp External file referenced in this input. tennis_ef2.inp External file referenced in this input. tennis_ef3.inp External file referenced in this input.

Figures Figure 2.1.4-1 Undeformed mesh.

2-759

Dynamic Stress/Displacement Analyses

Figure 2.1.4-2 Original position of ball and strings.

Figure 2.1.4-3 Deformed shape at 2.5 milliseconds.

Figure 2.1.4-4 Deformed shape at 5 milliseconds.

2-760

Dynamic Stress/Displacement Analyses

Figure 2.1.4-5 Deformed shape at 7.5 milliseconds.

Figure 2.1.4-6 Deformed shape at 10 milliseconds.

Figure 2.1.4-7 Deformed shape at 15 milliseconds.

2-761

Dynamic Stress/Displacement Analyses

Figure 2.1.4-8 Energy histories.

Figure 2.1.4-9 History of the gas pressure inside the tennis ball.

2-762

Dynamic Stress/Displacement Analyses

Figure 2.1.4-10 History of the ball volume.

Sample listings

2-763

Dynamic Stress/Displacement Analyses

Listing 2.1.4-1 *HEADING RACKET AND BALL IMPACT ******************** ** ** Strings. ** ******************** *NODE ** Bottom curve. 104, -2.700,-6.625,0. 109, 0.000,-8.500,0. 114, 2.700,-6.625,0. ** Left side curve. 501, -4.020,-3.750,0. 1201, -4.520, 0.000,0. 1901, -3.780, 3.750,0. ** Right side curve. 517, 4.020,-3.750,0. 1217, 4.520, 0.000,0. 1917, 3.780, 3.750,0. ** Top curve. 2103, -3.240, 4.500,0. 2109, 0.000, 5.500,0. 2115, 3.240, 4.500,0. ** Rectangular portion. 202, -3.780,-6.625,0. 216, 3.780,-6.625,0. 502, -3.780,-3.750,0. 516, 3.780,-3.750,0. 1902, -3.780, 3.750,0. 1916, 3.780, 3.750,0. 2002, -3.780, 4.500,0. 2016, 3.780, 4.500,0. *NGEN,NSET=N200 202,216,1 *NGEN,NSET=N500 502,516,1 *NGEN,NSET=N1900 1902,1916,1 *NGEN 2002,2016,1

2-764

Dynamic Stress/Displacement Analyses

*NFILL,NSET=STRINGS N200,N500,3,100 N500,N1900,14,100 *NGEN,NSET=STRINGS,LINE=P 104,114,1,109 517,1917,100,1217 501,1901,100,1201,0.,0.,1. 2103,2115,1,2109,0.,0.,1. *NSET,NSET=MIDPLANE,GEN 105,113,1 2104,2114,1 501,1801,100 517,1817,100 *NSET,NSET=MIDPLANE 204,303,402,214,315,416 1902,2003,1916,2015 ** *ELEMENT,TYPE=T3D2,ELSET=STRINGS 1, 204, 205 11, 303, 304 23, 402, 403 247,2003,2004 1001, 402, 502 1016, 303, 403 1033, 204, 304 1231, 315, 415 1248, 416, 516 2001, 501, 502 2015, 516, 517 2029, 105, 205 2038,2004,2104 *ELGEN,ELSET=STRINGS 1, 10,1,1 11, 12,1,1 23, 14,1,1, 16,100,14 247, 12,1,1 1001, 15,100,1 1016, 17,100,1 1033, 18,100,1, 11,1,18 1231, 17,100,1 1248, 15,100,1 2001, 14,100,1 2015, 14,100,1

2-765

Dynamic Stress/Displacement Analyses

2029, 9,1,1 2038, 11,1,1 *SOLID SECTION,ELSET=STRINGS,MATERIAL=STRING ** Diameter of strings is 0.1 in. 7.854E-3, ** *NSET, NSET=NCONTACT, GENERATE 205,213,1 304,314,1 403,415,1 502,516,1 602,616,1 702,716,1 802,816,1 902,916,1 1002,1016,1 1102,1116,1 1202,1216,1 1302,1316,1 1402,1416,1 1502,1516,1 1602,1616,1 1702,1716,1 1802,1816,1 1903,1915,1 2004,2014,1 ******************** ** ** Frame. ** ******************** *NCOPY,CHANGE NUMBER=10000,OLD SET=MIDPLANE,SHIFT, NEW SET=FRONT 0.,0.,.25 0.,0.,0., 0.,0.,1., 0.0 *NCOPY,CHANGE NUMBER=20000,OLD SET=MIDPLANE,SHIFT, NEW SET=BACK 0.,0.,-.25 0.,0.,0., 0.,0.,1., 0.0 *NODE 10000, 0,0.,0. *ELEMENT,TYPE=R3D4,ELSET=FRAME 3001, 105, 106, 10106, 10105

2-766

Dynamic Stress/Displacement Analyses

3009, 113, 214, 3010, 214, 315, 3011, 315, 416, 3012, 416, 517, 3013, 517, 617, 3036, 1817, 1916, 3037, 1916, 2015, 3038, 2015, 2114, 3039, 2105, 2104, 3049, 2104, 2003, 3050, 2003, 1902, 3051, 1902, 1801, 3052, 601, 501, 3065, 501, 402, 3066, 402, 303, 3077, 303, 204, 3078, 204, 105, 4001, 105, 106, 4009, 113, 214, 4010, 214, 315, 4011, 315, 416, 4012, 416, 517, 4013, 517, 617, 4036, 1817, 1916, 4037, 1916, 2015, 4038, 2015, 2114, 4039, 2105, 2104, 4049, 2104, 2003, 4050, 2003, 1902, 4051, 1902, 1801, 4052, 601, 501, 4065, 501, 402, 4066, 402, 303, 4077, 303, 204, 4078, 204, 105, ** *ELGEN,ELSET=FRAME 3001, 8,1,1 3013, 13,100,1 3039, 10,1,1 3052, 13,100,1 4001, 8,1,1 4013, 13,100,1

10214, 10315, 10416, 10517, 10617, 11916, 12015, 12114, 12104, 12003, 11902, 11801, 10501, 10402, 10303, 10204, 10105, 20106, 20214, 20315, 20416, 20517, 20617, 21916, 22015, 22114, 22104, 22003, 21902, 21801, 20501, 20402, 20303, 20204, 20105,

10113 10214 10315 10416 10517 11817 11916 12015 12105 12104 12003 11902 10601 10501 10402 10303 10204 20105 20113 20214 20315 20416 20517 21817 21916 22015 22105 22104 22003 21902 20601 20501 20402 20303 20204

2-767

Dynamic Stress/Displacement Analyses

4039, 10,1,1 4052, 13,100,1 *NODE,NSET=SPHERE,INPUT=tennis_ef1.inp ** *ELEMENT,TYPE=S4R,ELSET=SPHERE, INPUT=tennis_ef2.inp *SHELL SECTION,ELSET=SPHERE,MATERIAL=RUBBER .2,3 ** *PHYSICAL CONSTANTS, ABSOLUTE ZERO=-273.16 *ELEMENT,TYPE=F3D4,ELSET=CAVITY, INPUT=tennis_ef3.inp *FLUID PROPERTY,ELSET=CAVITY,REF NODE=30001, AMBIENT=14.7 *FLUID DENSITY 0.1E-4, ******************** ** ** Material definitions. ** ******************** *MATERIAL,NAME=RUBBER *DENSITY 1.E-4, *HYPERELASTIC,N=1 100.,25.,1.E-4 *MATERIAL,NAME=STRING ** Nylon type 6 general purpose. *DENSITY 1.07E-4, *ELASTIC 1.E6, ******************** ** ** Initial conditions, boundary conditions. ** ******************** *INITIAL CONDITIONS,TYPE=STRESS ** Tension in strings is 10 lb. STRINGS,1273. SPHERE,22.5,22.5 *INITIAL CONDITIONS,TYPE=VELOCITY ** Initial velocity of ball is 22 fps at a

2-768

Dynamic Stress/Displacement Analyses

** 15 degree angle of attack. SPHERE, 1, 68.3 SPHERE, 2, 0. SPHERE, 3,-255. *BOUNDARY 10000,1,6 *INITIAL CONDITIONS,TYPE=FLUID PRESSURE 30001,6. ** *RESTART,WRITE,NUM=30 ******************** ** *SURFACE,TYPE=ELEMENT,NAME=SPHERE SPHERE,SPOS *SURFACE,TYPE=NODE,NAME=STRINGS NCONTACT, *RIGID BODY,ELSET=FRAME,REF NODE=10000 *STEP *DYNAMIC,EXPLICIT ,15.E-3 ******************** ** ** Contact definitions. ** ******************** *SURFACE INTERACTION,NAME=SPH_STRING *FRICTION 0.1, *CONTACT PAIR,INTERACTION=SPH_STRING SPHERE,STRINGS ******************** ** ** Output requests. ** ******************** *FILE OUTPUT, NUM=2, TIMEMARKS=YES *EL FILE ELEN, S,LE,ERV *NODE FILE U,V *OUTPUT,FIELD,OP=NEW,NUMBER INTERVAL=5, TIMEMARKS=NO

2-769

Dynamic Stress/Displacement Analyses

*ELEMENT OUTPUT S, *NODE OUTPUT U, *OUTPUT,HISTORY,OP=NEW,TIME INTERVAL=3.E-5 *ENERGY OUTPUT ALLAE,ALLIE,ALLKE,ALLPD,ALLSE,ALLVD,ALLWK,ETOTAL *END STEP

2.1.5 Pressurized fuel tank with variable shell thickness Product: ABAQUS/Standard This problem demonstrates the variable shell thickness capability in ABAQUS. The example is based on an analysis conducted by SOLVAY RESEARCH & TECHNOLOGY (see reference) of a blow-molded, plastic fuel tank with dimensions similar to those considered here.

Geometry and model The mesh shown in Figure 2.1.5-1 is used in this example to model a fuel tank and its support straps. The mesh uses 2812 3-node shell elements ( S3R), with the support straps modeled with 32 2-node beam elements (B31). Depending on the desired accuracy and detail of the solution, the analyst may identify some regions of the mesh in which additional refinement, or second-order elements, would be appropriate. The fuel tank would fit within a box of dimensions 450 mm ´ 200 mm ´ 680 mm. An internal pressure of 7 ´ 10-3 MPa is applied statically to the tank. Analyses are conducted for a uniform shell thickness of 5 mm and for a spatially varying shell thickness in the range 1.38 mm to 9.35 mm (see Figure 2.1.5-2), which is a more accurate representation of the tank. The uniform thickness analysis provides a comparison to judge the effects of variable thickness. The overall volume of plastic modeled in the variable thickness analysis is about 93% of that in the uniform thickness analysis. For the variable thickness analysis the presence of the NODAL THICKNESS parameter on the *SHELL SECTION option indicates that the shell thickness is to be interpolated from nodal values specified with the *NODAL THICKNESS option. For elements with more than one integration point, this approach results in a thickness that can vary over the element. The materials are modeled as isotropic elastic. The plastic fuel tank has a Young's modulus of 0.6 GPa and a Poisson's ratio of 0.3. The steel support straps have a Young's modulus of 206.8 GPa and a Poisson's ratio of 0.29. Geometrically nonlinear effects are significant in this example, so the NLGEOM parameter is included on the *STEP option.

Results and discussion Contour plots of the Mises stress at the inner surface of the fuel tank (section point 1 in the shell elements) for the variable shell thickness and uniform shell thickness analyses are shown in Figure 2.1.5-3 and Figure 2.1.5-4. The ratio of the maximum Mises stress found in the variable thickness

2-770

Dynamic Stress/Displacement Analyses

analysis to that found in the uniform thickness analysis is 1.5. For the variable thickness analysis, the maximum Mises stress occurs at a location where the fuel tank skin is relatively thin (see Figure 2.1.5-2 and Figure 2.1.5-3). Examination of the y-component of displacement shows that the overall expansion of the tank in the y-direction is about 1.5% greater in the variable thickness analysis.

Input files pressfueltank_variablethick.inp Example using variable shell thickness. pressfueltank_uniformthick.inp Example using uniform shell thickness. pressfueltank_node.inp Nodal coordinate data for both models. pressfueltank_shellelement.inp Shell element connectivity data for both models. pressfueltank_beamelement.inp Beam element connectivity data for both models. pressfueltank_shellthickness.inp Shell thickness data for the variable shell thickness model.

Reference · SOLVAY RESEARCH & TECHNOLOGY, Plastic Processing Department, Rue de Ransbeek, 310, B-1120 Brussels, Belgium.

Figures Figure 2.1.5-1 Fuel tank mesh with S3R and B31 elements.

2-771

Dynamic Stress/Displacement Analyses

Figure 2.1.5-2 Shell thickness for variable thickness analysis.

2-772

Dynamic Stress/Displacement Analyses

Figure 2.1.5-3 Mises stress solution for variable shell thickness analysis.

2-773

Dynamic Stress/Displacement Analyses

Figure 2.1.5-4 Mises stress solution for uniform shell thickness analysis.

2-774

Dynamic Stress/Displacement Analyses

Sample listings

2-775

Dynamic Stress/Displacement Analyses

Listing 2.1.5-1 *HEADING FUEL TANK - VARIABLE THICKNESS *PREPRINT,MODEL=NO ** **READ MESH DATA FROM SEPARATE FILES *NODE, INPUT=pressfueltank_node.inp *ELEMENT, TYPE=S3R, ELSET=TANK, INPUT=pressfueltank_shellelement.inp *ELEMENT, TYPE=B31, ELSET=STRAPS, INPUT=pressfueltank_beamelement.inp ** **READ VARIABLE SHELL THICKNESS DATA FROM **SEPARATE FILE *SHELL SECTION,ELSET=TANK,MATERIAL=MTANK, NODAL THICKNESS 5. , 3 *NODAL THICKNESS, INPUT=pressfueltank_shellthickness.inp ** *BEAM SECTION,SECTION=RECT,ELSET=STRAPS, MATERIAL=MSTRAP 40.,1.5 0.,0.,-1. ** *MATERIAL,NAME=MTANK *ELASTIC 600., 0.3 ** *MATERIAL,NAME=MSTRAP *ELASTIC 2.068E+05, 0.29 ** *NSET,NSET=APPUI1 112, 164, 168, 169, 170, 171, 172, 173, 177, 180, 214, 233, 236, 237, 238, 239, 240, 241, 242, 245, 271, 272, 279, 284, 285, 288, 310, 311, 312, 313, 342 *NSET,NSET=APPUI2 1455, 1458, 1459, 1512, 1513, 1514, 1515, 1518, 1519, 1520, 1579, 1580, 1583, 1584, 1585, 1586, 1639, 1640

2-776

Dynamic Stress/Displacement Analyses

*NSET,NSET=ENDSTR 1740, 1743, 1746, 1747 ** *BOUNDARY ENDSTR,1,6,0. APPUI1,2,2,0. APPUI2,2,2,0. ** *ELSET,ELSET=SAMPLE,GENERATE 200,1400,200 ** *RESTART,WRITE,FREQUENCY=10 ** ** *STEP,NLGEOM *STATIC 0.1,1. *DLOAD,OP=NEW TANK, P, 7.E-3 *NODE PRINT,FREQUENCY=0 *EL PRINT,FREQUENCY=0 *EL FILE,ELSET=SAMPLE STH, SINV, *OUTPUT,FIELD,VAR=PRESELECT,FREQ=10 *ELEMENT OUTPUT STH, *OUTPUT,FIELD *ELEMENT OUTPUT,ELSET=SAMPLE STH, SINV, *OUTPUT,HISTORY *ELEMENT OUTPUT,ELSET=SAMPLE STH, SINV, *END STEP

2-777

Dynamic Stress/Displacement Analyses

Listing 2.1.5-2 *HEADING FUEL TANK - UNIFORM THICKNESS *PREPRINT,MODEL=NO ** **READ MESH DATA FROM SEPARATE FILES *NODE, INPUT=pressfueltank_node.inp *ELEMENT, TYPE=S3R, ELSET=TANK, INPUT=pressfueltank_shellelement.inp *ELEMENT, TYPE=B31, ELSET=STRAPS, INPUT=pressfueltank_beamelement.inp ** *SHELL SECTION,ELSET=TANK,MATERIAL=MTANK 5. , 3 ** *BEAM SECTION,SECTION=RECT,ELSET=STRAPS, MATERIAL=MSTRAP 40.,1.5 0.,0.,-1. ** *MATERIAL,NAME=MTANK *ELASTIC 600., 0.3 ** *MATERIAL,NAME=MSTRAP *ELASTIC 2.068E+05, 0.29 ** *NSET,NSET=APPUI1 112, 164, 168, 169, 170, 171, 172, 173, 177, 180, 214, 233, 236, 237, 238, 239, 240, 241, 242, 245, 271, 272, 279, 284, 285, 288, 310, 311, 312, 313, 342 *NSET,NSET=APPUI2 1455, 1458, 1459, 1512, 1513, 1514, 1515, 1518, 1519, 1520, 1579, 1580, 1583, 1584, 1585, 1586, 1639, 1640 *NSET,NSET=ENDSTR 1740, 1743, 1746, 1747 ** *BOUNDARY ENDSTR,1,6,0.

2-778

Dynamic Stress/Displacement Analyses

APPUI1,2,2,0. APPUI2,2,2,0. ** *ELSET,ELSET=SAMPLE,GENERATE 200,1400,200 ** *RESTART,WRITE,FREQUENCY=10 ** ** *STEP,NLGEOM *STATIC 0.1,1. *DLOAD,OP=NEW TANK, P, 7.E-3 *NODE PRINT,FREQUENCY=0 *EL PRINT,FREQUENCY=0 *EL FILE,ELSET=SAMPLE STH, SINV, *OUTPUT,FIELD,VAR=PRESELECT,FREQ=10 *ELEMENT OUTPUT STH, *OUTPUT,FIELD *ELEMENT OUTPUT,ELSET=SAMPLE STH, SINV, *OUTPUT,HISTORY *ELEMENT OUTPUT,ELSET=SAMPLE STH, SINV, *END STEP

2.1.6 Modeling of an automobile suspension Product: ABAQUS/Standard This example illustrates the use of JOINTC elements. It is repeated to illustrate the use of connector elements. JOINTC elements (``Flexible joint element,'' Section 17.4.1 of the ABAQUS/Standard User's Manual) can be used to model the interaction between two nodes that are almost coincident geometrically and that represent a joint that has internal stiffness and/or damping. The behavior of the joint is defined in a local coordinate system, defined by an *ORIENTATION option (``Orientations,'' Section 2.2.4 of the ABAQUS/Standard User's Manual). This system rotates with the motion of the first node of the element and may consist of linear or nonlinear springs and dashpots arranged in parallel, coupling the corresponding components of relative displacement and of relative rotation in the

2-779

Dynamic Stress/Displacement Analyses

joint. This feature can be used to model, for example, a rubber bearing in a car suspension. In the connector element model the JOINTC elements are replaced by connector elements (see ``Connectors,'' Section 17.1.1 of the ABAQUS/Standard User's Manual) with connection types CARTESIAN to define the translational behavior and ROTATION to define the rotational behavior. These connection types allow linear or nonlinear spring and dashpot behavior to be defined in a local coordinate system that rotates with the first node on the element. Several different connection types can be used to model the finite rotational response. See ``Connection-type library,'' Section 17.1.3 of the ABAQUS/Standard User's Manual, for connection types using different finite rotation parametrizations. In this model the rotation magnitudes are assumed small. Hence, a rotation vector parametrization of the joint using ROTATION is appropriate. The primary objective of this example is to verify the accuracy of JOINTC and connector elements in a structure undergoing rigid rotation motions. A secondary objective of this example is to demonstrate the use of equivalent rigid body motion output variables in ABAQUS/Standard.

Geometry and model The structure analyzed is an automobile's left front suspension subassembly (see Figure 2.1.6-1). The physical components included in the assemblage are the tire, the wheel, the axle (hub), the A-arm (wishbone), the coil spring, and the frame. The tire is modeled with a JOINTC or connector element; a curved bar element has been attached for visualization. (The JOINTC or connector element is used because it is a convenient way of defining the tire's nonlinear stiffness in a local coordinate system.) The vertical stiffness of the wheel is represented by a beam element. The axle and A-arm are both modeled with beam elements. The axle is connected to the A-arm by a pin-type MPC in the JOINTC model or with connection type JOIN in the connector model. The coil spring is modeled by a SPRINGA element in the JOINTC model or with connection type AXIAL in the connector model. The automobile frame is represented by a MASS element. The top of the coil spring is connected directly to the frame, while the A-arm is connected to the frame by two JOINTC elements or two connector elements with connection types CARTESIAN and ROTATION (representing the A-arm bushings). The initial position represents a fully weighted vehicle, and the tire and coil spring have a corresponding initial preload. The first step in the analysis allows the suspension system to reach equilibrium. The second step models the tire moving over a bump in the road. The bump is idealized as a triangular shape 100 mm high by 400 mm long, and the vehicle is assumed to travel at 5 km/hr. A second input file is used to show the effects of large rotation on the suspension response. This file includes an initial rotation step, which rigidly rotates the model by 90° about the vertical axis but is otherwise identical to the first input file. We expect the response from the two analyses to be the same. In this example we are primarily interested in the equivalent rigid body motion of the A-arm and, in particular, in the average displacement and rotation.

Results and discussion The results from the connector element models are qualitatively and quantitatively equivalent to the JOINTC models. Hence, only the JOINTC results are discussed further.

2-780

Dynamic Stress/Displacement Analyses

The vertical displacement histories in Step 2 are shown in Figure 2.1.6-2for the contact point of the tire with the ground, the wheel center, and the frame. Figure 2.1.6-3 shows a series of overlaid displaced plots as the tire rolls up the bump. To verify the behavior of the JOINTC elements with large rotations, the second model rigidly rotates the entire structure by 90° before applying the bump excitation. Figure 2.1.6-4shows the displacement time histories from the two models overlaid on the same plot. They are nearly identical. In the analysis of deformable bodies undergoing large motions it is convenient to obtain information about the equivalent rigid body motions: average displacement and rotation, as well as linear and angular momentum about the center of mass. For this purpose ABAQUS provides a set of equivalent rigid body output variables. As indicated above, a secondary objective of this example is to demonstrate the use of these output variables, which represent the average motion of the specified element set. The variables are requested using the *EL PRINT and *EL FILE commands. If no element set is specified, the average motion of the entire model is given. This type of output can only be requested in a *DYNAMIC analysis, and only elements that have a mass will contribute to the equivalent rigid body motion. For a precise definition of the equivalent rigid body motion of a deformable body, see ``Equivalent rigid body dynamic motion,'' Section 2.4.4 of the ABAQUS Theory Manual. Figure 2.1.6-5 and Figure 2.1.6-6have been generated using the equivalent rigid body output variables. Figure 2.1.6-5 shows the vertical motion of node 5001 (bearing point "A" of the A-arm), node 5080 (point of A-arm nearest the tire), and the average vertical motion of the A-arm (output variable UC3). As expected, the displacement of the center of mass of the component lies between the displacements of its two ends. Figure 2.1.6-6shows the average rigid body rotation of the A-arm component about its center of mass. Rigid body rotations are available about the three global axes. Here we are interested in the rotation about the global X-axis (output variable URC1). The standard output for rotations is radians, but the results have been scaled to plot the rotation in degrees.

Input files jointcautosuspension.inp Suspension analysis with JOINTC elements. jointcautosuspension_rotated.inp Rotated suspension analysis with JOINTC elements. This input file includes one extra (rotation) step but is otherwise identical to jointcautosuspension.inp. jointcautosuspension_depend.inp Identical to jointcautosuspension.inp, except that field-variable-dependent linear and nonlinear spring properties are used in the JOINTC elements. connautosuspension.inp Suspension analysis with connector elements. connautosuspension_rotated.inp

2-781

Dynamic Stress/Displacement Analyses

Rotated suspension analysis with connector elements. This input file includes one extra (rotation) step but is otherwise identical to connautosuspension.inp. connautosuspension_depend.inp Identical to connautosuspension.inp, except that field-variable-dependent linear and nonlinear spring properties are used in the connector elements with connection types CARTESIAN, ROTATION, and AXIAL.

Figures Figure 2.1.6-1 Left front automobile suspension.

Figure 2.1.6-2 Displacement histories of tire, wheel center, and frame.

2-782

Dynamic Stress/Displacement Analyses

Figure 2.1.6-3 Displaced shapes during positive vertical tire motion.

Figure 2.1.6-4 Overlay of unrotated and rotated suspension analyses.

Figure 2.1.6-5 Vertical motion of the A-arm: average and nodal motions.

2-783

Dynamic Stress/Displacement Analyses

Figure 2.1.6-6 Average rotation of the A-arm about its center of mass.

Sample listings

2-784

Dynamic Stress/Displacement Analyses

Listing 2.1.6-1 *HEADING JOINTC ELEMENTS; MODELING AN AUTOMOBILE SUSPENSION *RESTART, WRITE, FREQUENCY=5 ** ** Auto suspension sub-assembly modeled in ** sprung condition. Coil spring and tire ** spring have initial preload as given by ** their respective spring load-deflection ** curves. Weight of frame (by gravity load) ** rests on the coil spring top and the two ** wishbone bearing (pivot) points. ** ** FRAME ** ** Model frame as lumped mass at auto centerline *NODE, NSET=FRAME 1001, 0.00, 0.00, 0.00 *ELEMENT, TYPE=MASS, ELSET=FRAME 1001, 1001 ** Mass used is one quarter of total auto mass *MASS, ELSET=FRAME 0.423, *BOUNDARY 1001, 1,2, 0.0 1001, 4,6, 0.0 ** ** WHEEL ** ** 3001 is lower rim, 3002 is wheel center *NODE, NSET=WHEEL 3001, 0.00, -779.50, -315.00 3002, 0.00, -779.50, 0.00 *ELEMENT, TYPE=B31, ELSET=WHEEL 3001, 3001, 3002 *BEAM SECTION, SECTION=CIRC, MATERIAL=STEEL, ELSET=WHEEL 24.0, 0.0, 1.0, 0.0 *BOUNDARY WHEEL, 6,6, 0.0

2-785

Dynamic Stress/Displacement Analyses

** ** TIRE ** *NODE, NSET=GROUND 2000, 0.00, 0.00, -335.00 *NODE, NSET=TIRE 2001, 0.00, -779.50, -335.00 2091, 167.50, -779.50, -290.11 2092, -167.50, -779.50, -290.11 *ORIENTATION, NAME=XYZ 1.0, 0.,0.,0.,1.,0. 3, 0.0 *ELEMENT, TYPE=JOINTC, ELSET=TIRE 2001, 3001, 2001 *JOINT, ELSET=TIRE, ORIENTATION=XYZ *SPRING 1, 175., *SPRING 2, 175., *SPRING, NONLINEAR 3, -10000., -24.21 0., -19.21 4150., 0.00 10630., 30.00 ** for visualization only *ELEMENT, TYPE=T3D3, ELSET=PLOTA 2091, 2091, 2001, 2092 *SOLID SECTION, MATERIAL=STEEL, ELSET=PLOTA 0.0005, *MPC BEAM, 2091, 2001 BEAM, 2092, 2001 ** ** Tie bottom of tire to ground (makes global ** rotation possible) *MPC BEAM, 2001, 2000 ** ** AXLE **

2-786

Dynamic Stress/Displacement Analyses

*NODE, NSET=AXLE 4001, 0.00, -705.30, 0.00 4002, 0.00, -736.30, 0.00 4003, 2.56, -750.00, -116.00 4004, 152.00, -695.61, -13.81 4005, 152.00, -695.61, -13.81 *ELEMENT, TYPE=B31, ELSET=AXLE1 4020, 3002, 4001 4021, 4001, 4002 *BEAM SECTION, SECTION=CIRC, MATERIAL=STEEL, ELSET=AXLE1 13.0, *ELEMENT, TYPE=B31, ELSET=AXLE2 4022, 4002, 4003 *BEAM SECTION, SECTION=CIRC, MATERIAL=STEEL, ELSET=AXLE2 15.0, 1.0, 0.0, 0.0 *ELEMENT, TYPE=B31, ELSET=AXLE3 4023, 4002, 4004 *BEAM GENERAL SECTION, SECTION=GENERAL, ELSET=AXLE3, DENSITY=7.8E-9 391.0, 17000.0, 0.0, 9400.0,22600.0 0.0, 0.0, -1.0 2.1E+05, 8.077E+04 *BOUNDARY AXLE, 5,5, 0.0 ** ** WISHBONE ** *NODE, NSET=WBONE 5001, -73.00, -351.00, -90.00 5002, 325.00, -351.00, -90.00 5011, -17.00, -540.00, -128.00 5012, -73.00, -398.60, -110.70 5013, 325.00, -398.60, -110.70 5080, 2.56, -750.00, -116.00 *ELEMENT, TYPE=B31, ELSET=WB1 5001, 5080, 5011 5002, 5011, 5012 5003, 5011, 5013 *BEAM GENERAL SECTION, SECTION=GENERAL, ELSET=WB1, DENSITY=7.8E-9

2-787

Dynamic Stress/Displacement Analyses

542.0, 449591.0, 0.0, 196281.0, 639175.0 0.0, 0.0, -1.0 2.1E+05, 8.077E+04 *ELEMENT, TYPE=B31, ELSET=WB2 5033, 5012, 5001 5034, 5013, 5002 *BEAM GENERAL SECTION, SECTION=GENERAL, ELSET=WB2, DENSITY=7.8E-9 342.0, 81077.0, 0.0, 81077.0, 162155.0 0.0, 0.0, -1.0 2.1E+05, 8.077E+04 *ELEMENT, TYPE=B31, ELSET=WB3 5035, 5012, 5013 *BEAM SECTION, SECTION=CIRC, MATERIAL=STEEL, ELSET=WB3 13.0, ** *ELSET, ELSET=WBONE WB1, WB2, WB3 ** Pin axle and wishbone together *MPC PIN, 4003, 5080 ** ** COIL SPRING ** *NODE, NSET=CTOP 6001, -8.50, -514.00, 214.00 *ELEMENT, TYPE=SPRINGA, ELSET=CSPRG 6001, 5011, 6001 *SPRING, ELSET=CSPRG, NONLINEAR -13600.0, -100.00 -8900.0, 0.00 -4600.0, 100.00 ** Tie top of spring to frame *MPC BEAM, 6001, 1001 ** for visualization only *ELEMENT, TYPE=T3D2, ELSET=PLOTB 6091, 5011, 6001 *SOLID SECTION, MATERIAL=STEEL, ELSET=PLOTB 0.0005, **

2-788

Dynamic Stress/Displacement Analyses

** BEARING POINT A ** *NODE, NSET=A-PVT 7001, -73.00, -351.00, -90.00 *ELEMENT, TYPE=JOINTC, ELSET=APVT 7001, 7001, 5001 ** Tie fixed side of jointc to frame *MPC BEAM, 7001, 1001 *JOINT, ELSET=APVT, ORIENTATION=XYZ *SPRING, NONLINEAR 1, -16000.0, -4.8 -10000.0, -3.8 -6000.0, -2.6 -3000.0, -1.1 0.0, 0.0 3000.0, 1.1 6000.0, 2.6 10000.0, 3.8 16000.0, 4.8 *SPRING, NONLINEAR 2, -10000.0, -1.80 -6000.0, -1.25 -2000.0, -0.53 0.0, 0.00 2000.0, 0.53 6000.0, 1.25 10000.0, 1.80 *SPRING, NONLINEAR 3, -10000.0, -2.40 -5000.0, -1.45 -2000.0, -0.68 0.0, 0.00 2000.0, 0.68 5000.0, 1.45 10000.0, 2.40 *SPRING 4, 1.142E5, *SPRING

2-789

Dynamic Stress/Displacement Analyses

5, 2.8568E6, *SPRING 6, 2.8568E6, ** ** BEARING POINT B ** *NODE, NSET=B-PVT 7002, 325.00, -351.00, -90.00 *ELEMENT, TYPE=JOINTC, ELSET=BPVT 7002, 7002, 5002 ** Tie fixed side of jointc to frame *MPC BEAM, 7002, 1001 *JOINT, ELSET=BPVT, ORIENTATION=XYZ *SPRING, NONLINEAR 1, -1600.0, -6.00 -1000.0, -2.50 -700.0, -1.50 -500.0, -1.00 -300.0, -0.50 0.0, 0.00 300.0, 0.50 500.0, 1.00 700.0, 1.50 1000.0, 2.50 1600.0, 6.00 *SPRING, NONLINEAR 2, -6800.0, -4.00 -4800.0, -3.75 -3600.0, -3.50 -2800.0, -3.25 -1700.0, -2.75 -1000.0, -2.25 -700.0, -1.75 0.0, 0.00 700.0, 1.75 1000.0, 2.25 1700.0, 2.75 2800.0, 3.25

2-790

Dynamic Stress/Displacement Analyses

3600.0, 3.50 4800.0, 3.75 6800.0, 4.00 *SPRING,NONLINEAR 3, -6400.0, -2.00 -5200.0, -1.75 -4160.0, -1.50 -2400.0, -1.00 1000.0, 0.00 4400.0, 1.00 6160.0, 1.50 7200.0, 1.75 8400.0, 2.00 *SPRING 4, 4.3082E4, *SPRING 5, 1.1467E6, *SPRING 6, 3.1311E5, ** *MATERIAL, NAME=STEEL *ELASTIC 2.1E+05,0.3 *DENSITY 7.8E-9, *ELSET, ELSET=ALL 1001, ** ** Idealized triangular speed bump 400mm long ** and 100mm high. Time data based on 5km/hr ** auto speed *AMPLITUDE, NAME=BUMP, TIME=STEP TIME 0.0, 0.0, 0.05, 0.0, 0.20, 100.0, 0.35, 0.0 0.40, 0.0 ** ** *STEP, NLGEOM, INC=100 Auto Weight/Tire Compression/Coil spring Equilibrium

2-791

Dynamic Stress/Displacement Analyses

*STATIC 0.2, 0.2 *BOUNDARY 2000, 1,6, 0.0 *DLOAD ALL, GRAV, 9815.0, 0.0, 0.0, -1.0 *EL PRINT,FREQUENCY=0 *NODE PRINT,FREQUENCY=0 *NSET, NSET=PLOT 2000, 3002, 1001 *NODE FILE, NSET=PLOT U, *END STEP ** ** *STEP, NLGEOM, INC=200 Apply "bump" to tire bottom with boundary condition *DYNAMIC, HAFTOL=5000 5.0E-4, 0.40, , 0.01 *BOUNDARY, AMPLITUDE=BUMP 2000, 3,3, 1.0 *EL FILE, ELSET=WBONE XC, UC, VC, HC, HO, RI, MASS, VOL *END STEP

2.1.7 Explosive pipe closure Product: ABAQUS/Explicit This problem illustrates the following concepts: large deformation kinematics, equations of state, elastic-plastic material, transformations, detonation points.

Problem description The units used in this analysis are referred to as c.g. ¹sec. Using these units, length is given in centimeters (cm), mass in grams (gm), and time is measured in microseconds (¹sec). The stresses have units of mega bars (M bar). These units are commonly used in shock wave physics applications because the pressures tend to have values on the order of unity.

2-792

Dynamic Stress/Displacement Analyses

In this example problem two concentric pipes have the annulus between them filled with high explosive (HE). The inside radius of the inner pipe is 10 mm. The inside radius of the outer pipe is 20 mm. Both pipes are steel with a wall thickness of 2 mm. Each pipe is modeled with 6 elements in the radial direction, while the HE is modeled with 24 elements in the radial direction. The steel pipe is an elastic, perfectly plastic material with Young's modulus of 221.1 GPa (.02211 M bar), Poisson's ratio of 0.279, yield strength of 430 MPa (.0043 M bar), and density of 7846 kg/m2 (7.846 gm/cm3). The explosive material is modeled using the JWL equation of state with detonation wave speed = 7596 m/sec (.7596 cm/microsecond), A = 520.6 GPa (5.206 M bar), B = 5.3 GPa (0.053 M bar), R1 = 4.1, R2 = 1.2, !=.35, density of 1900 kg/m3 (1.9 gm/cm3), and initial specific energy of 3.63 Joule/kg (0.0363 T erg/gm). The tension cutoff pressure is assumed to be zero and is specified using the *TENSILE FAILURE option. Refer to ``Equation of state,'' Section 9.5.1 of the ABAQUS/Explicit User's Manual, for a description of this material model. The explosive material is detonated at four points around the circumference of the cylinder. Because of the symmetry in this problem, only one-eighth of the pipe is modeled. Figure 2.1.7-1 shows the original geometry and the location of the detonation point for the model. A transformed coordinate system is used to define the symmetry conditions along the sloping boundary. This analysis is run in two steps to reduce the amount of output written to the restart file. In the early part of the analysis, the deformations are not of much interest. Hence, the first step has a duration of 6 ¹sec and requests only 1 restart interval (*RESTART, WRITE, NUMBER INTERVAL=1). After 6 ¹sec the deformations are becoming significant. The second step has a duration of 1.5 ¹sec and requests 3 restart intervals (*RESTART, WRITE, NUMBER INTERVAL=3). This analysis is run as both a two-dimensional case using CPE4R elements and as a three-dimensional case using C3D8R elements. In the three-dimensional case the displacements are constrained to be zero in the out-of-plane direction.

Results and discussion Figure 2.1.7-2 through Figure 2.1.7-5show a sequence of the deformed shapes computed by ABAQUS/Explicit for the two-dimensional case. Although not shown here, the results of the three-dimensional analysis are indistinguishable from those of the two-dimensional analysis. This problem tests the features listed, but it does not provide independent verification of them.

Input files eoscyl2d.inp Two-dimensional case. eoscyl3d.inp Three-dimensional case.

Figures 2-793

Dynamic Stress/Displacement Analyses

Figure 2.1.7-1 Original geometry.

Figure 2.1.7-2 Deformed configuration after 6.0 ¹sec.

Figure 2.1.7-3 Deformed configuration after 6.5 ¹sec.

2-794

Dynamic Stress/Displacement Analyses

Figure 2.1.7-4 Deformed configuration after 7.0 ¹sec.

Figure 2.1.7-5 Deformed configuration after 7.5 ¹sec.

2-795

Dynamic Stress/Displacement Analyses

Sample listings

2-796

Dynamic Stress/Displacement Analyses

Listing 2.1.7-1 *HEADING EXPLOSIVE PIPE CLOSURE *NODE 1,1.0,0. 7,1.2,0. 31,2.0,0. 37,2.2,0. 3001, .707107, .707107 3007, .848528, .848528 3031,1.414213,1.414213 3037,1.555634,1.555634 *NGEN,LINE=C,NSET=A 1,3001,100,,0.,0.,0. *NGEN,LINE=C,NSET=B 7,3007,100,,0.,0.,0. *NGEN,LINE=C,NSET=C 31,3031,100,,0.,0.,0. *NGEN,LINE=C,NSET=D 37,3037,100,,0.,0.,0. *NFILL A,B,6,1 B,C,24,1 C,D,6,1 *NSET,NSET=XAXIS,GEN 1,37,1 *NSET,NSET=TAXIS,GEN 3001,3037,1 *TRANSFORM,NSET=TAXIS .707107,.707107,0., -.707107,.707107,0. *ELEMENT,TYPE=CPE4R,ELSET=PIPE 1, 1, 2,102,101 901,31,32,132,131 *ELGEN,ELSET=PIPE 1, 6,1,1, 30,100,6 901, 6,1,1, 30,100,6 *SOLID SECTION,ELSET=PIPE,MATERIAL=STEEL *ELEMENT,TYPE=CPE4R,ELSET=HE 181, 7,8,108,107 *ELGEN,ELSET=HE 181, 24,1,1, 30,100,24 *SOLID SECTION,ELSET=HE,MATERIAL=HE

2-797

Dynamic Stress/Displacement Analyses

*MATERIAL,NAME=STEEL *DENSITY 7.846, *ELASTIC 2.211E-2,.279 *PLASTIC .0043,0. *MATERIAL,NAME=HE *DENSITY 1.9, *EOS,TYPE=JWL 0.7596,5.206,.053,.35,4.1,1.2,3.63E-2 *DETONATION POINT 1.414213,1.414213,0.,0. *TENSILE FAILURE,ELEMENT DELETION=NO, PRESSURE=BRITTLE,SHEAR=BRITTLE 0., ** *BOUNDARY XAXIS,YSYMM TAXIS,YSYMM *STEP *DYNAMIC,EXPLICIT ,2. *RESTART,TIMEMARKS=YES,WRITE,NUM=1 *FILE OUTPUT,NUMBER INTERVAL=2, TIMEMARKS=YES *EL FILE PRESS,S,LE *NODE FILE U, *ENERGY FILE *HISTORY OUTPUT,TIME=2.0E-3 *ENERGY HISTORY ALLKE,ALLIE,ALLSE,ALLAE,ALLVD,ALLCD,ALLPD, ALLFD,ALLWK,ETOTAL,DT *END STEP *STEP *DYNAMIC,EXPLICIT ,0.4 *RESTART,TIMEMARKS=YES,WRITE,NUM=3 *FILE OUTPUT,NUM=2, TIMEMARKS=YES *EL FILE PRESS,S,LE

2-798

Dynamic Stress/Displacement Analyses

*NODE FILE U, *ENERGY FILE *HISTORY OUTPUT,TIME=0.4E-3 *ENERGY HISTORY ALLKE,ALLIE,ALLSE,ALLAE,ALLVD,ALLCD,ALLPD, ALLFD,ALLWK,ETOTAL,DT *END STEP

2.1.8 Knee bolster impact with double-sided surface contact Product: ABAQUS/Explicit This example illustrates the use of the double-sided surface contact capability in a simulation involving large relative motion between potentially contacting surfaces. Double-sided surface contact is required because large deformations during the course of the analysis cause several slave nodes to displace around and then behind their originally opposing master surfaces.

Problem description This model represents an automobile knee bolster assembly--the portion of the instrument panel that the occupant's legs impact in the event of a crash. The assembly consists of a hard plastic cover (the knee bolster) supported by a stiff steel substructure. Proper design of this assembly ensures that the occupant's energy is dissipated with a minimum of injury causing forces. In this simulation the legs approach the knee bolster at 6 m/s, representing unrestrained motion following a 15 mph to dead stop crash event. The components of the instrument panel are modeled using S3R and S4R shell elements. The bolster is made up of 2690 shell elements, with the material modeled as a von Mises elastic strain hardening plastic material with a Young's modulus of 2.346 GPa, a Poisson's ratio of 0.4, a density of 1140 kg/m3, and a yield stress of 11.7 MPa. The steel substructure is made up of 1648 elements, with the material modeled as a strain hardening steel with a Young's modulus of 207 GPa, a Poisson's ratio of 0.3, a density of 7700 kg/m3, and a yield stress of 207 MPa. Contact between the instrument panel assembly components is modeled by defining double-sided surfaces on 2536 shell elements in the bolster and on 213 shell elements on the steel substructure. Figure 2.1.8-1 shows the model geometry from the rear of the knee bolster prior to impact, and Figure 2.1.8-2shows where a double-sided surface definition is needed because of large motions of the bolster structure. Figure 2.1.8-3 shows the knee bolster and knee/leg assembly from a position outboard and behind the driver prior to impact. The legs are represented as structural members with a surrounding rigid surface. The structural members, representing the bones, are modeled with B31 beam elements and T3D2 truss elements, with the material modeled as elastic with a Young's modulus of 207 GPa, a Poisson's ratio of 0.3, and a density of 7.7 kg/m3. The rigid surfaces, representing the knee and shin, are modeled with R3D4 rigid elements. A single-sided surface definition is used in this case. The body mass is modeled by distributing mass elements at various locations among the nodes of the structural elements. Contact between the legs and the instrument panel is defined using node-based surfaces on the bolster and rigid

2-799

Dynamic Stress/Displacement Analyses

surfaces to represent the knees and shins. Initial velocities are defined on the leg components to approximate a 15 mph (6 m/s) crash condition. The hips are constrained to translate in the plane of the seat. The ankles are constrained consistent with fixed planting of the feet on the floor of the car. The dashboard substructure is fixed at locations where it would be welded to the automobile frame; deformations due to this impact are assumed to be confined to the explicitly modeled structure.

Results and discussion Figure 2.1.8-4 shows the deformed shape of the bolster assembly after 30.0 ms. This analysis would not be possible with single-sided surfaces because nodes move around the edge of the steel structure and shift from the positive side of the surface to the negative side as the surfaces deform. Such motions are allowed with double-sided surfaces but not with single-sided surfaces. Figure 2.1.8-5 shows the energy time history of the whole model: internal energy, kinetic energy, recoverable strain energy, and plastic dissipation. This figure shows that roughly one-half of the body's initial kinetic energy has been transferred by the end of this simulation. Of this transferred amount roughly one-quarter has been transferred to elastic deformations in the instrument panel structure and bones, and the balance is lost to plastic dissipation; the crash event cannot be considered complete at 30 ms. Figure 2.1.8-6 shows the total knee and shin contact forces measured against the displacement into the bolster. Consistent with the observations of the energy quantities, it is not clear that these forces have peaked or that the crash event is complete.

Acknowledgment HKS would like to thank GE Plastics for supplying the model used in this example.

Input files knee_bolster.inp Input data for this analysis. knee_bolster_ef1.inp External file referenced by this analysis. knee_bolster_ef2.inp External file referenced by this analysis. knee_bolster_ef3.inp External file referenced by this analysis.

Figures

2-800

Dynamic Stress/Displacement Analyses

Figure 2.1.8-1 Initial configuration of the knee bolster model (view from behind the bolster).

Figure 2.1.8-2 Location of node that moves from initially opposing one side of a shell element in the steel substructure to opposing the opposite side following large deformation of the bolster structure.

Figure 2.1.8-3 Initial configuration of the knee bolster model (view from outboard and behind the driver).

2-801

Dynamic Stress/Displacement Analyses

Figure 2.1.8-4 Deformed shape after 30 ms.

Figure 2.1.8-5 Time histories of the whole model: internal energy, kinetic energy, recoverable strain energy, and plastic dissipation.

2-802

Dynamic Stress/Displacement Analyses

Figure 2.1.8-6 Front leg reaction forces measured against impact displacement.

Sample listings

2-803

Dynamic Stress/Displacement Analyses

Listing 2.1.8-1 *HEADING KNEE BOLSTER IMPACT SIMULATION ** **This example simulates the impact of a knee **and leg structure into a knee bolster assembly ** ** READ NODE AND NODE SET DEFINITIONS ** FROM EXTERNAL FILE: *INCLUDE,INPUT=knee_bolster_ef1.inp ** ** READ ELEMENT AND ELSET DEFINITIONS ** FROM EXTERNAL FILE: *INCLUDE,INPUT=knee_bolster_ef2.inp ** ** Material definitions ** *MATERIAL, NAME=STEEL *DENSITY 7.7E-09, *ELASTIC, TYPE=ISO 207000.0, 0.3 *PLASTIC 207.0, 0.0 276.0, 0.22 ** *MATERIAL, NAME=BONE *DENSITY 7.7E-12, *ELASTIC, TYPE=ISO 207000.0, 0.3 ** *MATERIAL,NAME=MC8002 *ELASTIC .2346E+04, .4000 *PLASTIC 11.7, 0.00 32.8, 0.00114 47.0, 0.0052 53.5, 0.0227 *DENSITY 1.14E-09,

2-804

Dynamic Stress/Displacement Analyses

** *SHELL SECTION,ELSET=STEEL ,MATERIAL=STEEL 1.50000, 5 *SHELL SECTION,ELSET=TOPBRKT ,MATERIAL=STEEL 1.50000, 5 *SHELL SECTION,ELSET=FLRBRKT ,MATERIAL=STEEL 1.50000, 5 *SHELL SECTION,ELSET=SDBRKT ,MATERIAL=STEEL 1.50000, 5 *SHELL SECTION,ELSET=FRONT ,MATERIAL=MC8002 3.00000, 5 *SHELL SECTION,ELSET=CORR ,MATERIAL=MC8002 2.50000, 5 *SHELL SECTION,ELSET=RIBS ,MATERIAL=MC8002 1.88000, 5 ** ** READ BOUNDARY CONDITION DEFINITIONS ** FROM EXTERNAL FILE: *INCLUDE,INPUT=knee_bolster_ef3.inp ** *MPC BEAM, 6447, 3253 BEAM, 6264, 2540 BEAM, 6366, 2555 ** ** Below are beam elements for lower torso. ** *BEAM SECTION,ELSET=TIBCHK,MATERIAL=BONE, SECTION=CIRC 25.4, *ELEMENT,TYPE=B31,ELSET=TIBCHK ** Left Tibia 8000, 9000, 9001 ** Right Tibia 8100, 9100, 9101 ** Left Hip 8400, 9200, 9400 ** Right Hip 8500, 9400, 9300 *SOLID SECTION,ELSET=FEMUR,MATERIAL=BONE 2027.0, *ELEMENT, TYPE=T3D2,ELSET=FEMUR ** Left Femur

2-805

Dynamic Stress/Displacement Analyses

8200, 9200, 9001 ** Right Femur 8300, 9300, 9101 ** ** ** Initial Conditions and Definitions. ** ** *MASS,ELSET=WT .0082, ** ** Left Shin ** *NSET, NSET=LSHIN, GENERATE 8000, 8121, 1 *ELEMENT,TYPE=MASS,ELSET=WT 10000, 9001 *NSET,NSET=LKNE 9001, *NSET, NSET=RSHIN, GENERATE 8200, 8321, 1 *ELEMENT,TYPE=MASS,ELSET=WT 10001, 9101 *NSET,NSET=RKNE 9101, *NSET,NSET=KNEES 9001, 9101 *INITIAL CONDITIONS,TYPE=VELOCITY KNEES, 1, -5364.48 KNEES, 3, 2839.18 KNEES, 5, -14.1725 ** ** Left hip mass ** *NSET,NSET=M3 9200, *ELEMENT,TYPE=MASS,ELSET=WT 10002, 9200 *BOUNDARY M3, 3, , 0. *INITIAL CONDITIONS, TYPE=VELOCITY M3, 1, -6593.58 **

2-806

Dynamic Stress/Displacement Analyses

** Center mass ** *NSET,NSET=M4 9400, *ELEMENT,TYPE=MASS,ELSET=WT 10003, 9400 *BOUNDARY M4, 2, 3, 0. *INITIAL CONDITIONS, TYPE=VELOCITY M4, 1, -6593.58 ** ** Right torso mass ** *NSET,NSET=M5 9300, *ELEMENT,TYPE=MASS,ELSET=WT 10004, 9300 *BOUNDARY M5, 3,, 0. *INITIAL CONDITIONS, TYPE=VELOCITY M5, 1, -6593.58 ** ** Ankles ** *NSET,NSET=ANKLE 9000, 9100 *TRANSFORM,NSET=ANKLE 142.200, 0.0, 393.900, 0.0, 100.0, 0.0 *BOUNDARY ANKLE, 1,3, 0.0 ANKLE, 4,, 0.0 *INITIAL CONDITIONS,TYPE=VELOCITY ANKLE, 5, -14.1725 ** ** History Section ** *RESTART,WRITE,NUMBER INTERVAL=30 *SURFACE,TYPE=NODE,NAME=LNODE LNODE, *SURFACE,TYPE=ELEMENT, NAME=RMETAL RMETAL, *SURFACE,TYPE=ELEMENT, NAME=CORR CORR,

2-807

Dynamic Stress/Displacement Analyses

*SURFACE,TYPE=ELEMENT,NAME=LK LKSHIN2,SPOS *SURFACE,TYPE=NODE,NAME=RNODE RNODE, *SURFACE,TYPE=ELEMENT, NAME=FRONT FRONT, *SURFACE,TYPE=ELEMENT,NAME=RK RKSHIN2,SPOS *SURFACE,TYPE=ELEMENT, NAME=LMETAL LMETAL, *RIGID BODY,ELSET=LKSHIN2,REF NODE=9001 *RIGID BODY,ELSET=RKSHIN2,REF NODE=9101 *STEP *DYNAMIC, EXPLICIT ,.030 *CONTACT CONTROLS,GLOBTRKINC=1000,CPSET=CPAIR ** *FILE OUTPUT, NUMBER INTERVAL = 2 *EL FILE, ELSET = FRONT S, *ENERGY FILE ALLIE, ALLKE, ETOTAL, ALLWK, ALLAE, ALLSE, ALLPD *NODE FILE, NSET = KNEES U,V *NODE FILE, NSET = M3 U,V *NODE FILE, NSET = M4 U,V *NODE FILE, NSET = M5 U,V ** ** Surface Definition ** *CONTACT PAIR, INTERACTION=FRIC,CPSET=CPAIR LK, LNODE RK, RNODE ** FRONT, CORR FRONT, RMETAL FRONT, LMETAL CORR, RMETAL CORR, LMETAL **

2-808

Dynamic Stress/Displacement Analyses

*SURFACE INTERACTION, NAME=FRIC *FRICTION 0.2, ** ** Output ** *HISTORY OUTPUT,TIME=0.0001 RF,BONDSTAT,BONDLOAD *NODE HISTORY,NSET=LSHIN RF, *NODE HISTORY,NSET=RSHIN RF, *NODE HISTORY,NSET=LKNE U,V,A *NODE HISTORY,NSET=RKNE U,V,A *NODE HISTORY,NSET=M4 U,V,A *ENERGY HISTORY ALLIE, ALLKE, ETOTAL, ALLWK, ALLAE, ALLSE, ALLPD *MONITOR, NODE=9400,DOF=1 *ENDSTEP

2.1.9 Cask drop with foam impact limiter Product: ABAQUS/Explicit A containment cask is partially filled with fluid and a foam impact limiter. The complete package is dropped a distance of 9.09 m (30 ft) onto a rigid surface, which results in an impact speed of 13.35 m/sec (525.3 in/sec). The problem illustrates the use of an initial velocity condition and the analysis of a structure containing liquid and incorporating crushable foam to absorb impact energy. Experimental and numerical results for this problem have been reported by Sauvé et al. (1993). The numerical results given in the reference were obtained using a relatively coarse finite element mesh. In this example results are presented for the same coarse mesh as the reference and also for a more refined mesh.

Model description The containment cask shown in Figure 2.1.9-2consists of two compartments. The upper compartment surrounds the fluid and is made of stainless steel ( 304L). It has a height of 580 mm (22.8 in), a diameter of 300 mm (11.8 in), and a wall thickness of 4.76 mm (0.187 in). The top mild steel cover has a thickness of 9.52 mm (0.375 in). The water is filled to a depth of 522 mm (20.55 in), which is 90% of the container's capacity. Figure 2.1.9-3shows the original, coarse mesh of C3D8R elements used to model the fluid. Contact conditions are defined between the fluid and the inside of the upper compartment.

2-809

Dynamic Stress/Displacement Analyses

An impact limiter made of polyurethane foam is contained within the bottom mild steel compartment of the cask. The height of the foam impact limiter is 127.3 mm (5.01 in). Figure 2.1.9-4shows the coarse mesh used to model the foam. Contact conditions are defined between the foam and the inside of the bottom compartment of the cask. The foam impact limiter and the fluid/stainless steel liner are separated by a mild steel bulkhead with a thickness of 12.7 mm (0.5 in). A 12.7 mm (0.5 in) air gap exists between the top of the foam surface and this bulkhead. In the experiment a pressure transducer is located in the polyurethane foam on the centerline of the cask at the top of the impact limiter. This result is compared with vertical stress-time histories taken from the element at the top of the foam model on the centerline. Both axisymmetric and three-dimensional models are analyzed. Figure 2.1.9-5shows the three-dimensional model formed by assembling the parts shown in Figure 2.1.9-2through Figure 2.1.9-4. The equivalent axisymmetric model is shown in Figure 2.1.9-6. Contact pairs are defined between the solids and the shells. Element-based surfaces are defined on the shells, and node-based surfaces are defined containing the nodes on the outer surfaces of the solid elements. The shell thickness was not taken into account when the original meshes were designed, and the outer surface of the solids usually coincides with the midsurface of the enclosing shell. This would lead to an initial overclosure of one-half the shell thickness, unless the NO THICK parameter is used to enforce contact at the midsurface of the shell, as if it had zero thickness. The use of a node-based surface implies a pure master-slave relationship for the contact pair. This is important in this problem because the default in ABAQUS/Explicit when contact is defined between shells and solids is to define a pure master-slave relationship with the solids as the master and the shells as the slave. In this case the shell structures are much stiffer than the fluid and foam structures, so the master-slave roles must be reversed. For the axisymmetric model two cases using different section control options for the foam and fluid elements are analyzed. The first case uses the COMBINED hourglass control option; the second case uses the default section control options (the RELAX STIFFNESS hourglass control). The three-dimensional model also has two cases with different section control options for the foam and fluid elements. The first case uses the ORTHOGONAL kinematic option and COMBINED hourglass control; the second three-dimensional case uses the default section control options (the AVERAGE STRAIN kinematic option and the RELAX STIFFNESS hourglass control). The options used are summarized in Table 2.1.9-4. Coarse and refined meshes are used for all analysis cases.

Material description The general material properties are listed in Table 2.1.9-1. The material models for the water and foam are further described below. Water: The water is treated as a simple hydrodynamic material model. This provides zero shear strength and a bulk response given by p = K"vol ;

2-810

Dynamic Stress/Displacement Analyses

where K is the bulk modulus with a value 2068 MPa (300000 psi). This model is defined using the linear Us ¡ Up equation of state model provided in ABAQUS/Explicit. The linear Us ¡ Up Hugoniot form, p = f (½) + g (½)Em , is p=

½0 c20 ´ ¡0 ´ ) + ¡0 ½0 Em ; (1 ¡ 2 (1 ¡ s´) 2

where ´ = 1 ¡ ½0 =½ is the same as the nominal volumetric strain measure, "vol . Since K = ½0 c20 , setting the parameters s = 0:0 and ¡0 = 0:0 gives the simple hydrostatic bulk response defined earlier. In this analysis c0 = 1450.6 m/sec (57100 in/sec) and ½0 = 983.2 kg/m3 (0.92 ´ 10-4 lb sec2in-4). The tension cutoff pressure is assumed to be zero and is specified using the *TENSILE FAILURE option. Refer to ``Equation of state,'' Section 9.5.1 of the ABAQUS/Explicit User's Manual, for a description of this material model. Foam: The crushable foam model is used for the polyurethane foam. In this model the flow potential, h, is chosen as h=

r

9 2 p + q2 ; 2

where q is the Mises equivalent stress and p is the hydrostatic pressure. The yield surface is defined as "µ

¶2 ³ ´ # 12 pt ¡ pc q 2 pc + pt +p + = : 2 M 2 Sauvé et al. use the "soils and crushable foams" model, which was originally defined in an unpublished report by Krieg (1978) and is based upon a Mises plasticity model in which the yield stress depends upon the mean volumetric pressure. The volumetric deformation allows for plastic behavior, defined by tabular data defining pressure versus volume strain. This model is easy to implement in an explicit dynamics algorithm and useful because the deviatoric and volumetric terms are only loosely coupled. However, it requires an experienced analyst to ensure that meaningful results are obtained, mainly because the model does not match physical behavior well under deviatoric straining. To define the initial shape of the yield surface, the ABAQUS/Explicit crushable foam model requires the initial yield surface position, "pl vol j0 ; the initial yield stress in uniaxial compression, ¾0 ; and the magnitude of the strength in hydrostatic tension, pt . Sauvé et al. define the pressure-dependent yield surface for the foam model as ¾y2 = 3:18 + 2:06p;

2-811

Dynamic Stress/Displacement Analyses

where the units of stress are MPa and pressure is positive in compression. To calibrate the ABAQUS/Explicit crushable foam model to this pressure-dependent data, we observe that p = 13 ¾y for the uniaxial compression case. Substituting this value for p in the above equation and solving for ¾y gives ¾0 =2.16 MPa (313.3 psi). The value of pt is obtained by solving the above equation for ¾y = 0, giving pt = 1.54 MPa (223.8 psi). The value of "pl vol j0 is chosen to be zero because tensile experimental data are not given in the reference and the foam is almost always under hydrostatic compression. If the foam were subjected to triaxial tension, it would be necessary to define pressure-plastic volumetric strain data to account for strain softening, as discussed in ``Crushable foam plasticity model,'' Section 10.3.3 of the ABAQUS/Explicit User's Manual. The pressure/volumetric strain data in the reference are given in Table 2.1.9-2. Table 2.1.9-3shows the values as converted to the form required for ABAQUS/Explicit. Each form of the data is plotted in Figure 2.1.9-1.

Results and discussion The deformed geometries for the three-dimensional and the axisymmetric models at 5 msec are shown in Figure 2.1.9-7and Figure 2.1.9-8. The axisymmetric model is analyzed using COMBINED hourglass control. The three-dimensional model uses the ORTHOGONAL kinematics and COMBINED hourglass control. Figure 2.1.9-9 shows plots of the vertical stress versus time for the element located at the pressure transducer in the foam; results from the models with the previous section control options, as well as results from analyses using the default section control options, are reported for comparison (see Table 2.1.9-4). Axisymmetric and three-dimensional results are compared to the experimental pressure trace. The time origin of the experimental curve is not defined in the reference; therefore, the experimental curve is shifted so that the time when pressure in the transducer changes to a positive value is assumed to be the time at which impact occurs. The numerical pressure results show significant oscillations about the experimental results during the first 2 msec of the response. This is partly because the meshes are quite coarse and partly because pressure transducers in experiments exhibit inertia in their response and will not report sharp gradients in time. During the next 3 msec the numerical results correspond more closely with the experimental results. The analyses run with different section control options compare very well. A more refined three-dimensional mesh is shown in Figure 2.1.9-10. The refined axisymmetric model is the same model used in the r-z plane. The deformed geometries for these models are shown in Figure 2.1.9-11(using the ORTHOGONAL kinematics and COMBINED hourglass control) and Figure 2.1.9-12(using the COMBINED hourglass control). The vertical stress histories for the refined models are shown in Figure 2.1.9-13for the same options used for the coarse meshes (see Table 2.1.9-4). The numerical results show less oscillation about the experimental results than those obtained with the coarse mesh. They compare well with the experimental results during the following 3 msec of the response. In addition, Figure 2.1.9-11shows that the refined mesh eliminates much of the fluid's hourglass-like response due to its zero shear strength.

Input files

2-812

Dynamic Stress/Displacement Analyses

cask_drop_axi_cs.inp Coarse axisymmetric model using the COMBINED hourglass control. cask_drop_3d_ocs.inp Coarse three-dimensional model using the ORTHOGONAL kinematic and the COMBINED hourglass control. cask_drop_axi.inp Coarse axisymmetric mesh using the default section controls. cask_drop_3d.inp Coarse three-dimensional mesh using the default section controls. cask_drop_axi_r_cs.inp Refined axisymmetric model using the COMBINED hourglass control. cask_drop_3d_r_ocs.inp Refined three-dimensional model using the ORTHOGONAL kinematic and the COMBINED hourglass control. cask_drop_axi_r.inp Refined axisymmetric mesh using the default section controls. cask_drop_3d_r.inp Refined three-dimensional mesh using the default section controls.

References · Krieg, R. D., ``A Simple Constitutive Description for Soils and Crushable Foams ,'' SC-DR-72-0883, Sandia National Laboratories, Albuquerque, NM , 1978. · Sauvé, R. G., G. D. Morandin, and E. Nadeau, ``Impact Simulation of Liquid-Filled Containers Including Fluid-Structure Interaction,'' Journal of Pressure Vessel Technology, vol. 115, pp. 68-79, 1993.

Tables Table 2.1.9-1 Material properties. Properties A36

304L

8032 193. 1 0.28 206.

8032 193. 1 0.28 305.

Density, ½ (kg m-3) Young's modulus, E (GPa) Poisson's ratio, º Yield stress, ¾y0 (MPa)

Liqui d 983

Foa m 305 .129 0

2-813

Dynamic Stress/Displacement Analyses

8 Bulk modulus, K (GPa) Hardening modulus, Et (GPa)

4 2.07

0

1.52

Table 2.1.9-2 Pressure-volumetric strain data. ²v 0 .01 .02 .03 .04 .05 .06 p 0 2.7 4.1 5.1 5.5 5.8 6.2 (MPa) 6 4 7 2 6 1

.385 10.3 4

Table 2.1.9-3 Modified pressure-volumetric strain data. ²pv 0 .01 .02 .345 .44 .49 pc + pt (MPa) 7.0 7.4 7.7 11.8 20.8 40.8 6 0 5 9 5 4

.48 19.3 1

.51 84.2 8

.53 39.3 0

.55 82.7 4

2 5516 .

Table 2.1.9-4 Analysis options tested. Analysis Section Controls Kinematic Hourglass Label AXI n/a relax AXI CS n/a combined 3D average relax 3D OCS orthogonal combined

Figures Figure 2.1.9-1 Foam hardening curves.

Figure 2.1.9-2 Containment structure mesh in the three-dimensional model (coarse mesh).

2-814

Dynamic Stress/Displacement Analyses

Figure 2.1.9-3 Fluid mesh in the three-dimensional model (coarse mesh).

Figure 2.1.9-4 Foam mesh in the three-dimensional model (coarse mesh).

Figure 2.1.9-5 The complete three-dimensional model (coarse mesh).

2-815

Dynamic Stress/Displacement Analyses

Figure 2.1.9-6 Axisymmetric model (coarse mesh).

Figure 2.1.9-7 Three-dimensional deformed geometry using ORTHOGONAL element kinematics and COMBINED hourglass control (coarse mesh).

2-816

Dynamic Stress/Displacement Analyses

Figure 2.1.9-8 Axisymmetric deformed geometry using COMBINED hourglass control (coarse mesh).

Figure 2.1.9-9 Vertical stress history in the foam (coarse mesh).

Figure 2.1.9-10 Refined mesh for the three-dimensional model.

2-817

Dynamic Stress/Displacement Analyses

Figure 2.1.9-11 Three-dimensional deformed geometry using ORTHOGONAL element kinematics and COMBINED hourglass control (refined mesh).

Figure 2.1.9-12 Axisymmetric deformed geometry using COMBINED hourglass control (refined mesh).

2-818

Dynamic Stress/Displacement Analyses

Figure 2.1.9-13 Vertical stress history in the foam (refined mesh).

Sample listings

2-819

Dynamic Stress/Displacement Analyses

Listing 2.1.9-1 *HEADING CASK DROP PROBLEM AXISYMMETRIC MODEL (coarse mesh) SECTION CONTROLS USED (HOURGLASS=COMBINED) ** ** Create liner mesh ** *NODE,NSET=NSHE1 1, 0.0,28.3461 2, 2.3622,28.3461 3, 4.7244,28.3461 4, 7.0865,28.3461 5, 9.4487,28.3461 6, 11.8109,28.3461 7, 11.8109,27.1650 8, 11.8109,25.1965 9, 11.8109,23.2281 10, 11.8109,21.2596 11, 11.8109,19.2911 12, 11.8109,17.3226 13, 11.8109,15.3541 14, 11.8109,13.3857 15, 11.8109,11.4172 16,11.8109,9.4487 17,11.8109,8.4645 18,11.8109,7.4802 19,11.8109,6.4960 20,11.8109,5.5117 21,9.4487,5.5117 22,7.0865,5.5117 23,4.7244,5.5117 24,2.3622,5.5117 25, 0.0,5.5117 26,11.8109,4.4094 27,11.8109,3.3070 28,11.8109,2.2047 29,11.8109,1.1023 30,11.8109,0.0 31,9.4487,0.0 32,7.0865,0.0 33,4.7244,0.0

2-820

Dynamic Stress/Displacement Analyses

34,2.3622,0.0 35,0.0,0.0 *ELEMENT, TYPE=SAX1 1, 1,2 6, 6,7 20, 20,26 21, 26,27 30, 20,21 *ELGEN, ELSET=S1 1,5,1,1 *ELGEN, ELSET=S2 6,14,1,1 *ELGEN, ELSET=S3 30, 5,1,1 *ELSET,ELSET=S4 20, *ELGEN, ELSET=S4 21,9,1,1 *ELSET,ELSET=SSTEEL S1,S2,S3, *ELSET,ELSET=MSTEEL S4, ** ** Shell material definition ** *SHELL SECTION,MATERIAL=A2,ELSET=S1, SECTION INTEGRATION=GAUSS 0.3748,5 *SHELL SECTION,MATERIAL=A1,ELSET=S2, SECTION INTEGRATION=GAUSS 0.1874,5 *SHELL SECTION,MATERIAL=A2,ELSET=S3, SECTION INTEGRATION=GAUSS 0.5,5 *SHELL SECTION,MATERIAL=A2,ELSET=S4, SECTION INTEGRATION=GAUSS 0.0591,5 ** ** Stainless steel (304L) ** *MATERIAL,NAME=A1 *DENSITY 0.00075163,

2-821

Dynamic Stress/Displacement Analyses

*ELASTIC 28E6,0.28 *PLASTIC 44300.0,0. 66300.0,0.1 ** ** Mild steel (A36) ** *MATERIAL,NAME=A2 *DENSITY 0.00075163, *ELASTIC 28E6,0.28 *PLASTIC 30000.0,0. ** ** Create fluid mesh ** *NODE, NSET=WTOP 101, 0.0,26.0627 102, 2.36218,26.0627 103, 4.72436,26.0627 104, 7.08654,26.0627 105, 9.44872,26.0627 106, 11.8109,26.0627 *NODE, NSET=WMID 155, 0.0,9.2482 156, 2.36218,9.2482 157, 4.72436,9.2482 158, 7.08654,9.2482 159, 9.44872,9.2482 160, 11.8109,9.2482 *NODE, NSET=WBOT 179, 0.0,5.5117 180, 2.36218,5.5117 181, 4.72436,5.5117 182, 7.08654,5.5117 183, 9.44872,5.5117 184, 11.8109,5.5117 *NFILL,NSET=NWATER WTOP,WMID,9,6 *NFILL,NSET=NWATER WMID,WBOT,4,6

2-822

Dynamic Stress/Displacement Analyses

*ELEMENT, TYPE=CAX4R 101, 102,101,107,108 *ELGEN, ELSET=WATER 101, 5,1,1,13,6,5 *MATERIAL, NAME=MWATER *DENSITY 9.2E-5, *EOS, TYPE=USUP 57100.874,0.0,0.0 *TENSILE FAILURE,ELEMENT DELETION=NO, PRESSURE=BRITTLE,SHEAR=BRITTLE 0., *SOLID SECTION, ELSET=WATER, MATERIAL=MWATER, CONTROL=B *SECTION CONTROLS, HOURGLASS=COMBINED, NAME=B ** ** Create foam mesh ** *NODE, NSET=FTOP 201, 0.0,5.0117 202, 2.36218,5.0117 203, 4.72436,5.0117 204, 7.08654,5.0117 205, 9.44872,5.0117 206, 11.8109,5.0117 *NODE,NSET=FBOT 231, 0.0,0.0 232, 2.36218,0.0 233, 4.72436,0.0 234, 7.08654,0.0 235, 9.44872,0.0 236, 11.8109,0.0 *NFILL, NSET=NFOAM FTOP,FBOT,5,6 *ELEMENT, TYPE=CAX4R 201, 202,201,207,208 *ELGEN, ELSET=FOAM 201, 5,1,1,5,6,5 *MATERIAL, NAME=MFOAM *ELASTIC 18738,0.0 *DENSITY 2.85E-5,

2-823

Dynamic Stress/Displacement Analyses

*FOAM 0.0,223.84,313.35 *FOAM HARDENING 1023.84,0.00 1073.84,0.01 1123.84,0.02 1723.84,0.345 3023.84,0.44 5923.84,0.49 12223.84,0.51 8E5,2.00 *SOLID SECTION, ELSET=FOAM, MATERIAL=MFOAM, CONTROL=B ** ** Define fluid and foam contact node set ** *NSET, NSET=WCON1 101,102,103,104,105,106,112,118,124,130,136,142, 148,154,160,166,172,178,179,180,181,182,183,184 *NSET,NSET=FCON1 201,202,203,204,205,206,212,218,224,230,231,232, 233,234,235,236 ** ** Define boundary condition ** *NSET, NSET=FEND 30,31,32,33,34,35 *NSET, NSET=WAXI, GENERATE 101,179,6 *NSET, NSET=FAXI, GENERATE 201,231,6 *BOUNDARY FEND,2,2 35,XSYMM 25,XSYMM 1,XSYMM WAXI,XSYMM FAXI,XSYMM ** ** Define initial condition ** *NSET,NSET=NALL, GENERATE 1,29,1

2-824

Dynamic Stress/Displacement Analyses

101,184,1 201,236,1 *INITIAL CONDITIONS, TYPE=VELOCITY NALL, 2, -523.3 ** ** Define history output element set ** *ELSET,ELSET=FLUID 161, *ELSET,ELSET=SOLID 201, *ELSET,ELSET=MIDEL 161,201 *ELSET,ELSET=SHELL 22, *ELSET,ELSET=ELOUT MIDEL, SHELL, *NSET, NSET=NOUT 27,201 *RESTART, WRITE, NUM=1, TIMEMARKS=NO *SURFACE,TYPE=NODE,NAME=FCON1 FCON1, *SURFACE,TYPE=NODE,NAME=WCON1 WCON1, *SURFACE,TYPE=ELEMENT, NAME=SSIDE1, NO THICK S1,SNEG S2,SNEG S3,SNEG *SURFACE,TYPE=ELEMENT, NAME=SSIDE2, NO THICK S3,SPOS S4,SNEG *STEP *DYNAMIC, EXPLICIT ,0.005 *CONTACT PAIR SSIDE1,WCON1 *CONTACT PAIR SSIDE2,FCON1 *FILE OUTPUT, NUM=4, TIMEMARKS=NO *EL FILE, ELSET=FLUID PRESS, *EL FILE, ELSET=SOLID

2-825

Dynamic Stress/Displacement Analyses

PEEQ,PE,LE MISES,PRESS *EL FILE, ELSET=SHELL PEEQ,PE,LE MISES,PRESS SF,STH *NODE FILE, NSET=NOUT U,V *HISTORY OUTPUT,TIME=0.0 *ENERGY HISTORY ALLAE,ALLIE,ALLKE,ALLPD,ALLSE,ALLVD,ALLWK,ETOTAL *NODE HISTORY, NSET=NOUT U,V *EL HISTORY,ELSET=MIDEL S22,PEEQ,MISES,ERV *EL HISTORY,ELSET=ELOUT PRESS, *EL HISTORY,ELSET=SHELL SF,STH *EL HISTORY,ELSET=SHELL,SECTION POINT=1 S22,PEEQ,MISES *EL HISTORY,ELSET=SHELL,SECTION POINT=2 S22,PEEQ,MISES *EL HISTORY,ELSET=SHELL,SECTION POINT=3 S22,PEEQ,MISES *OUTPUT,FIELD,OP=NEW,NUM=4,TIMEMARKS=NO *ELEMENT OUTPUT,ELSET=FLUID PRESS, *ELEMENT OUTPUT,ELSET=SOLID PEEQ,PE,LE MISES,PRESS *ELEMENT OUTPUT,ELSET=SHELL PEEQ,PE,LE MISES,PRESS SF,STH *NODE OUTPUT U,V *OUTPUT,HISTORY,OP=NEW,TIME INTERVAL=0.0 *ENERGY OUTPUT ALLAE,ALLIE,ALLKE,ALLPD,ALLSE,ALLVD,ALLWK,ETOTAL *NODE OUTPUT,NSET=NOUT U,V *ELEMENT OUTPUT,ELSET=MIDEL

2-826

Dynamic Stress/Displacement Analyses

S22,PEEQ,MISES,ERV *ELEMENT OUTPUT,ELSET=ELOUT PRESS, *ELEMENT OUTPUT,ELSET=SHELL SF,STH *ELEMENT OUTPUT,ELSET=SHELL S22,PEEQ,MISES *ELEMENT OUTPUT,ELSET=SHELL S22,PEEQ,MISES *ELEMENT OUTPUT,ELSET=SHELL S22,PEEQ,MISES *END STEP

2-827

Dynamic Stress/Displacement Analyses

Listing 2.1.9-2 *HEADING CASK DROP PROBLEM 3D MODEL (coarse mesh) SECTION CONTROLS USED (KINEMA=ORTHOGONAL, HOURGLASS=COMBINED) ** ** Create liner mesh ** ** Top shell mesh *NODE,NSET=N1 1, 0.0,0.0,28.3461 2, 2.3622,0.0,28.3461 3, 0.0,2.3622,28.3461 4, 2.3622,2.3622,28.3461 *NODE,NSET=N2 5, 4.7244,0.0,28.3461 6, 4.7244,2.3622,28.3461 7, 4.7244,4.7244,28.3461 8, 2.3622,4.7244,28.3461 9, 0.0,4.7244,28.3461 *NODE,NSET=N3 20, 11.8109,0.0,28.3461 21,10.911849,4.5198358,28.3461 22,8.3515675,8.3515675,28.3461 23,4.5198358,10.911849,28.3461 24, 0.0,11.8109,28.3461 *NFILL,NSET=N31 N2,N3,3,5 *ELEMENT,TYPE=S4R,ELSET=ETSHELL 1, 1,2,4,3 2, 2,5,6,4 3, 3,4,8,9 4, 4,6,7,8 5, 5,10,11,6 *NSET,NSET=NTSHELL N1,N2,N3,N31 *ELGEN, ELSET=ETSHELL 5,4,1,1,3,5,4 ** First shell wall and middle shell mesh *NCOPY,OLD SET=N3, NEW SET=N4, CHANGE NUMBER=5, SHIFT

2-828

Dynamic Stress/Displacement Analyses

0.0,0.0,-1.1811 0.0,0.0,0.0,0.0,0.0,0.0,0.0,0.0,0.0 *NCOPY,OLD SET=N4, NEW SET=N5, CHANGE NUMBER=45, SHIFT 0.0,0.0,-17.7163 0.0,0.0,0.0,0.0,0.0,0.0,0.0,0.0,0.0 *NCOPY,OLD SET=NTSHELL, NEW SET=NMSHELL, CHANGE NUMBER=89, SHIFT 0.0,0.0,-22.8344 0.0,0.0,0.0,0.0,0.0,0.0,0.0,0.0,0.0 *NFILL N4,N5,9,5 *NCOPY,OLD SET=N4, NEW SET=N6, CHANGE NUMBER=60, SHIFT 0.0,0.0,-20.669 0.0,0.0,0.0,0.0,0.0,0.0,0.0,0.0,0.0 *NFILL N5,N6,3,5 ** Second shell wall and bottom shell mesh *NCOPY,OLD SET=NTSHELL, NEW SET=NBSHELL, CHANGE NUMBER=133, SHIFT 0.0,0.0,-28.3461 0.0,0.0,0.0,0.0,0.0,0.0,0.0,0.0,0.0 *NCOPY,OLD SET=N4, NEW SET=N7, CHANGE NUMBER=104, SHIFT 0.0,0.0,-26.0627 0.0,0.0,0.0,0.0,0.0,0.0,0.0,0.0,0.0 *NSET,NSET=N61 109,110,111,112,113 *NFILL N61,N7,4,5 *ELEMENT,TYPE=S4R 17, 25,26,21,20 69, 109,110,86,85 89, 114,115,110,109 105,153,154,130,129 *ELGEN, ELSET=W1SHELL 17, 4,1,1,13,5,4 *ELGEN, ELSET=W1SHELL 69, 4,1,1 *ELCOPY, ELEMENT SHIFT=72, OLD SET=ETSHELL, SHIFT NODE=89, NEW SET=EMSHELL *ELCOPY, ELEMENT SHIFT=36, OLD SET=EMSHELL,

2-829

Dynamic Stress/Displacement Analyses

SHIFT NODE=44, NEW SET=EBSHELL *ELGEN,ELSET=W2SHELL 89,4,1,1,4,5,4 *ELGEN,ELSET=W2SHELL 105, 4,1,1 *ELSET,ELSET=SHELL1 ETSHELL,W1SHELL,EMSHELL,W2SHELL,EBSHELL ** ** Shell material definition ** *SHELL SECTION,MATERIAL=A2,ELSET=ETSHELL, SECTION INTEGRATION=GAUSS 0.3748,5 *SHELL SECTION,MATERIAL=A1,ELSET=W1SHELL, SECTION INTEGRATION=GAUSS 0.1874,5 *SHELL SECTION,MATERIAL=A2,ELSET=EMSHELL, SECTION INTEGRATION=GAUSS 0.5,5 *SHELL SECTION,MATERIAL=A2,ELSET=W2SHELL, SECTION INTEGRATION=GAUSS 0.0591,5 *SHELL SECTION,MATERIAL=A2,ELSET=EBSHELL, SECTION INTEGRATION=GAUSS 0.0591,5 ** ** Stainless steel (304L) ** *MATERIAL,NAME=A1 *DENSITY 0.00075163, *ELASTIC 28E6,0.28 *PLASTIC 44300.0,0. 66300.0,0.1 ** ** Mild steel (A36) ** *MATERIAL,NAME=A2 *DENSITY 0.00075163, *ELASTIC

2-830

Dynamic Stress/Displacement Analyses

28E6,0.28 *PLASTIC 30000.0,0. ** ** Create fluid mesh ** *NCOPY,OLD SET=NTSHELL,CHANGE NUMBER=200, NEW SET=WTOP,SHIFT 0.0,0.0,-2.2834 0.0,0.0,0.0,0.0,0.0,0.0,0.0,0.0,0.0 *NCOPY,OLD SET=WTOP, NEW SET=WMID, CHANGE NUMBER=216, SHIFT 0.0,0.0,-16.8145 0.0,0.0,0.0,0.0,0.0,0.0,0.0,0.0,0.0 *NCOPY,OLD SET=WTOP, NEW SET=WBOT, CHANGE NUMBER=312, SHIFT 0.0,0.0,-20.551 0.0,0.0,0.0,0.0,0.0,0.0,0.0,0.0,0.0 *NFILL WTOP,WMID,9,24 *NFILL WMID,WBOT,4,24 *ELEMENT,TYPE=C3D8R,ELSET=E1 201, 225,226,228,227,201,202,204,203 202, 226,229,230,228,202,205,206,204 203, 227,228,232,233,203,204,208,209 204, 228,230,231,232,204,206,207,208 205, 229,234,235,230,205,210,211,206 206, 230,235,236,231,206,211,212,207 207, 231,236,237,232,207,212,213,208 208, 232,237,238,233,208,213,214,209 209, 234,239,240,235,210,215,216,211 210, 235,240,241,236,211,216,217,212 211, 236,241,242,237,212,217,218,213 212, 237,242,243,238,213,218,219,214 213, 239,244,245,240,215,220,221,216 214, 240,245,246,241,216,221,222,217 215, 241,246,247,242,217,222,223,218 216, 242,247,248,243,218,223,224,219 *ELCOPY,OLD SET=E1,ELEMENT SHIFT=16, SHIFT NODE=24 *ELCOPY,OLD SET=E1,ELEMENT SHIFT=32, SHIFT NODE=48

2-831

Dynamic Stress/Displacement Analyses

*ELCOPY,OLD SET=E1,ELEMENT SHIFT=48, SHIFT NODE=72 *ELCOPY,OLD SET=E1,ELEMENT SHIFT=64, SHIFT NODE=96 *ELCOPY,OLD SET=E1,ELEMENT SHIFT=80, SHIFT NODE=120 *ELCOPY,OLD SET=E1,ELEMENT SHIFT=96, SHIFT NODE=144 *ELCOPY,OLD SET=E1,ELEMENT SHIFT=112, SHIFT NODE=168 *ELCOPY,OLD SET=E1,ELEMENT SHIFT=128, SHIFT NODE=192 *ELCOPY,OLD SET=E1,ELEMENT SHIFT=144, SHIFT NODE=216 *ELCOPY,OLD SET=E1,ELEMENT SHIFT=160, SHIFT NODE=240 *ELCOPY,OLD SET=E1,ELEMENT SHIFT=176, SHIFT NODE=264 *ELCOPY,OLD SET=E1,ELEMENT SHIFT=192, SHIFT NODE=288 *ELSET,ELSET=WATER,GENERATE 201,408,1 *MATERIAL, NAME=MWATER *DENSITY 9.2E-5, *EOS, TYPE=USUP 57100.874,0.0,0.0 *TENSILE FAILURE,ELEMENT DELETION=NO, PRESSURE=BRITTLE,SHEAR=BRITTLE 0., *SOLID SECTION, ELSET=WATER, MATERIAL=MWATER, CONTROL=C *SECTION CONTROLS, KINEMA=ORTHOGONAL, HOURGLASS=COMBINED, NAME=C ** ** Create foam mesh ** *NCOPY,OLD SET=NMSHELL,CHANGE NUMBER=511, NEW SET=FTOP,SHIFT 0.0,0.0,-0.5 0.0,0.0,0.0,0.0,0.0,0.0,0.0,0.0,0.0 *NCOPY,OLD SET=NBSHELL,CHANGE NUMBER=587, NEW SET=FBOT,SHIFT

2-832

Dynamic Stress/Displacement Analyses

0.0,0.0,0.0 0.0,0.0,0.0,0.0,0.0,0.0,0.0,0.0,0.0 *NFILL FTOP,FBOT,5,24 *ELCOPY,OLD SET=E1,ELEMENT SHIFT=300, SHIFT NODE=400,NEW SET=E2 *ELCOPY,OLD SET=E2,ELEMENT SHIFT=16, SHIFT NODE=24 *ELCOPY,OLD SET=E2,ELEMENT SHIFT=32, SHIFT NODE=48 *ELCOPY,OLD SET=E2,ELEMENT SHIFT=48, SHIFT NODE=72 *ELCOPY,OLD SET=E2,ELEMENT SHIFT=64, SHIFT NODE=96 *ELSET,ELSET=FOAM,GENERATE 501,580,1 *MATERIAL, NAME=MFOAM *ELASTIC 18738,0.0 *DENSITY 2.85E-5, *FOAM 0.0,223.84,313.35 *FOAM HARDENING 1023.84,0.00 1073.84,0.01 1123.84,0.02 1723.84,0.345 3023.84,0.44 5923.84,0.49 12223.84,0.51 8E5,2.00 *SOLID SECTION, ELSET=FOAM, MATERIAL=MFOAM, CONTROL=C ** ** Define fluid and foam contact node set ** *NSET, NSET=WCONT, GENERATE 201,224,1 220,532,24 221,533,24 222,534,24 223,535,24

2-833

Dynamic Stress/Displacement Analyses

224,536,24 513,536,1 *NSET, NSET=FCONT, GENERATE 601,624,1 620,740,24 621,741,24 622,742,24 623,743,24 624,744,24 721,744,1 ** ** Define boundary condition ** *NSET,NSET=FEND, GENERATE 134,157,1 *NSET,NSET=YANODES 1,2,5,10,15,20,25,30,35,40,45,50,55,60,65,70, 75,80,85,90,91,94,99,104,109,114,119,124,129, 134,135,138,143,148,153,513,514,517,522,527, 532,721,722,725,730,735,740, *NSET,NSET=YANODES,GENERATE 201,513,24 202,514,24 205,517,24 210,522,24 215,527,24 220,532,24 601,721,24 602,722,24 605,725,24 610,730,24 615,735,24 620,740,24 *NSET,NSET=XANODES 1,3,9,14,19,24,29,34,39,44,49,54,59,64,69,74, 79,84,89,90,92,98,103,108,113,118,123,128,133, 134,136,142,147,152,157,513,515,521,526,531, 536,721,723,729,734,739,744, *NSET,NSET=XANODES,GENERATE 201,513,24 203,515,24 209,521,24 214,526,24

2-834

Dynamic Stress/Displacement Analyses

219,531,24 224,536,24 601,721,24 603,723,24 609,729,24 614,734,24 619,739,24 624,744,24 *BOUNDARY FEND,ZSYMM XANODES,XSYMM YANODES,YSYMM ** ** Define initial condition ** *NSET,NSET=NALL,GENERATE 1,133,1 201,536,1 601,720,1 *INITIAL CONDITIONS, TYPE=VELOCITY NALL, 3, -523.3 ** ** Define history output element set ** *ELSET,ELSET=FLUID 393, *ELSET,ELSET=SOLID 501, *ELSET,ELSET=MIDEL 393,501 *ELSET,ELSET=SHELL 97, *ELSET,ELSET=ELOUT MIDEL, SHELL, *NSET, NSET=NOUT 119,601 *NSET, NSET=NOUT, ELSET=ELOUT *RESTART, WRITE, NUM=1, TIMEMARKS=NO *SURFACE,TYPE=ELEMENT, NAME=SSIDE1, NO THICK ETSHELL,SNEG W1SHELL,SNEG EMSHELL,SPOS

2-835

Dynamic Stress/Displacement Analyses

*SURFACE,TYPE=NODE,NAME=FCONT FCONT, *SURFACE,TYPE=ELEMENT, NAME=SSIDE2, NO THICK EMSHELL,SNEG W2SHELL,SNEG EBSHELL,SPOS *SURFACE,TYPE=NODE,NAME=WCONT WCONT, *STEP *DYNAMIC, EXPLICIT ,0.005 *CONTACT PAIR SSIDE1,WCONT *CONTACT PAIR SSIDE2,FCONT *FILE OUTPUT, NUM=4, TIMEMARKS=NO *EL FILE, ELSET=FLUID PRESS, *EL FILE, ELSET=SOLID PEEQ,PE,LE MISES,PRESS *EL FILE, ELSET=SHELL PEEQ,PE,LE MISES,PRESS SF,STH *NODE FILE, NSET=NOUT U,V *HISTORY OUTPUT,TIME=0.0 *ENERGY HISTORY ALLAE,ALLIE,ALLKE,ALLPD,ALLSE,ALLVD,ALLWK,ETOTAL *NODE HISTORY, NSET=NOUT U,V *EL HISTORY,ELSET=MIDEL S33,PEEQ,MISES,ERV *EL HISTORY,ELSET=ELOUT PRESS, *EL HISTORY,ELSET=SHELL SF,STH *EL HISTORY,ELSET=SHELL,SECTION POINT=1 S33,PEEQ,MISES *EL HISTORY,ELSET=SHELL,SECTION POINT=2 S33,PEEQ,MISES *EL HISTORY,ELSET=SHELL,SECTION POINT=3

2-836

Dynamic Stress/Displacement Analyses

S33,PEEQ,MISES *OUTPUT,FIELD,VARIABLE=PRESELECT,OP=NEW,NUM=1, TIMEMARKS=NO *OUTPUT,FIELD,OP=NEW,NUM=4,TIMEMARKS=NO *ELEMENT OUTPUT,ELSET=FLUID PRESS, *ELEMENT OUTPUT,ELSET=SOLID PEEQ,PE,LE MISES,PRESS *ELEMENT OUTPUT,ELSET=SHELL PEEQ,PE,LE MISES,PRESS SF,STH *NODE OUTPUT,NSET=NOUT U,V *OUTPUT,HISTORY,OP=NEW,TIME INTERVAL=0.0 *ENERGY OUTPUT ALLAE,ALLIE,ALLKE,ALLPD,ALLSE,ALLVD,ALLWK,ETOTAL *NODE OUTPUT,NSET=NOUT U,V *ELEMENT OUTPUT,ELSET=MIDEL S33,PEEQ,MISES,ERV *ELEMENT OUTPUT,ELSET=ELOUT PRESS, *ELEMENT OUTPUT,ELSET=SHELL SF,STH *ELEMENT OUTPUT,ELSET=SHELL S33,PEEQ,MISES *ELEMENT OUTPUT,ELSET=SHELL S33,PEEQ,MISES *ELEMENT OUTPUT,ELSET=SHELL S33,PEEQ,MISES *END STEP

2.1.10 Oblique impact of a copper rod Product: ABAQUS/Explicit This example simulates a high velocity, oblique impact of a copper rod into a rigid wall. Extremely high plastic strains develop at the crushed end of the rod, resulting in severe local mesh distortion. Adaptive meshing is used to reduce element distortion and to obtain an accurate and economical solution to the problem.

Problem description

2-837

Dynamic Stress/Displacement Analyses

The model geometry is depicted in Figure 2.1.10-1. A cylindrical rod, measuring 32.4 ´ 3.2 mm, impacts a rigid wall with an initial velocity of vy =340 m/sec. The wall is perpendicular to the x-z plane and makes an angle of 30° with the x-y plane. The half-symmetric finite element model is shown in Figure 2.1.10-2. Symmetry boundary conditions are applied at the y=0 plane. The rod is meshed with CAX4R elements, and the wall is modeled as an analytical rigid surface using the *SURFACE, TYPE=CYLINDER option in conjunction with the *RIGID BODY option. Coulomb friction is assumed between the rod and the wall, with a friction coefficient of 0.2. The analysis is performed for a period of 120 microseconds. The rod is modeled as a Johnson-Cook, elastic-plastic material with a Young's modulus of 124 GPa, a Poisson's ratio of 0.34, and a density of 8960 kg/m 3. The Johnson-Cook model is appropriate for modeling high-rate impacts involving metals. The Johnson-Cook material parameters are taken from Johnson and Cook (1985) in which the following constants are used: A = 90 MPa, n = 0.31, m = 1.09, C = 0.025, and "_o = 1 s-1. Furthermore, the melting temperature is 1058°C, and the transition temperature is 25°C. Adiabatic conditions are assumed with a heat fraction of 50%. The specific heat of the material is 383 J/Kg°C, and the thermal expansion coefficient is 0.00005°C -1.

Adaptive meshing A single adaptive mesh domain that incorporates the entire rod is defined. Symmetry boundary conditions are defined as Lagrangian surfaces (the default), and contact surfaces are defined as sliding contact surfaces (the default). Because the impact phenomenon modeled in this example is an extremely dynamic event with large changes in geometry occurring over a relatively small number of increments, it is necessary to increase the frequency and intensity of adaptive meshing. The frequency value is reduced to 5 increments from a default value of 10, and the number of mesh sweeps used to smooth the mesh is increased to 3 from the default value of 1. The default values are used for all other adaptive mesh controls.

Results and discussion Deformed shape plots at 40, 80, and 120 microseconds are shown in Figure 2.1.10-3, Figure 2.1.10-4, and Figure 2.1.10-5, respectively. The rod rebounds from the wall near the end of the analysis. High-speed collisions such as these result in significant amounts of material flow in the impact zone. A pure Lagrangian analysis of this finite element model fails as a result of excessive distortions. Continuous adaptive meshing allows the analysis to run to completion while retaining a high-quality mesh. The kinetic and internal energy histories are plotted in Figure 2.1.10-6. Most of the initial kinetic energy is converted to internal energy as the rod is plastically deformed. Both energy curves plateau as the rod rebounds from the wall.

Input files ale_rodimpac_inclined.inp Analysis using adaptive meshing. ale_rodimpac_inclined_nodelem.inp

2-838

Dynamic Stress/Displacement Analyses

External file referenced by this analysis.

Reference · Johnson, G. R. and W. H. Cook, "Fracture Characteristics of Three Metals Subjected to Various Strains, Strain Rates, Temperatures and Pressures, " Engineering Fracture Mechanics, 21, pp. 31-48, 1985.

Figures Figure 2.1.10-1 Model geometry.

Figure 2.1.10-2 Initial configuration.

2-839

Dynamic Stress/Displacement Analyses

Figure 2.1.10-3 Deformed configuration at 40 microseconds.

Figure 2.1.10-4 Deformed configuration at 80 microseconds.

Figure 2.1.10-5 Deformed configuration at 120 microseconds.

2-840

Dynamic Stress/Displacement Analyses

Figure 2.1.10-6 Time history of kinetic and internal energies of the rod.

Sample listings

2-841

Dynamic Stress/Displacement Analyses

Listing 2.1.10-1 *HEADING ADAPTIVE MESHING EXAMPLE OBLIQUE IMPACT OF A COPPER ROD(3D MODEL) Units - N, m ,second ** *RESTART,WRITE,NUMBER INTERVAL=30 *INCLUDE,INPUT=ale_rodimpac_inclined_nodelem.inp ** ** Representative material properties for copper ** *MATERIAL,NAME=COPPER *ELASTIC 124.E9, 0.34 ** Young's modulus unit: Pa *PLASTIC,HARDENING=JOHNSON COOK 90.E6, 292.E6, 0.31, 1.09, 1058., 25. ** A & B unit: Pa *RATE DEPENDENT,TYPE=JOHNSON COOK 0.025, 1.0 **unit:reference strain rate has a unit of s^(-1) *INELASTIC HEAT FRACTION 0.5, ** dimensionless *SPECIFIC HEAT 383., ** unit: J/kgK *EXPANSION 5.E-5, ** unit: K^(-1) *DENSITY 8.96E3, ** unit: kg/m^3 *SOLID SECTION,ELSET=ROD,MATERIAL=COPPER, CONTROLS=SECT *SECTION CONTROLS,NAME=SECT, KINEMATICS=ORTHOGONAL,HOURGLASS=VISCO *BOUNDARY SPLANE1, 2 200000, 1, 6 *INITIAL CONDITIONS,TYPE=TEMPERATURE ROD0, 25.

2-842

Dynamic Stress/Displacement Analyses

*INITIAL CONDITIONS,TYPE=VELOCITY BODY, 3, -340. ** ** Run the problem for 120 microseconds ** *SURFACE,TYPE=CYLINDER,NAME=RSURF -20.E-3,0.,-13.3945E-3,20.E-3,0.,-13.3945E-3 -20.E-3,1.,-13.3945E-3 START, 0., 0. LINE, 40.E-3, 23.094E-3 *SURFACE,TYPE=ELEMENT,NAME=RODSURF, REGION TYPE=SLIDING ROD, *RIGID BODY,REFNODE=200000, ANALYTICAL SURFACE =RSURF *STEP *DYNAMIC,EXPLICIT,ADIABATIC ,120.E-6 *CONTACT PAIR,INTERACTION=INTER RSURF,RODSURF *SURFACE INTERACTION,NAME=INTER *FRICTION 0.2, *FILE OUTPUT,TIMEMARKS=YES,NUM=1 *EL FILE PEEQ,MISES, *NODE FILE U, *ENERGY FILE ** *ADAPTIVE MESH,ELSET=ROD,FREQUENCY=5, MESH SWEEPS=3 ** *END STEP

2.1.11 Water sloshing in a baffled tank Product: ABAQUS/Explicit This example illustrates the use of adaptive meshing to model an inviscid fluid sloshing inside a baffled tank. The overall structural response resulting from the coupling between the water and tank, rather than a detailed solution in the fluid, is sought. Adaptive meshing permits the investigation of this response over longer time periods than a pure Lagrangian approach would because the mesh entanglement that occurs in the latter case is prevented.

2-843

Dynamic Stress/Displacement Analyses

Problem description The geometry for the problem is shown in Figure 2.1.11-1. The model consists of a baffled tank filled with water. The baffle, which is attached to the sides and top of the tank, does not penetrate the entire depth of the water. The tank measures 508 ´ 152.4 ´ 152.4 mm (20 ´ 6 ´ 6 inches), and the baffle measures 3.048 ´ 152.4 ´ 121.92 mm (0.12 ´ 6 ´ 4.8 inches). The tank is filled with 101.6 mm (4 inches) of water. A cutaway view of the finite element model that displays the baffle and the water is shown in Figure 2.1.11-2. The top of the tank is not modeled because the water is not expected to come into contact with it. The tank is modeled as a rigid body and is meshed with R3D4 elements. The baffle is modeled as a deformable body and is meshed with S4R elements. A graded mesh of C3D8R elements is used for the water, with more refinement adjacent to the baffle where significant deformations are expected. In sloshing problems water can be considered an incompressible and inviscid material. An effective method for modeling water in ABAQUS/Explicit is to use a simple Newtonian viscous shear model and a linear Us ¡ Up equation of state for the bulk response. The bulk modulus functions as a penalty parameter for the incompressible constraint. Since sloshing problems are unconfined, the bulk modulus chosen can be two or three orders of magnitude less than the actual bulk modulus and the water will still behave as an incompressible medium. The shear viscosity also acts as a penalty parameter to suppress shear modes that could tangle the mesh. The shear viscosity chosen should be small because water is inviscid; a high shear viscosity will result in an overly stiff response. An appropriate value for the shear viscosity can be calculated based on the bulk modulus. To avoid an overly stiff response, the internal forces arising due to the deviatoric response of the material should be kept several orders of magnitude below the forces arising due to the volumetric response. This can be done by choosing an elastic shear modulus that is several orders of magnitude lower than the bulk modulus. If the Newtonian viscous deviatoric model is used, the shear viscosity specified should be on the order of an equivalent shear modulus, calculated as mentioned earlier, scaled by the stable time increment. The expected stable time increment can be obtained from a datacheck analysis of the model. This method is a convenient way to approximate a shear strength that will not introduce excessive viscosity in the material. In addition, if a shear model is defined, the hourglass control forces are calculated based on the shear stiffness of the material. Thus, in materials with extremely low or zero shear strengths such as inviscid fluids, the hourglass forces calculated based on the default parameters are insufficient to prevent spurious hourglass modes. Therefore, a sufficiently high hourglass scaling factor is used to increase the resistance to such modes. This analysis methodology is verified in ``Water sloshing in a pitching tank,'' Section 1.11.6 of the ABAQUS Benchmarks Manual. For this example the linear Us ¡ Up equation of state is used with a wave speed of 45.85 m/sec (1805

in/sec) and a density of 983.204 kg/m 3 (0.92 ´ 10-4 lb sec2/in4). The wave speed corresponds to a bulk modulus of 2.07 MPa (300 psi), three orders of magnitude less than the actual bulk modulus of water, 2.07 GPa (3.0 ´ 105 psi). The shear viscosity is chosen as 1.5 ´ 10-8 sec-1. The baffle is modeled as a Mooney-Rivlin elastomeric material with hyperelastic constants C10 = 689480 Pa (100 psi) and C01 = 172370 Pa (25 psi) and a density of 10900.74 kg/m 3 (1.02 ´ 10-3 lb sec2/in4).

2-844

Dynamic Stress/Displacement Analyses

Pure master-slave contact is defined between the tank and the water; balanced master-slave contact is defined between the baffle and the water. The bottom edge of the baffle has nodes in common with the underlying water surface. This prevents relative slip between the bottom edge of the baffle and the water immediately below it. The motion of the other edges of the baffle coincides with that of the tank. The water is subjected to gravity loading. Consequently, an initial geostatic stress field is defined to equilibrate the stresses caused by the self-weight of the water. A velocity pulse in the form of a sine wave with an amplitude of 63.5 mm (2.5 inches) and a period of 2 seconds is prescribed for the tank in both the x- and y-directions simultaneously. All remaining degrees of freedom for the tank are fully constrained. The sloshing analysis is performed for two seconds.

Adaptive meshing A single adaptive mesh domain that incorporates the water is defined. Sliding boundary regions are used for all contact surface definitions on the water (the default). Because the sloshing phenomenon modeled in this example results in large mesh motions, it is necessary to increase the frequency and intensity of adaptive meshing. The frequency value is reduced to 5 increments from a default value of 10, and the number of mesh sweeps used to smooth the mesh is increased to 3 from a default value of 1. The SMOOTHING OBJECTIVE parameter on the *ADAPTIVE MESH CONTROLS option is set to GRADED so that the initial mesh gradation of the water is preserved while continuous adaptive meshing is performed. The default values are used for all other parameters and controls.

Results and discussion Figure 2.1.11-3, Figure 2.1.11-4, and Figure 2.1.11-5 show the deformed mesh configuration at t = 1.2 s, t = 1.6 s, and t = 2.0 s, respectively. Four time histories of the vertical displacement of the water level are shown in Figure 2.1.11-6; these correspond to the water level at the baffle in the front and back of the left and right bays. The locations at which the time histories are measured are denoted A, B, C, and D in Figure 2.1.11-1. An analysis such as this could be used to design a baffle that attenuates sloshing at certain frequencies. Using adaptivity in ABAQUS/Explicit is appropriate for sloshing problems in which the structural response is of primary interest. It is generally not possible to model such flow behaviors as splashing or complex free surface interactions. Furthermore, surface tension is not modeled.

Input file ale_water_sloshing.inp Input data for this analysis. ale_water_sloshingel.inp Element data.

Figures

2-845

Dynamic Stress/Displacement Analyses

Figure 2.1.11-1 Model geometry.

Figure 2.1.11-2 Initial configuration (front of rigid tank is not shown).

Figure 2.1.11-3 Deformed configuration of the water and the baffle at 1.2 seconds.

2-846

Dynamic Stress/Displacement Analyses

Figure 2.1.11-4 Deformed configuration of the water and the baffle at 1.6 seconds.

Figure 2.1.11-5 Deformed configuration of the water and the baffle at 2.0 seconds.

Figure 2.1.11-6 Time histories of the vertical displacement of the water at the baffle at both the front and back of the left and right bays.

2-847

Dynamic Stress/Displacement Analyses

Sample listings

2-848

Dynamic Stress/Displacement Analyses

Listing 2.1.11-1 *HEADING ADAPTIVE MESHING EXAMPLE WATER SLOSHING IN A BAFFLED TANK Unit lb, in, sec *RESTART, WRITE, NUMBER=30 *NODE 1, 10.00, 0.0, 0.0 21, 20.00, 0.0, 0.0 127, 10.00, 0.0, 1.2 147, 20.00, 0.0, 1.2 316, 10.00, 0.0, 4.0 336, 20.00, 0.0, 4.0 5041,10.00, 6.0, 0.0 5061,20.00, 6.0, 0.0 5167,10.00, 6.0, 1.2 5187,20.00, 6.0, 1.2 5356,10.00, 6.0, 4.0 5376,20.00, 6.0, 4.0 75000, 25.00, 20.0 *NGEN, NSET=A1 1, 127,21 *NGEN, NSET=A2 5041, 5167,21 *NFILL, NSET=A A1,A2,15,336 *NGEN, NSET=B1 21,147,21 *NGEN, NSET=B2 5061,5187,21 *NFILL, NSET=B B1,B2,15,336 *NFILL,NSET=RIGHT1,BIAS=.9 A, B, 20, 1 *NGEN, NSET=C1 127, 316,21 *NGEN, NSET=C2 5167, 5356,21 *NFILL, NSET=C C1,C2,15,336 *NGEN, NSET=D1 147,336,21

2-849

Dynamic Stress/Displacement Analyses

*NGEN, NSET=D2 5187,5376,21 *NFILL, NSET=D D1,D2,15,336 *NFILL,NSET=RIGHT2,BIAS=.9 C, D, 20, 1 *NSET,NSET=RIGHT RIGHT1,RIGHT2 *ELEMENT, TYPE=C3D8R 1,1,2,338,337,22,23,359,358 *ELGEN, ELSET=WATER1 1,20,1,1,15,21,20,15,336,300, ***************************************** *NCOPY,CHANGE NUMBER=5376,OLD SET=RIGHT, NEW SET=LEFT,REFLECT=MIRROR 10.,0., 20.,10.,3., 20. 10.,0., -5., *ELCOPY,ELEMENT SHIFT=4500,OLD SET=WATER1, SHIFT NODES=5376,REFLECT,NEW SET=WATER2 *ELSET,ELSET=WATER WATER1,WATER2 *NODE 10753, 0.0,0.0,0.0 10754,20.0,0.0,0.0 10755,20.0,0.0,6.0, 10756,0.00,0.0,6.0, 10757, 0.0,6.0,0.0, 10758,20.0,6.0,0.0, 10759,20.0,6.0,6.0, 10760,0.00,6.0,6.0, *ELEMENT, TYPE=R3D4, ELSET=RIGID 9001,10756,10755,10754,10753 9002,10757,10758,10759,10760 9003,10755,10759,10758,10754 9004,10753,10757,10760,10756 9005,10753,10754,10758,10757 *NODE 10761,10.00,-0.1,1.2 10776,10.00,6.1,1.2 11001,10.00,-0.1,6.0 11016,10.00,6.1,6.0 *NGEN, NSET=S1 10761,10776,1

2-850

Dynamic Stress/Displacement Analyses

*NGEN, NSET=S2 11001,11016,1 *NFILL,NSET=S S1,S2,15, 16 *NSET,NSET=EDGES, GEN 10777,11001,16 10792,11016,16 11001,11016,1 *NSET,NSET=OUT 316,5356,5692,10732 *ELEMENT, TYPE=S4R 9006,10761,10777,10778,10762 *ELGEN, ELSET=BAFFLE 9006,15,1,1,15,16,15 *INCLUDE, INPUT=ale_water_sloshingel.inp *SHELL SECTION, ELSET=BAFFLE, MATERIAL=BAFFLE .12, *MATERIAL, NAME=BAFFLE *HYPERELASTIC,POLYNOMIAL, N=1 100., 25. *DENSITY 1.07E-3, *SOLID SECTION, ELSET=WATER, MATERIAL=WATER, CONTROLS=SECT *SECTION CONTROLS, NAME=SECT, KINEMATICS=ORTHOGONAL, HOURGLASS=STIFFNESS 10000., ***K=300,K/G=1.E+6, (Actual K of water = 300000) *MATERIAL, NAME=WATER *EOS, TYPE=USUP 1805.7878,0.,0. *EOS SHEAR, TYPE=VISCOUS 1.5E-8, *DENSITY .92E-4, *BOUNDARY 75000,3,6,0.0 EDGES,3,6,0.0 *AMPLITUDE,NAME=AMP,DEFINITION=SMOOTH STEP 0.,0.,.25,1.76777,.5,2.5,.75,1.76777, 1.0,0.0,10.0,0.0 *INITIAL CONDITIONS, TYPE=STRESS, GEOSTATIC WATER,0.,4.,-.1420,0.,1.,1.,

2-851

Dynamic Stress/Displacement Analyses

*SURFACE,TYPE=ELEMENT, NAME=BAFFLESURF1,NOTHICK BAFFLE,SNEG *SURFACE,TYPE=ELEMENT, NAME=BAFFLESURF2,NOTHICK BAFFLE,SPOS *SURFACE,TYPE=ELEMENT, NAME=RSURF RIGID,SPOS *SURFACE,TYPE=ELEMENT, NAME=WATSURF1 WATER, *SURFACE,TYPE=ELEMENT, NAME=WATSURF2 OUT1,S6 OUT11,S2 *SURFACE,TYPE=ELEMENT, NAME=WATSURF3 OUT2,S3 OUT21,S2 *RIGID BODY, REF NODE=75000, POSITION=CENTER OF MASS,ELSET=RIGID *STEP *DYNAMIC, EXPLICIT ,2.0 *DLOAD WATER, GRAV, 386., 0., 0.,-1. *BOUNDARY,TYPE=VELOCITY,AMPLITUDE=AMP 75000,1,2,1. EDGES,1,2,1. *CONTACT PAIR,INTERACTION=WATRIG RSURF,WATSURF1 *CONTACT PAIR,INTERACTION=WATBAFFLE,WEIGHT=1.0,MECHANICAL CONSTRAINT=PENA BAFFLESURF1,WATSURF2 *CONTACT PAIR,INTERACTION=WATBAFFLE,WEIGHT=1.0,MECHANICAL CONSTRAINT=PENA BAFFLESURF2,WATSURF3 *SURFACE INTERACTION, NAME=WATRIG *SURFACE INTERACTION, NAME=WATBAFFLE *FILE OUTPUT, NUMBER=4, TIMEMARKS=YES *EL FILE,ELSET=OUT S, PRESS, *NODE FILE,NSET=EDGES U,V *HISTORY OUTPUT,TIME=1.0E-2 *NODE HISTORY,NSET=EDGES U,V *NODE HISTORY, NSET=OUT U,V

2-852

Dynamic Stress/Displacement Analyses

*EL HISTORY,ELSET=OUT S, PRESS, SHRMOD, DILMOD *ENERGY HISTORY ALLKE,ALLIE,ALLAE,ALLVD,ALLWK,ETOTAL, DT, *ADAPTIVE MESH,ELSET=WATER,CONTROLS=CONTROLS, FREQUENCY=5,MESH SWEEPS=3 *ADAPTIVE MESH CONTROLS,NAME=CONTROLS, SMOOTHING=GRADED,TRANSITION FEATURE ANGLE=0.0 *END STEP

2.1.12 Rigid multi-body mechanism Products: ABAQUS/Standard ABAQUS/Explicit This example illustrates the use of connector elements to model kinematic constraints between rigid bodies in a multi-body mechanism.

Problem description The crank mechanism considered here transmits a rotational motion through two universal joints and then converts the rotation into translational motion of two slides. The mechanism is modeled using nine rigid components attached with eight connector elements. The various kinematic constraints modeled with connector elements include TRANSLATOR, which allows relative translation along a line but no rotations; HINGE, which allows one relative rotation and fixes relative translations; CYLINDRICAL, which allows relative translation along a line and relative rotation about that line; JOIN, which fixes relative translations but leaves the rotations free; PLANAR, which keeps a point on a plane and allows only relative rotations about the normal to that plane; and UJOINT, which fixes the relative translations and enforces a universal constraint on the relative rotations. The complete model is shown in Figure 2.1.12-1. The axes of rotation of the small and large disks are parallel but offset. A constant angular velocity of the small disk is specified about its axis with a velocity boundary condition on its rigid body reference node. All other degrees of freedom of the rigid body reference node are fixed. The rotational motion of the small disk is transmitted to the large disk through two UJOINT connections and a rigid link. A UJOINT connection, or a universal rotation constraint with shared translational degrees of freedom, between two nonaligned shafts will not transmit constant angular velocity. However, two symmetrically placed universal constraints, as here, will produce constant angular velocity coupling between the two disks. The large disk is connected to a rigid circular rod with a JOIN connection. A JOIN connection is equivalent to a ball-and-socket or a spherical joint. The circular rod connects through a sleeve to a flat block. The rod and sleeve constraint is modeled with a CYLINDRICAL connection, which allows the sleeve to translate along and rotate about the rod. The attachment of the circular rod to the flat block is a HINGE connection, which allows only a single relative rotation about

2-853

Dynamic Stress/Displacement Analyses

the shared hinge axis. The flat block, in turn, is assumed to slide between two fixed parallel plates. This sliding constraint is modeled with a PLANAR connection. The sleeve on the circular rod is connected to a square-section sleeve on the square rod with a HINGE connection. The square rod is fixed in space. The square-section sleeve slides along the square bar without rotating. This sliding constraint is modeled with a TRANSLATOR connection.

Results and discussion Figure 2.1.12-2 shows the position of the mechanism at various times. By visual inspection it can be observed that the connector elements are enforcing the correct kinematic constraints. In this model there are nine rigid bodies with 6 degrees of freedom each, accounting for 54 rigid body degrees of freedom. The eight connector elements eliminate 33 rigid body degrees of freedom through kinematic constraints (enforced via Lagrange multipliers) as itemized in Table 2.1.12-1. Hence, the model has 21 rigid body degrees of freedom to be specified as boundary conditions or determined by the solution. In this case all remaining rigid body degrees of freedom are specified as boundary conditions, with the z-component of angular velocity specified for the small disk and 20 additional fixed boundary conditions used.

Input files rigmultimech_exp.inp ABAQUS/Explicit analysis. rigmultimech_std.inp ABAQUS/Standard analysis. rigmultimech_bulk.inp Node and element bulk data for the rigid bodies.

Table Table 2.1.12-1 Rigid body degrees of freedom eliminated by kinematic constraints. Total rigid body dofs Connection type Number of eliminated from kinematic model constraints UJOINT (2) 4 8 JOIN 3 3 CYLINDRICAL 4 4 HINGE (2) 5 10 PLANAR 3 3 TRANSLATOR 5 5 Total eliminated: 33

Figures

2-854

Dynamic Stress/Displacement Analyses

Figure 2.1.12-1 Rigid mechanism model.

Figure 2.1.12-2 Time history of the motion of the mechanism during the first revolution.

2-855

Dynamic Stress/Displacement Analyses

Sample listings

2-856

Dynamic Stress/Displacement Analyses

Listing 2.1.12-1 *HEADING Rigid, multi-body mechanism - connector elements ** node and element definitions: *INCLUDE, INPUT=rigmultimech_bulk.inp ***************************** *ELSET, ELSET=SQUAREROD, GEN 1,4,1 *ELSET, ELSET=SQUARESLEAVE, GEN 5,92,1 *ELSET, ELSET=ROUNDROD, GEN 93,172,1 *ELSET, ELSET=ROUNDSLEAVE, GEN 173,260,1 *ELSET, ELSET=SLIDINGBLOCK, GEN 261,272,1 *ELSET, ELSET=RACEWAY, GEN 273,278,1 *ELSET, ELSET=LARGEDISK, GEN 1001,1174,1 *ELSET, ELSET=DISKLINK, GEN 1175, 1194,1 *ELSET, ELSET=SMALLDISK, GEN 1195, 1368,1 ***************************** ** Square rod *NSET, NSET=ADD1 19 *RIGID BODY,ELSET=SQUAREROD,REF NODE=10000, POSITION=CENTER OF MASS,TIE NSET=ADD1 ** Square sleave *NSET, NSET=ADD2 20,218 *RIGID BODY,ELSET=SQUARESLEAVE,REF NODE=20000, POSITION=CENTER OF MASS,TIE NSET=ADD2 ** Round rod *NSET, NSET=ADD3 385,746,1034 *RIGID BODY,ELSET=ROUNDROD,REF NODE=30000, POSITION=CENTER OF MASS,TIE NSET=ADD3 ** Round sleave *NSET, NSET=ADD4

2-857

Dynamic Stress/Displacement Analyses

219,386 *RIGID BODY,ELSET=ROUNDSLEAVE,REF NODE=40000, POSITION=CENTER OF MASS,TIE NSET=ADD4 ** Large disk *NSET, NSET=ADD5 747,768 *RIGID BODY,ELSET=LARGEDISK,REF NODE=70000, POSITION=CENTER OF MASS,TIE NSET=ADD5 ** Sliding block *NSET, NSET=ADD6 1035, 1040 *RIGID BODY,ELSET=SLIDINGBLOCK,REF NODE=50000, POSITION=CENTER OF MASS,TIE NSET=ADD6 ** Raceway *NSET,NSET=ADD7 1041, *RIGID BODY,ELSET=RACEWAY,REF NODE=60000, POSITION=CENTER OF MASS,TIE NSET=ADD7 ** DiskLink *NSET,NSET=ADD8 795,798 *RIGID BODY,ELSET=DISKLINK,REF NODE=80000, POSITION=CENTER OF MASS,TIE NSET=ADD8 ** Smalldisk *NSET,NSET=ADD9 821, *RIGID BODY,ELSET=SMALLDISK,REF NODE=90000, POSITION=CENTER OF MASS,TIE NSET=ADD9 ** *NSET, NSET=REF 10000,20000,30000,40000,50000,60000,70000,80000, 90000 ***************************** ** Square rod - square sleave ***************************** *ELEMENT, TYPE = CONN3D2, ELSET=SR-SS 5001, 19, 20 *ORIENTATION, DEFINITION=COORDINATES, NAME=SR-SS 1, 0, 0, 0, 1, 0 *CONNECTOR SECTION, ELSET=SR-SS translator, SR-SS, *****************************

2-858

Dynamic Stress/Displacement Analyses

** Square sleave - round sleave ***************************** *ELEMENT, TYPE = CONN3D2, ELSET=SS-RS 5002, 218, 219 *ORIENTATION, DEFINITION=COORDINATES, 0, 0, 1, 1, 0, 0 *CONNECTOR SECTION, ELSET=SS-RS hinge, SS-RS, ***************************** ** Round rod - round sleave ***************************** *ELEMENT, TYPE = CONN3D2, ELSET=RR-RS 5003, 385, 386 *ORIENTATION, DEFINITION=COORDINATES, 0, 1, 0, 0, 0, 1 *CONNECTOR SECTION, ELSET=RR-RS cylindrical, RR-RS ***************************** ** Round rod - large disk ***************************** *ELEMENT, TYPE = CONN3D2, ELSET=RR-LD 5004, 746, 747 *ORIENTATION, DEFINITION=COORDINATES, 1, 0, 0, 0, 1, 0 *CONNECTOR SECTION, ELSET=RR-LD join, RR-LD ***************************** ** Round rod - sliding block ***************************** *ELEMENT, TYPE = CONN3D2, ELSET=RR-SB 5005, 1034, 1035 *ORIENTATION, DEFINITION=COORDINATES, 0, 0, 1, 1, 0, 0 *CONNECTOR SECTION, ELSET=RR-SB hinge, RR-SB ***************************** ** Sliding block - raceway ***************************** *ELEMENT, TYPE = CONN3D2, ELSET=SB-R

NAME=SS-RS

NAME=RR-RS

NAME=RR-LD

NAME=RR-SB

2-859

Dynamic Stress/Displacement Analyses

5006, 1040, 1041 *ORIENTATION, DEFINITION=COORDINATES, NAME=SB-R 1, 0, 0, 0, 1, 0 *CONNECTOR SECTION, ELSET=SB-R slideplane, revolute SB-R, ***************************** ** Large disk - disklink ***************************** *ELEMENT, TYPE = CONN3D2, ELSET=LD-DL 5007, 768, 795 *ORIENTATION, DEFINITION=COORDINATES, NAME=LD-DL -1, 0, 0, 0, 0, 1 *ORIENTATION, DEFINITION=COORDINATES, NAME=DL-LD -.8660254,0.,.5,.5,0.,.8660254 *CONNECTOR SECTION, ELSET=LD-DL ujoint, LD-DL,DL-LD ***************************** ** Small Disk - Disk Link ***************************** *ELEMENT, TYPE = CONN3D2, ELSET=SD-DL 5008, 821, 798 *ORIENTATION, DEFINITION=COORDINATES, NAME=SD-DL -1, 0, 0, 0, 0, 1 *ORIENTATION, DEFINITION=COORDINATES, NAME=DL-SD -.8660254,0.,.5,.5,0.,.8660254 *CONNECTOR SECTION, ELSET=SD-DL ujoint, SD-DL,DL-SD *BOUNDARY 10000,1,2,0.0 10000,4,6,0.0 70000,1,5,0.0 90000,1,2,0.0 90000,4,5,0.0 60000,1,6,0.0 *AMPLITUDE, NAME=AMP, DEFINITION=SMOOTH STEP 0.0,0.0,.00375,23.26,3.0,23.26 *********************************** *NSET, NSET=CONNECTIONNODES 746,747,386,385,20,19, 219,218,1034,1035,1040,1041,

2-860

Dynamic Stress/Displacement Analyses

768,795,798,821 *NSET,NSET=OUT CONNECTIONNODES,REF *STEP,NLGEOM=YES *DYNAMIC,EXPLICIT,DIRECT 1.8E-4,0.18 *BOUNDARY, TYPE=VELOCITY, AMPLITUDE=AMP 90000,6,6,5.0 *************************************** *FILE OUTPUT,TIMEMARKS=NO,NUM=10 *NODE FILE,NSET=OUT U,V,A *ENERGY FILE *OUTPUT,FIELD,NUM=300 *NODE OUTPUT U,V,A *OUTPUT,HISTORY,FREQUENCY=100 *NODE OUTPUT,NSET=OUT U,V,A *END STEP

2.2 Mode-based dynamic analyses 2.2.1 Analysis of a rotating fan using superelements and cyclic symmetry model Product: ABAQUS/Standard This example illustrates the single and multi-level substructure capability of ABAQUS for problems where the part being modeled consists of repeated structures. It also demonstrates the capability of ABAQUS to analyze cyclic symmetric models using the *CYCLIC SYMMETRY MODEL option. Some of the limitations of modeling a structure using superelements or using cyclic symmetry are also discussed.

Geometry and material The structure is a fan consisting of a central hub and four blades, as shown in Figure 2.2.1-1. The blades and the hub are made up of S4R shell elements. The material is elastic, with a Young's modulus of 2 ´ 1011 Pa and a Poisson's ratio of 0.29. The density of the material is 7850 kg/m 3. All nodes along the mounting hole in the hub are fixed.

Models Four different models are considered, as follows: 1. The fan is modeled as a single structure (no superelements).

2-861

Dynamic Stress/Displacement Analyses

2. One quadrant of the fan, consisting of a quarter of the hub and a single blade, is reduced to a superelement. The fan is then modeled with four superelements (a single-level superelement structure). During superelement generation all degrees of freedom are retained for the nodes along the edges of the hub in each quadrant as well as one node at the blade tip (see Figure 2.2.1-2). 3. A single fan blade is reduced to a superelement, which is then combined with one-quarter of the hub to form a higher level superelement. Four of these superelements are then combined to form the fan (similar to the single-level superelement), thus forming a multi-level superelement structure. Nodes along the base of the fan blade and one node at the tip of the blade have all their degrees of freedom retained during generation of the fan blade superelement as shown in Figure 2.2.1-2. At the higher level superelement generation stage, nodes along the edge of the hub in each quadrant as well as the node at the blade tip have their degrees of freedom retained. 4. One quadrant of the fan, consisting of a quarter of the hub and a single blade, is modeled with and without superelements as a datum sector for the *CYCLIC SYMMETRY MODEL option. Two surfaces, which are at 90° to each other, are chosen to serve as the slave and master surfaces for the *TIE, CYCLIC SYMMETRY option. The finite element mesh contains matching nodes on the symmetry surfaces; therefore, both surfaces are defined with the *SURFACE, TYPE=NODE option. The axis of cyclic symmetry is parallel to the global z-axis and passes through the point on the x-y plane with coordinates (3.0, 3.0). The cyclic symmetry model is shown in Figure 2.2.1-3. The entire model consists of four repetitive sectors. Both a frequency analysis and a static analysis are performed on the first three models. Stress- and load-stiffening effects due to the centrifugal loading on the fan are built into the superelement stiffness during generation using the *PRELOAD HISTORY option with the NLGEOM parameter included on the *STEP option. To get the proper stress stiffening in the hub of the multi-level superelement, the centrifugal load defined in the lowest level superelement (the blade) needs to be captured with the *SLOAD CASE option and must be applied as a preload with the *SLOAD option in the next level superelement. The reduced mass matrix for each superelement is generated by including the *SUPER MASS option during the superelement generation. To improve the representation of the superelement's dynamic behavior in the global analysis, dynamic modes are extracted by including the MODES=m parameter on the *SUPER MASS option and running a *FREQUENCY preload step that extracts at least m frequencies. The reduced mass matrix obtained by the default value of m = 0 corresponds to the Guyan reduction technique, while m > 0 corresponds to the restrained mode addition technique. In the "Results and discussion" section below the solution obtained for the model without superelements (the "full model") is used as the reference solution. For the cyclic symmetry model without superelements, the eigenvalue extraction procedure was performed on the preloaded structure. The nonlinear static step has the centrifugal load applied to the blade. Fifty eigenvalues were requested using the Lanczos eigenvalue solver, which is the only eigensolver that can be used for *FREQUENCY analysis with the *CYCLIC SYMMETRY MODEL option. The *SELECT CYCLIC SYMMETRY MODES option is omitted; therefore, the eigenvalues are being extracted for all possible (three) cyclic symmetry modes. In the discussion that follows the

2-862

Dynamic Stress/Displacement Analyses

solution obtained for the cyclic symmetry model is compared with the solution for the entire 360° model as the reference solution. A similar simulation was performed for the cyclic symmetry model with superelements but without the preload step. Twenty eigenvalues were extracted and compared with the reference solution obtained for the entire 360° model with superelements.

Results and discussion Results for the frequency analysis and the static analysis appear below.

Frequency analysis for models with superelements Frequencies corresponding to the 15 lowest eigenvalues have been extracted and are tabulated in Table 2.2.1-1 for each model. To study the effect of retaining dynamic modes during superelement generation, the superelement models were run after extracting 0, 5, and 20 dynamic modes during superelement generation. While the Guyan reduction technique (m =0) yields frequencies that are reasonable compared to those of the full model, the values obtained with 5 retained modes are much closer to full model predictions, especially for the higher eigenvalues. Increasing the number of retained modes to 20 does not yield a significant improvement in the results, consistent with the fact that in the Guyan reduction technique the choice of retained degrees of freedom affects accuracy, while for the restrained mode addition technique the modes corresponding to the lowest frequencies are by definition optimal. When superelements are used in an eigenfrequency analysis, it is to be expected that the lowest eigenfrequency in the superelement model is higher than the lowest eigenfrequency in the corresponding model without superelements. This is indeed the case for the single-level superelement analysis, but for the multi-level superelement analysis the lowest eigenfrequency is below the one for the full model. This occurs because the stress and load stiffness for the lowest level superelement (the blade) are generated with the root of the blade fixed, whereas in the full model the root of the blade will move radially due to the deformation of the hub under the applied centrifugal load. Hence, the superelement stiffness is somewhat inaccurate. Since the radial displacements at the blade root are small compared to the overall dimensions of the model (of order 10 -3), the resulting error should be small, as is observed from the results. Table 2.2.1-2 shows what happens if the NLGEOM parameter is omitted during the preloading steps. It is clear that the results are significantly different from the ones that take the effect of the preload on the stiffness into account. Note that in this case the lowest eigenfrequency in the superelement models is indeed above the lowest eigenfrequency in the model without superelements.

Static analysis for models with superelements A static analysis of the fan is carried out about the preloaded base state by applying a pressure load of 105 Pa normal to the blades of the fan. The axial displacement of the outer edge of the fan blade due to the pressure load is monitored at nodes along path AB, as shown in Figure 2.2.1-1. The results are shown in Figure 2.2.1-4; there is good agreement between the solutions for the superelement models and the full model. While superelements can be generated from models that exhibit nonlinear response, it must be noted

2-863

Dynamic Stress/Displacement Analyses

that, once created, a superelement always exhibits linear response at the usage level. Hence, a preloaded superelement will produce a response equivalent to that of the response to a linear perturbation load on a preloaded full model. Consequently, the full model is analyzed by applying the centrifugal preload in a general step and the pressure load in a linear perturbation step. Since an analysis using superelements is equivalent to a perturbation step, the results obtained do not incorporate the preload deformation. Thus, if the total displacement of the structure is desired, the results of this perturbation step need to be added to the base state solution of the structure.

Static analysis and eigenvalue extraction for the cyclic symmetry model In the general static step that includes nonlinear geometry, the centrifugal load is applied to the datum sector. Only symmetric loads can be applied in general static steps with the *CYCLIC SYMMETRY MODEL option. The computed eigenvalues are identical with those obtained for the entire 360° model, as shown in the Table 2.2.1-1. The additional information obtained during the eigenvalue extraction is the cyclic symmetry mode number associated with each eigenvalue. In the case of 4 repetitive sectors, all the eigenvalues corresponding to cyclic symmetry mode 1 appear in pairs; the eigenvalues corresponding to modes 0 and 2 are single. The lowest first two eigenvalues correspond to cyclic symmetry mode 1, followed by the single eigenvalues corresponding to cyclic symmetry modes 2 and 0. For a comparison with the cyclic symmetry model option, the problem is also modeled with *MPC type CYCLSYM (see fansuperelem_mpc.inp). To verify the use of superelements with the cyclic symmetry model, it was determined that the results obtained with fansuperelem_cyclic.inp were identical to the results obtained with fansuperelem_1level_freq.inp.

Input files fan_cyclicsymmodel.inp Cyclic symmetry model with static and eigenvalue extraction steps. fansuperelem_1level_freq.inp Single-level superelement usage analysis with a frequency extraction step. fansuperelem_1level_static.inp Single-level superelement usage analysis with a static step. fansuperelem_multi_freq.inp Multi-level superelement usage analysis with a frequency extraction step. fansuperelem_multi_static.inp Multi-level superelement usage analysis with a static step. fansuperelem_freq.inp Frequency extraction without superelements. fansuperelem_static.inp

2-864

Dynamic Stress/Displacement Analyses

Static analysis without superelements. fansuperelem_mpc.inp Single-level usage analysis demonstrating the use of cyclic symmetry MPCs. fansuperelem_gen1.inp Superelement generation for a single blade used in the multi-level superelement generation file fansuperelem_gen2.inp. fansuperelem_gen2.inp Multi-level superelement generation used in fansuperelem_multi_freq.inp and fansuperelem_multi_static.inp. fansuperelem_gen3.inp Single-level superelement generation used infansuperelem_1level_freq.inp, fansuperelem_1level_static.inp, and fansuperelem_mpc.inp. fansuperelem_cyclic.inp Single-level superelement with the cyclic symmetry model used in a frequency analysis.

Tables Table 2.2.1-1 Comparison of natural frequencies for single-level and multi-level superelements with the values for the model without superelements. With substructuring: 1 With substructuring: 2 Eigenvalue level levels no. cycles/sec m=0 m=5 m=20 m=0 m=5 m=20 1 6.9464 6.7893 6.7882 6.9191 6.7665 6.7654 2 6.9464 6.7893 6.7882 6.9191 6.7665 6.7654 3 8.0024 7.7148 7.7139 8.0082 7.7228 7.7219 4 8.2007 7.8817 7.8810 8.2079 7.8909 7.8903 5 11.343 11.021 11.010 11.308 10.986 10.976 6 11.343 11.021 11.010 11.308 10.986 10.976 7 12.513 11.916 11.897 12.291 11.760 11.741 8 14.683 14.354 14.301 14.671 14.303 14.252 9 17.862 14.432 14.432 17.745 14.470 14.470 10 18.921 14.776 14.772 18.913 14.814 14.810 11 21.150 14.776 14.772 21.010 14.814 14.810 12 21.150 15.990 15.952 21.010 16.001 15.963 13 28.449 17.773 17.696 28.417 17.652 17.575 14 28.986 19.029 19.012 29.001 19.030 19.013 15 28.986 21.234 21.077 29.001 21.082 20.928

Full model 6.7881 6.7881 7.7139 7.8810 11.009 11.009 11.895 14.303 14.432 14.771 14.771 15.948 17.696 19.001 21.075

Table 2.2.1-2 Comparison of natural frequencies for single-level and two-level superelements with

2-865

Dynamic Stress/Displacement Analyses

the full model values without the use of the NLGEOM parameter. With Full Eigenvalue substructuring model no. cycles/sec 1 level 2 levels 1 4.4811 4.4811 4.4809 2 4.4811 4.4811 4.4809 3 4.5489 4.5489 4.5487 4 4.8916 4.8916 4.8914 5 9.5519 9.5519 9.5423 6 9.5519 9.5519 9.5423 7 9.7893 9.7894 9.7758 8 12.611 12.611 12.570 9 14.006 14.006 14.003 10 14.332 14.332 14.325 11 14.332 14.332 14.325 12 15.475 15.475 15.455 13 16.962 16.963 16.897 14 18.244 18.245 18.220 15 19.040 19.041 18.933

Figures Figure 2.2.1-1 Mesh used for the complete fan model.

Figure 2.2.1-2 Superelements generated.

2-866

Dynamic Stress/Displacement Analyses

Figure 2.2.1-3 Datum sector for cyclic symmetry model.

2-867

Dynamic Stress/Displacement Analyses

Figure 2.2.1-4 Displacements due to pressure loading along path AB.

2-868

Dynamic Stress/Displacement Analyses

Sample listings

2-869

Dynamic Stress/Displacement Analyses

Listing 2.2.1-1 *HEADING Superelement analysis of a fan Frequency analysis : One level superelement. Usage level: FAN=HUB+4xBLADES ** Z100: a superelement for a single blade; Z200: a superelement which contains the 1/4 hub and a superelement blade (Z100); Z300: a superelement which contains the 1/4 hub and a full blade. Requires superelement generation file fansuperelem_gen3.inp ** *RESTART,WRITE,FRE=1 ** *NODE 1, 3.50000, 3.00000, 4.00000 3, 3.46638, 3.18024, 4.00000 7, 3.18024, 3.46638, 4.00000 9, 3.00000, 3.50000, 4.00000 ** 31, 6.00000, 3.00000, 4.00000 33, 5.79830, 4.08144, 4.00000 37, 4.08144, 5.79830, 4.00000 39, 3.00000, 6.00000, 4.00000 ** 91, 6.00000, 3.00000, 0.00000 93, 5.79830, 4.08144, 0.00000 97, 4.08144, 5.79830, 0.00000 99, 3.00000, 6.00000, 0.00000 ** 100, 7.89643, 8.00249, 2.59810 9998, 3.00000, 3.00000, 4.00000 9999, 3.00000, 3.00000, 0.00000 *NGEN,LINE=C,NSET=NHUB 1,3,1,9998 3,7,1,9998 7,9,1,9998 *NGEN,LINE=C,NSET=RINGF 31,33,1,9998 33,37,1,9998

2-870

Dynamic Stress/Displacement Analyses

37,39,1,9998 *NGEN,LINE=C,NSET=RINGB 91,93,1,9999 93,97,1,9999 97,99,1,9999 *NFILL,NSET=HUB NHUB,RINGF,3,10 RINGF,RINGB,6,10 ** *NSET,NSET=PART1,GENERATE 1,91,10 9,99,10 2,8,1 32,38,1 100,100,1 ** *NCOPY,CHANGE NUMBER=100,OLD SET=PART1,SHIFT 0.,0.,0. 3.,3.,-1.,3.,3.,1.,90. *NCOPY,CHANGE NUMBER=200,OLD SET=PART1,SHIFT 0.,0.,0. 3.,3.,-1.,3.,3.,1.,180. *NCOPY,CHANGE NUMBER=300,OLD SET=PART1,SHIFT 0.,0.,0. 3.,3.,-1.,3.,3.,1.,270. ** *NSET,NSET=PART1X,GENERATE 1,91,10 *NSET,NSET=PART1Y,GENERATE 9,99,10 *NSET,NSET=PART2X,GENERATE 109,199,10 *NSET,NSET=PART2Y,GENERATE 101,191,10 *NSET,NSET=PART3X,GENERATE 201,291,10 *NSET,NSET=PART3Y,GENERATE 209,299,10 *NSET,NSET=PART4X,GENERATE 309,399,10 *NSET,NSET=PART4Y,GENERATE 301,391,10 *MPC

2-871

Dynamic Stress/Displacement Analyses

TIE,PART4X,PART1X TIE,PART2Y,PART1Y TIE,PART2X,PART3X TIE,PART4Y,PART3Y ** *NSET,NSET=NODEHUB,GENERATE 1, 9, 1 102, 108, 1 201, 209, 1 302, 308, 1 ** *ELEMENT,TYPE=Z300,ELSET=P1,FILE=FAN 901,1,2,3,4,5,6,7,8,9,11,19,21,29,31,32, 33,34,35,36,37,38,39,41,49,51,59,61,69,71,79,81, 89,91,99,100 *ELCOPY,ELEMENT SHIFT=1,OLD SET=P1, SHIFT NODES=100,NEW SET=P2 *ELCOPY,ELEMENT SHIFT=2,OLD SET=P1, SHIFT NODES=200,NEW SET=P3 *ELCOPY,ELEMENT SHIFT=3,OLD SET=P1, SHIFT NODES=300,NEW SET=P4 ** *SUPER PROPERTY,ELSET=P1 0.,0.,0. *SUPER PROPERTY,ELSET=P2 0.,0.,0. 3.,3.,0.,3.,3.,3.,90. *SUPER PROPERTY,ELSET=P3 0.,0.,0. 3.,3.,0.,3.,3.,3.,180. *SUPER PROPERTY,ELSET=P4 0.,0.,0. 3.,3.,0.,3.,3.,3.,270. ** *STEP Step 1: Eigenfrequency extraction *FREQUENCY 20, *BOUNDARY NODEHUB,ENCASTRE ** *EL PRINT,FREQ=0 *EL FILE,FREQ=0

2-872

Dynamic Stress/Displacement Analyses

*NODE PRINT,FREQ=0 *MODAL FILE,FREQ=99 ** *END STEP

2.2.2 Linear analysis of the Indian Point reactor feedwater line Product: ABAQUS/Standard This example concerns the linear analysis of an actual pipeline from a nuclear reactor and is intended to illustrate some of the issues that must be addressed in performing seismic piping analysis. The pipeline is the Indian Point Boiler Feedwater Pipe fitted with modern supports, as shown in Figure 2.2.2-1. This pipeline was tested experimentally in EPRI's full-scale testing program. The model corresponds to Configuration 1 of the line in Phase III of the testing program. The experimental results are documented in EPRI Report NP-3108 Volume 1 (1983). We first verify that the geometric/kinematic model is adequate to simulate the dynamic response accurately. For this purpose we compare predictions of the natural frequencies of the system using a coarse model and a finer model, as well as two substructure models created from the coarse mesh. These analyses are intended to verify that the models used in subsequent runs provide accurate predictions of the lower frequencies of the pipeline. We then perform linear dynamic response analysis in the time domain for one of the "snap-back" loadings applied in the physical test ( EPRI NP-3108, 1983) and compare the results with the experimental measurements. The linear dynamic response analysis results are also compared with the results of direct integration analysis (integration of all variables in the entire model, as would be performed for a generally nonlinear problem). This is done primarily for cross-verification of the two analysis procedures. These snap-back response analyses correspond to a load of 31136 N (7000 lb) applied at node 25 in the z-direction, with the pipe filled with water. This load case is referred to as test S138R1SZ in EPRI NP-3108. We also compute the pipeline's response in the frequency domain to steady excitation at node 27 in the z-direction. Experimental data are also available for comparison with these results.

Geometry and model Geometrical and material properties are taken from EPRI NP-3108 (1983). The supports are assumed to be linear springs for the purpose of these linear analyses, although their actual response is probably nonlinear. The spring stiffness values are those recommended by Tang et al. (1985). The pipe is assumed to be completely restrained in the vertical direction at the wall penetration. In the experimental snap-back test used for the comparison (test S138R1SZ), the pipe is full of water. The DENSITY parameter on the *BEAM GENERAL SECTION option is, therefore, adjusted to account for the additional mass of the water by computing a composite (steel plus water) mass per unit length of pipe. The pipeline is modeled with element type B31. This is a shear flexible beam element that uses linear interpolation of displacement and rotation between two nodes, with transverse shear behavior modeled according to Timoshenko beam theory. The element uses a lumped mass matrix because this provides

2-873

Dynamic Stress/Displacement Analyses

more accurate results in test cases. The coarse finite element model uses at least two beam elements along each straight run, with a finer division around the curved segments of the pipe to describe the curvature of the pipe with reasonable accuracy. Separate nodes are assigned for all spring supports, external loading locations, and all the points where experimental data have been recorded. The model is shown in Figure 2.2.2-2. This mesh has 74 beam elements. In typical piping systems the elbows play a dominant role in the response because of their flexibility. This could be incorporated in the model by using the ELBOW elements. However, ELBOW elements are intended for applications that involve nonlinear response within the elbows themselves and are an expensive option for linear response of the elbows, which is the case for this study. Therefore, instead of using elbow elements, we modify the geometrical properties of beam elements to model the elbows with correct flexibility. This is done by calculating the flexibility factor, k, for each elbow and modifying the moments of inertia of the beam cross-sections in these regions. The flexibility factor for an elbow is a function of two parameters. One is a geometric parameter, ¸, defined as ¸=

tR p ; r2 1 ¡ º 2

where t is the wall thickness of the curved pipe, R is the bend radius of the centerline of the curved pipe, r is the mean cross-sectional radius of the curved pipe, and º is Poisson's ratio. The other parameter is an internal pressure loading parameter, Ã. For thick sections (like the ones used in this pipe), Ã has negligible effect unless the pressures are very high and the water in this case is not pressurized. Consequently, the flexibility factor is a function of ¸ only. For the elbows in this pipeline ¸ = 0.786 for the 203 mm (8 in) section and ¸ = 0.912 for the 152 mm (6 in) section. The corresponding flexibility factors obtained from Dodge and Moore (1972) are 2.09 and 1.85. These are implemented in the model by modifying the moments of inertia of the beam cross-sections in the curved regions of the pipeline. ABAQUS provides two different options for introducing geometrical properties of a beam cross-section. One is the *BEAM GENERAL SECTION option, in which all geometric properties (area, moments of inertia) can be given without specifying the shape of the cross-section. The material data, including the density, are given on the same option. Alternatively, the geometrical properties of the cross-section can be given by using the *BEAM SECTION option. With this option the cross-section dimensions are given, and ABAQUS calculates the corresponding cross-sectional behavior by numerical integration, thus allowing for nonlinear material response in the section. When this option is used, the material properties--including density and damping coefficients--are introduced in the *MATERIAL option associated with the section. This approach is more expensive for systems in which the cross-sectional behavior is linear, since numerical integration over the section is required each time the stress must be computed. Thus, in this case we use the *BEAM GENERAL SECTION option. To verify that the mesh will provide results of adequate accuracy, the natural frequencies predicted with this model are compared with those obtained with another mesh that has twice as many elements

2-874

Dynamic Stress/Displacement Analyses

in each pipe segment. Table 2.2.2-1 shows that these two meshes provide results within 2% for the first six modes and generally quite similar frequencies up to about 30 Hz. Based on this comparison the smaller model, with 74 beam elements, is used for the remaining studies (although the larger model would add little to the cost of the linear analyses, which for either case would be based on the same number of eigenmodes: only in direct integration would the cost increase proportionally with the model size).

Superelement models In ABAQUS the dynamic response of a superelement is defined by a combination of Guyan reduction and the inclusion of some natural modes of the fully restrained superelement. Guyan reduction consists of choosing additional physical degrees of freedom to retain in the dynamic model that are not needed to connect the superelement to the rest of the mesh. In this example we use only Guyan reduction since the model is small and it is easy to identify suitable degrees of freedom to retain. A critical modeling issue with this method is the choice of retained degrees of freedom: enough degrees of freedom must be retained so that the dynamic response of the substructure is modeled with sufficient accuracy. The retained degrees of freedom should be such as to distribute the mass evenly in each substructure so that the lower frequency response of each substructure is modeled accurately. Only frequencies up to 33 Hz are generally considered important in the seismic response of piping systems such as the one studied in this example, so the retained degrees of freedom must be chosen to provide accurate modeling of the response up to that frequency. In this case the pipeline naturally divides into three segments in terms of which kinematic directions participate in the dynamic response, because the response of a pipeline is generally dominated by transverse displacement. The lower part of the pipeline, between nodes 1 and 23, is, therefore, likely to respond predominantly in degrees of freedom 1 and 2; the middle part, between nodes 23 and 49, should respond in degrees of freedom 2 and 3; and the top part, above node 49, should respond in degrees of freedom 1 and 3. Comparative tests (not documented) have been run to verify these conjectures, and two superelement models have been retained for further analysis: one in which the entire pipeline is treated as a single superelement, and one in which it is split into three superelements. In the latter case all degrees of freedom must be retained at the interface nodes to join the superelements correctly. At other nodes only some translational degrees of freedom are retained, based on the arguments presented above. The choice of which degrees of freedom to retain can be investigated inexpensively in a case such as this by numerical experiments--extracting the modes of the reduced system for the particular set of retained degrees of freedom and comparing these modes with those of the complete model. The choices made in the superelement models used here are based somewhat on such tests, although insufficient tests have been run to ensure that they are close to the optimal choice for accuracy with a given number of retained variables. For linear analysis of a model as small as this one, achieving an optimal selection of retained degrees of freedom is not critical because computer run times are short: it becomes more critical when the reduced model is used in a nonlinear analysis or where the underlying model is so large that comparative eigenvalue tests cannot be performed easily. In such cases the inclusion of natural modes of the superelement is desirable. The superelement models are shown in Figure 2.2.2-2.

2-875

Dynamic Stress/Displacement Analyses

Damping "Damping" plays an essential role in any practical dynamic analysis. In nonlinear analysis the "damping" is often modeled by introducing dissipation directly into the constitutive definition as viscosity or plasticity. In linear analysis equivalent linear damping is used to approximate dissipation mechanisms that are not modeled explicitly. Experimental estimates of equivalent linear damping, based on three different methods, are found in EPRI NP-3108 (see Table 7-6, Table 7-7, and Figure 7-15 of that report). For the load case and pipe configuration analyzed here, those results suggest that linear damping corresponding to 2.8% of critical damping in the lowest mode of the system matches the measured behavior of the structure, with the experimental results also showing that the percentage of critical damping changes from mode to mode. In spite of this all the numerical analyses reported here assume the same damping ratio for all modes included in the model, this choice being made for simplicity only. For linear dynamic analysis based on the eigenmodes, ABAQUS allows damping to be defined as a percentage of critical damping in each mode, as structural damping (proportional to nodal forces), or as Rayleigh damping (proportional to the mass and stiffness of the structure). Only the last option is possible when using direct integration, although other forms of damping can be added as discrete dashpots or in the constitutive models. In this case, results are obtained for linear dynamic analysis with modal and Rayleigh damping and for direct integration with Rayleigh damping.

Results and discussion Results are shown for four geometric models: the "coarse" (74 element) model, which has a total of 435 degrees of freedom; a finer (148 element) model, which has a total of 870 degrees of freedom; a model in which the pipeline is modeled as a single superelement (made from the coarse model), with 59 retained degrees of freedom; and a model in which the pipeline is modeled with three superelements (made from the coarse model), with 65 retained degrees of freedom. The first comparison of results is the natural frequencies of the system, as they are measured and as they are predicted by the various models. The first 24 modes are shown in Table 2.2.2-1. These modes span the frequency range from the lowest frequency (about 4.3 Hz) to about 43 Hz. In typical seismic analysis of systems such as this, the frequency range of practical importance is up to 33 Hz; on this basis these modes are more than sufficient. Only the first six modes of the actual system have been measured, so any comparison at higher frequencies is between the numerical calculations reported here and other similar computations. The results obtained with the four models correlate quite well between themselves, suggesting that the mesh and the choices of retained degrees of freedom in the superelement models are reasonable. It is particularly noteworthy that the results for the superelement models correspond extremely well with those provided by the original model, considering the large reduction in the number of degrees of freedom for the substructures. The results also correlate roughly with the analysis results obtained by EDS and reported in EPRI NP-3108: except for modes 3 and 4 the frequencies are within 10% of the EDS numbers. For the first three modes the ABAQUS results are lower than those reported by EDS. This suggests the possibility that the ABAQUS model may be too flexible. The SUPERPIPE values are

2-876

Dynamic Stress/Displacement Analyses

significantly higher than any of the other data for most modes, and the ABAQUS and the EDS results diverge from the test results after the first four modes. The results of the time history analyses are summarized in Table 2.2.2-2to Table 2.2.2-5. These analyses are based on using all 24 modes of the coarse model. Typical predicted response plots are shown in Figure 2.2.2-3 to Figure 2.2.2-7. In many cases of regular, beam-type, one-dimensional structures, the first few modes will generally establish the dynamic behavior. Although the pipeline has an irregular shape, it is worth checking how much the higher modes influence the results. This is done in this case by comparing the results using the first six modes only with the results obtained with 24 modes. The highest discrepancy (20%) is found in the predicted accelerations at certain degrees of freedom. All other results show at most 5-10% differences (see Figure 2.2.2-3and Figure 2.2.2-4). This conclusion is also supported by the steady-state results. All the ABAQUS results are reasonably self-consistent, in the sense that Rayleigh and modal damping and modal dynamics and direct integration all predict essentially the same values. The choice of 2.8% damping seems reasonable, in that oscillations caused by the snap-back are damped out almost completely in 10 seconds, which corresponds to the measurements. Unfortunately there is poor correlation between predicted and measured support reactions and maximum recorded displacements. The test results and the corresponding computations are shown in Table 2.2.2-2and Table 2.2.2-3. All the models give essentially the same values. The initial reactions and displacements are computed for a snap-back load of 31136 N (7000 lb) applied at node 25 (node 417 in EPRI report NP-3108) in the z-direction. The maximum recorded displacements occur at node 27 (node 419 in EPRI report NP-3108) in the y- and z-directions. It is assumed that the supports are in the positions relative to the pipe exactly as shown in Figure 2.2.2-1. The scatter in the experimental measurements makes it difficult to assess the validity of the stiffness chosen for the spring supports. The maximum displacement predicted at node 27 in the z-direction is almost twice that measured. This again implies the possibility that, at least in the area near this node, the model is too flexible. The generally satisfactory agreement between the natural frequency predictions and poor agreement between the maximum displacements and reactions suggests that improved modeling of the supports may be necessary. In this context it is worthwhile noting that the experimental program recorded significantly different support parameters in different tests on the pipeline system. Table 2.2.2-4 shows the results for displacement and acceleration for node 27 (which has the largest displacement). All the computed results are higher than the experimental values. The largest discrepancies between the measurements and the analysis results are in the predictions of peak forces in the springs, summarized in Table 2.2.2-5. Results obtained with the various models differ by less than 10%: these differences are caused by the differences in the models, different types of damping, and--for the direct integration results--errors in the time integration (for the modal dynamic procedure the time integration is exact). The principal cause of the discrepancies between the measurements and the computed values is believed to be the assumption of linear response in the springs in the numerical models. In reality the spring supports are either rigid struts or mechanical snubbers (Configuration 2). Especially when snubbers are used, the supports perform as nonlinear elements and must be modeled as such to reflect the support behavior accurately. Interestingly, even with the assumption of linear support behavior, the character of the oscillation is well-predicted for many variables.

2-877

Dynamic Stress/Displacement Analyses

The last group of numerical results are frequency domain calculations obtained using the *STEADY STATE DYNAMICS linear dynamic response option. The response corresponds to steady harmonic excitation at node 27 in the z-direction by a force with a peak amplitude of 31136 N (7000 lb). Such frequency domain results play a valuable role in earthquake analysis because they define the frequency ranges in which the structure's response is most amplified by the excitation. Although it is expected that the first few natural frequencies will be where the most amplification occurs, the results show clearly that some variables are strongly amplified by the fifth and sixth modes. This is observed both in the simulations and in the experimental measurements. Measured experimental results are available for the acceleration of node 33 (node 419 in EPRI NO-3108) in the z-direction and for the force in spring FW-R-21. The character of curves obtained with ABAQUS agrees well with the experimental results (see Figure 2.2.2-8and Figure 2.2.2-9), but the values differ significantly, as in the time domain results. The peak acceleration recorded is 2.0 m/s 2 (78.47 in/s 2), at the first natural frequency, while the analysis predicts 4.0 m/s 2 (157.5 in/s 2). Likewise, the peak force value recorded is 2.0 kN (450 lb), compared to 5.9 kN (1326 lb) predicted. The discrepancies are again attributed to incorrect estimates of the support stiffness or to nonlinearities in the supports.

Input files indianpoint_modaldyn_coarse.inp *MODAL DYNAMIC analysis with modal damping using the coarse model. indianpoint_modaldyn_3sub.inp *MODAL DYNAMIC analysis using the three substructure model. indianpoint_3sub_gen1.inp First superelement generation referenced by the analysis indianpoint_modaldyn_3sub.inp. indianpoint_3sub_gen2.inp Second superelement generation referenced by the analysis indianpoint_modaldyn_3sub.inp. indianpoint_3sub_gen3.inp Third superelement generation referenced by the analysis indianpoint_modaldyn_3sub.inp. indianpoint_sstate_sinedwell.inp *STEADY STATE DYNAMICS analysis corresponding to the sine dwell test performed experimentally using the coarse model. indianpoint_direct_beam_coarse.inp Direct integration analysis using the coarse model with the *BEAM SECTION option. indianpoint_sstate_modaldamp.inp *STEADY STATE DYNAMICS analysis with modal damping, covering a range of frequencies using the coarse model. indianpoint_modaldyn_1sub.inp

2-878

Dynamic Stress/Displacement Analyses

*MODAL DYNAMIC analysis with one substructure. indianpoint_1sub_gen1.inp Superelement generation referenced by the analysis indianpoint_modaldyn_1sub.inp. indianpoint_direct_beamgensect.inp Direct integration using the coarse model with *BEAM GENERAL SECTION instead of *BEAM SECTION, which, thus, runs faster on the computer since numerical integration of the cross-section is avoided. indianpoint_modaldyn_elmatrix1.inp *MODAL DYNAMIC analysis that reads and uses the superelement matrix written to the results file in indianpoint_3sub_gen1.inp, indianpoint_3sub_gen2.inp, and indianpoint_3sub_gen3.inp. indianpoint_modaldyn_elmatrix2.inp Reads and uses the element matrix written to the results file in indianpoint_modaldyn_3sub.inp. indianpoint_modaldyn_elmatrix3.inp Reads and uses the superelement matrix written to the results file in indianpoint_1sub_gen1.inp. indianpoint_modaldyn_elmatrix4.inp Reads and uses the element matrix written to the results file in indianpoint_modaldyn_1sub.inp. indianpoint_modaldamp_rayleigh.inp *MODAL DAMPING analysis with modal Rayleigh damping using the coarse mesh with the *BEAM SECTION option. indianpoint_dyn_rayleigh_3sub.inp *DYNAMIC analysis with Rayleigh damping using the three substructure model. indianpoint_rayleigh_3sub_gen1.inp First superelement generation referenced by the analysis indianpoint_dyn_rayleigh_3sub.inp. indianpoint_rayleigh_3sub_gen2.inp Second superelement generation referenced by the analysis indianpoint_dyn_rayleigh_3sub.inp. indianpoint_rayleigh_3sub_gen3.inp Third superelement generation referenced by the analysis indianpoint_dyn_rayleigh_3sub.inp. indianpoint_modaldyn_unsorted.inp One substructure *MODAL DYNAMIC analysis with unsorted node sets and unsorted retained degrees of freedom. indianpoint_unsorted_gen1.inp Superelement generation with unsorted node sets and unsorted retained degrees of freedom referenced by the analysis indianpoint_modaldyn_unsorted.inp.

2-879

Dynamic Stress/Displacement Analyses

indianpoint_lanczos.inp Same as indianpoint_modaldyn_coarse.inp, except that it uses the Lanczos solver and the eigenvectors are normalized with respect to the generalized mass. indianpoint_restart_normdisp.inp Restarts from indianpoint_lanczos.inp and continues the eigenvalue extraction with the eigenvectors normalized with respect to the maximum displacement. indianpoint_restart_bc.inp Restarts from indianpoint_lanczos.inp and continues the eigenvalue extraction with modified boundary conditions. indianpoint_overlapfreq.inp Contains two steps, which extract eigenvalues with overlapping frequency ranges.

References · Consolidated Edison Company of New York, Inc., EDS Nuclear, Inc., and Anco Engineers, Inc., Testing and Analysis of Feedwater Piping at Indian Point Unit 1, Volume 1: Damping and Frequency, EPRI NP-3108, vol. 1, July 1983. · Dodge, W. G., and S. E. Moore, "Stress Indices and Flexibility Factors for Moment Loadings in Elbows and Curved Pipe," WRC Bulletin, no. 179, December 1972. · Tang, Y. K., M. Gonin, and H. T. Tang, "Correlation Analysis of In-situ Piping Support Reactions," EPRI correspondence with HKS, May 1985.

Tables Table 2.2.2-1 Comparison of natural frequencies (Hz). Anco EDS SUPE ABAQUS R Mod (experiment PIPE coarse finer single e mesh mes super ) h 1 4.20 4.30 5.30 4.25 4.26 4.25 2 6.80 6.80 8.10 6.27 6.25 6.27 3 8.30 8.80 12.00 7.29 7.29 7.30 4 12.60 10.6 13.30 12.80 12.6 12.87 0 6 5 15.40 13.0 14.40 13.18 13.1 13.19 0 4 6 16.70 14.5 15.90 13.90 13.7 13.91 0 5 7 16.2 18.30 15.11 15.9 14.34

2-880

three super s 4.25 6.27 7.30 12.86 13.20 13.92 14.39

Dynamic Stress/Displacement Analyses

0 8

19.40

16.30

9

20.20

16.89

10

22.20

17.43

11

18.02

12

19.58

13

23.43

14

23.99

15

24.27

16

24.80

17

26.82

18

29.53

19

30.61

20

30.95

21

31.52

22

33.50

23

39.09

24

39.86

8 16.0 7 16.8 1 17.8 2 19.0 7 20.1 0 21.4 5 22.1 3 23.5 8 24.1 5 26.8 4 30.1 8 30.6 0 32.5 8 33.1 1 35.0 8 39.6 5 43.2 5

16.24

16.31

16.43

16.43

17.17

17.20

18.10

18.10

20.05

20.01

23.98

24.00

24.47

24.47

24.97

24.96

25.34

25.28

27.63

27.56

30.31

30.55

31.08

31.06

31.43

31.43

32.00

31.98

33.76

33.77

39.75

39.97

42.98

42.97

Table 2.2.2-2 Comparison of initial support reactions. Snap-back Test No. S138R1SZ; 31136 N (7000 lb) at node 25, z-direction. NOD SUPPOR Anco TEST N (lb) E T 15 FW-R-11 -8000 (-1798.6 ) 22 FW-R-13 30000 (6744.6) 23 FW-R-14 -252 (-56.7) 35 FW-R-17 23625 (5311.4)

ABAQUS N (lb) -11712 (-2633) 29352 -3754 102

(6599) (-844) (-22.8)

2-881

Dynamic Stress/Displacement Analyses

35 39 39

FW-R-18 FW-R-20 FW-R-21

49 53 53 56 56

FW-R-23 FW-R-24 FW-R-25 FW-R-27 FW-R-28

10025 24000 -2450 0 8000 -4324 2000 432 156

(2553.8) (5395.7) (-5508.1 ) (1798.6) (-972.1) (449.6) (97.1) (35.1)

-18468 4212 25016

(-4152) ( 947) (5624)

24348 -4057 -816 -1801 -799

(5474) (-912) (-183) (-405) (-180)

Table 2.2.2-3 Comparison of maximum displacements. ABAQUS Anco Measured ABAQUS NODE NODE No. No. mm (in) mm (in) 27 419-Y -16.0 (-.630) -26.85 (-1.057) 27 419-Z 37.81 (1.49) 65.72 (2.587)

Table 2.2.2-4 Peak displacement and acceleration values at node 27. Variable Measured ABAQUS Modal, Modal, Direct (Anco) 2.8% modal Rayleigh integration damping damping uy (mm) -0.024/0.024 -0.029/0.029 -0.031/0.03 -0.031/0.031 1 uz (mm) -0.038/0.038 -0.058/0.066 -0.062/0.05 -0.063/0.068 9 -47.6/40.9 -42.1/50.8 -49.6/49.9 -83.8/91.0 u Äz (m/s2) The high acceleration amplitude reported for the ABAQUS direct integration analysis occurs only during the first few increments, after which it reduces to -31.6/48.6 m/s 2.

Table 2.2.2-5 Peak reaction forces at supports (in kN). Support Measured ABAQUS Modal, Modal, number (Anco) 2.8% modal Rayleigh damping damping FW-R-11 -16.44/19.22 -19.80/13.42 -19.90/14.26 FW-R-13 -15.10/29.91 -18.94/24.45 -19.46/23.61 FW-R-14 -7.22/12.00 -9.34/7.35 -10.23/10.00 FW-R-17 34.40/26.20 -7.50/10.59 -.17/9.25 FW-R-18 -14.30/14.40 -33.26/32.06 -33.58/31.61 FW-R-20 -25.60/26.90 -7.54/8.79 -7.98/8.50 FW-R-21 -24.50/23.80 -25.55/24.47 -26.38/25.30 FW-R-23 -15.30/16.00 -25.39/24.63 -26.06/25.36

2-882

Direct integration -21.82/15.76 -28.50/21.98 -12.54/9.03 -7.91/10.97 -33.46/32.63 -8.07/10.60 -27.78/25.26 -25.40/24.35

Dynamic Stress/Displacement Analyses

FW-R-24 FW-R-25 FW-R-27 FW-R-28

-9.61/7.30 -6.77/6.21 -3.76/3.04 -1.10/1.82

-7.17/6.87 -3.48/4.36 -4.12/4.00 -1.53/1.08

-7.69/7.20 -3.34/4.55 -3.78/3.80 -1.62/1.15

-8.23/8.64 -7.13/4.71 -4.29/4.43 -1.79/1.44

Figures Figure 2.2.2-1 Indian Point boiler feedwater line: modern supports, Configuration 1.

Figure 2.2.2-2 Basic mesh and superelement models.

2-883

Dynamic Stress/Displacement Analyses

Figure 2.2.2-3 z-displacement at node 27, modal analysis with 24 modes.

Figure 2.2.2-4 z-displacement at node 27, modal analysis with 6 modes.

2-884

Dynamic Stress/Displacement Analyses

Figure 2.2.2-5 z-displacement at node 27, direct integration analysis.

Figure 2.2.2-6 z-direction acceleration at node 27, modal analysis with 24 modes.

2-885

Dynamic Stress/Displacement Analyses

Figure 2.2.2-7 Force in spring support FW-R-11, modal analysis with 24 modes.

Figure 2.2.2-8 Comparison of z-direction acceleration at node 33 between experimental steady-state results (solid line) and ABAQUS (dashed line).

2-886

Dynamic Stress/Displacement Analyses

Figure 2.2.2-9 Comparison of force in spring support FW-R-21, between experimental steady-state results (solid line) and ABAQUS (dashed line).

2-887

Dynamic Stress/Displacement Analyses

Sample listings

2-888

Dynamic Stress/Displacement Analyses

Listing 2.2.2-1 *HEADING INDIAN POINT FEEDWATER LINE WITH SPRING SUPPORTS ** BEAM ELEMENTS WITH MODAL DYNAMICS, ** MODAL DAMPING *NODE 1, 0., 423., -234.96 3, 0., 423., -150.96 5, 0., 435., -138.96 6, 0., 474., -138.96 8, 0., 486., -126.96 10, 0., 486., -75.96 11, 0., 486., -51.96 12, 0., 486., -18.00 13, 0., 486., 9.00 15, 0., 486., 144.5 16, 0., 486., 159. 18, 8.484, 494.484, 171. 19, 8.484,494.484,171. 21, 16.93, 497.96, 171. 22, 19.8125, 497.96 , 171. 23, 29.125 ,497.96, 171. 25, 200.72, 497.96, 171.00 27, 260.72, 497.96, 171. 29, 272.72, 509.96, 171.00 31, 272.72, 569.964, 171.00 33, 280.44, 581.96, 180.19 35, 330.1 , 581.96, 239.3 36, 335.21, 581.96, 245.46 38, 342.91, 593.96, 254.65 39, 342.91 , 628. , 254.65 40, 342.91, 660., 254.65 42, 342.91, 706., 254.65 44, 340.22, 714.48, 256.91 46, 296.57, 771.47, 293.54 48, 282.36, 779.95, 289.80 49, 278.50, 779.95, 285.20 50,274.644, 779.95, 280.61 52, 266.93, 791.95, 271.42 53, 266.93, 801., 271.42 54, 266.93, 876.00, 271.42 56, 266.93, 990.96, 271.42

2-889

Dynamic Stress/Displacement Analyses

57, 266.93, 1000.27, 271.42 59, 278.88, 1012.27, 272.46 61, 335.26, 1012.27, 277.39 63, 343.40, 1012.27, 281.64 64, 366.97, 1012.27, 309.73 65, 369.52, 1012.27, 312.76 66, 379.16, 1012.27, 324.25 67, 388.8, 1012.27, 335.74 68, 389.11, 1012.27, 336.11 70, 396.83, 1024.27, 345.3 71, 396.83, 1027.27, 345.3 72, 396.83, 1033.27, 345.3 73, 396.83, 1040.95, 345.3 75, 389.93, 1049.95, 351.08 76, 380.74, 1049.95, 358.8 *NGEN 1,3 8,10 13,15 23,25 25,27 29,31 33,35 40,42 44,46 54,57 59,61 *NGEN,LINE=C 3,5,1,, 0., 435., -150.96 6,8,1,, 0., 474., -126.96 16,18,1,, 8.484, 494.48, 159.00 19, 21,1,, 16.932, 485.96, 171.00 27,29,1,, 260.724, 509.96, 171.00 31,33,1,, 280.44, 569.96, 180.19 36,38,1,, 335.21, 593.96, 245.46 42,44,1,, 333.71, 706.00, 262.37 46,48,1,, 288.85, 771.47, 284.35 50,52,1,, 274.64, 791.95, 280.61 57,59,1,, 278.88, 1000.27, 272.46 61,63,1,, 334.21, 1012.27, 289.34 68,70,1,, 389.11, 1024.27, 336.11 73,75,1,, 389.93, 1040.95, 351.08 **

2-890

Dynamic Stress/Displacement Analyses

** SPRING DEFINITIONS ** *NODE,NSET=SPRS 115, 24.91, 475.93, 144.5 122, 19.81, 497.96, 219.5 123, 29.13, 597.41, 160.55 135, 299.94, 555., 239.30 235, 330.10, 599.46, 239.30 139, 364.74, 628.00, 220.25 239, 359.58, 628.00, 291.83 149,278.50, 792.45, 285.20 153, 321.48, 801.00, 318.12 253, 314.43, 801.00, 212.09 156, 311.81, 990.96, 215.36 256,290.46, 1008.88, 299.46 *ELEMENT,TYPE=SPRINGA,ELSET=FWR11 1001,15,115 *ELEMENT,TYPE=SPRINGA,ELSET=FWR13 1002,22,122 *ELEMENT,TYPE=SPRINGA,ELSET=FWR14 1003,23,123 *ELEMENT,TYPE=SPRINGA,ELSET=FWR17 1004,35,135 *ELEMENT,TYPE=SPRINGA,ELSET=FWR18 1005,35,235 *ELEMENT,TYPE=SPRINGA,ELSET=FWR20 1006,39,139 *ELEMENT,TYPE=SPRINGA,ELSET=FWR21 1007,39,239 *ELEMENT,TYPE=SPRINGA,ELSET=FWR23 1008,49,149 *ELEMENT,TYPE=SPRINGA,ELSET=FWR25 1009,53,153 *ELEMENT,TYPE=SPRINGA,ELSET=FWR24 1010,53,253 *ELEMENT,TYPE=SPRINGA,ELSET=FWR27 1011,56,156 *ELEMENT,TYPE=SPRINGA,ELSET=FWR28 1012,56,256 *ELSET,ELSET=SPRINGS FWR11, FWR13, FWR14, FWR17, FWR18, FWR20, FWR21, FWR23, FWR24, FWR25, FWR27, FWR28 *SPRING ,ELSET=FWR11

2-891

Dynamic Stress/Displacement Analyses

17700. , *SPRING,ELSET=FWR13 119600., *SPRING ,ELSET=FWR14 403000., *SPRING ,ELSET=FWR17 97900., *SPRING,ELSET=FWR18 228000., *SPRING ,ELSET=FWR20 86300., *SPRING,ELSET=FWR21 86300., *SPRING,ELSET=FWR23 319000., *SPRING,ELSET=FWR24 56800., *SPRING,ELSET=FWR25 39100., *SPRING,ELSET=FWR27 55500., *SPRING,ELSET=FWR28 68000., ** ** PIPE DEFINITIONS ** *ELEMENT,TYPE=B31 1,1,2 14,13,14 20,19,20 28,25,26

2-892

Dynamic Stress/Displacement Analyses

53,49,50 *ELEMENT,TYPE=B31,ELSET=ONE 24,22,23 *ELGEN 1,12 14,5 20,3 24,3 28,24 53,27 *MPC BEAM,18,19 *ELSET,ELSET=D8 1,2,5,8,9,10,11,12,14,16,22 ,15 24,25,26,28,29,32,33,36,37,38,41,42,43,44,47,48 51,53,56,57,58,59,60,63,64,67,68,71 74, *ELSET,ELSET=D8E 3, 4, 6, 7,17,18,20,21,30,31,34,35,39,40 45,46,49,50,54,55,61,62,65,66,72,73 *ELSET,ELSET=BF57 69,70 *ELSET,ELSET=BWR 75, *ELSET,ELSET=D6 76,79 *ELSET,ELSET=D6E 77,78 *BEAM GENERAL SECTION,ELSET=D8 ,SECTION=GENERAL, DENSITY= .0010691 12.763 , 105.317 , , 105.317 , 210.635 1. , , -1. 27.9E6 , 10.73E6 *BEAM GENERAL SECTION,ELSET=D8E,SECTION=GENERAL, DENSITY=.0010691 12.763 , 50.439 , , 50.439 , 210.635 1. , , -1. 27.9E6 , 10.73E6 *BEAM GENERAL SECTION,ELSET=D6 ,SECTION=GENERAL, DENSITY=0.00102423 8.405 , 40.295 , , 40.295 , 80.589 1., 27.9E6 , 10.73E6

2-893

Dynamic Stress/Displacement Analyses

*BEAM GENERAL SECTION,ELSET=D6E,SECTION=GENERAL, DENSITY=0.00102423 8.405 , 21.828, ,21.828, 80.589 1., 27.9E6 , 10.73E6 *BEAM GENERAL SECTION,ELSET=BWR,SECTION=GENERAL, DENSITY=0.0013266 10.4806 , 67.143 , , 67.143 , 134.29 1. , , -1. 27.9E6 , 10.73E6 *BEAM GENERAL SECTION,ELSET=BF57,SECTION=GENERAL, DENSITY=0.002591 30.631 ,161.77 , , 161.77 , 323.53 1. , , -1. 27.9E6 , 10.73E6 *NSET,NSET=SMALL 1,25,27,45,55 *BOUNDARY 1,1,6 76,1,6 70,1 70,2 10,2 SPRS,1,3 *RESTART,WRITE,FREQUENCY=100 *STEP *FREQUENCY 24, *EL PRINT,ELSET=SPRINGS,FREQUENCY=1 S11,E11 *EL FILE,ELSET=SPRINGS ELEN, *EL PRINT,ELSET=ONE,FREQUENCY=1 SENER, ELSE, *EL FILE,ELSET=ONE ENER, ELEN, *NODE PRINT,FREQUENCY=0 *OUTPUT,FIELD *ELEMENT OUTPUT,ELSET=SPRINGS ELEN, *ELEMENT OUTPUT,ELSET=ONE

2-894

Dynamic Stress/Displacement Analyses

ENER, ELEN, *NODE OUTPUT *END STEP *STEP,PERTURBATION SNAP LOAD---APPLIED STATICALLY *STATIC *EL PRINT,ELSET=SPRINGS,FREQUENCY=1 S,E *CLOAD 25,3,7000. *NODE PRINT U, RF, *NODE FILE,NSET=SMALL,FREQUENCY=1 U,RF *OUTPUT,FIELD, FREQUENCY=1 *ELEMENT OUTPUT, ELSET=SPRINGS ELEN, ENER, S,E *ELEMENT OUTPUT,ELSET=ONE ELEN, ENER, S,E *NODE OUTPUT,NSET=SMALL U, RF, *OUTPUT,HISTORY,FREQUENCY=1 *NODE OUTPUT,NSET=SMALL U,RF *END STEP *STEP RELEASE LOAD *MODAL DYNAMIC,CONTINUE=YES 0.02,10.0 *MODAL DAMPING,MODAL=DIRECT 1,24,0.028 *PRINT,FREQUENCY=100 *NODE PRINT,NSET=SMALL,FREQUENCY=100 U, *NODE FILE,NSET=SMALL,FREQUENCY=100 U,V,A,RF

2-895

Dynamic Stress/Displacement Analyses

*EL FILE,ELSET=SPRINGS,FREQUENCY=100 S, *EL PRINT,ELSET=SPRINGS,FREQUENCY=100 S, *OUTPUT,FIELD,FREQUENCY=100 *NODE OUTPUT,NSET=SMALL U,V,A,RF *ELEMENT OUTPUT,ELSET=SPRINGS S, *OUTPUT,HISTORY,FREQUENCY=100 *NODE OUTPUT,NSET=SMALL U,V,A,RF *ELEMENT OUTPUT,ELSET=SPRINGS S, *END STEP

2-896

Dynamic Stress/Displacement Analyses

Listing 2.2.2-2 *HEADING INDIAN POINT FEEDWATER LINE WITH SPRING SUPPORTS ** BEAM ELEMENTS WITH STEADY STATE SINE DWELL *NODE 1, 0., 423., -234.96 3, 0., 423., -150.96 5, 0., 435., -138.96 6, 0., 474., -138.96 8, 0., 486., -126.96 10, 0., 486., -75.96 11, 0., 486., -51.96 12, 0., 486., -18.00 13, 0., 486., 9.00 15, 0., 486., 144.5 16, 0., 486., 159. 18, 8.484, 494.484, 171. 19, 8.484,494.484,171. 21, 16.93, 497.96, 171. 22, 19.8125, 497.96 , 171. 23, 29.125 ,497.96, 171. 25, 200.72, 497.96, 171.00 27, 260.72, 497.96, 171. 29, 272.72, 509.96, 171.00 31, 272.72, 569.964, 171.00 33, 280.44, 581.96, 180.19 35, 330.1 , 581.96, 239.3 36, 335.21, 581.96, 245.46 38, 342.91, 593.96, 254.65 39, 342.91 , 628. , 254.65 40, 342.91, 660., 254.65 42, 342.91, 706., 254.65 44, 340.22, 714.48, 256.91 46, 296.57, 771.47, 293.54 48, 282.36, 779.95, 289.80 49, 278.50, 779.95, 285.20 50,274.644, 779.95, 280.61 52, 266.93, 791.95, 271.42 53, 266.93, 801., 271.42 54, 266.93, 876.00, 271.42 56, 266.93, 990.96, 271.42 57, 266.93, 1000.27, 271.42

2-897

Dynamic Stress/Displacement Analyses

59, 278.88, 1012.27, 272.46 61, 335.26, 1012.27, 277.39 63, 343.40, 1012.27, 281.64 64, 366.97, 1012.27, 309.73 65, 369.52, 1012.27, 312.76 66, 379.16, 1012.27, 324.25 67, 388.8, 1012.27, 335.74 68, 389.11, 1012.27, 336.11 70, 396.83, 1024.27, 345.3 71, 396.83, 1027.27, 345.3 72, 396.83, 1033.27, 345.3 73, 396.83, 1040.95, 345.3 75, 389.93, 1049.95, 351.08 76, 380.74, 1049.95, 358.8 *NGEN 1,3 8,10 13,15 23,25 25,27 29,31 33,35 40,42 44,46 54,57 59,61 *NGEN,LINE=C 3,5,1,, 0., 435., -150.96 6,8,1,, 0., 474., -126.96 16,18,1,, 8.484, 494.48, 159.00 19, 21,1,, 16.932, 485.96, 171.00 27,29,1,, 260.724, 509.96, 171.00 31,33,1,, 280.44, 569.96, 180.19 36,38,1,, 335.21, 593.96, 245.46 42,44,1,, 333.71, 706.00, 262.37 46,48,1,, 288.85, 771.47, 284.35 50,52,1,, 274.64, 791.95, 280.61 57,59,1,, 278.88, 1000.27, 272.46 61,63,1,, 334.21, 1012.27, 289.34 68,70,1,, 389.11, 1024.27, 336.11 73,75,1,, 389.93, 1040.95, 351.08 ** ** SPRING DEFINITIONS

2-898

Dynamic Stress/Displacement Analyses

** *NODE,NSET=SPRS 115, 24.91, 475.93, 144.5 122, 19.81, 497.96, 219.5 123, 29.13, 597.41, 160.55 135, 299.94, 555., 239.30 235, 330.10, 599.46, 239.30 139, 364.74, 628.00, 220.25 239, 359.58, 628.00, 291.83 149,278.50, 792.45, 285.20 153, 321.48, 801.00, 318.12 253, 314.43, 801.00, 212.09 156, 311.81, 990.96, 215.36 256,290.46, 1008.88, 299.46 *NSET,NSET=NPDR 25,27,33,36,42,1,76,15,22,23,35,39,49,53,56 *ELEMENT,TYPE=SPRINGA,ELSET=FWR11 1001,15,115 *ELEMENT,TYPE=SPRINGA,ELSET=FWR13 1002,22,122 *ELEMENT,TYPE=SPRINGA,ELSET=FWR14 1003,23,123 *ELEMENT,TYPE=SPRINGA,ELSET=FWR17 1004,35,135 *ELEMENT,TYPE=SPRINGA,ELSET=FWR18 1005,35,235 *ELEMENT,TYPE=SPRINGA,ELSET=FWR20 1006,39,139 *ELEMENT,TYPE=SPRINGA,ELSET=FWR21 1007,39,239 *ELEMENT,TYPE=SPRINGA,ELSET=FWR23 1008,49,149 *ELEMENT,TYPE=SPRINGA,ELSET=FWR25 1009,53,153 *ELEMENT,TYPE=SPRINGA,ELSET=FWR24 1010,53,253 *ELEMENT,TYPE=SPRINGA,ELSET=FWR27 1011,56,156 *ELEMENT,TYPE=SPRINGA,ELSET=FWR28 1012,56,256 *ELSET,ELSET=SPRINGS FWR11, FWR13, FWR14, FWR17, FWR18, FWR20, FWR21, FWR23, FWR24, FWR25, FWR27, FWR28

2-899

Dynamic Stress/Displacement Analyses

*SPRING ,ELSET=FWR11 17700. , *SPRING,ELSET=FWR13 119600., *SPRING ,ELSET=FWR14 403000., *SPRING ,ELSET=FWR17 97900., *SPRING,ELSET=FWR18 228000., *SPRING ,ELSET=FWR20 86300., *SPRING,ELSET=FWR21 86300., *SPRING,ELSET=FWR23 319000., *SPRING,ELSET=FWR24 56800., *SPRING,ELSET=FWR25 39100., *SPRING,ELSET=FWR27 55500., *SPRING,ELSET=FWR28 68000., ** ** PIPE DEFINITIONS ** *ELEMENT,TYPE=B31 1,1,2 14,13,14 20,19,20

2-900

Dynamic Stress/Displacement Analyses

24,22,23 28,25,26 53,49,50 *ELGEN 1,12 14,5 20,3 24,3 28,24 53,27 *MPC BEAM,18,19 *ELSET,ELSET=D8 1,2,5,8,9,10,11,12,14,16,22 ,15 24,25,26,28,29,32,33,36,37,38,41,42,43,44,47,48 51,53,56,57,58,59,60,63,64,67,68,71 74, *ELSET,ELSET=D8E 3, 4, 6, 7,17,18,20,21,30,31,34,35,39,40 45,46,49,50,54,55,61,62,65,66,72,73 *ELSET,ELSET=BF57 69,70 *ELSET,ELSET=BWR 75, *ELSET,ELSET=D6 76,79 *ELSET,ELSET=D6E 77,78 *BEAM GENERAL SECTION,ELSET=D8 ,SECTION=GENERAL, DENSITY= .0010691 12.763 , 105.317 , , 105.317 , 210.635 1. , , -1. 27.9E6 , 10.73E6 *BEAM GENERAL SECTION,ELSET=D8E,SECTION=GENERAL, DENSITY=.0010691 12.763 , 50.439 , , 50.439 , 210.635 1. , , -1. 27.9E6 , 10.73E6 *BEAM GENERAL SECTION,ELSET=D6 ,SECTION=GENERAL, DENSITY=0.00102423 8.405 , 40.295 , , 40.295 , 80.589 1., 27.9E6 , 10.73E6

2-901

Dynamic Stress/Displacement Analyses

*BEAM GENERAL SECTION,ELSET=D6E,SECTION=GENERAL, DENSITY=0.00102423 8.405 , 21.828, ,21.828, 80.589 1., 27.9E6 , 10.73E6 *BEAM GENERAL SECTION,ELSET=BWR,SECTION=GENERAL, DENSITY=0.0013266 10.4806 , 67.143 , , 67.143 , 134.29 1. , , -1. 27.9E6 , 10.73E6 *BEAM GENERAL SECTION,ELSET=BF57,SECTION=GENERAL, DENSITY=0.002591 30.631 ,161.77 , , 161.77 , 323.53 1. , , -1. 27.9E6 , 10.73E6 *NSET,NSET=SMALL 25,27,33 *BOUNDARY 1,1,6 76,1,6 70,1 70,2 10,2 SPRS,1,3 *AMPLITUDE,NAME=AMP 0.0,1.0,2.0,18.46,2.4,26.54,2.8,36.16, 3.0,41.55,3.4,53.35,3.8,66.64,4.0,73.84, 4.1,77.58,4.2,81.44,4.3,85.34,4.4,89.35, 4.6,97.66,4.8,106.34,5.0,115.38,5.2,124.79, 5.4,134.58,5.6,144.73,5.8,155.26,6.0,166.15, 6.1,171.73,6.2,177.41,6.35,186.1,6.4,189.04, 6.6,201.04,6.8,213.41,7.0,226.15,7.2,239.26, 7.4,252.73,7.8,280.79,8.0,295.38 *STEP *FREQUENCY 24, *EL PRINT,ELSET=SPRINGS S11,E11 *NODE PRINT,FREQUENCY=0 *END STEP *STEP *STEADY STATE DYNAMICS,FREQUENCY SCALE=LINEAR 0.02,2.0,3,,

2-902

Dynamic Stress/Displacement Analyses

2.4,8.0,27,1.0 *CLOAD,AMPLITUDE=AMP 27,3,1.0 *MODAL DAMPING,MODAL=DIRECT 1,24,0.028 *EL PRINT,ELSET=SPRINGS,FREQUENCY=10 S11,E11 *NODE PRINT,NSET=SMALL,FREQUENCY=10 U, *NODE FILE,NSET=SMALL,FREQUENCY=10 U,V,A *MODAL PRINT,FREQUENCY=10 GU, GA, GPU, *EL FILE,ELSET=SPRINGS,FREQUENCY=10 S, *OUTPUT,FIELD,FREQUENCY=10 *NODE OUTPUT,NSET=SMALL U,V,A *ELEMENT OUTPUT,ELSET=SPRINGS S, *OUTPUT,HISTORY,FREQUENCY=10 *NODE OUTPUT,NSET=SMALL U,V,A *ELEMENT OUTPUT,ELSET=SPRINGS S, *END STEP

2.2.3 Response spectra of a three-dimensional frame building Product: ABAQUS/Standard The purpose of this example is to verify the different summation methods for natural modes in the *RESPONSE SPECTRUM procedure. To compare the five different methods that are available in ABAQUS, a three-dimensional model with closely spaced modes is examined.

Geometry and model A four-story steel-frame building is analyzed. All columns in the building have the same geometric properties. However, as shown in Figure 2.2.3-1, the properties of the beams in Frames 1 and 2 are different, as compared to those in Frames 3 and 4, to move the center of mass of the structure away from its geometric center. Eigenvalue extraction performed on the model shows that many of the 30 modes that cover the frequency range up to 40 Hz are closely spaced. An acceleration spectrum based on the El Centro earthquake record is applied in the x-y plane. The FORTRAN program given in

2-903

Dynamic Stress/Displacement Analyses

frameresponsespect_acc.f is used to generate the spectrum. The frequency range is chosen between 0.1 Hz and 40 Hz, and the number of points at which the spectrum is calculated is set at 501. Only one spectrum curve is requested for 2% damping.

Results and discussion As described in ``Linear analysis of a rod under dynamic loading,'' Section 1.4.9 of the ABAQUS Benchmarks Manual, for structures with well-separated modes the TENP and the CQC methods reduce to the SRSS method, while the NRL and the ABS methods give similar results. Hence, for such structures, two summation rules would suffice, with ABS providing the more conservative results. However, when structures with closely spaced modes are analyzed, all five summation rules can yield very different results. This is even more apparent in three-dimensional problems. In the present example, the plane of the earthquake motion lies along the x-axis, so we expect that the structural response will be dominated by Frames 1 and 3 and will result in a significant base shear in the x-direction. All five methods are compared against a modal time history response using the same El Centro acceleration record in Table 2.2.3-1, where the base shear forces are summed up in the plane of each frame Si , where i is the frame number. This comparison shows that the best approximation is generated by the CQC method. The other methods overestimate the shear in the y-direction, and some of them underestimate the base shear in the x-direction. The CQC method is generally recommended for asymmetrical three-dimensional problems with closely spaced structural modes. This method takes into account the sign of the mode shapes through cross-modal correlation factors and can correctly predict the response in directions perpendicular to the direction of excitation.

Input files frameresponsespect_freq.inp *FREQUENCY analysis. frameresponsespect_rs.inp *RESPONSE SPECTRUM analysis. frameresponsespect_modal.inp *MODAL DYNAMIC analysis. frameresponsespect_acc.f FORTRAN program that will produce the acceleration spectrum needed to run frameresponsespect_rs.inp.

Table Table 2.2.3-1 Comparison of base shear forces for different summation methods. Method S1 (kip) S2 (kip) S3 (kip) S4 (kip) Time history -25.5 14.0 -37.0 -22.8 ABS 52.5 52.5 69.6 69.6

2-904

Dynamic Stress/Displacement Analyses

SRSS TENP NRL CQC

20.9 33.1 29.3 26.6

20.9 33.1 29.3 14.6

26.8 38.8 37.2 31.6

26.8 38.8 37.2 22.1

Figure Figure 2.2.3-1 Three-dimensional frame system.

Sample listings

2-905

Dynamic Stress/Displacement Analyses

Listing 2.2.3-1 *HEADING 3-D BUILDING SUBJECTED TO EARTHQUAKE RESP. SPECTRUM *RESTART,WRITE,FREQUENCY=99 *NODE,NSET=BOT 1, 5,200.,0.,0.,0. 9,350.,0.,0.,0. 13,550.,0.,0.,0. 17,550.,200.,0. 21,550.,350.,0. 25,550.,550.,0. 29,350.,550.,0. 33,200.,550.,0. 37,0.,550.,0. 41,0.,350.,0. 45,0.,200.,0. *NCOPY,OLD SET=BOT,NEW SET=TOP,SHIFT, CHANGE NUMBER=16000 0.,0.,400. 0.,0.,0.,0.,0.,10.,0. *NFILL BOT,TOP,16,1000 *NGEN 4021,4025,1 *NGEN,NSET=B1 4001,4005,1 4005,4009,1 4009,4013,1 *NGEN,NSET=B3 4013,4017,1 4017,4021,1 4021,4024,1 *NCOPY,OLD SET=B1,NEW SET=B2,REFLECT=POINT, CHANGE NUMBER=24 275.,275,100. *NCOPY,OLD SET=B3,NEW SET=B4,REFLECT=POINT, CHANGE NUMBER=24 275.,275,100. *NSET,NSET=BOT1 B1,B2,B3,B4

2-906

Dynamic Stress/Displacement Analyses

*NCOPY,OLD SET=BOT1,NEW SET=TOP1,SHIFT, CHANGE NUMBER=12000 0.,0.,300. 0.,0.,0.,0.,0.,10.,0. *NFILL BOT1,TOP1,3,4000 ** ** NODE USED TO DEFINE THE SECTION ORIENTATION ** OF ELSET C1 *NODE 50001,1000,0 ** **CREATE ALL COLUMNS *ELEMENT,TYPE=B32,ELSET=C1 1,1,1001,2001,50001 *ELGEN,ELSET=C1 1,8,2000,1,12,4,8 **CREATE BEAMS IN FRAME 1 *ELEMENT,TYPE=B32,ELSET=B1 101,4001,4002,4003 *ELGEN,ELSET=B1 101,4,4000,1,6,2,4 **CREATE BEAMS IN FRAME 2 *ELEMENT,TYPE=B32,ELSET=B2 125,4013,4014,4015 *ELGEN,ELSET=B2 125,4,4000,1,6,2,4 **CREATE BEAMS IN FRAME 3 *ELEMENT,TYPE=B32,ELSET=B3 149,4025,4026,4027 *ELGEN,ELSET=B3 149,4,4000,1,6,2,4 **CREATE BEAMS IN FRAME 4 *ELEMENT,TYPE=B32,ELSET=B4 173,4037,4038,4039 *ELGEN,ELSET=B4 173,4,4000,1,5,2,4 *ELEMENT,TYPE=B32,ELSET=B4 193,4047,4048,4001 194,8047,8048,8001 195,12047,12048,12001 196,16047,16048,16001 *ELSET,ELSET=THREE

2-907

Dynamic Stress/Displacement Analyses

1,9,104 *MATERIAL,NAME=STEEL *ELASTIC 30.E6, *DENSITY 0.000728, *BEAM SECTION,SECTION=BOX,MATERIAL=STEEL,ELSET=C1 14.,14.,1.5,1.5,1.5,1.5 *BEAM SECTION,SECTION=BOX,MATERIAL=STEEL,ELSET=B1 8.0,10.,1.0,1.0,1.0,1.0 0.,1.,0. *BEAM SECTION,SECTION=BOX,MATERIAL=STEEL,ELSET=B2 8.0,10.,1.0,1.0,1.0,1.0 -1.,0.,0. *BEAM SECTION,SECTION=BOX,MATERIAL=STEEL,ELSET=B3 12.,14.,1.2,1.2,1.2,1.2 0.,-1.,0. *BEAM SECTION,SECTION=BOX,MATERIAL=STEEL,ELSET=B4 12.,14.,1.2,1.2,1.2,1.2 1.,0.,0. *BOUNDARY BOT,1,6 *STEP *FREQUENCY 30, *NODE PRINT,NSET=TOP U, *EL PRINT,FREQUENCY=0 *EL FILE,ELSET=THREE SF, *OUTPUT,FIELD *ELEMENT OUTPUT,ELSET=THREE SF, *NODE FILE,NSET=TOP U, *OUTPUT,FIELD *NODE OUTPUT,NSET=TOP U, *MODAL FILE *OUTPUT,HISTORY,FREQUENCY=1 *MODAL OUTPUT *END STEP

2-908

Dynamic Stress/Displacement Analyses

Listing 2.2.3-2 *HEADING RESPONSE SPECTRUM FOR 3-D BUILDING *RESTART,READ,STEP=1,INC=1,WRITE,FREQUENCY=0 *ELSET,ELSET=SMALL 1,9,104,112,116,148,152,160,172,176 *SPECTRUM,TYPE=ACCELERATION,INPUT=SPECTRUM.ACC, NAME=SPEC *STEP *RESPONSE SPECTRUM,SUM=ABS,COMP=ALGEBRAIC SPEC,1.,0.,0.,1. *MODAL DAMPING,MODAL=DIRECT 1,30, 0.02 *EL PRINT,ELSET=SMALL SF, *NODE PRINT,NSET=TOP U, *NODE PRINT RF, *NODE FILE,NSET=TOP U, *NODE FILE RF, *EL FILE,ELSET=SMALL SF, *END STEP *STEP *RESPONSE SPECTRUM,SUM=SRSS,COMP=ALGEBRAIC SPEC,1.,0.,0.,1. *MODAL DAMPING,MODAL=DIRECT 1,30, 0.02 *END STEP *STEP *RESPONSE SPECTRUM,SUM=SRSS,COMP=SRSS SPEC,1.,0.,0.,1. *MODAL DAMPING,MODAL=DIRECT 1,30, 0.02 *END STEP *STEP *RESPONSE SPECTRUM,SUM=CQC,COMP=ALGEBRAIC SPEC,1.,0.,0.,1.

2-909

Dynamic Stress/Displacement Analyses

*MODAL DAMPING,MODAL=DIRECT 1,30, 0.02 *END STEP *STEP *RESPONSE SPECTRUM,SUM=NRL,COMP=ALGEBRAIC SPEC,1.,0.,0.,1. *MODAL DAMPING,MODAL=DIRECT 1,30, 0.02 *END STEP *STEP *RESPONSE SPECTRUM,SUM=NRL,COMP=SRSS SPEC,1.,0.,0.,1. *MODAL DAMPING,MODAL=DIRECT 1,30, 0.02 *END STEP *STEP *RESPONSE SPECTRUM,SUM=TENP,COMP=SRSS SPEC,1.,0.,0.,1. *MODAL DAMPING,MODAL=DIRECT 1,30, 0.02 *END STEP *STEP *RESPONSE SPECTRUM,SUM=TENP,COMP=ALGEBRAIC SPEC,1.,0.,0.,1. *MODAL DAMPING,MODAL=DIRECT 1,30, 0.02 *END STEP **************************** **multidirectional spectra** **************************** *STEP *RESPONSE SPECTRUM,SUM=SRSS,COMP=ALGEBRAIC SPEC,1.,0.,0.,1. SPEC,0.,1.,0.,1. *MODAL DAMPING,MODAL=DIRECT 1,30, 0.02 *END STEP *STEP *RESPONSE SPECTRUM,SUM=SRSS,COMP=SRSS SPEC,1.,0.,0.,1. SPEC,0.,1.,0.,1. *MODAL DAMPING,MODAL=DIRECT 1,30, 0.02

2-910

Dynamic Stress/Displacement Analyses

*END STEP *STEP *RESPONSE SPECTRUM,SUM=TENP,COMP=SRSS SPEC,1.,0.,0.,1. SPEC,0.,1.,0.,1. *MODAL DAMPING,MODAL=DIRECT 1,30, 0.02 *END STEP *STEP *RESPONSE SPECTRUM,SUM=CQC,COMP=SRSS SPEC,1.,0.,0.,1. SPEC,0.,1.,0.,1. SPEC,0.,0.,1.,1. *MODAL DAMPING,MODAL=DIRECT 1,30, 0.02 *END STEP

2-911

Dynamic Stress/Displacement Analyses

Listing 2.2.3-3 *HEADING 3-D BUILDING SUBJECTED TO EARTHQUAKE RECORD *RESTART,READ,STEP=1,INC=1,WRITE,FREQUENCY=0 *AMPLITUDE,VALUE=ABSOLUTE,TIME=STEP TIME, INPUT=QUAKE.AMP,NAME=EQ *ELSET,ELSET=ALL 104,112,116,120,124,128,136, 148,152,160,172,176,184,196 *STEP *MODAL DYNAMIC 0.01,10. *MODAL DAMPING,MODAL=DIRECT 1,30,0.02 *BASE MOTION,AMPLITUDE=EQ,DOF=1,SCALE=386.09 *NODE PRINT,NSET=TOP,FREQUENCY=100 U, *EL PRINT,ELSET=ALL,FREQUENCY=100 SF, *NODE PRINT,FREQUENCY=50 RF, ** IN ORDER TO GET RESULTS FOR TABLE 3.1.16-1, ** THE NODE FILE SHOULD BE WRITTEN WITH A ** FREQUENCY=2 **NODE FILE,FREQUENCY=2 *NODE FILE,FREQUENCY=100 RF, *END STEP

2-912

Tire Analyses

3. Tire Analyses 3.1 Tire analyses 3.1.1 Symmetric results transfer for a static tire analysis Product: ABAQUS/Standard This example illustrates the use of the *SYMMETRIC RESULTS TRANSFER option as well as the *SYMMETRIC MODEL GENERATION option to model the static interaction between a tire and a flat rigid surface. The *SYMMETRIC MODEL GENERATION option (``Symmetric model generation,'' Section 7.7.1 of the ABAQUS/Standard User's Manual) can be used to create a three-dimensional model by revolving an axisymmetric model about its axis of revolution or by combining two parts of a symmetric model, where one part is the original model and the other part is the original model reflected through a line or a plane. Both model generating techniques are demonstrated in this example. The *SYMMETRIC RESULTS TRANSFER option (``Transferring results from a symmetric mesh to a three-dimensional mesh,'' Section 7.7.2 of the ABAQUS/Standard User's Manual) allows the user to transfer the solution obtained from an axisymmetric analysis onto a three-dimensional model with the same geometry. It also allows the transfer of a symmetric three-dimensional solution to a full three-dimensional model. Both these results transfer features are demonstrated in this example. The results transfer capability can significantly reduce the analysis cost of structures that undergo symmetric deformation, followed by nonsymmetric deformation later during the loading history. The purpose of this example is to obtain the footprint solution of a 175 SR14 tire subjected to an inflation pressure and a concentrated load on the axle, which represents the weight of the vehicle. The footprint solution is used as a starting point in ``Steady-state rolling analysis of a tire,'' Section 3.1.2, where the free rolling state of the tire rolling at 10 km/h is determined, and in ``Subspace-based steady-state dynamic tire analysis,'' Section 3.1.3, where a frequency response analysis is performed.

Problem description The different components of the tire are shown in Figure 3.1.1-1. The tread and sidewalls are made of rubber, and the belts and carcass are constructed from fiber reinforced rubber composites. The rubber is modeled as an incompressible hyperelastic material, and the fiber reinforcement is modeled as a linear elastic material. A small amount of skew symmetry is present in the geometry of the tire due to the placement and §20.0° orientation of the reinforcing belts. Two simulations are performed in this example. The first simulation exploits the symmetry in the tire model and utilizes the results transfer capability; the second simulation does not use the results transfer capability. Comparisons between the two methodologies are made. The first simulation is broken down into three separate analyses. In the first analysis the inflation of the tire by a uniform internal pressure is modeled. Due to the anisotropic nature of the tire construction, the inflation loading gives rise to a circumferential component of deformation. The resulting stress field is fully three-dimensional, but the problem remains axisymmetric in the sense that the solution 3-913

Tire Analyses

does not vary as a function of position along the circumference. ABAQUS provides axisymmetric elements with twist (CGAX) for such situations. These elements are used to model the inflation loading. Only half the tire cross-section is needed for the inflation analysis due to a reflection symmetry through the vertical line that passes through the tire axle (see Figure 3.1.1-2). We refer to this model as the axisymmetric model. The second part of the simulation entails the computation of the footprint solution, which represents the static deformed shape of the pressurized tire due to a vertical dead load (modeling the weight of a vehicle). A three-dimensional model is needed for this analysis. The finite element mesh for this model is obtained by revolving the axisymmetric cross-section about the axis of revolution. A nonuniform discretization along the circumference is used as shown in Figure 3.1.1-3. In addition, the axisymmetric solution is transferred to the new mesh where it serves as the initial or base state in the footprint calculations. As with the axisymmetric model, only half of the cross-section is needed in this simulation, but skew-symmetric boundary conditions must be applied along the mid-plane of the cross-section to account for antisymmetric stresses that result from the inflation loading and the concentrated load on the axle. We refer to this model as the partial three-dimensional model. In the last part of this analysis the footprint solution from the partial three-dimensional model is transferred to a full three-dimensional model and brought into equilibrium. This full three-dimensional model is used in the steady-state transport example that follows. The model is created by combining two parts of the partial three-dimensional model, where one part is the mesh used in the second analysis and the other part is the partial model reflected through a line. We refer to this model as the full three-dimensional model. A second simulation is performed in which the same loading steps are repeated, except that the full three-dimensional model is used for the entire analysis. Besides being used to validate the results transfer solution, this second simulation allows us to demonstrate the computational advantage afforded by the ABAQUS results transfer capability in problems with rotational and/or reflection symmetries.

Model definition In the first simulation the inflation step is performed on the axisymmetric model and the results are stored in the results files ( .res, .mdl, .stt, and .prt). The axisymmetric model is discretized with CGAX4H and CGAX3H elements. The belts and carcass are modeled by defining rebar in the continuum elements, and the road is defined as an analytical rigid surface. The axisymmetric results are read into the subsequent footprint analysis, and the partial three-dimensional model is generated by ABAQUS by revolving the axisymmetric model cross-section about the rotational symmetry axis. The *SYMMETRIC MODEL GENERATION, REVOLVE option is used for this purpose. The road is defined in the partial three-dimensional model. The results of the footprint analysis are read into the final equilibrium analysis, and the full three-dimensional model is generated by reflecting the partial three-dimensional model through a vertical line using the *SYMMETRIC MODEL GENERATION, REFLECT=LINE option. The line used in the reflection is the vertical line in the symmetry plane of the tire, which passes through the axis of rotation. The REFLECT=LINE parameter is used, as opposed to the REFLECT=PLANE parameter, to take into account the skew symmetry of the tire. The analytical rigid surface as defined in the partial three-dimensional model is transferred to the full

3-914

Tire Analyses

model without change. The three-dimensional finite element mesh of the full model is shown in Figure 3.1.1-4. In the second simulation a datacheck analysis is performed to write the axisymmetric model information to the results files. The full tire cross-section is meshed in this model. No analysis step is performed. The axisymmetric model information is read in a subsequent run, and a full three-dimensional model is generated by ABAQUS by revolving the cross-section about the rotational symmetry axis. The *SYMMETRIC MODEL GENERATION, REVOLVE option is again used for this purpose. The road is defined in the full model. The three-dimensional finite element mesh of the full model is identical to the one generated in the first analysis. However, the inflation load and concentrated load on the axle are applied to the full model without making use of the results transfer capability. During the model generation from the axisymmetric to the three-dimensional meshes in both analyses, the axisymmetric CGAX4H and CGAX3H elements are converted into C3D8H and C3D6H elements, respectively. The footprint calculations in both analyses are performed with a friction coefficient of zero in anticipation of eventually performing a steady-state rolling analysis of the tire using the *STEADY STATE TRANSPORT option, as explained in ``Steady-state rolling analysis of a tire,'' Section 3.1.2. Since the results from the static analyses performed in this example are used in a subsequent time-domain dynamic example, there are a few features in the input files that would not ordinarily be included for purely static analyses. It is instructive to point out and to discuss these features briefly. The TRANSPORT parameter is included with the *SYMMETRIC MODEL GENERATION option to define streamlines in the model, which are needed by ABAQUS to perform streamline calculations during the *STEADY STATE TRANSPORT analysis in the next example problem. The TRANSPORT parameter is not required for any other analysis type except for *STEADY STATE TRANSPORT. The hyperelastic material, which models the rubber, has a *VISCOELASTIC, TIME=PRONY option included. This enables us to model viscoelasticity in the steady-state transport example that follows. As a consequence of defining a time-domain viscoelastic material property, the *HYPERELASTIC option includes the LONG TERM parameter to indicate that the elastic properties defined in the associated data lines define the long-term behavior of the rubber. In addition, all *STATIC steps include the LONG TERM parameter to ensure that the static solutions are based upon the long-term elastic moduli.

Loading As discussed in the previous sections, the loading on the tire is applied over several steps. In the first simulation the inflation of the tire to a pressure of 200.0 kPa is modeled using the axisymmetric tire model (tiretransfer_axi_half.inp) with a *STATIC analysis procedure. The results from this axisymmetric analysis are then transferred to the partial three-dimensional model (tiretransfer_symmetric.inp) in which the footprint solution is computed in two sequential *STATIC steps. The first of these static steps establishes the initial contact between the road and the tire by

3-915

Tire Analyses

prescribing a vertical displacement of 0.02 m on the rigid body reference node. Since this is a static analysis, it is recommended that contact be established with a prescribed displacement, as opposed to a prescribed load, to avoid potential convergence difficulties that might arise due to unbalanced forces. The prescribed boundary condition is removed in the second static step, and a vertical load of N = 1.65 kN is applied to the rigid body reference node. The 1.65 kN load in the partial three-dimensional model represents a 3.3 kN load in the full three-dimensional model. The transfer of the results from the axisymmetric model to the partial three-dimensional model is accomplished by using the *SYMMETRIC RESULTS TRANSFER option. Once the static footprint solution for the partial three-dimensional model has been established, the *SYMMETRIC RESULTS TRANSFER option is used once again to transfer the solution to the full three-dimensional model ( tiretransfer_full.inp), where the footprint solution is brought into equilibrium in a single *STATIC increment. The results transfer sequence is illustrated in Figure 3.1.1-5. It is important to note that boundary conditions and loads are not transferred with the *SYMMETRIC RESULTS TRANSFER option; they must be carefully redefined in the new analysis to match the loads and boundary conditions from the transferred solution. Due to numerical and modeling issues the element formulation for the two-dimensional and three-dimensional elements are not identical. As a result, there may be slight differences between the equilibrium solutions generated by the two- and three-dimensional models. In addition, small numerical differences may occur between the symmetric and full three-dimensional solutions because of the presence of symmetry boundary conditions in the symmetric model that are not used in the full model. Therefore, it is advised that in a results transfer simulation an initial step be performed where equilibrium is established between the transferred solution and loads that match the state of the model from which the results are transferred. Since the transferred solution is applied in full at time t = 0, the external loads must also be applied in full at the beginning of the initial step. There is no benefit in reducing the magnitude of the loads to overcome convergence problems. To ensure that ABAQUS does not waste computational time by attempting smaller time increments if equilibrium cannot be attained, it is recommended that the initial step should consist of a *STATIC, DIRECT procedure with the initial time increment set to the total step time. In the second simulation identical inflation and the footprint steps are repeated. The only difference is that the entire analysis is performed on the full three-dimensional model (tiretransfer_full_footprint.inp). The full three-dimensional model is generated using the restart information from a datacheck analysis on an axisymmetric model of the full tire cross-section (tiretransfer_axi_full.inp).

Solution controls Since the three-dimensional tire model has a small loaded area and, thus, rather localized forces, the default averaged flux values for the convergence criteria produce very tight tolerances and cause more iteration than is necessary for an accurate solution. To decrease the computational time required for the analysis, the *CONTROLS option can be used to override the default values for average forces and moments. The default controls are used in this example.

Results and discussion

3-916

Tire Analyses

The results from the two simulations are essentially identical. The peak Mises stresses and displacement magnitudes in the two models agree within 0.3% and 0.2%, respectively. The final deformed shape of the tire is shown in Figure 3.1.1-6. The computational cost of each simulation is shown in Table 3.1.1-1. The simulation performed on the full three-dimensional model took 2.5 times longer than the results transfer simulation --clearly demonstrating the computational advantage that can be attained by exploiting the symmetry in the model using the *SYMMETRIC RESULTS TRANSFER option.

Input files tiretransfer_axi_half.inp Axisymmetric model, inflation analysis (simulation 1). tiretransfer_symmetric.inp Partial three-dimensional model, footprint analysis (simulation 1). tiretransfer_full.inp Full three-dimensional model, final equilibrium analysis (simulation 1). tiretransfer_axi_full.inp Axisymmetric model, datacheck analysis (simulation 2). tiretransfer_full_footprint.inp Full three-dimensional model, complete analysis (simulation 2). tiretransfer_node.inp Nodal coordinates for both axisymmetric models.

Table Table 3.1.1-1 Comparison of normalized CPU times to perform the footprint analysis (normalized with respect to the total "No results transfer" analysis). No results Use results transfer transfer and symmetry conditions Inflation 0.002(a)+0.039(b) 0.36(e) (c) (d) Footprint 0.29 +0.061 0.64(e) Total 0.39 1.0 (a) axisymmetric model (b) equilibrium step in partial three-dimensional model (c) footprint analysis in partial three-dimensional model (d) equlibrium step in full three-dimensional model

3-917

Tire Analyses

(e) full three-dimensional model

Figures Figure 3.1.1-1 Tire cross-section.

Figure 3.1.1-2 Axisymmetric tire mesh.

Figure 3.1.1-3 Partial three-dimensional tire mesh.

3-918

Tire Analyses

Figure 3.1.1-4 Full three-dimensional tire mesh.

Figure 3.1.1-5 Results transfer analysis sequence.

3-919

Tire Analyses

Figure 3.1.1-6 Deformed three-dimensional tire (Deformations scaled by a factor of 2).

Sample listings

3-920

Tire Analyses

Listing 3.1.1-1 *HEADING SYMMETRIC RESULTS TRANSFER FOR TIRE MODEL TIRETRANSFER_AXI_HALF AXISYMMETRIC HALF TIRE MODEL STEP 1: INFLATE TIRE TO 200 KPa UNITS: KG, M *RESTART,WRITE,FREQ=100 *NODE,NSET=NTIRE,INP=tiretransfer_node.inp *ELEMENT,TYPE=CGAX4H,ELSET=TREAD 1, 50, 55, 54, 49 2, 45, 50, 49, 44 3, 40, 45, 44, 39 5, 35, 40, 39, 34 7, 31, 35, 34, 30 *ELEMENT,TYPE=CGAX3H,ELSET=TREAD 4, 27, 31, 30 *ELEMENT,TYPE=CGAX4H,ELSET=SIDE 15, 27, 30, 28, 25 16, 24, 27, 25, 22 17, 21, 24, 22, 19 18, 18, 21, 19, 16 19, 15, 18, 16, 13 20, 12, 15, 13, 10 21, 30, 34, 32, 28 29, 9, 12, 10, 7 30, 6, 9, 7, 4 31, 3, 6, 4, 1 *ELEMENT,TYPE=CGAX4H,ELSET=BELT 35, 49, 54, 51, 46 36, 44, 49, 46, 41 37, 39, 44, 41, 36 38, 34, 39, 36, 32 *REBAR,ELEMENT=CONTINUUM,MATERIAL=BELT, GEOMETRY=ISO,NAME=BELT1 BELT, 0.2118683E-6, 1.16E-3, 70.0, 0.50, *REBAR,ELEMENT=CONTINUUM,MATERIAL=BELT, GEOMETRY=ISO,NAME=BELT2 BELT, 0.2118683E-6, 1.16E-3, 110.0, 0.83, *REBAR,ELEMENT=CONTINUUM,MATERIAL=CARCASS, GEOMETRY=ISO,NAME=CARCASS BELT, 0.4208352E-6, 1.00E-3, 0.0, 0.0, 3

3-921

3

3

Tire Analyses

SIDE, 0.4208352E-6, 1.00E-3, 0.0, 0.0, 3 *SOLID SECTION,ELSET=TREAD,MATERIAL=RUBBER *SOLID SECTION,ELSET=SIDE,MATERIAL=RUBBER *SOLID SECTION,ELSET=BELT,MATERIAL=RUBBER *MATERIAL,NAME=RUBBER *HYPERELASTIC,N=1,MODULI=LONG TERM 1.0e6, *VISCOELASTIC,TIME=PRONY 0.3, 0.0, 0.1 *DENSITY 1100., *MATERIAL,NAME=BELT *ELASTIC,TYPE=ISO 172.2E+09, 0.3 *DENSITY 5900., *MATERIAL,NAME=CARCASS *ELASTIC,TYPE=ISO 9.87E+9, 0.3 *DENSITY 1500., *NSET,NSET=RIM 6, 3, 1 *NSET,NSET=SYM 51, 54, 55 *ELSET,ELSET=SOLID,GENERATE 1, 76,1 *SURFACE,NAME=INSIDE BELT, S3 SIDE, S3 *********************************** *STEP,INC=100,NLGEOM=YES 1: INFLATION *STATIC, LONG TERM 0.25, 1.0 *BOUNDARY RIM, 1, 2 RIM, 5, SYM, 2, SYM, 5, *DSLOAD INSIDE, P, 200.E3 *EL FILE,FREQUENCY=50,POSITION=NODES

3-922

Tire Analyses

S, E *NODE FILE,FREQUENCY=50 U *EL PRINT,FREQUENCY=50,REBAR,ELSET=SOLID S *NODE PRINT,FREQUENCY=100,TOTAL=YES U, RF *OUTPUT,FIELD,VARIABLE=PRESELECT,FREQ=50 *OUTPUT,HISTORY,FREQ=1 *END STEP

3-923

Tire Analyses

Listing 3.1.1-2 *HEADING SYMMETRIC RESULTS TRANSFER FOR TIRE MODEL 3D HALF TIRE MODEL STEP 0: TRANSFER TIRE INFLATION RESULTS FROM tiretransfer_axi_half AND GENERATE MODEL USING *SYMMETRIC MODEL GENERATION STEP 1: BRING TRANSFERRED AXISYMMETRIC RESULTS TO EQUILIBRIUM STEP 2: FOOTPRINT ANALYSIS (DISPLACEMENT CONTROL) STEP 3: FOOTPRINT ANALYSIS (LOAD CONTROL) UNITS: KG, M *RESTART,WRITE,FREQ=100 *NODE,NSET=ROAD 9999, 0.0, 0.0, -0.02 *SYMMETRIC MODEL GENERATION,REVOLVE,ELEMENT=200, NODE=200,TRANSPORT 0.0, 0.0, 0.0, 0.0, 1.0, 0.0 0.0, 0.0, 1.0 90.0, 3 70.0, 3 15.0, 7 10.0, 4 15.0, 7 70.0, 3 90.0, 3 *SYMMETRIC RESULTS TRANSFER, STEP=1, INC=4 *ELSET,ELSET=FOOT,GEN 1001, 4801, 200 1002, 4802, 200 1003, 4803, 200 1004, 4804, 200 1005, 4805, 200 1007, 4807, 200 *SURFACE,TYPE=CYLINDER,NAME=SROAD 0., 0.,-0.31657, 1., 0.,-0.31657 0., 1.,-0.31657 START, -0.3, 0. LINE, 0.3, 0. *RIGID BODY,REF NODE=9999,ANALYTICAL SURFACE=SROAD *SURFACE,NAME=STREAD FOOT, S3

3-924

Tire Analyses

*CONTACT PAIR,INTERACTION=SRIGID STREAD, SROAD *SURFACE INTERACTION,NAME=SRIGID *FRICTION 0.0 *ELSET,ELSET=SECT,GENERATE 2800, 3200, 1 *NSET,NSET=SECT,GENERATE 2800, 3400, 1 *NSET,NSET=FOOT,ELSET=FOOT *NSET,NSET=NOUTP,GENERATE 1055, 5055, 200 *NSET,NSET=SYM1 51,54,55,3051,3054,3055 ** ** NODE SETS ASYMA,ASYMB,ASYMC, and ASYMD ** USED FOR ANTI_SYMMETRY BC's ** *NSET,NSET=ASYMA,GENERATE,UNSORTED 255, 2855, 200 254, 2854, 200 251, 2851, 200 *NSET,NSET=ASYMB,GENERATE,UNSORTED 5855, 3255, -200 5854, 3254, -200 5851, 3251, -200 *NSET,NSET=ASYMC,GENERATE,UNSORTED 255, 1055, 200 254, 2854, 200 251, 2851, 200 *NSET,NSET=ASYMD,GENERATE,UNSORTED 5855, 5055, -200 5854, 3254, -200 5851, 3251, -200 *EQUATION 2 ASYMA, 1, 1.0, ASYMB, 1, 1.0 *EQUATION 2 ASYMA, 2, 1.0, ASYMB, 2, 1.0 *EQUATION 2 ASYMC, 3, 1.0, ASYMD, 3, -1.0

3-925

Tire Analyses

*FILE FORMAT,ZERO INCREMENT ******************************************** *STEP,INC=100,NLGEOM=YES 1: BRING TRANSFERRED RESULTS TO EQUILIBRIUM *STATIC, LONG TERM 1.0, 1.0 *BOUNDARY,OP=NEW RIM, 1, 3 ROAD, 1, 6 SYM1, 1, 2 *DSLOAD,OP=NEW INSIDE, P, 200.E3 *NODE PRINT,NSET=ROAD,FREQ=100 U, RF, *EL PRINT,FREQ=0 *NODE FILE,NSET=ROAD U, RF *OUTPUT,FIELD,VARIABLE=PRESELECT *END STEP ****************************************** *STEP,INC=100,NLGEOM=YES 2: FOOTPRINT (Displacement controlled) *STATIC, LONG TERM 0.2, 1.0 *BOUNDARY,OP=NEW RIM, 1, 3 ROAD, 1, 2 ROAD, 4, 6 SYM1, 1, 2 ROAD, 3, , 0.02 *NODE PRINT,NSET=ROAD,FREQ=100 U, RF, *EL PRINT,FREQ=0 *NODE FILE,NSET=ROAD U, RF *NODE FILE,NSET=FOOT,FREQ=100 *OUTPUT,FIELD,VARIABLE=PRESELECT,FREQ=5 *OUTPUT,HISTORY,FREQ=1 *NODE OUTPUT, NSET=ROAD U, RF *END STEP

3-926

Tire Analyses

**************************************** *STEP,INC=100,NLGEOM=YES 3: FOOTPRINT (Load controlled) *STATIC, LONG TERM 1.0, 1.0 *BOUNDARY,OP=NEW RIM, 1, 3 ROAD, 1, 2 ROAD, 4, 6 SYM1, 1, 2 *CLOAD, OP=NEW ROAD, 3, 1650. *END STEP

3.1.2 Steady-state rolling analysis of a tire Product: ABAQUS/Standard This example illustrates the use of the *STEADY STATE TRANSPORT option in ABAQUS (``Steady-state transport analysis,'' Section 6.4.1 of the ABAQUS/Standard User's Manual) to model the steady-state dynamic interaction between a rolling tire and a flat rigid surface. A steady-state transport analysis uses a moving reference frame in which rigid body rotation is described in an Eulerian manner and the deformation is described in a Lagrangian manner. This kinematic description converts the steady moving contact problem into a pure spatially dependent simulation. Thus, the mesh need be refined only in the contact region--the steady motion transports the material through the mesh. Frictional effects, inertia effects, and history effects in the material can all be accounted for in a *STEADY STATE TRANSPORT analysis. The purpose of this analysis is to obtain free rolling equilibrium solutions of a 175 SR14 tire traveling at a ground velocity of 10.0 km/h (2.7778 m/s) at different slip angles. The slip angle is the angle between the direction of travel and the plane normal to the axle of the tire. Straight line rolling occurs at a 0.0° slip angle. An equilibrium solution for the rolling tire problem that has zero torque, T , applied around the axle is referred to as a free rolling solution. An equilibrium solution with a nonzero torque is referred to as either a traction or a braking solution depending upon the sense of T . Braking occurs when the angular velocity of the tire is small enough such that some or all of the contact points between the tire and the road are slipping and the resultant torque on the tire acts in an opposite sense from the angular velocity of the free rolling solution. Similarly, traction occurs when the angular velocity of the tire is large enough such that some or all of the contact points between the tire and the road are slipping and the resultant torque on the tire acts in the same sense as the angular velocity of the free rolling solution. Full braking (traction) occurs when all of the contact points between the tire and the road are slipping. A wheel in free rolling, traction, or braking will spin at different angular velocities, !, for the same ground velocity, v0 : Usually the combination of ! and v0 that results in free rolling is not known in

3-927

Tire Analyses

advance. Since the steady-state transport analysis capability requires that both the rotational spinning velocity, !, and the traveling ground velocity, v0 , be prescribed, the free rolling solution must be found in an indirect manner. One such indirect approach is illustrated in this example. A finite element analysis of this problem, together with experimental results, have been published by Koishi et al. (1997).

Problem description and model definition A description of the tire and finite element model has been given in ``Symmetric results transfer for a static tire analysis,'' Section 3.1.1. To take into account the effect of the skew symmetry of the actual tire in the dynamic analysis, the steady-state rolling analysis will be performed on the full three-dimensional model, also referred to as the full model. Inertia effects are ignored since the rolling speed is low (v0 = 10 km/h). As stated earlier, the *STEADY STATE TRANSPORT capability in ABAQUS uses a mixed Eulerian/Lagrangian approach in which, to an observer in the moving reference frame, the material appears to flow through a stationary mesh. The paths that the material points follow through the mesh are referred to as streamlines and must be computed before a steady-state transport analysis can be performed. As discussed in ``Symmetric results transfer for a static tire analysis,'' Section 3.1.1, the streamlines needed for the steady-state transport analyses in this example were computed using the *SYMMETRIC MODEL GENERATION, REVOLVE, TRANSPORT option. This option generated the three-dimensional mesh by revolving the two-dimensional tire cross-section about the symmetry axis so that the streamlines followed the mesh lines. The incompressible hyperelastic material used to model the rubber in this example includes a time-domain viscoelastic component, which is enabled by the *VISCOELASTIC, TIME=PRONY option. A simple 1-term Prony series model is used. For an incompressible material a 1-term Prony series in ABAQUS is defined by providing a single value for the shear relaxation modulus ratio, g¹1P , and its associated relaxation time, ¿1 . In this example g¹1P = 0:3 and ¿1 = 0:1. The viscoelastic--i.e., material history--effects are included in a *STEADY STATE TRANSPORT step unless the LONG TERM parameter is used. See ``Time domain viscoelasticity,'' Section 10.6.1 of the ABAQUS/Standard User's Manual, for a more detailed discussion on modeling time-domain viscoelasticity in ABAQUS.

Loading As discussed in ``Symmetric results transfer for a static tire analysis,'' Section 3.1.1, it is recommended that the footprint analyses be obtained with a friction coefficient of zero (so that no frictional forces are transmitted across the contact surface). The frictional stresses for a rolling tire are very different from the frictional stresses in a stationary tire, even if the tire is rolling at very low speed; therefore, discontinuities may arise in the solution between the last *STATIC analysis and the first *STEADY STATE TRANSPORT analysis. Furthermore, varying the friction coefficient from zero at the beginning of the steady-state transport step to its final value at the end of the steady-state transport step ensures that the changes in frictional forces reduce with smaller load increments. This is important if ABAQUS must take a smaller load increment to overcome convergence difficulties while trying to obtain the steady-state rolling solution. 3-928

Tire Analyses

Once the static footprint solution for the tire has been computed, the steady-state rolling contact problem can be solved using the *STEADY STATE TRANSPORT option. The objective of the first simulation in this example is to obtain the straight-line, steady-state rolling solutions, including full braking and full traction, at different spinning velocities. We also compute the straight-line, free rolling solution. In the second simulation, free rolling solutions at different slip angles are computed. In the first and second simulations, material history effects are ignored by including the LONG TERM parameter on the *STEADY STATE TRANSPORT steps. The third simulation repeats a portion of the straight-line, steady-state rolling analysis from the first simulation; however, material history effects are included by omitting the LONG TERM parameter. A steady ground velocity of 10.0 km/h is maintained for all three simulations. In simulation 1 (rollingtire_brake_trac.inp) the full traction solution is obtained in the first *STEADY STATE TRANSPORT step by setting the friction coefficient, ¹, to its final value of 1.0 using the *CHANGE FRICTION option and applying the translational ground velocity together with a spinning angular velocity that will result in full braking. The *TRANSPORT VELOCITY and *MOTION options are used for this purpose. An estimate of the angular velocity corresponding to full braking is obtained as follows. A free rolling tire generally travels farther in one revolution than determined by its center height, H, but less than determined by the free tire radius. In this example the free radius is 316.2 mm and the vertical deflection is approximately 20.0 mm, so H = 294.2 mm. Using the free radius and the effective height, it is estimated that free rolling occurs at an angular velocity between ! = 8.78 rad/s and ! = 9.44 rad/s. Smaller angular velocities would result in braking, and larger angular velocities would result in traction. We use an angular velocity ! = 8.0 rad/s to ensure that the solution in the first steady-state transport step is a full braking solution (all contact points are slipping, so the magnitude of the total frictional force across the contact surface is ¹N ). In the second steady-state transport analysis step of the full model, the angular velocity is increased gradually to ! = 10.0 rad/s while the ground velocity is held constant. The solution at each load increment is a steady-state solution to the loads acting on the structure at that instant so that a series of steady-state solutions between full braking and full traction is obtained. In the second simulation (rollingtire_slipangles.inp) the free rolling solutions at different slip angles are computed. The slip angle, µ, is the angle between the direction of travel and the plane normal to the axle of the tire. In the first step the straight-line free rolling solution from the first simulation is brought into equilibrium. This step is followed by a *STEADY STATE TRANSPORT step where the slip angle is gradually increased from µ =0.0° at the beginning of the step to µ =3.0° at the end of the step, so a series of steady-state solutions at different slip angles are obtained. This is accomplished by prescribing a traveling velocity vector with components vx = v0 cos µ and vy = v0 sin µ on the *MOTION option, where µ =0.0° in the first steady-state transport step and µ =3.0° at the end of the second steady-state transport step. The final simulation in this example (rollingtire_materialhistory.inp) includes a series of steady-state solutions between full braking and full traction in which the material history effects are included.

Results and discussion Figure 3.1.2-1 and Figure 3.1.2-2 show the reaction force parallel to the ground (referred to as rolling 3-929

Tire Analyses

resistance) and the torque, T , on the tire axle at different angular spinning velocities. The figures show that free rolling, T = 0.0, occurs at an angular velocity of approximately 9.0 rad/s. Full braking occurs at spinning velocities smaller than 8.2 rad/s, and full traction occurs at velocities larger than 9.7 rad/s. At these spinning velocities all contact points are slipping, and the rolling resistance reaches the limiting value ¹N: Figure 3.1.2-3 and Figure 3.1.2-4 show shear stress along the centerline of the tire surface in the free rolling and full traction states, respectively. The distance along the centerline is measured as an angle with respect to a plane parallel to the ground passing through the tire axle. The dashed line is the maximum or limiting shear stress, ¹p, that can be transmitted across the surface, where p is the contact pressure. The figures show that all contact points are slipping during full traction. During free rolling all points stick. A better approximation to the angular velocity that corresponds to free rolling can be made by using the results generated by rollingtire_brake_trac.inp to refine the search about an angular velocity of 9.0 rad/s. The file rollingtire_trac_res.inp restarts the previous analysis from Step 3, Increment 11 (corresponding to an angular velocity of 9.006 rad/s) and performs a refined search up to 9.04 rad/s. Figure 3.1.2-5 shows the torque, T , on the tire axle computed in the refined search, which leads to a more precise value for the free rolling angular velocity of approximately 9.025 rad/s. This result is used for the model where the free rolling solutions at different slip angles are computed. Figure 3.1.2-6 shows the transverse force (force along the tire axle) measured at different slip angles. The figure compares the steady-state transport analysis prediction with the result obtained from a pure Lagrangian analysis. The Lagrangian solution is obtained by performing an explicit transient analysis using ABAQUS/Explicit. With this analysis technique a prescribed constant traveling velocity is applied to the tire, which is free to roll along the rigid surface. Since more than one revolution is necessary to obtain a steady-state configuration, fine meshing is required along the full circumference; hence, the Lagrangian solution is much more costly than the steady-state solutions shown in this example. The figure shows good agreement between the results obtained from the two analysis techniques. Figure 3.1.2-7 compares the free rolling solutions with and without material history effects included. The solid lines in the diagram represent the rolling resistance (force parallel to the ground along the traveling direction); and the broken lines, the torque (normalized with respect to the free radius) on the axle. The figure shows that free rolling, marked with bullet points, occurs at a higher angular velocity when history effects are included. It also shows that the rolling resistance increases when history effects are included. The influence of material history effects on a steady-state rolling solution is discussed in detail in ``Steady-state spinning of a disk in contact with a foundation, '' Section 1.5.2 of the ABAQUS Benchmarks Manual.

Acknowledgments HKS gratefully acknowledges Hankook Tire and Yokohama Rubber Company for their cooperation in developing the steady-state transport capability used in this example. HKS thanks Dr. Koishi of Yokohama Rubber Company for supplying the geometry and material properties used in this example.

3-930

Tire Analyses

Input files rollingtire_brake_trac.inp Three-dimensional full model for the full braking and traction analyses. rollingtire_trac_res.inp Three-dimensional full model for the refined braking and traction analyses. rollingtire_slipangles.inp Three-dimensional full model for the slip angle analysis. rollingtire_materialhistory.inp Three-dimensional full model with material history effects.

Reference · Koishi, M., K. Kabe, and M. Shiratori, "Tire Cornering Simulation using Explicit Finite Element Analysis Code," 16th annual conference of the Tire Society at the University of Akron, 1997.

Figures Figure 3.1.2-1 Rolling resistance at different angular velocities.

Figure 3.1.2-2 Torque at different angular velocities.

3-931

Tire Analyses

Figure 3.1.2-3 Shear stress along tire center (free rolling).

Figure 3.1.2-4 Shear stress along tire center (full traction).

3-932

Tire Analyses

Figure 3.1.2-5 Torque at different angular velocities (refined search).

Figure 3.1.2-6 Transverse force as a function of slip angle.

3-933

Tire Analyses

Figure 3.1.2-7 Rolling resistance and normalized torque as a function of angular velocity ( R=0.3162 m).

Sample listings

3-934

Tire Analyses

Listing 3.1.2-1 *HEADING STEADY-STATE ROLLING ANALYSIS OF A TIRE: ROLLINGTIRE_BRAKE_TRAC 3D FULL TIRE MODEL STEP 0: TRANSFER TIRE INFLATION FOOTPRINT RESULTS FROM TIRETRANSFER_FULL STEP 1: FULL BRAKING ANAYLSIS STEP 2: FULL TRACTION ANALYSIS UNITS: KG, M *RESTART,READ,STEP=1,INC=1 *FILE FORMAT,ZERO INCREMENT ****************************************** *STEP,INC=300,NLGEOM=YES,UNSYMM=YES 1: STRAIGHT LINE ROLLING (Full braking) *STEADY STATE TRANSPORT, LONG TERM 0.5, 1.0 *CHANGE FRICTION,INTERACTION=SRIGID *FRICTION,SLIP=0.01 1.0 *TRANSPORT VELOCITY NTIRE, 8.0 *MOTION,TYPE=VELOCITY,TRANSLATION NTIRE, 1, , 2.7778 *CONTACT PRINT,FREQ=100,NSET=NOUTP *CONTACT FILE,NSET=NOUTP,FREQ=100 *NODE FILE,NSET=NOUTP,FREQ=100 V, COORD *NODE FILE,NSET=ROAD U, RF *OUTPUT,HISTORY,FREQ=100,OP=ADD *NODE OUTPUT,NSET=NOUTP V, COORD *CONTACT OUTPUT,NSET=NOUTP CSTRESS, *END STEP ******************************************* *STEP,INC=300,NLGEOM=YES,UNSYMM=YES 2: STRAIGHT LINE ROLLING (Full traction) *STEADY STATE TRANSPORT, LONG TERM 0.1, 1.0, , 0.1 *RESTART,WRITE,FREQ=11

3-935

Tire Analyses

*TRANSPORT VELOCITY NTIRE, 10.00 *END STEP

3-936

Tire Analyses

Listing 3.1.2-2 *HEADING STEADY-STATE ROLLING ANALYSIS OF A TIRE: STEP 0: RESTART FROM rollingtire_trac_res STEP 1: GET EQUILIBRIUM STEP 2: FREE ROLLING AT DIFFERENT SLIP ANGLES UNITS: KG, M *RESTART,READ,STEP=5,INC=2,END STEP *FILE FORMAT,ZERO INCREMENT ****************************************** *STEP,INC=300,NLGEOM,UNSYMM=YES 1: STRAIGHT LINE FREE ROLLING *STEADY STATE TRANSPORT, LONG TERM 1.0, 1.0, *TRANSPORT VELOCITY NTIRE, 9.023 *END STEP ****************************************** *STEP,INC=300,NLGEOM,UNSYMM=YES 2: SLIP (3 degrees) *STEADY STATE TRANSPORT, LONG TERM 0.1, 1.0, , 0.1 *MOTION,TYPE=VELOCITY,TRANSLATION NTIRE, 1, , 2.774 NTIRE, 2, , 0.14538 *END STEP

3.1.3 Subspace-based steady-state dynamic tire analysis Product: ABAQUS/Standard This example illustrates the use of the *STEADY STATE DYNAMICS, SUBSPACE PROJECTION option to model the frequency response of a tire about a static footprint solution. The *STEADY STATE DYNAMICS, SUBSPACE PROJECTION option (``Subspace-based steady-state dynamic analysis,'' Section 6.3.7 of the ABAQUS/Standard User's Manual) is an analysis procedure that can be used to calculate the steady-state dynamic response of a system subjected to harmonic excitation. It does so by the direct solution of the steady-state dynamic equations projected onto a reduced-dimensional subspace spanned by a set of eigenmodes of the undamped system. If the dimension of the subspace is small compared to the dimension of the original problem--i.e., if a relatively small number of eigenmodes are used, the subspace method can offer a very cost-effective alternative to a direct-solution steady-state analysis. The purpose of this analysis is to obtain the frequency response of a 175 SR14 tire subjected to a 3-937

Tire Analyses

harmonic load excitation about the footprint solution discussed in ``Symmetric results transfer for a static tire analysis,'' Section 3.1.1). The *SYMMETRIC RESULTS TRANSFER and *SYMMETRIC MODEL GENERATION options are used to generate the footprint solution, which serves as the base state in the steady-state dynamics calculations.

Problem description A description of the tire being modeled has been given in ``Symmetric results transfer for a static tire analysis,'' Section 3.1.1. In this example we exploit the symmetry in the tire model and utilize the results transfer capability in ABAQUS to compute the footprint solution for the full three-dimensional model in a manner identical to that discussed in ``Symmetric results transfer for a static tire analysis,'' Section 3.1.1. Once the footprint solution has been computed, several steady-state dynamic steps are performed. Both the *STEADY STATE DYNAMICS, DIRECT and the *STEADY STATE DYNAMICS, SUBSPACE PROJECTION options are used. Besides being used to validate the subspace projection results, the direct steady-state procedure allows us to demonstrate the computational advantage afforded by the subspace projection capability in ABAQUS.

Model definition The model used in this analysis is essentially identical to that used in the first simulation discussed in ``Symmetric results transfer for a static tire analysis,'' Section 3.1.1, with CGAX4H and CGAX3H elements used in the axisymmetric model and rebar in the continuum elements for the belts and carcass. However, since no *STEADY STATE TRANSPORT steps are performed in this example, the TRANSPORT parameter is not needed during the symmetric model generation phase. In addition, instead of using a nonuniform discretization about the circumference, the uniform discretization shown in Figure 3.1.3-1 is used. The analysis procedures available with the *STEADY STATE DYNAMICS option are all frequency-domain procedures. In contrast, the *STEADY STATE TRANSPORT option discussed in ``Steady-state rolling analysis of a tire,'' Section 3.1.2, is a time-domain procedure. The incompressible hyperelastic material used to model the rubber in this example includes a frequency-domain viscoelastic model, which is activated by the *VISCOELASTIC, FREQUENCY=TABULAR option. This is different from the time-domain viscoelastic model (*VISCOELASTIC, TIME=PRONY) that was used in the steady-state transport example. The FREQUENCY=TABULAR option requires the user to provide tabular values of !<(g¤ ) and !=(g¤ ) as functions of frequency, where g ¤ is the Fourier transform of the nondimensional shear relaxation function g (t) = GGR1(t) ¡ 1 . For consistency, the 1-term Prony series viscoelastic model used in the

steady-state rolling example was converted into an equivalent frequency-domain viscoelastic model for this example using the following relationships: !<(g¤ ) =

g¹1P !¿1 ; P 1 + !2 ¿ 2 1 ¡ g¹1 1

3-938

Tire Analyses

!=(g¤ ) = ¡

g¹1P ! 2 ¿12 ; 1 ¡ g¹1P 1 + ! 2 ¿12

where g¹1P = 0:3 is the modulus ratio for the first term in the Prony series expansion for the shear relaxation modulus and ¿1 = 0:1 is the relaxation time for the first term in the Prony series expansion. Since the material is incompressible, no viscoelastic data are needed for the volumetric behavior. See ``Frequency domain viscoelasticity,'' Section 10.6.2 of the ABAQUS/Standard User's Manual, for a more detailed discussion on frequency-domain viscoelasticity.

Loading The loading sequence for computing the footprint solution is identical to that discussed in ``Symmetric results transfer for a static tire analysis,'' Section 3.1.1, with the axisymmetric model contained in tiredynamic_axi_half.inp, the partial three-dimensional model in tiredynamic_symmetric.inp, and the full three-dimensional model in tiredynamic_freqresp.inp. Since the NLGEOM=YES parameter is active for the *STATIC steps used in computing the footprint solution, the steady-state dynamic analyses, which are linear perturbation procedures, are performed about the nonlinear deformed shape of the footprint solution. The first frequency response analyses of the tire are performed using the *STEADY STATE DYNAMICS, SUBSPACE PROJECTION option. The excitation is due to a harmonic vertical load of 200 N, which is applied to the analytical rigid surface through its reference node. The frequency is swept from 80 Hz to 130 Hz. The rim of the tire is held fixed throughout the analysis. Prior to the subspace analysis being performed, the eigenmodes that are used for the subspace projection are computed in a *FREQUENCY step. In the frequency step the first 20 eigenpairs are extracted, for which the computed eigenvalues range from 50 to 185 Hz. The accuracy of the subspace analysis can be improved by including some of the stiffness associated with frequency-dependent material properties--i.e., viscoelasticity--in the eigenmode extraction step. This is accomplished by using the PROPERTY EVALUATION parameter with the *FREQUENCY option. In general, if the material response does not vary significantly over the frequency range of interest, the value for the PROPERTY EVALUATION parameter can be set to the center of the frequency span. Otherwise, more accurate results will be obtained by running several separate frequency analyses over smaller frequency ranges with appropriate settings for the PROPERTY EVALUATION parameter. In this example a single frequency sweep is performed with PROPERTY EVALUATION=105 Hz. The main advantage that the subspace projection method offers over mode-based techniques (``Mode-based steady-state dynamic analysis,'' Section 6.3.6 of the ABAQUS/Standard User's Manual) is that it allows frequency-dependent material properties, such as viscoelasticity, to be included directly in the analysis. However, there is a cost involved in assembling the projected equations, and this cost must be taken into account when deciding between a subspace solution and a direct solution. ABAQUS offers four different parameter values that may be assigned to the SUBSPACE PROJECTION option to control how often the projected subspace equations are recomputed. These values are ALL FREQUENCIES, in which new projected equations are computed for every frequency in the analysis; EIGENFREQUENCY, in which projected equations are recomputed only at the 3-939

Tire Analyses

eigenfrequencies; PROPERTY CHANGE, in which projected equations are recomputed when the stiffness and/or damping properties have changed by a user-specified percentage; and CONSTANT, which computes the projected equations only once at the center of the frequency range specified in the data lines of the *STEADY STATE DYNAMICS option. Setting SUBSPACE PROJECTION=ALL FREQUENCIES is, in general, the most accurate option; however, the computational overhead associated with recomputing the projected equations at every frequency can significantly reduce the cost benefit of the subspace method versus a direct solution. The SUBSPACE PROJECTION=CONSTANT option is the most inexpensive choice, but it should be chosen only when the material properties do not depend strongly on frequency. In general, the accuracy and cost associated with the four SUBSPACE PROJECTION parameter values are strongly problem dependent. In this example problem the results and computational expense of all four parameter values for SUBSPACE PROJECTION are discussed. The results from the various subspace analyses are compared to the results from a *STEADY STATE DYNAMICS, DIRECT analysis.

Results and discussion Each of the subspace analyses utilizes all 20 modes extracted in the *FREQUENCY step. Figure 3.1.3-2 shows the frequency response plots of the vertical displacements of the road's reference node for the direct solution along with the four subspace solutions using each of the SUBSPACE PROJECTION parameter values discussed above. Similarly, Figure 3.1.3-3 shows the frequency response plots of the horizontal displacement of a node on the tire's sidewall for the same five analyses. As illustrated in Figure 3.1.3-2 and Figure 3.1.3-3, all four of the subspace projection methods yield almost identical solutions; except for small discrepancies in the vertical displacements at 92 and 120 Hz, the subspace projection solutions closely match the direct solution as well. Timing results shown in Table 3.1.3-1 show that the SUBSPACE PROJECTION method results in savings in CPU time versus the direct solution.

Input files tiredynamic_axi_half.inp Axisymmetric model, inflation analysis. tiredynamic_symmetric.inp Partial three-dimensional model, footprint analysis. tiredynamic_freqresp.inp Full three-dimensional model, steady-state dynamic analyses. tiretransfer_node.inp Nodal coordinates for axisymmetric model.

Table

3-940

Tire Analyses

Table 3.1.3-1 Comparison of normalized CPU times (normalized with respect to the DIRECT analysis) to perform frequency sweep from 80 Hz to 130 Hz and the *FREQUENCY step. Normalized CPU time SUBSPACE PROJECTION=ALL FREQUENCIES 0.89 SUBSPACE PROJECTION=EIGENFREQUENCY 0.54 SUBSPACE PROJECTION=PROPERTY CHANGE 0.49 SUBSPACE PROJECTION=CONSTANT 0.36 DIRECT 1.0 *FREQUENCY 0.073

Figures Figure 3.1.3-1 Uniform three-dimensional tire mesh.

Figure 3.1.3-2 Frequency response of the vertical road displacement due to a vertical harmonic point load of 200 N applied to the reference node.

3-941

Tire Analyses

Figure 3.1.3-3 Frequency response of the horizontal sidewall displacement due to a vertical harmonic point load of 200 N applied to the reference node.

Sample listings

3-942

Tire Analyses

Listing 3.1.3-1 *HEADING SYMMETRIC RESULTS TRANSFER FOR STATIC TIRE ANALYSIS: TIREDYNAMIC_FREQRESP 3D FILE TIRE MODEL STEP 0: TRANSFER TIRE FOOTPRINT RESULTS FROM TIREDYNAMIC_SYMMETRIC AND GENERATE MODEL USING *SYMMETRIC MODEL GENERATION STEP 1: BRING TRANSFERRED RESULTS TO EQUILIBRIUM STEP 2: FREQUENCY ANALYSIS STEP 3: STEADY STATE DYNAMICS, SUBSPACE PROJECTION=ALL FREQUENCIES STEP 4: STEADY STATE DYNAMICS, SUBSPACE PROJECTION=EIGENFREQUENCY STEP 5: STEADY STATE DYNAMICS, SUBSPACE PROJECTION=CONSTANT STEP 6: STEADY STATE DYNAMICS, SUBSPACE PROJECTION=PROPERTY CHANGE STEP 7: STEADY STATE DYNAMICS,DIRECT UNITS: KG, M *RESTART,WRITE,FREQ=100 *SYMMETRIC MODEL GENERATION,REFLECT=LINE, ELEMENT=100000,NODE=100000 0.0, 0.0, 0.0, 0.0, 0.0, 1.0 *SYMMETRIC RESULTS TRANSFER,STEP=3,INC=1 *NSET,NSET=SIDE 6015, *FILE FORMAT,ZERO INCREMENT *********************************************** *STEP,INC=100,NLGEOM=YES 1: BRING TRANSFERRED RESULTS TO EQUILIBRIUM *STATIC 1.0, 1.0 *BOUNDARY,OP=NEW RIM, 1, 3 ROAD, 1, 2 ROAD, 4, 6 *DSLOAD,OP=NEW INSIDE, P, 200.E3 *CLOAD,OP=NEW ROAD, 3, 3300. *NODE PRINT,NSET=ROAD,FREQ=1

3-943

Tire Analyses

U, RF, *EL PRINT,FREQ=0 *NODE FILE,NSET=ROAD,FREQ=1 U,RF *EL FILE,FREQ=0 *OUTPUT,FIELD,VARIABLE=PRESELECT,FREQ=1 *OUTPUT,HISTORY,FREQ=1 *NODE OUTPUT, NSET=ROAD U,RF *END STEP ************************************************ *STEP 2: FREQUENCY ANALYSIS *FREQUENCY,EIGENSOLVER=LANCZOS, PROPERTY EVALUATION=105 20,0.,200.,1.0 ** 50,0.,200.,1.0 ** For QA use 20,0.,200.,1.0 *EL FILE, FREQ=0 *NODE FILE, FREQ=0 *EL PRINT, FREQ=0 *NODE PRINT, FREQ=0 *OUTPUT,HISTORY,FREQ=0 *END STEP ************************************************ *STEP 3: FREQUENCY RESPONSE: STEADY STATE DYNAMICS, SUBSPACE SUBSPACE PROJECTION=ALL FREQUENCIES *STEADY STATE DYNAMICS, SUBSPACE PROJECTION=ALL FREQUENCIES, INTERVAL=EIGENFREQUENCY,FREQUENCY SCALE=LINEAR 80,130,3 ** 80,130,7, ** For QA use 80,130,3 *CLOAD ROAD,3,200. *EL PRINT, FREQ=0 *EL FILE, FREQ=0 *NODE PRINT,FREQ=0 *NODE FILE,NSET=SIDE,FREQ=1 U,

3-944

Tire Analyses

*NODE FILE,NSET=ROAD,FREQ=1 U,RF *OUTPUT,FIELD,VARIABLE=PRESELECT,FREQ=0 *OUTPUT,HISTORY,FREQ=1 *NODE OUTPUT,NSET=ROAD U,RF *NODE OUTPUT,NSET=SIDE U, *END STEP ************************************************* *STEP 4: FREQUENCY RESPONSE: STEADY STATE DYNAMICS, SUBSPACE SUBSPACE PROJECTION=EIGENFREQUENCY *STEADY STATE DYNAMICS, SUBSPACE PROJECTION=EIGENFREQUENCY, INTERVAL=EIGENFREQUENCY,FREQUENCY SCALE=LINEAR 80,130,3 ** 80,130,7, ** For QA use 80,130,3 *CLOAD ROAD,3,200. *END STEP ************************************************** *STEP 5: FREQUENCY RESPONSE: STEADY STATE DYNAMICS, SUBSPACE SUBSPACE PROJECTION=CONSTANT *STEADY STATE DYNAMICS, SUBSPACE PROJECTION=CONSTANT, INTERVAL=EIGENFREQUENCY,FREQUENCY SCALE=LINEAR 80,130,3 ** 80,130,7, ** For QA use 80,130,3 *CLOAD ROAD,3,200. *END STEP ************************************************** *STEP 6: FREQUENCY RESPONSE: STEADY STATE DYNAMICS, SUBSPACE SUBSPACE PROJECTION=PROPERTY CHANGE *STEADY STATE DYNAMICS,

3-945

Tire Analyses

SUBSPACE PROJECTION=PROPERTY CHANGE, INTERVAL=EIGENFREQUENCY,FREQUENCY SCALE=LINEAR 80,130,3 ** 80,130,7, ** For QA use 80,130,3 *CLOAD ROAD,3,200. *END STEP ************************************************** *STEP,NLGEOM=YES 7: FREQUENCY RESPONSE: STEADY STATE DYNAMICS, DIRECT *STEADY STATE DYNAMICS,DIRECT, INTERVAL=EIGENFREQUENCY,FREQUENCY SCALE=LINEAR 80,130,3 ** 80,130,7, ** For QA use 80,130,3 *CLOAD ROAD,3,200. *END STEP

3-946

Heat Transfer and Thermal-Stress Analyses

4. Heat Transfer and Thermal-Stress Analyses 4.1 Heat transfer and thermal-stress analyses 4.1.1 Thermally coupled analysis of a disc brake Products: ABAQUS/Standard ABAQUS/Explicit Disc brakes operate by pressing a set of composite material brake pads against a rotating steel disc: the frictional forces cause deceleration. The dissipation of the frictional heat generated is critical for effective braking performance. Temperature changes of the brake cause axial and radial deformation; and this change in shape, in turn, affects the contact between the pads and the disc. Thus, the system should be analyzed as a fully coupled thermo-mechanical system. In this example two thermally coupled disc brake analysis examples are discussed. The first example is an axisymmetric model in which the brake pads and the frictional heat generated by braking are "smeared" out over all 360° of the model. This problem is solved using only ABAQUS/Standard. The heat generation is supplied by user subroutine FRIC, and the analysis models a linear decrease in velocity as a result of braking. The second example is a three-dimensional model of the entire disc with pads touching only part of the circumference. The disc is rotated so that the heat is generated by friction. This problem is solved using both ABAQUS/Standard and ABAQUS/Explicit. It is also possible to perform uncoupled analysis of a brake system. The heat fluxes can be calculated and applied to a thermal model, and then the resulting temperatures can be applied to a stress analysis. However, since the thermal and stress analyses are uncoupled, this approach does not account for the effect of the thermal deformation on the contact which, in turn, affects the heat generation. Another type of geometrical model for a disc brake is used by Gonska and Kolbinger (1993). They model a "vented" disc brake (Figure 4.1.1-1) and take advantage of radial repetition by modeling a pie-slice segment (Figure 4.1.1-2). Like the axisymmetric model, this requires the effect of the pads to be smeared, but it allows the modeling of radial cooling ducts while still reducing the model size relative to a full model.

Geometry and model Both models analyzed in this example have solid discs, which allows the models to use coarser meshes than would be required to model the detail of a typical disc brake that has complicated geometrical features such as cooling ducts and bolt holes. The first example further simplifies the model by considering the pads to be "smeared" around the entire 360° so that the system is axisymmetric. The second example is a full three-dimensional model of the entire annular disc with pads touching only part of the circumference. However, the geometry of the disc has been simplified by making it symmetrical about a plane normal to the axis. Therefore, only half of the disc and one brake pad is modeled, and symmetry boundary conditions are applied. The dimensions of the axisymmetric model are taken from a typical car disc brake. The disc has a thicker friction ring connected to a conical section that, in turn, connects to an inner hub. The inner 4-947

Heat Transfer and Thermal-Stress Analyses

radius of the friction ring is 100.0 mm, the outer radius is 135.0 mm, and it is 10.0 mm thick. The conical section is 32.5 mm deep and 5.0 mm thick. The hub has an inner radius of 60.0 mm, an outer radius of 80.0 mm, and is 5.0 mm thick. The pads are 20.0 mm thick and initially cover the entire friction ring surfaces. The pads and disc of the axisymmetric model are modeled with CAX4T elements. Frictional contact between the pads and the disc is modeled by contact pairs between surfaces defined on the element faces in the contact region. Small sliding is assumed. The mesh is shown in Figure 4.1.1-3, with the pads drawn in a darker gray than the disc. There are six elements through the thickness of the friction ring and four elements through the thickness of each of the pads. The mesh is somewhat coarse but is optimized by using thinner elements near the surfaces of the disc and pads where contact occurs for better resolution of the thermal gradients in these areas. The disc for the three-dimensional model has an outer radius of 135.0 mm, an inner radius of 90.0 mm, and a thickness of 10.0 mm (the half-model has a thickness of 5.0 mm). The ring has a thinner section out to a radius of 100.0 mm, which has a thickness of 6.0 mm (the half-model has a thickness of 3.0 mm). The pad is 10.0 mm thick and covers a little less than one-tenth the circumference. The pad does not quite reach to the edge of the thicker part of the friction ring. The pad and disc of the three-dimensional model are modeled with C3D8T elements in ABAQUS/Standard and with C3D8RT elements in ABAQUS/Explicit; the contact and friction between the pad and the disc are modeled by contact pairs between surfaces defined on the element faces in the contact region. The same mesh is used in both ABAQUS/Standard and ABAQUS/Explicit. It is shown in Figure 4.1.1-4, with the pad drawn in a darker gray than the disc. The disc is a simple annulus with a thinner inner ring. This mesh is also rather coarse with only three elements through the thickness of the disc and three elements through the pad. The elements on the contact sides are thinner since they will be in the areas of higher thermal gradients. There are 36 elements in the circumferential direction of the disc.

Material properties The thermal mechanical properties for the axisymmetric model were taken from a paper by Day and Newcomb (1984) describing the analysis of an annular disc brake. The pad is made of a resin-bonded composite friction material, and the disc is made of steel. Although Day and Newcomb note that material changes occur in the pad material because of thermal degradation, the pad in the axisymmetric model has the properties of the unused pad material. For the axisymmetric model the modulus, density, conductivity, and coefficient of friction are divided by 18 since the pads actually cover only a 20° section of the disc, even though they are modeled as being smeared around the entire circumference. The pad for the three-dimensional model is also a resin-bonded composite friction material whose thermal mechanical properties are listed in Table 4.1.1-1 and coefficient of friction is listed in Table 4.1.1-2. The properties were taken from a paper by Day (1984). It is noted that above certain temperatures, approximately 400°C, the pad material becomes thermally degraded and ¹ is assumed constant from this point on. It is assumed that all the frictional energy is dissipated as heat and distributed equally between the disc and the pad; therefore, the *GAP HEAT GENERATION option is set to 1.0, and the default

4-948

Heat Transfer and Thermal-Stress Analyses

distribution is used. The *GAP HEAT GENERATION option allows the user to specify an unequal distribution, which is particularly important if the heat conduction across the interface is poor. In this example the conductivity value specified with the *GAP CONDUCTANCE option is quite high; hence, the results are not very sensitive to changes in distribution. In ABAQUS/Explicit arbitrarily high gap conductivity values may cause the stable time increment associated with the thermal part of the problem to control the time incrementation, possibly resulting in a very inefficient analysis. In this problem the gap conductivity value used in the ABAQUS/Explicit simulation is 20 times smaller than the one used in the ABAQUS/Standard simulation. This allows the stable time increment associated with the mechanical part of the problem to control the time incrementation, thus permitting a more efficient solution while hardly affecting the results.

Loading The pads of the axisymmetric model are first pressed against the disc. The magnitude of the load is divided by 18 since the pads are not actually axisymmetric. The frictional forces are then applied through user subroutine FRIC to simulate a linear decrease in velocity of the disc relative to the pads. The braking is done over three steps; then, when the velocity is zero, a final step shows the continued heat conduction through the model. The pad of the three-dimensional model is fixed in the nonaxial degrees of freedom and is pressed against the disc with a distributed load applied to the back of the pad. In ABAQUS/Standard the disc is then rotated by 60° using an applied boundary condition to the center ring. In ABAQUS/Explicit this boundary condition is prescribed using the *AMPLITUDE, TYPE=SMOOTH STEP option to minimize the effects of centrifugal forces at the beginning and end of the step. Frictional forces between the surfaces generate heat in the brake. The initial temperature of both models is 20°C.

Solution controls (ABAQUS/Standard only) Since the three-dimensional model has a small loaded area and, thus, rather localized forces and heat fluxes, the default averaged flux values for the convergence criteria produce very tight tolerances and cause more iteration than is necessary for an accurate solution. To decrease the computational time required for the analysis, the *CONTROLS option is used to override the automatic calculation of the average forces and heat fluxes. The option is first used with the FIELD=DISPLACEMENT parameter. The convergence criterion ratio is set to 1%, and the time-average and average fluxes are set to a typical nodal force (displacement flux): fd = pA = (1:7E6)(1:77E-4) ¼ 300; where p is the pressure and A is the area of a typical pad element. The option is next used with the FIELD=TEMPERATURE parameter. The convergence criterion ratio is set to 1%, and the time-average and average fluxes are set to the nodal heat flux (temperature flux) for a typical pad element. The heat flux density generated by an interface element due to frictional heat generation is qg = ´¿ v, where ´ is the gap heat generation factor, ¿ is the frictional stress, and v is the velocity. Therefore, the nodal heat flux is

4-949

Heat Transfer and Thermal-Stress Analyses

ft = qg A = ´ (¹p)(!r )A; where A is the contact area of a typical pad element, ¹ is the friction coefficient, and p is the contact pressure. The angular velocity, !, is obtained as the total rotation, ¼=3, divided by the total time, 0.015 sec. The radius, r, is set to 0.120 m, which is the distance from the axis to a point approximately in the middle of the pad surface. This yields (1:0)(:37)(1:7E6)( ¼3 )(0:12)(1:77E-4) ft = ¼ 900: 0:015

Additional solution controls can reduce the solver cost for an increment by improving the initial solution guess, solving thermal and mechanical equations separately, and reducing the wavefront of three-dimensional finite-sliding contact analysis. These features are discussed below. The impact of combining these features is also discussed. When the default convergence controls are used, it is possible to obtain faster convergence by setting the EXTRAPOLATION parameter on the *STEP option to PARABOLIC. For the three-dimensional model the use of this feature yields a 14% enhancement in computational speed per increment. The coupling between the thermal and mechanical fields in this problem is relatively weak. It is, therefore, possible to obtain a more efficient solution by specifying separate solutions for the thermal and mechanical equations each increment. This technique, which is specified by using the *SOLUTION TECHNIQUE, TYPE=SEPARATED option, results in faster per-iteration solution times at the expense of poorer convergence when a strong interfield coupling is present. Use of this technique also permits the use of the symmetric solver and storage scheme, which is invoked by specifying UNSYMM=NO on the *STEP option. The resulting symmetric approximation of the mechanical equations was also found to be cost effective for this problem, when combined with a quality initial solution guess obtained by specifying EXTRAPOLATION=PARABOLIC on the *STEP option. Neither of these approximations impacts solution accuracy. For the three-dimensional model the use of *SOLUTION TECHNIQUE, TYPE=SEPARATED and *STEP, UNSYMM=NO, EXTRAPOLATION=PARABOLIC yields a 50% decrease in the total solution time. In the three-dimensional model the deformable master surface is defined from a large number of connecting elements resulting in a large wavefront. By default, ABAQUS/Standard employs an automated contact patch algorithm to reduce the wavefront and solution time. For instance, in the coupled thermal-mechanical analysis a substantial savings in solution time (a 30% to 50% decrease) is obtained when the automatic contact patch algorithm is employed compared to an analysis that uses a fixed contact patch encompassing the entire master surface. The reduction in solution time is system dependent and depends on several factors, such as CPU type, system memory, and IO speed. This solution time savings is in addition to any of the other savings discussed in this section. The additional savings is, therefore, realized when the separated solution scheme and parabolic extrapolation are also specified.

Results and discussion

4-950

Heat Transfer and Thermal-Stress Analyses

The temperature distribution of the axisymmetric model at an early time increment is shown in Figure 4.1.1-5. The temperature is greatest at the interfaces between the disc and pads, and the heat has just started to conduct into the disc. Figure 4.1.1-6 shows the temperature distribution at the end of the analysis when the velocity is zero. The heat has conducted through the friction ring of the disc. Figure 4.1.1-7 is a displaced plot of the model at the end of the analysis and shows the characteristic conical deformation due to thermal expansion. The displacement has been magnified by a factor of 128 to show the deformation more clearly. The temperature distribution of the disc surface of the three-dimensional model after a rotation of 60° is shown in Figure 4.1.1-8 (ABAQUS/Standard) and Figure 4.1.1-9 (ABAQUS/Explicit). The agreement between the two results is excellent. The hottest region is the area under the pad, while the heat in the regions that the pad has passed over has dissipated somewhat. Figure 4.1.1-10 shows the temperature distribution of the inside of the brake pad predicted by ABAQUS/Standard, while Figure 4.1.1-11 shows the same result obtained with ABAQUS/Explicit. Again excellent agreement between the two results is noted. Figure 4.1.1-12 shows the temperature distribution in the disc predicted by ABAQUS/Standard with the thickness magnified by a factor of 20. The heat has conducted into the disc in the regions that the pad has passed over. The stresses predicted by ABAQUS/Standard do not account for the effects of centrifugal loads (*COUPLED TEMPERATURE-DISPLACEMENT is a quasi-static procedure), while the stresses predicted by ABAQUS/Explicit do. These effects can be significant, especially during the early transient portion of the simulation when the initially stationary disc is brought up to speed. To compare the stress results between ABAQUS/Standard and ABAQUS/Explicit, we gradually initiated and ended the disc rotation in the ABAQUS/Explicit simulation; thus, in ABAQUS/Explicit, the centrifugal stresses at the beginning and end of the step are small compared with the thermal stresses. At points in between, however, the effects of centrifugal loading are more pronounced and differences between the stress states predicted by ABAQUS/Standard and ABAQUS/Explicit are observed. The overall effect on the thermal response, however, is negligible. The ABAQUS/Explicit analysis did not include mass scaling because its presence would artificially scale the stresses due to the centrifugal loads. It is possible to include mass scaling to make the analysis more economical, but any results obtained with mass scaling must be interpreted carefully in this problem.

Input files ABAQUS/Standard input files discbrake_axi.inp Axisymmetric model. discbrake_axi.f User subroutine FRIC used in discbrake_axi.inp. discbrake_3d.inp Three-dimensional model.

4-951

Heat Transfer and Thermal-Stress Analyses

discbrake_postoutput.inp *POST OUTPUT analysis of the three-dimensional model. discbrake_3d_extrapara.inp Three-dimensional model with the second step run with *STEP, EXTRAPOLATION=PARABOLIC and with the default *CONTROLS option. discbrake_3d_extrapara_300c.inp Three-dimensional model with the second step run with *STEP, EXTRAPOLATION=PARABOLIC. It is assumed that several revolutions occurred and the initial temperature for the disc brake and pad is 300°C. discbrake_3d_separated.inp Three-dimensional model run using the *SOLUTION TECHNIQUE, TYPE=SEPARATED option. ABAQUS/Explicit input file discbrake_3d_xpl.inp Three-dimensional model.

References · Day, A. J., "An Analysis of Speed, Temperature, and Performance Characteristics of Automotive Drum Brakes," Journal of Tribology, vol. 110, pp. 295-305, 1988. · Day, A. J., and T. J. Newcomb, "The Dissipation of Frictional Energy from the Interface of an Annular Disc Brake," Proc. Instn. Mech. Engrs, vol. 198D, no. 11, pp. 201-209, 1984. · Gonska, H. W., and H. J. Kolbinger, "ABAQUS Application Example: Temperature and Deformation Calculation of Passenger Car Brake Disks," ABAQUS Users' Conference Proceedings, 1993.

Tables Table 4.1.1-1 Thermal-mechanical properties. Temperature of property measurement 20 (°C) 2200 Young's modulus, E (N/mm2) Poisson's ratio, º 0.25 3 1550 ½ Density, (kg/m ) 10e-6 Thermal expansion coefficient (K -1) Thermal conductivity, ∙ (w/mK) 0.5 Specific heat, Cp (J/kgK) 1200

100

200

300

1300 0.25 1550 0.5 1200

530 0.25 1550 30e-6 0.5 1200

320 0.25 1550 0.5 1200

4-952

Heat Transfer and Thermal-Stress Analyses

Table 4.1.1-2 Brake lining temperature characteristic. Temperature of property measurement 100 200 (°C) Friction coefficient, ¹ 0.38 0.41

300

400

0.42

0.24

Figures Figure 4.1.1-1 A vented brake disc design.

Figure 4.1.1-2 Modeling a segment of a brake disc.

Figure 4.1.1-3 Mesh for the axisymmetric model, ABAQUS/Standard.

4-953

Heat Transfer and Thermal-Stress Analyses

Figure 4.1.1-4 Mesh for the three-dimensional model.

Figure 4.1.1-5 Isotherms of the axisymmetric model at t =0.675, ABAQUS/Standard.

4-954

Heat Transfer and Thermal-Stress Analyses

Figure 4.1.1-6 Isotherms of the axisymmetric model when braking has ended, ABAQUS/Standard.

Figure 4.1.1-7 Deformation of the axisymmetric disc, displacement magnified by 128, ABAQUS/Standard.

Figure 4.1.1-8 Isotherms of the disc surface, ABAQUS/Standard.

4-955

Heat Transfer and Thermal-Stress Analyses

Figure 4.1.1-9 Isotherms of the disc surface, ABAQUS/Explicit.

Figure 4.1.1-10 Isotherms of the inside of the brake pad, ABAQUS/Standard.

4-956

Heat Transfer and Thermal-Stress Analyses

Figure 4.1.1-11 Isotherms of the inside of the brake pad, ABAQUS/Explicit.

Figure 4.1.1-12 Isotherms of the disc with the thickness magnified 20 times, ABAQUS/Standard.

4-957

Heat Transfer and Thermal-Stress Analyses

Sample listings

4-958

Heat Transfer and Thermal-Stress Analyses

Listing 4.1.1-1 *HEADING AXISYMMETRIC DISC BRAKE ANALYSIS *NODE,NSET=CENTER 1, 60.E-3, 30.E-3 2, 60.E-3, 27.5E-3 3, 60.E-3, 25.E-3 *NODE 801, 80.E-3, 30.E-3 802, 80.E-3, 27.5E-3 803, 80.E-3, 25.E-3 611, 85.E-3, 2.5E-3 612, 85.E-3, 0.E-3 613, 85.E-3, -2.5E-3 1011, 95.E-3, 2.5E-3 1012, 95.E-3, 0.E-3 1013, 95.E-3, -2.5E-3 *NODE,NSET=INNER 1204,100.E-3, 15.E-3 1205,100.E-3, 10.E-3 1206,100.E-3, 7.E-3 1207,100.E-3, 5.5E-3 1208,100.E-3, 5.E-3 ** 1209,100.E-3, 5.E-3 1210,100.E-3, 4.5E-3 1211,100.E-3, 3.E-3 1212,100.E-3, 0.E-3 1213,100.E-3, -3.E-3 1214,100.E-3, -4.5E-3 1215,100.E-3, -5.E-3 ** 1216,100.E-3, -5.E-3 1217,100.E-3, -5.5E-3 1218,100.E-3, -7.E-3 1219,100.E-3,-10.E-3 1220,100.E-3,-15.E-3 *NODE,NSET=OUTER 2404,135.E-3, 15.E-3 2405,135.E-3, 10.E-3 2406,135.E-3, 7.E-3 2407,135.E-3, 5.5E-3

4-959

Heat Transfer and Thermal-Stress Analyses

2408,135.E-3, 5.E-3 ** 2409,135.E-3, 5.E-3 2410,135.E-3, 4.5E-3 2411,135.E-3, 3.E-3 2412,135.E-3, 0.E-3 2413,135.E-3, -3.E-3 2414,135.E-3, -4.5E-3 2415,135.E-3, -5.E-3 ** 2416,135.E-3, -5.E-3 2417,135.E-3, -5.5E-3 2418,135.E-3, -7.E-3 2419,135.E-3,-10.E-3 2420,135.E-3,-15.E-3 *NGEN,NSET=ALL 1, 801,100 2, 802,100 3, 803,100 611,1011,100 612,1012,100 613,1013,100 1011,1211,100 1012,1212,100 1013,1213,100 603, 611, 1 703, 711, 1 803, 811, 1 *NFILL,NSET=ALL INNER, OUTER, 12, 100 *NSET, NSET=PADS, GENERATE 1204, 2404, 100 1205, 2405, 100 1206, 2406, 100 1207, 2407, 100 1208, 2408, 100 1216, 2416, 100 1217, 2417, 100 1218, 2418, 100 1219, 2419, 100 1220, 2420, 100 *NSET, NSET=PADBACK, GENERATE 1204, 2404, 100

4-960

Heat Transfer and Thermal-Stress Analyses

1220, 2420, 100 *ELEMENT, TYPE=CAX4T 1, 1, 2, 102, 101 1209,1209,1210,1310,1309 *ELGEN,ELSET=DISK 1, 2,1,1, 8,100,100 601,12,1,1, 2,100,100 611, 2,1,1, 6,100,100 1209, 6,1,1,12,100,100 *ELSET,ELSET=SURF1 611, 612, 1209, 1210, 1213, 1214 *ELSET,ELSET=SURF2, GENERATE 612, 1112, 100 1214, 2314, 100 *ELSET,ELSET=SURF3, GENERATE 701, 710, 1 2309, 2314, 1 *ELSET,ELSET=SURF4, GENERATE 1, 701, 100 811, 1111, 100 1209, 2309, 100 *ELEMENT, TYPE=CAX4T 1204,1204,1205,1305,1304 1216,1216,1217,1317,1316 *ELGEN,ELSET=PAD1 1204, 4,1,1,12,100,100 *ELGEN,ELSET=PAD2 1216, 4,1,1,12,100,100 *ELSET,ELSET=PADS PAD1,PAD2 *ELSET,ELSET=PADBACK1,GENERATE 1204, 2304, 100 *ELSET,ELSET=PADBACK2,GENERATE 1219, 2319, 100 *ELSET,ELSET=FRIC1, GENERATE 1209, 2309,100 *ELSET, ELSET=FRIC2,GENERATE 1214,2314,100 *ELSET, ELSET=PAD1EL,GENERATE 1207,2307,100 *ELSET, ELSET=PAD2EL,GENERATE 1216,2316,100 *SOLID SECTION,ELSET=DISK,MATERIAL=STEEL

4-961

Heat Transfer and Thermal-Stress Analyses

*MATERIAL, NAME=STEEL *ELASTIC 210.E9, .3 *EXPANSION 11.E-6, *DENSITY 7800., *SPECIFIC HEAT 452., *CONDUCTIVITY 48., *SOLID SECTION,ELSET=PADS,MATERIAL=PAD *MATERIAL, NAME=PAD ** THE MODULUS, DENSITY AND CONDUCTIVITY HAVE BEEN ** DIVIDED BY 18 TO ACCOUNT FOR THE FACT THAT THE ** PADS ARE NOT AXISYMMETRIC *ELASTIC 16.66667E6, .25 *EXPANSION 57.E-6, *DENSITY 125., *SPECIFIC HEAT 1000., *CONDUCTIVITY 0.05, *surface, NAME=RING1 FRIC1,S4 *surface, NAME=RING2 FRIC2,S2 *surface, NAME=PAD1SURF PAD1EL,S2 *surface, NAME=PAD2SURF PAD2EL,S4 *SURFACE INTERACTION, NAME=INT *FRICTION,USER,PROPERTIES=1 0.37, *GAP CONDUCTANCE 1.0E9, 0. 1.0E9, 1. *GAP HEAT GENERATION 1.0,0.5 *CONTACT PAIR, INTERACTION=INT,SMALL SLIDING

4-962

Heat Transfer and Thermal-Stress Analyses

**PAD1SURF,RING1 **PAD2SURF,RING2 RING1,PAD1SURF RING2,PAD2SURF *INITIAL CONDITIONS, TYPE=TEMPERATURE ALL,20. ***** *RESTART,WRITE,FREQUENCY=5 ** *STEP, AMPLITUDE=RAMP START BRAKING: VELOCITY DECREASES LINEARLY OVER TIME IN 4.5 SECS *COUPLED TEMPERATURE-DISPLACEMENT,DELTMX=100. 0.005, 0.01 *BOUNDARY CENTER, 1, 2 PADBACK, 1 ** PRESSURE LOAD DIVIDED BY 18 AS WELL *DLOAD PADBACK1, P4, 0.09444444E6 PADBACK2, P2, 0.09444444E6 *FILM SURF1, F1, 20., 100. SURF2, F2, 20., 100. SURF3, F3, 20., 100. SURF4, F4, 20., 100. *PRINT, CONTACT=YES *EL PRINT, FREQUENCY=100 S, E, *NODE PRINT, NSET=PADS, FREQUENCY=100 U1, U2, NT11, RF1, RF2 *NODE FILE, NSET=PADS, FREQUENCY=100 U, NT, RF *END STEP ** *STEP, INC=100, AMPLITUDE=RAMP CONTINUE BRAKING: 0.01 TO 0.04 SECS *COUPLED TEMPERATURE-DISPLACEMENT,DELTMX=10. 0.01, 0.04 *END STEP ** *STEP, INC=100, AMPLITUDE=RAMP

4-963

Heat Transfer and Thermal-Stress Analyses

CONTINUE BRAKING: 0.04 TO 4.5 SECS *COUPLED TEMPERATURE-DISPLACEMENT,DELTMX=50. 0.1, 4.0, , .4 *END STEP ** *STEP, INC=100, AMPLITUDE=RAMP HEAT CONDUCTION WITH ZERO VELOCITY *COUPLED TEMPERATURE-DISPLACEMENT,DELTMX=50. 1., 20.0, , 4. *END STEP

4-964

Heat Transfer and Thermal-Stress Analyses

Listing 4.1.1-2 *HEADING THERMALLY COUPLED ANALYSIS OF A SYMMETRIC DISC BRAKE *NODE 1, 90.0000000E-3, 0.00000000E-3, 0.0E-3 36, 88.6326978E-3, -15.62833599E-3, 0.0E-3 101, 100.0000000E-3, 0.00000000E-3, 0.0E-3 136, 98.4807753E-3, -17.36481777E-3, 0.0E-3 401, 135.0000000E-3, 0.00000000E-3, 0.0E-3 436, 132.9490467E-3, -23.44250399E-3, 0.0E-3 1001, 90.0000000E-3, 0.00000000E-3, 3.0E-3 1036, 88.6326978E-3, -15.62833599E-3, 3.0E-3 1101, 100.0000000E-3, 0.00000000E-3, 3.0E-3 1136, 98.4807753E-3, -17.36481777E-3, 3.0E-3 1401, 135.0000000E-3, 0.00000000E-3, 3.0E-3 1436, 132.9490467E-3, -23.44250399E-3, 3.0E-3 2101, 100.0000000E-3, 0.00000000E-3, 4.5E-3 2136, 98.4807753E-3, -17.36481777E-3, 4.5E-3 2401, 135.0000000E-3, 0.00000000E-3, 4.5E-3 2436, 132.9490467E-3, -23.44250399E-3, 4.5E-3 3101, 100.0000000E-3, 0.00000000E-3, 5.0E-3 3136, 98.4807753E-3, -17.36481777E-3, 5.0E-3 3401, 135.0000000E-3, 0.00000000E-3, 5.0E-3 3436, 132.9490467E-3, -23.44250399E-3, 5.0E-3 *NODE, NSET=CENTER 1000, 0., 0., 0., *NGEN, LINE=C, NSET=SUPPORT 1, 36, 1, , 0., 0., 0.0E-3, 0., 0., 100.E-3 1001, 1036, 1, , 0., 0., 3.0E-3, 0., 0., 100.E-3 *NGEN, LINE=C, NSET=INNER1 101, 136, 1, , 0., 0., 0.0E-3, 0., 0., 100.E-3 1101, 1136, 1, , 0., 0., 3.0E-3, 0., 0., 100.E-3 *NGEN, LINE=C, NSET=INNER2 2101, 2136, 1, , 0., 0., 4.5E-3, 0., 0., 100.E-3 3101, 3136, 1, , 0., 0., 5.0E-3, 0., 0., 100.E-3 *NSET, NSET=INNER INNER1, INNER2 *NGEN, LINE=C, NSET=OUTER 401, 436, 1, , 0., 0., 0.0E-3, 0., 0., 100.E-3 1401, 1436, 1, , 0., 0., 3.0E-3, 0., 0., 100.E-3 2401, 2436, 1, , 0., 0., 4.5E-3, 0., 0., 100.E-3

4-965

Heat Transfer and Thermal-Stress Analyses

3401, 3436, 1, , 0., 0., 5.0E-3, 0., 0., 100.E-3 *NFILL, NSET=DISK INNER, OUTER, 3, 100 *NSET, NSET=SYMM, GENERATE 101, 436 *ELEMENT, TYPE=C3D8T, ELSET=SUPPORT 1, 1, 101, 102, 2, 1001, 1101, 1102, 1002 36, 36, 136, 101, 1, 1036, 1136, 1101, 1001 *ELEMENT, TYPE=C3D8T, ELSET=DISK 101, 101, 201, 202, 102, 1101, 1201, 1202, 1102 136, 136, 236, 201, 101, 1136, 1236, 1201, 1101 *ELGEN, ELSET=SUPPORT 1, 35, 1, 1 *ELGEN, ELSET=DISK 101, 35, 1, 1, 3, 100, 100, 3, 1000, 1000 136, 1, 1, 1, 3, 100, 100, 3, 1000, 1000 *ELSET, ELSET=FULLDISK SUPPORT, DISK *ELSET, ELSET=DISKSURF, GENERATE 2101, 2436 *SOLID SECTION, ELSET=FULLDISK, MATERIAL=STEEL, ORIENTATION=CYL *MATERIAL, NAME=STEEL *ELASTIC 209.E9, .3 *EXPANSION 11.E-6, *DENSITY 7800., *SPECIFIC HEAT 452., *CONDUCTIVITY 48., *ORIENTATION, SYSTEM=CYLINDRICAL, NAME=CYL 0., 0., 0., 0., 0., 1. 3, 0. *MPC BEAM, SUPPORT, 1000 *NODE 10001, 29.E-3, 97.26895702E-3, 5.0E-3 10005, -29.E-3, 97.26895702E-3, 5.0E-3 10301, 38.E-3, 127.4558747E-3, 5.0E-3 10305, -38.E-3, 127.4558747E-3, 5.0E-3

4-966

Heat Transfer and Thermal-Stress Analyses

11001, 29.E-3, 97.26895702E-3, 5.5E-3 11005, -29.E-3, 97.26895702E-3, 5.5E-3 11301, 38.E-3, 127.4558747E-3, 5.5E-3 11305, -38.E-3, 127.4558747E-3, 5.5E-3 12001, 29.E-3, 97.26895702E-3, 7.0E-3 12005, -29.E-3, 97.26895702E-3, 7.0E-3 12301, 38.E-3, 127.4558747E-3, 7.0E-3 12305, -38.E-3, 127.4558747E-3, 7.0E-3 13001, 29.E-3, 97.26895702E-3, 10.0E-3 13005, -29.E-3, 97.26895702E-3, 10.0E-3 13301, 38.E-3, 127.4558747E-3, 10.0E-3 13305, -38.E-3, 127.4558747E-3, 10.0E-3 14001, 29.E-3, 97.26895702E-3, 15.0E-3 14005, -29.E-3, 97.26895702E-3, 15.0E-3 14301, 38.E-3, 127.4558747E-3, 15.0E-3 14305, -38.E-3, 127.4558747E-3, 15.0E-3 *NGEN, LINE=C, NSET=INPAD 10001,10005,1,,0.,0.,5.0E-3,0.,0.,100.E-3 11001,11005,1,,0.,0.,5.5E-3,0.,0.,100.E-3 12001,12005,1,,0.,0.,7.0E-3,0.,0.,100.E-3 13001,13005,1,,0.,0.,10.0E-3,0.,0.,100.E-3 14001,14005,1,,0.,0.,15.0E-3,0.,0.,100.E-3 *NGEN, LINE=C, NSET=OUTPAD 10301,10305,1,,0.,0.,5.0E-3,0.,0.,100.E-3 11301,11305,1,,0.,0.,5.5E-3,0.,0.,100.E-3 12301,12305,1,,0.,0.,7.0E-3,0.,0.,100.E-3 13301,13305,1,,0.,0.,10.0E-3,0.,0.,100.E-3 14301,14305,1,,0.,0.,15.0E-3,0.,0.,100.E-3 *NFILL, NSET=NPAD INPAD, OUTPAD, 3, 100 *NSET, NSET=NPADBACK, GENERATE 14001, 14305 *NSET, NSET=ALL DISK, NPAD, SUPPORT *ELEMENT, TYPE=C3D8T 10001, 10001, 10101, 10102, 10002, 11001, 11101, 11102, 11002 *ELGEN, ELSET=EPAD 10001, 4, 1, 1, 3, 100, 100, 4, 1000, 1000 *ELSET, ELSET=EPADBACK, GENERATE 13001, 13204 *SOLID SECTION, ELSET=EPAD, MATERIAL=PADMAT, ORIENTATION=CYL

4-967

Heat Transfer and Thermal-Stress Analyses

*MATERIAL, NAME=PADMAT *ELASTIC 2200.E6, .25, 20.0 1300.E6, .25, 100.0 530.E6, .25, 200.0 320.E6, .25, 300.0 *EXPANSION 10.E-6, 20.0 30.E-6,200.0 *DENSITY 1550., *SPECIFIC HEAT 1200., *CONDUCTIVITY 0.9, ** ** DEFINE SURFACES AND CONTACT PAIR ** *SURFACE, NAME=MASTER DISKSURF, S2 *SURFACE, NAME=SLAVE 10001, S1 10002, S1 10003, S1 10004, S1 10101, S1 10102, S1 10103, S1 10104, S1 10201, S1 10202, S1 10203, S1 10204, S1 *CONTACT PAIR, INTERACTION=INTERF SLAVE,MASTER *SURFACE INTERACTION, NAME=INTERF *FRICTION 0.37,,,20.0 0.38,,,100.0 0.41,,,200.0 0.39,,,300.0 0.24,,,400.0 *GAP CONDUCTANCE

4-968

Heat Transfer and Thermal-Stress Analyses

1.0E9, 0. 1.0E9, 1. *GAP HEAT GENERATION 1.0, *INITIAL CONDITIONS, TYPE=TEMPERATURE ALL,20. *RESTART, WRITE, FREQUENCY=100 ***** *STEP,NLGEOM,AMPLITUDE=RAMP,UNSYMM=YES PRESS THE PAD AGAINST THE DISK *COUPLED TEMPERATURE-DISPLACEMENT,DELTMX=100. 0.0005, 0.001 *BOUNDARY SYMM, 3, 3 CENTER, 1, 6 NPADBACK, 1, 2 *DLOAD EPADBACK, P2, 1.7E6 *FILM DISKSURF, F2, 20., 100. ** *PRINT, CONTACT=YES *CONTACT PRINT, FREQUENCY=5 *CONTACT FILE, FREQUENCY=5 *EL PRINT, FREQUENCY=100 S, E, *NODE PRINT, NSET=CENTER, FREQUENCY=1 UR3,RF *NODE PRINT, NSET=NPAD, FREQUENCY=100 U1, U2, U3, NT11, RF1, RF2, RF3 *NODE FILE, NSET=CENTER, FREQUENCY=1 U, RF *NODE FILE, NSET=NPAD, FREQUENCY=100 U, NT, RF *END STEP ***** *STEP, NLGEOM,INC=100,AMPLITUDE=RAMP,UNSYMM=YES ROTATE THE DISK BY 60 DEGREES *COUPLED TEMPERATURE-DISPLACEMENT, DELTMX=100. 0.001, 0.015, , .004 *CONTROLS,PARAMETERS=FIELD,FIELD=DISPLACEMENT 0.01,,300.,300.

4-969

Heat Transfer and Thermal-Stress Analyses

*CONTROLS,PARAMETERS=FIELD,FIELD=TEMPERATURE 0.01,,900.,900. *BOUNDARY CENTER, 6, 6, 1.04717 *END STEP

4-970

Heat Transfer and Thermal-Stress Analyses

Listing 4.1.1-3 *HEADING THERMALLY COUPLED ANALYSIS OF A SYMMETRIC DISC BRAKE (EXPLICIT) RIGID BODY (PIN NSET) *NODE 1, 90.0000000E-3, 0.00000000E-3, 0.0E-3 36, 88.6326978E-3, -15.62833599E-3, 0.0E-3 101, 100.0000000E-3, 0.00000000E-3, 0.0E-3 136, 98.4807753E-3, -17.36481777E-3, 0.0E-3 401, 135.0000000E-3, 0.00000000E-3, 0.0E-3 436, 132.9490467E-3, -23.44250399E-3, 0.0E-3 1001, 90.0000000E-3, 0.00000000E-3, 3.0E-3 1036, 88.6326978E-3, -15.62833599E-3, 3.0E-3 1101, 100.0000000E-3, 0.00000000E-3, 3.0E-3 1136, 98.4807753E-3, -17.36481777E-3, 3.0E-3 1401, 135.0000000E-3, 0.00000000E-3, 3.0E-3 1436, 132.9490467E-3, -23.44250399E-3, 3.0E-3 2101, 100.0000000E-3, 0.00000000E-3, 4.5E-3 2136, 98.4807753E-3, -17.36481777E-3, 4.5E-3 2401, 135.0000000E-3, 0.00000000E-3, 4.5E-3 2436, 132.9490467E-3, -23.44250399E-3, 4.5E-3 3101, 100.0000000E-3, 0.00000000E-3, 5.0E-3 3136, 98.4807753E-3, -17.36481777E-3, 5.0E-3 3401, 135.0000000E-3, 0.00000000E-3, 5.0E-3 3436, 132.9490467E-3, -23.44250399E-3, 5.0E-3 *NODE, NSET=CENTER 1000, 0., 0., 0., *NGEN, LINE=C, NSET=SUPPORT 1, 36, 1, , 0., 0., 0.0E-3, 0., 0., 100.E-3 1001, 1036, 1, , 0., 0., 3.0E-3, 0., 0., 100.E-3 *NGEN, LINE=C, NSET=INNER1 101, 136, 1, , 0., 0., 0.0E-3, 0., 0., 100.E-3 1101, 1136, 1, , 0., 0., 3.0E-3, 0., 0., 100.E-3 *NGEN, LINE=C, NSET=INNER2 2101, 2136, 1, , 0., 0., 4.5E-3, 0., 0., 100.E-3 3101, 3136, 1, , 0., 0., 5.0E-3, 0., 0., 100.E-3 *NSET, NSET=INNER INNER1, INNER2 *NGEN, LINE=C, NSET=OUTER 401, 436, 1, , 0., 0., 0.0E-3, 0., 0., 100.E-3 1401, 1436, 1, , 0., 0., 3.0E-3, 0., 0., 100.E-3

4-971

Heat Transfer and Thermal-Stress Analyses

2401, 2436, 1, , 0., 0., 4.5E-3, 0., 0., 100.E-3 3401, 3436, 1, , 0., 0., 5.0E-3, 0., 0., 100.E-3 *NFILL, NSET=DISK INNER, OUTER, 3, 100 *NSET, NSET=SYMM, GENERATE 101, 436 *ELEMENT, TYPE=C3D8RT, ELSET=SUPPORT 1, 1, 101, 102, 2, 1001, 1101, 1102, 1002 36, 36, 136, 101, 1, 1036, 1136, 1101, 1001 *ELEMENT, TYPE=C3D8RT, ELSET=DISK 101, 101, 201, 202, 102, 1101, 1201, 1202, 1102 136, 136, 236, 201, 101, 1136, 1236, 1201, 1101 *ELGEN, ELSET=SUPPORT 1, 35, 1, 1 *ELGEN, ELSET=DISK 101, 35, 1, 1, 3, 100, 100, 3, 1000, 1000 136, 1, 1, 1, 3, 100, 100, 3, 1000, 1000 *ELSET, ELSET=FULLDISK SUPPORT, DISK *ELSET, ELSET=DISKSURF, GENERATE 2101, 2436 *SOLID SECTION,ELSET=FULLDISK,MATERIAL=STEEL, ORIENTATION=CYL *MATERIAL, NAME=STEEL *ELASTIC 209.E9, .3 *EXPANSION 11.E-6, *DENSITY 7800., *SPECIFIC HEAT 452., *CONDUCTIVITY 48., *ORIENTATION, SYSTEM=CYLINDRICAL, NAME=CYL 0., 0., 0., 0., 0., 1. 3, 0. ** *RIGID BODY, REF NODE=1000, PIN NSET=SUPPORT ** *NODE 10001, 29.E-3, 97.26895702E-3, 5.0E-3 10005, -29.E-3, 97.26895702E-3, 5.0E-3

4-972

Heat Transfer and Thermal-Stress Analyses

10301, 38.E-3, 127.4558747E-3, 5.0E-3 10305, -38.E-3, 127.4558747E-3, 5.0E-3 11001, 29.E-3, 97.26895702E-3, 5.5E-3 11005, -29.E-3, 97.26895702E-3, 5.5E-3 11301, 38.E-3, 127.4558747E-3, 5.5E-3 11305, -38.E-3, 127.4558747E-3, 5.5E-3 12001, 29.E-3, 97.26895702E-3, 7.0E-3 12005, -29.E-3, 97.26895702E-3, 7.0E-3 12301, 38.E-3, 127.4558747E-3, 7.0E-3 12305, -38.E-3, 127.4558747E-3, 7.0E-3 13001, 29.E-3, 97.26895702E-3, 10.0E-3 13005, -29.E-3, 97.26895702E-3, 10.0E-3 13301, 38.E-3, 127.4558747E-3, 10.0E-3 13305, -38.E-3, 127.4558747E-3, 10.0E-3 14001, 29.E-3, 97.26895702E-3, 15.0E-3 14005, -29.E-3, 97.26895702E-3, 15.0E-3 14301, 38.E-3, 127.4558747E-3, 15.0E-3 14305, -38.E-3, 127.4558747E-3, 15.0E-3 *NGEN, LINE=C, NSET=INPAD 10001,10005,1,,0.,0.,5.0E-3,0.,0.,100.E-3 11001,11005,1,,0.,0.,5.5E-3,0.,0.,100.E-3 12001,12005,1,,0.,0.,7.0E-3,0.,0.,100.E-3 13001,13005,1,,0.,0.,10.0E-3,0.,0.,100.E-3 14001,14005,1,,0.,0.,15.0E-3,0.,0.,100.E-3 *NGEN, LINE=C, NSET=OUTPAD 10301,10305,1,,0.,0.,5.0E-3,0.,0.,100.E-3 11301,11305,1,,0.,0.,5.5E-3,0.,0.,100.E-3 12301,12305,1,,0.,0.,7.0E-3,0.,0.,100.E-3 13301,13305,1,,0.,0.,10.0E-3,0.,0.,100.E-3 14301,14305,1,,0.,0.,15.0E-3,0.,0.,100.E-3 *NFILL, NSET=NPAD INPAD, OUTPAD, 3, 100 *NSET, NSET=NPADBACK, GENERATE 14001, 14305 *NSET, NSET=ALL DISK, NPAD, SUPPORT *ELEMENT, TYPE=C3D8RT 10001, 10001, 10101, 10102, 10002, 11001, 11101, 11102, 11002 *ELGEN, ELSET=EPAD 10001, 4, 1, 1, 3, 100, 100, 4, 1000, 1000 *ELSET, ELSET=EPADBACK, GENERATE 13001, 13204

4-973

Heat Transfer and Thermal-Stress Analyses

*SOLID SECTION, ELSET=EPAD, MATERIAL=PADMAT, ORIENTATION=CYL *MATERIAL, NAME=PADMAT *ELASTIC 2200.E6, .25, 20.0 1300.E6, .25, 100.0 530.E6, .25, 200.0 320.E6, .25, 300.0 *EXPANSION 10.E-6, 20.0 30.E-6,200.0 *DENSITY 1550., *SPECIFIC HEAT 1200., *CONDUCTIVITY 0.9, *INITIAL CONDITIONS, TYPE=TEMPERATURE ALL,20. *ELSET,ELSET=EALL EPAD,FULLDISK ** ** DEFINE SURFACES ** *SURFACE, NAME=MASTER DISKSURF, S2 *SURFACE, NAME=SLAVE 10001, S1 10002, S1 10003, S1 10004, S1 10101, S1 10102, S1 10103, S1 10104, S1 10201, S1 10202, S1 10203, S1 10204, S1 ** *STEP PRESS THE PAD AGAINST THE DISK *DYNAMIC TEMPERATURE-DISPLACEMENT, EXPLICIT

4-974

Heat Transfer and Thermal-Stress Analyses

, 0.001 *BOUNDARY SYMM, 3, 3 CENTER, 1, 6 NPADBACK, 1, 2 ** ** DEFINE CONTACT PAIR ** *CONTACT PAIR, INTERACTION=INTERF,WEIGHT=0.0 SLAVE,MASTER *SURFACE INTERACTION, NAME=INTERF *FRICTION 0.37,,,20.0 0.38,,,100.0 0.41,,,200.0 0.39,,,300.0 0.24,,,400.0 *GAP CONDUCTANCE, PRESSURE 5.0E7,0.0 5.0E7,1000.0 *GAP HEAT GENERATION 1.0, ** *AMPLITUDE,NAME=RAMP 0.0,0.0,0.001,1.0 *DLOAD,AMP=RAMP EPADBACK, P2, 1.7E6 *FILM,AMP=RAMP DISKSURF, F2, 20., 100. ** *FILE OUTPUT,NUM=1 *NODE FILE NT, *EL FILE S, *END STEP ***** *STEP ROTATE THE DISK BY 60 DEGREES *DYNAMIC TEMPERATURE-DISPLACEMENT, EXPLICIT , 0.015 *AMPLITUDE,NAME=RAMP2,DEFINITION=SMOOTH STEP 0.,0.,0.015,1.0

4-975

Heat Transfer and Thermal-Stress Analyses

*BOUNDARY, TYPE=DISPLACEMENT,AMP=RAMP2 CENTER, 6, 6, 1.04717 *END STEP

4.1.2 Exhaust manifold assemblage Product: ABAQUS/Standard Engine exhaust manifolds are commonly subject to severe thermal cycles during operation and upon shutdown. Thermal expansion and contraction of the manifold is constrained by its interaction with the engine head to which it is bolted. These constraints govern the thermo-mechanical fatigue life of the manifold. The initial assembly procedure consists of bolting the flanges of the manifold to the engine head with prescribed bolt forces that produce uniform axial bolt stresses. Under subsequent operating conditions such as thermal cycling and creep, these bolt forces may increase or relax, possibly changing normal pressures and resulting in lateral slippage between the engine head and the manifold flanges. Thus, the boundary constraints on the manifold flanges are a function of the response of the entire assembly to its operating conditions. As such, these boundary constraints cannot be prescribed a priori. This example shows how to simulate these varying boundary constraints with the prescribed assembly load capability of ABAQUS. The problem scenario consists of three steps: 1. Apply prescribed bolt loads to fasten the exhaust manifold to the engine head. 2. Subject the assembly to the steady-state operating temperature distribution. 3. Return the assembly to ambient temperature conditions.

Geometry and model The exhaust manifold assemblage being analyzed is depicted in Figure 4.1.2-1. It consists of a four tube exhaust manifold with three flanges, bolted with seven bolts to a small section of the engine head. The manifold is cast from gray iron with a Young's modulus of 138 GPa, a Poisson's ratio of 0.283, and a coefficient of thermal expansion of 13.8 ´ 10-6 per °C. In this example the region of the manifold where the hot exhaust gases converge is subject to temperatures ranging from an initial value of 300 K to an extreme of 980 K. The elastic-plastic response of gray cast iron varies greatly over this range of temperatures, so the temperature-dependent plasticity curves shown in Figure 4.1.2-2 are used for the manifold material. Gray cast iron exhibits different behavior in tension and compression; therefore, these curves represent the average response. The Mises metal plasticity model with isotropic hardening is used. The three manifold flanges contain a total of seven bolt holes. The 9.0 mm diameter of these bolt holes is slightly greater than the 8.0 mm diameter of the bolt shanks to allow for some unobstructed lateral motion of the manifold. For simplicity, only a portion of engine head directly beneath the manifold flanges is modeled. The

4-976

Heat Transfer and Thermal-Stress Analyses

head is made from aluminum, with a Young's modulus of 69 GPa, a Poisson's ratio of 0.33, and a coefficient of thermal expansion of 22.9 ´ 10-6 per °C. The head has four exhaust ports leading into the manifold tubes. It has seven bolt holes used to secure the manifold. Seven bolts fasten the manifold to the head. The bolts are made from steel, with a Young's modulus of 207 GPa, a Poisson's ratio of 0.3, and a coefficient of thermal expansion of 13.8 ´ 10-6 per °C. The bolt shanks have a diameter of 8 mm. The bolt head diameters are 16 mm. Three-dimensional, deformable-to-deformable, small-sliding contact conditions apply to the model. The bottom of the bolt heads form contact bearing surfaces, with the top surfaces of the manifold flanges lying directly beneath them. In addition, the bottoms of the manifold flanges form contact bearing surfaces with the top of the engine head. Each of these surfaces is defined in ABAQUS with the *SURFACE option. Respective mating surfaces are paired together with the *CONTACT PAIR option. Normal pressures will be transmitted through these contact pairs as a result of the bolt tightening forces in Step 1. The forces carried by the bolts will vary as they respond to the thermal cycling of the assembly in subsequent steps. These fluctuations in bolt loads will result in varying normal pressures transmitted across the contact pairs. Lateral slip of the mating components will occur if the critical frictional shear stress limit is surpassed by lateral forces developed in the system. A friction coefficient of 0.2 is used between all contacting surfaces. Contact conditions are not necessary between the bolt shanks and the holes in the manifold flanges because of the design clearance between them. Contact between the bolt shanks and the holes in the engine head is not modeled. All three structural components (manifold, head, and bolts) are modeled with three-dimensional continuum elements. The model consists of 7450 first-order brick elements with incompatible deformation modes, C3D8I, and 282 first-order prism elements, C3D6. The C3D6 elements are used only where the complex geometry precludes the use of C3D8I elements. The C3D8I elements are selected to represent the bending of the manifold walls with only one element through the thickness of the tube walls.

Loading and boundary constraints It is assumed that the engine head is securely fixed to a stiff and bulky engine block, so the nodes along the base of the head are secured in the direction normal to the base (the global x-direction) but are free to move in the two lateral directions to account for thermal expansion. It is also assumed that the bolts are threaded tightly into the engine head, with the bolt threads beginning directly beneath the section of engine head modeled. Therefore, the nodes at the bottom of the bolt shanks are shared with the nodes of the surrounding engine head elements and are also secured in the global x-direction. The manifold flanges are sandwiched between the top of the engine head and the base of the bolt heads using the *CONTACT PAIR option. The line of action of the bolt forces (bolt shank axes) is along the global x degree of freedom. Soft springs acting in the global y- and z-directions are attached to the outlet end of the manifold and to the two ends of the head to suppress rigid body motions of the manifold and head, respectively. These springs have no influence on the solution. In the first step of the analysis each of the seven bolts is tightened to a uniform bolt force of 20 kN. In subsequent steps the variation of the bolt loads is monitored as the bolts respond to the thermal loading on the assembly as a whole. The "prescribed assembly load" capability of ABAQUS is used. For each

4-977

Heat Transfer and Thermal-Stress Analyses

bolt we define a "cut," or pre-tension section, and subject the section to a specified tensile load. As a result, the length of the bolt at the pre-tension section will change by the amount necessary to carry the prescribed load, while accounting for the compliance of the rest of the system. In the next step the prescribed bolt loads are replaced by the condition that the length changes calculated in the previous step remain fixed. The remainder of the bolt is free to deform. Then, during further external loading of the assembly the total force across each pre-tension section can be monitored as the reaction force required to hold the pre-tension section length change constant. The same procedure is used for all seven bolts. First, pre-tension sections are defined as "cuts" that are perpendicular to the bolt shank axes by using the *SURFACE option on the faces of a group of elements within each bolt shank, as shown in Figure 4.1.2-3. The line of action of the bolt force is in the direction that is normal to this surface. Next, each bolt is assigned an arbitrary, independent node that possesses one degree of freedom (dof 1), to which the bolt force will be applied. These nodes are called the "pre-tension nodes" (all seven bolt pre-tension nodes are placed into a node set named BOLTS). The spatial position of a pre-tension node is irrelevant. Finally, each surface is associated with the appropriate pre-tension node using the *PRE-TENSION SECTION option. A portion of the ABAQUS model definition section defining the pre-tension section is shown below: *ELSET, ELSET=BCUT1, GENERATE 19288,19307 *SURFACE, NAME=BOLT1 BCUT1,S2 *NODE, NSET=BOLTS 99991, 21.964 , -139.80 , -12.425 ... 99997, 21.964 , 137.38 , -12.226 *PRE-TENSION SECTION, SURFACE=BOLT1, NODE=99991

In Step 1 of the analysis a concentrated clamping load of 20 kN is applied to each of the pre-tension nodes in node set BOLTS. In Step 2 the concentrated load from Step 1 is removed and replaced by a "fixed" boundary condition on each pre-tension node that will hold the pre-tension section length changes from Step 1 fixed. The time period of this step is small so that it will not appear in time history plots of bolt loads. It is not a requirement that a separate step be used to replace the concentrated bolt force with a fixed boundary constraint; the replacement procedure can, in principle, be performed during the thermal load step. However, over the course of a step in which a load is replaced by a boundary condition, CF1 is ramped down, while RF1 is ramped up to replace it. Therefore, the total force across the bolt is the sum of the concentrated force ( CF1) and the reaction force (RF1) on the pre-tension node. In Step 3 of the analysis nodal temperatures depicting the steady-state temperature distribution in the manifold are read from an external file. The temperature distribution is shown in Figure 4.1.2-4. These nodal temperatures can be generated by an ABAQUS heat transfer analysis. Each of the nodes in the model has its temperature ramped up from the initial ambient temperature of 300 K to its final steady-state temperature. These nodal temperatures are interpolated to the element integration points so that the correct temperature-dependent plasticity data can be used in the constitutive calculations.

4-978

Heat Transfer and Thermal-Stress Analyses

Finally, in Step 4 the nodal temperatures are ramped back down to the initial ambient temperature of 300 K.

Results and discussion The analysis is performed as a small-displacement analysis. The nonlinearities in the problem are the result of changing contact conditions, frictional slip and stick, and temperature-dependent plasticity. Figure 4.1.2-5 shows the lateral displacement of the bottom surface of the flange at the end of the heat-up step. As a result of frictional sticking, the ends of the two outer manifold flanges have expanded outward relative to one another by only about 0.75 mm. Plastic yielding conditions result since thermal expansion of the remainder of the manifold is constrained by this limited lateral flange motion. A separate thermal-stress analysis of the manifold only, with no bolt constraints included, produced relative lateral expansions of about 1.1 mm and very little plasticity. Figure 4.1.2-6 is a plot of the forces carried by each of the seven bolts throughout the load history. This plot can be obtained with the X-Y plotting capabilities in ABAQUS/Viewer. The curves contain the values of the concentrated forces (CF1) for the pre-tension nodes in node set BOLTS for the first step of the analysis and the reaction forces (RF1) for subsequent steps. The loads carried by the bolts increase significantly during the heat-up step. The loads do not return precisely to the original bolt load specification upon cool down because of the residual stresses, plastic deformation, and frictional dissipation that developed in the manifold.

Input files manifold.inp Input data for the analysis. manifold_node_elem.inp Node and element definitions. manifold_nodaltemp.inp Nodal temperature data.

Figures Figure 4.1.2-1 Manifold assemblage.

4-979

Heat Transfer and Thermal-Stress Analyses

Figure 4.1.2-2 Gray cast iron temperature-dependent plasticity curves.

Figure 4.1.2-3 Pre-tension section.

4-980

Heat Transfer and Thermal-Stress Analyses

Figure 4.1.2-4 Steady-state temperature distribution.

Figure 4.1.2-5 Lateral expansion of manifold footprint.

Figure 4.1.2-6 History of bolt forces.

4-981

Heat Transfer and Thermal-Stress Analyses

Sample listings

4-982

Heat Transfer and Thermal-Stress Analyses

Listing 4.1.2-1 *HEADING BOLT DOWN AND THERMAL CYCLE OF EXHAUST MANIFOLD *PREPRINT, ECHO=NO ** ** read nodes and elements from external file ** 14682 nodes in nset NALL ** 7450 C3D8I elements ** 282 C3D6 elements ** create element sets: MANIFOLD, BOLTS, HEAD ** and HDTOP ** create node sets: MANI-N, BOLT-N, HEAD-N ** and HDBASE ** *INCLUDE, INPUT=manifold_node_elem.inp ** *NODE,NSET=BOLTS 99991, 21.964 , -139.80 , -12.425 99992, 21.964 , -87.632 , 23.730 99993, 21.964 , -54.143 , 24.577 99994, 21.964 , -6.2972 , -25.424 99995, 21.964 , 51.885 , 23.802 99996, 21.964 , 85.185 , 24.583 99997, 21.964 , 137.38 , -12.226 *ELSET,ELSET=BCUT1,GEN 19288,19307 *SURFACE,NAME=BOLT1 BCUT1,S2 *PRE-TENSION SECTION,SURFACE=BOLT1,NODE=99991 *ELSET,ELSET=BCUT2,GEN 19248,19267 *SURFACE,NAME=BOLT2 BCUT2,S2 *PRE-TENSION SECTION,SURFACE=BOLT2,NODE=99992 *ELSET,ELSET=BCUT3,GEN 19228,19247 *SURFACE,NAME=BOLT3 BCUT3,S2 *PRE-TENSION SECTION,SURFACE=BOLT3,NODE=99993 *ELSET,ELSET=BCUT4,GEN 19268,19287 *SURFACE,NAME=BOLT4

4-983

Heat Transfer and Thermal-Stress Analyses

BCUT4,S2 *PRE-TENSION SECTION,SURFACE=BOLT4,NODE=99994 *ELSET,ELSET=BCUT5,GEN 19308,19327 *SURFACE,NAME=BOLT5 BCUT5,S2 *PRE-TENSION SECTION,SURFACE=BOLT5,NODE=99995 *ELSET,ELSET=BCUT6,GEN 19190,19208 *SURFACE,NAME=BOLT6 BCUT6,S2 *PRE-TENSION SECTION,SURFACE=BOLT6,NODE=99996 *ELSET,ELSET=BCUT7,GEN 19209,19227 *SURFACE,NAME=BOLT7 BCUT7,S2 *PRE-TENSION SECTION,SURFACE=BOLT7,NODE=99997 ** ** SOFT SPRINGS ON MANIFOLD AND HEAD ** TO ELIMINATE RIGID BODY MOTION ** *ELEMENT, TYPE=SPRING1, ELSET=SOFT2 50002, 3550 60002, 3410 70002, 28794 80002, 28612 *ELEMENT, TYPE=SPRING1, ELSET=SOFT3 50003, 3550 60003, 3410 70003, 28794 80003, 28612 *SPRING, ELSET=SOFT2 2, 1.0, *SPRING, ELSET=SOFT3 3, 1.0, ** *ELSET, ELSET = B1, GEN 18810,18822 *SURFACE, NAME=B1S B1,S2 *ELSET, ELSET = F1, GEN

4-984

Heat Transfer and Thermal-Stress Analyses

11621,11633 *SURFACE, NAME=F1S F1,S1 *CONTACT PAIR, SMALL SLIDING,INTERACTION=BTOF, ADJUST=0.01 F1S, B1S ** *ELSET, ELSET = B2, GEN 18797,18809 *SURFACE, NAME=B2S B2,S2 *ELSET, ELSET = F2, GEN 11608,11620 *SURFACE, NAME=F2S F2,S1 *CONTACT PAIR, SMALL SLIDING,INTERACTION=BTOF, ADJUST=0.01 F2S, B2S ** *ELSET, ELSET = B3, GEN 18784,18796 *SURFACE, NAME=B3S B3,S2 *ELSET, ELSET = F3, GEN 11562,11574 *SURFACE, NAME=F3S F3,S1 *CONTACT PAIR, SMALL SLIDING,INTERACTION=BTOF, ADJUST=0.01 F3S, B3S ** *ELSET, ELSET = B4, GEN 18771,18783 *SURFACE, NAME=B4S B4,S2 *ELSET, ELSET = F4, GEN 11549,11561 *SURFACE, NAME=F4S F4,S1 *CONTACT PAIR, SMALL SLIDING,INTERACTION=BTOF, ADJUST=0.01 F4S, B4S **

4-985

Heat Transfer and Thermal-Stress Analyses

*ELSET, ELSET = B5, GEN 18758,18770 *SURFACE, NAME=B5S B5,S2 *ELSET, ELSET = F5, GEN 11521,11533 *SURFACE, NAME=F5S F5,S1 *CONTACT PAIR, SMALL SLIDING,INTERACTION=BTOF, ADJUST=0.01 F5S, B5S ** *ELSET, ELSET = B6, GEN 18745,18757 *SURFACE, NAME=B6S B6,S2 *ELSET, ELSET = F6, GEN 11492,11504 *SURFACE, NAME=F6S F6,S1 *CONTACT PAIR, SMALL SLIDING,INTERACTION=BTOF, ADJUST=0.01 F6S, B6S ** *ELSET, ELSET = B7, GEN 18732,18744 *SURFACE, NAME=B7S B7,S2 *ELSET, ELSET = F7, GEN 11472,11484 *SURFACE, NAME=F7S F7,S1 *CONTACT PAIR, SMALL SLIDING,INTERACTION=BTOF, ADJUST=0.01 F7S, B7S ** *SURFACE INTERACTION, NAME=BTOF *FRICTION 0.2, ** *SURFACE, NAME=HS HDTOP,S1 *ELSET, ELSET = FL1, GEN

4-986

Heat Transfer and Thermal-Stress Analyses

11766, 11795, 1 11874, 11899, 1 12044, 12073, 1 12076, 12101, 1 *SURFACE, NAME=FL1S FL1,S2 *CONTACT PAIR, SMALL SLIDING,INTERACTION=FTOH, ADJUST=0.01 FL1S, HS ** *ELSET, ELSET = FL2, GEN 11703, 11765, 1 11822, 11873, 1 11957, 12017, 1 12019, 12020, 1 12023, 12043, 1 12102, 12114, 1 *SURFACE, NAME=FL2S FL2,S2 *CONTACT PAIR, SMALL SLIDING,INTERACTION=FTOH, ADJUST=0.01 FL2S, HS ** *ELSET, ELSET = FL3, GEN 11679, 11702, 1 11796, 11821, 1 11900, 11956, 1 *SURFACE, NAME=FL3S FL3,S2 *CONTACT PAIR, SMALL SLIDING,INTERACTION=FTOH, ADJUST=0.01 FL3S, HS ** *SURFACE INTERACTION, NAME=FTOH *FRICTION 0.2, ** *SOLID SECTION,ELSET=MANIFOLD,MATERIAL=CASTFE *SOLID SECTION,ELSET=BOLTS,MATERIAL=STEEL *SOLID SECTION,ELSET=HEAD,MATERIAL=ALUM *MATERIAL, NAME=CASTFE *ELASTIC, TYPE=ISO 0.1380E+06, .2830

4-987

Heat Transfer and Thermal-Stress Analyses

*PLASTIC 325., 0., 293. 375., 0.000192, 293. 400., 0.000351, 293. 425., 0.000920, 293. 437.5,0.0018, 293. ** 262.5,0., 573 300., 0.000076, 573. 325., 0.000395, 573. 350., 0.0019, 573. ** 225., 0., 773. 250., 0.000188, 773. 262.5,0.0005978,773. 275., 0.001257, 773. 281.25,0.00196, 773. ** 25., 0.0, 973. 37.5, 0.000478, 973. 50., 0.0011376, 973. 51.5, 0.003627, 973. ** 12.5, 0.0,1173. 18.75, 0.0004889,1173. 25., 0.00082, 1173. 31.25, 0.00177, 1173. *EXPANSION, TYPE=ISO 0.0000138, ** *MATERIAL, NAME=STEEL *ELASTIC, TYPE=ISO 0.207E+06, 0.30 *EXPANSION, TYPE=ISO 0.0000138, ** *MATERIAL, NAME=ALUM *ELASTIC, TYPE=ISO 0.6900E+5, 0.33 *EXPANSION, TYPE=ISO 0.0000229, ** *INITIAL CONDITION, TYPE=TEMPERATURE

4-988

Heat Transfer and Thermal-Stress Analyses

NALL,300. ** *BOUNDARY HDBASE,1 ** *STEP STEP 1.) APPLY PRESCRIBED BOLT LOADS *STATIC 0.5,1.0 *CLOAD BOLTS,1,20000. *NODE FILE,NSET=BOLTS,FREQ=1 U,CF,RF *EL PRINT,FREQ = 0 S, PE, *NODE PRINT,FREQ = 0 U, RF, *PRINT,CONTACT=YES ** ** OUTPUT FOR ABAQUS/Safe ** *OUTPUT,FIELD,FREQUENCY=9999 *ELEMENT OUTPUT, ELSET=MANIFOLD, POSITION=NODES S, TEMP *NODE OUTPUT U, ** *END STEP ** *STEP, INC=1 STEP 2.) SUBSTITUTE BOLT LOAD WITH RESULTANT LENGTH CHANGE *STATIC 1.0E-10,1.0E-10,1.0E-10,1.0E-10 *BOUNDARY, FIXED BOLTS,1 *CLOAD, OP=NEW *ENDSTEP ** *STEP, INC=200 STEP 3.) APPLY PRESCRIBED THERMAL LOAD

4-989

Heat Transfer and Thermal-Stress Analyses

*STATIC 0.1, 1.0, 0.00001 *TEMPERATURE, INPUT=manifold_nodaltemp.inp *EL FILE, FREQ=100, ELSET=MANIFOLD, POSITION=CENTROID SP, *ENDSTEP ** *STEP, INC=200 STEP 4.) RETURN TO AMBIENT TEMPERATURES *STATIC 0.2, 1.0, 0.00001 *TEMPERATURE NALL,300. *ENDSTEP

4.1.3 Coolant manifold cover gasketed joint Product: ABAQUS/Standard Engine gaskets are used to seal the mating surfaces of engine components to maintain the integrity of the closed system throughout a wide range of operating loads and environmental conditions. Inadequate gasket performance leads to diminished engine pressure and fluid leakage, resulting in degradation of engine performance and potential engine damage. The gasket, the engine component flanges, and the fasteners--collectively referred to as a gasketed joint--must be considered as a unit when determining the system sealing performance because most gasketed joints do not obtain a uniform contact stress distribution due to nonuniform bolt spacing and flange distortion during assembly and subsequent operational loading. Engine gaskets are often complicated geometric constructs of various engineering materials and are subject to large compressive strains. The compressive response of the gasket is highly nonlinear. Such complexities make detailed modeling of gaskets with continuum elements difficult and impractical when analyzing complete assemblies. ABAQUS has a dedicated class of elements, referred to as gasket elements, that simplify the modeling of such components while maintaining the essential ingredients of the nonlinear response. Typical use of these gasket elements involves a tabular representation of the pressure versus closure relationship in the thickness direction of the gasket. The pressure versus closure models available in ABAQUS allow the modeling of very complex gasket behaviors, including nonlinear elasticity, permanent plastic deformation, and loading/unloading along different paths. These behaviors are usually calibrated directly from test data. In this manner a complex gasket can be modeled effectively using a single gasket element in the thickness direction. In this example a paper foam gasket with a silkscreened silicone bead is compressed between the lower engine intake manifold and the coolant manifold cover. The coolant manifold cover seals the lower intake manifold coolant passages so that the coolant can be distributed to the cylinder heads. An

4-990

Heat Transfer and Thermal-Stress Analyses

exploded view of the gasketed joint model is shown in Figure 4.1.3-1. It consists of two steel bolts, an aluminum coolant manifold cover, a paper foam gasket with a silicone bead, and--for simplicity--only a portion of the lower intake manifold, which is composed of steel. Symmetry conditions reduce the structure to a half model. The gasketed joint is subjected to the following mechanical and environmental load conditions: 1. Simulate the bolt loading sequence to fasten the joint. 2. Heat the assembly to the maximum operating temperature and apply interior cavity pressure. 3. Cool the assembly to the minimum operating temperature while maintaining interior cavity pressure. 4. Return the assembly to ambient conditions with the interior pressure removed. 5. Disassemble the gasketed joint.

Geometry and material The portion of the lower intake manifold that is modeled has two passages. Coolant flows from one passage into the manifold cover and back out through the other passage. Two steel bolts secure the cover to the manifold. The bolt shanks have a diameter of 6.0 mm, and the bolt heads have a diameter of 11.8 mm. The bolts and the lower intake manifold are assigned a Young's modulus of 2.0 ´ 105 MPa, a Poisson's ratio of 0.28, and a coefficient of thermal expansion of 1.6 ´ 10-5 per °C. The aluminum coolant manifold cover has a Young's modulus of 7.1 ´ 104 MPa, a Poisson's ratio of 0.33, and a coefficient of thermal expansion of 2.3 ´ 10-5 per °C. The metal components (bolts, cover, and intake manifold) are modeled with three-dimensional continuum elements: 1304 first-order brick elements with incompatible deformation modes ( C3D8I) and 208 first-order prism elements (C3D6). The C3D8I elements are chosen to capture the bending of the cover, using only one element through its thickness. The C3D6 elements are used only where geometric constraints preclude the use of C3D8I elements. The gasket schematic shown in Figure 4.1.3-2 has two distinct regions. The majority of the gasket is composed of a 0.79 mm thick, flat, crushable paper foam material. To ensure proper sealing pressures for this joint, a 0.076 mm thick silicone bead has been silkscreened along the top surface of the gasket encircling the interior cavity. Placing silicone beads on gaskets results in a change in the load transmitting characteristics of the gasket, which often improves both the recovery properties of the gasket and its potential to remain sealed for the long term. The entire gasket, including the bead, is modeled as a flat sheet with one gasket element through the thickness (see Figure 4.1.3-3). A fine mesh is used for the gasket to capture the in-plane variation of the gasket sealing pressure. This creates a mismatched mesh across the contacting surfaces, but ABAQUS contact definitions do not require one-to-one matching meshes across contact pairs. The gasket components (silicone bead region and paper foam region) are modeled with 973 first-order 8-node area elements (GK3D8) and 29 first-order 6-node area elements (GK3D6). The physical thickness of the entire sheet of gasket elements corresponds to the initial combined height of the paper

4-991

Heat Transfer and Thermal-Stress Analyses

foam and the silicone bead, 0.866 mm. The elements in the region of the gasket beneath the silicone bead are assigned different gasket properties from the rest of the elements in the gasket model. The paper foam region is initially not in contact with the cover. The initial gap is 0.076 mm. No pressure is generated in this portion of the gasket until the gap has closed. Gasket region property distinctions, such as initial gaps and different pressure versus closure relationships, are assigned to corresponding element sets by referring to different *GASKET SECTION options. Experimentally determined pressure versus closure curves for the two distinct gasket regions without the initial gap taken into account are shown in Figure 4.1.3-4. Tabular representations of these curves are specified using the *GASKET THICKNESS BEHAVIOR option that is associated with the respective *GASKET SECTION options. Creep/relaxation properties of the gasket and temperature-dependent pressure versus closure properties, capturing such effects as the glassy transition temperature of the silicone bead, are not accounted for in this example. Initially, ABAQUS considers the gasket behavior to be nonlinear elastic, such that loading and unloading occur along the same user-defined nonlinear path. ABAQUS considers yielding to occur once the slope of the pressure versus closure curve decreases by at least 10%. In addition to the single loading curve, whose closure increases monotonically, the user can define any number of unloading curves at different levels of plastic closure. Yielding occurs at a closure of 0.1118 mm for both regions of the gasket in this example, after which the gasket stiffness decreases slightly up to a closure of 0.15 mm, the final point on the loading curve. Beyond the data of the loading curve defined by the user, ABAQUS considers the gasket to behave with a fully crushed elastic response by linearly extrapolating the last segment of the last specified unloading curve (alternatively, the user could have specified a piecewise linear form). A single unloading curve is defined for each of the two gasket regions: the unloading curve for the silicone bead region is defined at 0.11 mm of plastic closure, and the unloading curve for the paper foam region is defined at 0.09 mm of plastic closure. Any unloading of the gasket beyond the yield point occurs along a curve interpolated between the two bounding unloading curves, which--for this example--are the initial, nonlinear elastic curve and the single unloading curve. Gasket materials often have higher coefficients of thermal expansion than most of the metals from which the bolts and flanges are made. For situations involving wide and rapid temperature fluctuations resultant differences in relative expansion and contraction can have a significant effect on the sealing properties of the gasket. The coefficient of thermal expansion for the silicone bead region is 1.2 ´ 10-4 per °C, and for the paper foam region it is 3.0 ´ 10-5 per °C. In this case, because of the differences in thermal expansion between the aluminum cover and the steel intake manifold, it is important to account for the membrane and transverse shear properties of the gasket and to model frictional effects between mating surfaces. For this analysis the silicone bead region of the gasket is defined to have a membrane stiffness of 75 MPa and a transverse shear stiffness of 40 MPa. The base foam material is defined with a value of 105 MPa for the membrane stiffness and a value of 55 MPa for the transverse shear stiffness. A friction coefficient of 0.2 is used between all mating surfaces. A separate analysis is included in this example problem using the "thickness-direction only" version of the gasket elements (GK3D8N and GK3D6N). These elements respond only in the thickness direction

4-992

Heat Transfer and Thermal-Stress Analyses

and have no membrane or transverse shear stiffness properties. They possess only one degree of freedom per node. As a result, frictional effects cannot be included at the surfaces of these elements. They are more economical than more general gasket elements that include membrane and transverse shear responses and may, thus, be preferable in models where lateral response can be considered negligible.

Loading and boundary constraints Symmetry boundary constraints are placed along the nodes on the symmetry plane. Furthermore, it is assumed that the intake manifold is a stiff and bulky component, so nodes along the base of the portion of the manifold modeled are secured in the normal direction (the global z-direction). Except for a soft spring constraint to eliminate rigid body motion, these manifold base nodes are free to displace laterally to allow for thermal expansion. Soft springs are also attached to the cover to eliminate rigid body motion in the x- and z-directions. The bottoms of the bolt heads form contact bearing surfaces with the top surface of the cover flange. In addition, the top of the gasket interacts with the bottom of the cover, while the bottom of the gasket contacts the top of the manifold. Each of these surfaces is defined with the *SURFACE option. Mating surfaces are paired together with the *CONTACT PAIR option. Three-dimensional, deformable-to-deformable, small-sliding contact conditions apply to each of these contact pairs. The gasket is attached to the manifold base using the *SURFACE BEHAVIOR, NO SEPARATION option, thus constraining it against rigid body motion in the global z-direction. The gasket membrane is allowed to stretch, contract, or shear as a result of frictional effects on both sides of the gasket. The bolts are assumed to be threaded tightly into the base. Therefore, the nodes at the bottom of the bolt shanks are shared with the intake manifold. Contact between the bolt shanks and the bolt holes is not modeled. The "prescribed assembly load" capability is used to define pre-tension loads in each of the bolts. For each of the two bolts we define a "cut" or pre-tension section and subject the section to a specified load. As a result, the length of the bolt at the pre-tension section changes by the amount necessary to carry the prescribed load, while accounting for the compliance of the rest of the joint. Once a bolt has been pre-tensioned, the applied concentrated bolt load is replaced with a "fixed" boundary condition, which specifies that the length change of the bolt at the "cut" remains fixed, while the remainder of the bolt is free to deform. Then, during further external loading of the assembly the total force across each pre-tension section (the load on the bolt) can be monitored as the reaction force required to hold the resultant length change of the pre-tension section constant. The sequence in which the bolts are tightened can have an impact on the distribution of the resultant contact area stress. A poorly specified bolt sequence can cause excessive distortion of the gasket and the flanges, which may lead to poor sealing performance. In the first step of the analysis the left bolt is pre-tensioned to a load of 6000 N using the *PRE-TENSION SECTION option. In the second step the right bolt is pre-tensioned to 6000 N. An interim step, referred to as Step 1a, is used to replace the prescribed load on the left bolt with a fixed boundary condition as described above. Since only half of each bolt is modeled, a total load of 12000 N is carried by each bolt. Following Step 2 another interim step, referred to as Step 2a, replaces the prescribed load on the pre-tension section of the right bolt with a fixed boundary condition.

4-993

Heat Transfer and Thermal-Stress Analyses

Step 3 is the beginning of the three-step thermo-mechanical operational cycle. In Step 3 the entire assembly is heated uniformly to its maximum operating temperature of 150°C, while simultaneously pressurizing the interior cavity to 0.689 MPa. In Step 4 the system temperature is decreased to the minimum operating temperature of -40°C while maintaining the interior pressure load of 0.689 MPa. In Step 5 the gasketed joint is returned to the ambient temperature conditions and the internal cavity pressure is removed. The sixth and final step in the analysis simulates disassembly of the gasketed joint by removing the bolt loads. This process demonstrates the interpolated unloading response for the different regions of the permanently deformed gasket.

Results and discussion The prime interest in this problem is the variation of bolt forces during the initial assembly and thermo-mechanical cycle and the resultant distribution and variation of the gasket sealing pressure. The function of the fasteners in a gasketed joint is to apply and maintain the load required to seal the joint. The bolt pattern and tension are directly related to the sealing pressure in the clamped gasket. At the maximum service temperature the bolt loads can be expected to be at their peak as a result of thermal expansion effects. It is important to ensure that the stress values of the metal engine components remain below yield and that there is no significant bending of the flanges, which may cause improper sealing of the gasket. At the minimum operating temperature the bolt loads are expected to reach a minimum as a result of thermal contraction effects. Hence, it is necessary to assess that adequate sealing pressure is retained throughout the gasket. Figure 4.1.3-5 shows the bolt load variation over the course of the six analysis steps. During the first step the pre-tension section node on the right bolt was prescribed a zero change of length constraint, which implies that the right bolt has just been placed in position but not torqued tightly. Hence, as the left bolt is tightened during Step 1, a small reaction load is generated in the right bolt. At the end of the second step during which the right bolt is tightened to carry a force of 6000 N, the force in the left bolt increases to 6200 N. In Step 3 the deformation of the assembly causes the bolt forces to increase to maximum values of 6800 N in the left bolt and 6600 N in the right bolt because of thermal expansion and interior pressurization. When the assembly is cooled to the minimum operating temperature, the bolt loads reach their minimum values. Due to thermal cycling and interior cavity pressure inducing inelastic response in the gasket, the bolt forces at the end of the operational cycle reduce to 6050 N in the left bolt and 5950 N in the right bolt. The gasket sealing pressure pattern depends on the rigidity of the flanges. Hence, it is useful to predict how the structure will deform due to the applied loading. Figure 4.1.3-6 shows the deformed shape of the coolant manifold cover at a displacement magnification factor of 50. Bowing of the cover from initial assembly and subsequent operational loads will lead to a nonuniform sealing pressure distribution in the gasket. Figure 4.1.3-7illustrates the gasket pressure distribution after initial fastening of the joint. Figure 4.1.3-8 shows the sealing pressure as a function of position along the perimeter of the silicone bead at the end of each of the analysis steps. The sealing pressure reaches a minimum at the point

4-994

Heat Transfer and Thermal-Stress Analyses

equidistant from the bolts, making this the critical point in the gasketed joint design. This figure also reflects the reduction in the sealing pressure near the bolt holes as a result of plastic deformation of the gasket body during the operational cycle. Figure 4.1.3-9 is a contour plot of the permanent deformation in the gasket after completion of the thermo-mechanical cycle. Figure 4.1.3-10 follows the pressure/closure history of one point in the gasket during this analysis in relation to the user-specified loading/unloading test data. The "mechanical closure" (total closure, E11, minus thermal closure, THE11) is plotted along the abscissa of this figure. The material point traced (element 18451, integration point 1) is located along the inside periphery of the silicone bead at the symmetry plane of the assembly nearest the left bolt. Step 1 shows that this point follows the initial elastic loading curve up to the closure of 0.1118 mm. After this amount of closure, further loading causes plastic deformation. In the second step the tightening of the bolt results in a very small amount of unloading for this material point. For purposes of clarity, this deformation is not shown in the figure. Step 3 involves heating the system to the maximum operating temperature and pressurizing the interior cavity so that further yielding of the material point occurs. Step 4 results in the partial unloading of the point due to the thermal contraction associated with cooling the assembly to the minimum operating temperature. For this case the unloading path is based on a curve interpolated between the initial, nonlinear elastic curve and the single unloading curve. The return of the assembly to ambient conditions partially reloads this point along the same path as the previous unloading; however, no further yielding of this material point occurs during this step. In the final step the gasket is unloaded completely. The analysis using the "thickness-direction only" gasket elements runs in nearly half the CPU time of the full three-dimensional gasket element model. Minimum gasket sealing pressures in Step 4 of this analysis are predicted to be about 20% lower because frictional effects are neglected.

Input files manifoldgasket.inp Input data for the analysis. manifoldgasket_mesh.inp Node, element, and surface definitions. manifoldgasket_thick.inp "Thickness-direction only" gasket element analysis. manifoldgasket_thick_mesh.inp Node, element, and surface definitions for the "thickness-direction only" gasket element analysis.

Reference · Czernik, D. E., Gasket Handbook, McGraw-Hill, New York, 1996.

Figures

4-995

Heat Transfer and Thermal-Stress Analyses

Figure 4.1.3-1 Coolant manifold assemblage.

Figure 4.1.3-2 Schematic representation of a silicone bead printed on the gasket body.

4-996

Heat Transfer and Thermal-Stress Analyses

Figure 4.1.3-3 Mesh of gasket with silicone bead highlighted.

Figure 4.1.3-4 Pressure versus closure behavior for the gasket and the gasket with silicone bead.

Figure 4.1.3-5 History of bolt force.

4-997

Heat Transfer and Thermal-Stress Analyses

Figure 4.1.3-6 Deformed shape of coolant manifold cover at a displacement magnification factor of 50.

Figure 4.1.3-7 Gasket pressure distribution after initial fastening sequence.

Figure 4.1.3-8 Sealing pressure along inside periphery of silicone bead region of gasket.

4-998

Heat Transfer and Thermal-Stress Analyses

Figure 4.1.3-9 Plastic closure in gasket after operational cycle.

Figure 4.1.3-10 Typical pressure-closure diagram for material point in silicone bead region of gasket.

Sample listings

4-999

Heat Transfer and Thermal-Stress Analyses

Listing 4.1.3-1 *HEADING BOLT DOWN AND OPERATIONAL CYCLE OF COOLANT MANIFOLD COVER Units: N-mm-sec-deg C ** *RESTART,WRITE,FREQ=999 ** ** read nodes, elements, and surfaces ** from external file ** 4639 nodes in nset NALL ** 1304 C3D8I elements ** 208 C3D6 elements ** 973 GK3D8 elements ** 29 GK3D6 elements ** create element sets: COVER1,COVER2,BASE1,BASE2, ** BOLT1,MATL1,BEAD1,COVER, ** BASE,COVERF1,COVERF2, ** COVERF3,COVERF4,COVERF5, ** COVERF6,BASEF1,BASEF3, ** BASEF4,BASEF5,BASEF6 ** create node sets: NALL,BASE_BOT ** create surfaces: SCOVER2,SBOLTL,SBOLTR,SCOV1L, ** SCOV1R,SGTOP,SGBOT,SBASE1 ** *INCLUDE,INPUT=manifoldgasket_mesh.inp ** ***** *GASKET SECTION, ELSET=BEAD1, BEHAVIOR=GBEAD1 *GASKET BEHAVIOR,NAME=GBEAD1 *GASKET ELASTICITY,COMPONENT=MEMBRANE 75., *GASKET ELASTICITY,COMPONENT=TRANSVERSE SHEAR 40.0, *GASKET THICKNESS BEHAVIOR,TYPE=ELASTIC-PLASTIC, DIRECTION=LOADING 0.0 ,0.0 3.27 ,0.0254 8.40 ,0.0508 18.52,0.0762 34.26,0.1016 41.69,0.1118

4-1000

Heat Transfer and Thermal-Stress Analyses

45.50,0.13 47.80,0.15 *GASKET THICKNESS BEHAVIOR,TYPE=ELASTIC-PLASTIC, DIRECTION=UNLOADING 0.0,0.11,0.11 10.0,0.13,0.11 20.0,0.14,0.11 30.0,0.145,0.11 40.0,0.1475,0.11 47.8,0.15,0.11 *EXPANSION 1.2E-4, *GASKET SECTION, ELSET=MATL1, BEHAVIOR=GMATL1 ,0.076 *GASKET BEHAVIOR,NAME=GMATL1 *GASKET ELASTICITY,COMPONENT=MEMBRANE 105., *GASKET ELASTICITY,COMPONENT=TRANSVERSE SHEAR 55., *GASKET THICKNESS BEHAVIOR,TYPE=ELASTIC-PLASTIC, DIRECTION=LOADING 0.0 ,0.0 4.83 ,0.0254 11.72,0.0508 25.17,0.0762 43.09,0.1016 52.75,0.1118 57.02,0.13 58.85,0.15 *GASKET THICKNESS BEHAVIOR,TYPE=ELASTIC-PLASTIC, DIRECTION=UNLOADING 0.0,0.09,0.09 10.0,0.108,0.09 20.0,0.122,0.09 30.0,0.131,0.09 40.0,0.142,0.09 50.0,0.147,0.09 58.85,0.15,0.09 *EXPANSION 3.E-5, ***** *SOLID SECTION, ELSET=COVER, MATERIAL=ALUM *SOLID SECTION, ELSET=BASE, MATERIAL=STEEL

4-1001

Heat Transfer and Thermal-Stress Analyses

*SOLID SECTION, ELSET=BOLT1, MATERIAL=STEEL ***** *MATERIAL, NAME=STEEL *ELASTIC 200000.,.28 *EXPANSION 1.6E-5, ***** *MATERIAL, NAME=ALUM *ELASTIC 71000.,.33 *EXPANSION 2.3E-5, ***** ** ** INITIAL TEMPERATURE -- 20 DEGREES CELSIUS ** *INITIAL CONDITIONS, TYPE=TEMPERATURE NALL,20.0 ** ** ** CONTACT DEFINITIONS ** *CONTACT PAIR,INTERACTION=IBOLT,SMALL SLIDING, ADJUST=.01 SBOLTL,SCOV1L SBOLTR,SCOV1R *CONTACT PAIR,INTERACTION=ITOP,SMALL SLIDING, ADJUST=.01 SGTOP,SCOVER2 *CONTACT PAIR,INTERACTION=IBOT,SMALL SLIDING, ADJUST=.01 SGBOT,SBASE1 *SURFACE INTERACTION,NAME=IBOLT *FRICTION 0.20, *SURFACE INTERACTION,NAME=ITOP *FRICTION 0.20, *SURFACE INTERACTION,NAME=IBOT *SURFACE BEHAVIOR,NO SEPARATION *FRICTION 0.20,

4-1002

Heat Transfer and Thermal-Stress Analyses

** ** PRE-TENSION SECTION DEFINITIONS ** *ELSET,ELSET=RCUT 3701,3702,3703,3708 *ELSET,ELSET=LCUT 3709,3710,3711,3716 *SURFACE,NAME=PREBOLTL LCUT, S1 *SURFACE,NAME=PREBOLTR RCUT, S1 *PRE-TENSION SECTION,SURFACE=PREBOLTL,NODE=1000001 *PRE-TENSION SECTION,SURFACE=PREBOLTR,NODE=1000002 ** ** SOFT SPRINGS ON COVER, BASE AND GASKET ** TO ELIMINATE RIGID BODY MOTION ** - Nodes 643 and 2012 are located on COVER ** - Nodes 5560 and 5689 are located on BASE ** - Nodes 15827 and 15737 are located on GASKET ** *ELEMENT,TYPE=SPRING1,ELSET=SP1 999001,643 999002,2012 999003,5560 999004,5689 999005,15827 999006,15737 *ELEMENT,TYPE=SPRING1,ELSET=SP3 999007,643 999008,2012 *SPRING,ELSET=SP1 1, 1., *SPRING,ELSET=SP3 3, 1., ** ** DISPLACEMENT BOUNDARY CONDITIONS ** *BOUNDARY BASE_BOT,3 YSYMM,2 **

4-1003

Heat Transfer and Thermal-Stress Analyses

** NODE SETS FOR OUTPUT ** *NSET,NSET=REFNODE 1000001,1000002 ***************************************** ** ** STEP 1 -- PRE-TENSION LEFT BOLT ** *STEP,INC=20 *STATIC 0.01,1.0 *CLOAD 1000001,1,6000. *BOUNDARY 1000002,1,,0.0 ** *MONITOR,NODE=15737,DOF=3 *NODE FILE,NSET=REFNODE,FREQ=1 U,RF,CF *EL FILE,ELSET=IBEAD,FREQ=1 S,E,THE *FILE FORMAT,ZERO INCREMENT *EL PRINT,FREQ=0 *NODE PRINT,FREQ=0 *END STEP ** ** STEP 1A -- SUBSTITUTE LEFT BOLT LOAD ** WITH RESULTANT LENGTH CHANGE ** *STEP,INC=1 *STATIC 1.E-10,1.0E-10,1.0E-10,1.0E-10 *BOUNDARY,FIXED 1000001,1 *CLOAD,OP=NEW *ENDSTEP ** ** STEP 2 -- PRE-TENSION RIGHT BOLT ** *STEP,INC=20 *STATIC 0.01,1.0 *CLOAD,OP=NEW

4-1004

Heat Transfer and Thermal-Stress Analyses

1000002,1,6000. *BOUNDARY,OP=NEW,FIXED 1000001,1 *BOUNDARY,OP=NEW BASE_BOT,3 YSYMM,2 *END STEP ** ** STEP 2A -- SUBSTITUTE RIGHT BOLT LOAD ** WITH RESULTANT LENGTH CHANGE ** *STEP,INC=1 *STATIC 1.E-10,1.0E-10,1.0E-10,1.0E-10 *BOUNDARY,FIXED 1000002,1 *CLOAD,OP=NEW *ENDSTEP ** ** STEP 3 -- INCREASE TEMPERATURE TO 150 ** DEGREES CELSIUS and PRESSURIZE ** INTERIOR CAVITY TO 0.6895 MPa ** *STEP,INC=20 *STATIC 0.125,1.0 *TEMPERATURE NALL,150. *DLOAD,OP=NEW coverf1,p1,0.6895 coverf2,p2,0.6895 coverf3,p3,0.6895 coverf4,p4,0.6895 coverf5,p5,0.6895 coverf6,p6,0.6895 basef1 ,p1,0.6895 basef3 ,p3,0.6895 basef4 ,p4,0.6895 basef5 ,p5,0.6895 basef6 ,p6,0.6895 *MONITOR,NODE=15737,DOF=1 *END STEP **

4-1005

Heat Transfer and Thermal-Stress Analyses

** STEP 4 -- DECREASE TEMPERATURE TO ** -40 DEGREES CELSIUS ** *STEP,INC=20 *STATIC 0.125,1.0 *TEMPERATURE NALL,-40.0 *END STEP ** ** STEP 5 -- INCREASE TEMPERATURE TO ** 20 DEGREES CELSIUS and ** REMOVE INTERNAL PRESSURE LOAD ** *STEP,INC=20 *STATIC 0.05,1.0 *TEMPERATURE NALL,20.0 *DLOAD,OP=NEW *END STEP ** ** STEP 6 -- UNLOAD THE GASKET ** *STEP,INC=20 *STATIC 0.125,1.0 *BOUNDARY,OP=NEW BASE_BOT,3 YSYMM,2 1000001,1,,0.005 1000002,1,,0.005 *END STEP

4.1.4 Radiation analysis of a plane finned surface Product: ABAQUS/Standard This example illustrates the ABAQUS capability to solve heat transfer problems including cavity radiation. We simulate the effects of a fire condition on a plane finned surface. This problem was proposed by Glass et al. (1989) as a benchmark for thermal radiation. We compare their results with those obtained using ABAQUS. The configuration shown in Figure 4.1.4-1 represents a plane wall with a uniform array of parallel rectangular fins attached. The problem represents three phases in a fire test. The first is the pretest, a

4-1006

Heat Transfer and Thermal-Stress Analyses

steady-state condition where heat is transferred by natural convection from an internal fluid at a fixed temperature of 100°C to the plane inside wall. Heat is conducted through the wall and dissipated by radiation and natural convection from the outside wall and fin surfaces to the surrounding medium which is at a temperature of 38°C. The second phase is a 30-minute fire transient, where heat is supplied by radiation and forced convection from a hot external fluid at 800°C. After conduction through the fins and wall, heat is rejected by natural convection to the internal fluid. Finally, the third phase is a 60-minute cool down period, where heat absorbed during the fire transient is rejected to the surroundings by the same process as that used to establish the initial steady-state condition.

Geometry and model The finite element mesh used for the wall and fins is shown in Figure 4.1.4-2. By making use of the radiation periodic symmetry capability in ABAQUS, we are able to represent the array of fins while meshing only one fin and corresponding wall section. The outside ambient is modeled with a single horizontal row of elements at some distance above the top of the fin (not shown in the figure). The varying ambient temperature is simulated by prescribing temperatures to the nodes of these elements. The elements representing the outside ambient are also assigned a surface emissivity of 1.0.

Material and boundary conditions The thermal conductivity of the wall and fins is 50 W/m°C (k), their specific heat is 500 J/kg°C (c), and the density is 7800 kg/m 3 (½). The surface emissivity of the wall and fins is 0.8, the Stefan-Boltzmann radiation constant is 5.6697 ´ 10-8 W/m2°K4, and the temperature of absolute zero is -273°C. The natural convection between the internal fluid and the inside of the wall is modeled with a film boundary condition where the film coefficient is given as 500( µw ¡ µf )1/3 W/m2°C, where µw is the inside wall temperature and µf is the temperature of the internal fluid. The film boundary condition user subroutine is used for this purpose since the film condition is temperature dependent. The natural convection between the outside finned surface and its surroundings is modeled with a film boundary condition where the film coefficient is given as 2(µs ¡ µa )1/3 W/m2°C, where µs is the temperature of the finned surface and µa is the outside ambient temperature. Again, the film boundary condition user subroutine is employed. The forced convection between the hot surroundings and the finned surface is modeled with a constant film coefficient of 10 W/m 2°C.

Loading The first simulation step is a steady-state heat transfer analysis to establish the initial pretest conditions. This is followed by a 30-minute transient heat transfer analysis during which time the ambient fire temperature is 800°C. Finally, a second transient heat transfer step is performed to simulate the 60-minute cool down period. The integration procedure used in ABAQUS for transient heat transfer analysis procedures introduces a relationship between the minimum usable time increment and the element size and material properties. The guideline given in the User's Manual is 4-1007

Heat Transfer and Thermal-Stress Analyses

¢t >

½c 2 ¢l ; 6k

where ¢l is the element size. This suggests that an initial time increment of 10 seconds is appropriate for the transient steps of this problem. Automatic time incrementation is chosen for the transient steps by setting DELTMX to 100°C. DELTMX controls the time integration by limiting the temperature change allowed at any point during an increment. A DELTMX of 100°C may seem rather coarse in comparison with temperature ranges of 800°C, but this is not expected to be the limiting factor; the strong nonlinearity of the radiation conditions is expected to dictate the time incrementation in the transient steps.

Results and discussion The results published by Glass et al. include those obtained by a number of different heat transfer codes, all of which give similar results. Since the most details are given for the results obtained with the program TAU (Johnson, 1987), we have chosen to compare the ABAQUS results to those of TAU. Figure 4.1.4-3 shows the history of the temperature at the top of the fin (point 1 in Figure 4.1.4-1). Figure 4.1.4-4 shows the histories of the temperature at the root of the fin (point 2 in Figure 4.1.4-1) and on the wall inside surface (point 3). In all cases the results obtained with ABAQUS match the TAU results quite well. In Figure 4.1.4-5 we show the temperature distribution around the fin perimeter (starting at point 1 and ending at point 2) at the end of the fire transient. Again, the ABAQUS and TAU results match closely. Finally, temperature contours at the end of the fire transient are shown in Figure 4.1.4-6.

Input file radiationfinnedsurf.inp Fire transient problem. radiationfinnedsurf.f User subroutine FILM used in radiationfinnedsurf.inp.

References · Glass, R. E., et al., "Standard Thermal Problem Set," Proceedings of the Ninth International Symposium on the Packaging of Radioactive Materials, pp. 275-282, June 1989. · Johnson, D., "Surface to Surface Radiation in the Program TAU, Taking Account of Multiple Reflection," United Kingdom Atomic Energy Authority Report ND-R-1444(R), 1987.

Figures Figure 4.1.4-1 Plane finned surface.

4-1008

Heat Transfer and Thermal-Stress Analyses

Figure 4.1.4-2 Finite element mesh of fin and inner wall.

Figure 4.1.4-3 Temperature history at top of fin.

4-1009

Heat Transfer and Thermal-Stress Analyses

Figure 4.1.4-4 Temperature history at root of fin and inside wall surface.

Figure 4.1.4-5 Temperature distribution along fin perimeter at end of fire transient.

4-1010

Heat Transfer and Thermal-Stress Analyses

Figure 4.1.4-6 Temperature contours at end of fire transient.

Sample listings

4-1011

Heat Transfer and Thermal-Stress Analyses

Listing 4.1.4-1 *HEADING PLANE FINNED SURFACE UNDER FIRE CONDITION ** ** FIN... *NODE 1, 5, 0.025D0 7, 0.035D0 11, 0.06D0 1001, 0.D0,0.1D0 1005,0.025D0,0.1D0 1007,0.035D0,0.1D0 1011,0.060D0,0.1D0 3001, 0D0,0.25D0 3005,0.025D0,0.25D0 3007,0.035D0,0.25D0 3011,0.060D0,0.25D0 *NGEN,NSET=N1 1,5 5,7 7,11 *NGEN,NSET=N2 1001,1005 1005,1007 1007,1011 *NGEN,NSET=N3 3001,3005 3005,3007 3007,3011 *NFILL,NSET=NALL N1,N2,10,100 N2,N3,20,100 *ELEMENT,TYPE=DC2D4 1,1,2,102,101 5000,1005,1006,1106,1105 *ELGEN,ELSET=STRUC 1,10,1,1,10,100,10 5000,2,1,1,20,100,2 ** ** AMBIENT... *NODE

4-1012

Heat Transfer and Thermal-Stress Analyses

5001, 0D0,0.550D0 5011,0.06D0,0.550D0 5101, 0D0,0.555D0 5111,0.06D0,0.555D0 *NGEN,NSET=NAMB 5001,5011 5101,5111 *ELEMENT,TYPE=DC2D4 8000,5001,5002,5102,5101 *ELGEN,ELSET=STRUC 8000,10,1,1 *ELSET,ELSET=EAMB,GENERATE 8000,8009 ** ** SURFACES... *ELSET,ELSET=BOTF1,GENERATE 1,10 *ELSET,ELSET=TOPF3,GENERATE 91,94 97,100 5038,5039 *ELSET,ELSET=TOPF4,GENERATE 5000,5038,2 *ELSET,ELSET=TOPF2,GENERATE 5001,5039,2 *surface,NAME=SRFS,PROPERTY=REFL TOPF3,S3 TOPF4,S4 TOPF2,S2 *surface,NAME=SAMB,PROPERTY=RAMB EAMB,S1 *SURFACE PROPERTY,NAME=REFL *EMISSIVITY 0.8D0, *SURFACE PROPERTY,NAME=RAMB *EMISSIVITY 1.0D0, *CAVITY DEFINITION,NAME=CAV2D SRFS,SAMB ** *SOLID SECTION,ELSET=STRUC,MATERIAL=MSTRUC *MATERIAL,NAME=MSTRUC *DENSITY

4-1013

Heat Transfer and Thermal-Stress Analyses

7800.0D0, *CONDUCTIVITY 50.0D0, *SPECIFIC HEAT 500.0D0, *RESTART,WRITE,FREQUENCY=100 *PHYSICAL CONSTANTS,STEFANBOLTZMANN=5.6697D-8, ABSOLUTE ZERO=-273.0 ** *INITIAL CONDITIONS,TYPE=TEMPERATURE NALL,77.D0 NAMB,77.D0 *NSET,NSET=THREE 11,1011,3006 ** ** *surface, NAME=BOTF1 BOTF1, S1 *STEP,INC=500 *HEAT TRANSFER,STEADY STATE 1.0, *BOUNDARY NAMB,11,,38.D0 *SFILM BOTF1,FNU *SFILM SRFS,FNU *RADIATION VIEWFACTOR,SYMMETRY=NSYMM *RADIATION SYMMETRY,NAME=NSYMM *PERIODIC,TYPE=2D,NR=20 0.0D0,0.555D0, 0.0D0,0.0D0, 0.06D0,0.0D0 *VIEWFACTOR OUTPUT, CAVITY=CAV2D, FREQUENCY=100 *RADIATION PRINT,CAVITY=CAV2D, FREQUENCY=10 RADFL,RADFLA,RADTL,RADTLA,VFTOT,FTEMP *RADIATION FILE,CAVITY=CAV2D, FREQUENCY=10 RADFL,RADFLA,RADTL,RADTLA,VFTOT,FTEMP *EL PRINT,FREQUENCY=0 *NODE PRINT,NSET=THREE NT, *NODE FILE,NSET=THREE NT, *END STEP *STEP,INC=500

4-1014

Heat Transfer and Thermal-Stress Analyses

*HEAT TRANSFER,DELTMX=100 10,1800 *BOUNDARY NAMB,11,,800.D0 *END STEP *STEP,INC=500 *HEAT TRANSFER,DELTMX=100 10,3600 *BOUNDARY NAMB,11,,38.D0 *END STEP

4-1015

Electrical Analyses

5. Electrical Analyses 5.1 Piezoelectric analyses 5.1.1 Eigenvalue analysis of a piezoelectric transducer Product: ABAQUS/Standard This problem performs an eigenspectrum analysis of a cylindrical transducer consisting of a piezoelectric material with brass end caps. Various elements are used in the analysis. The elements range from axisymmetric elements to three-dimensional elements, using both lower- and higher-order elements. The basis of the piezoelectric capability in ABAQUS is described in ``Piezoelectric analysis,'' Section 2.10.1 of the ABAQUS Theory Manual.

Geometry and material This problem is identical to the one discussed in a report by Mercer et al. (1987). The structure is shown in Figure 5.1.1-1and consists of a piezoelectric material PZT4 with brass end caps. The piezoelectric material is electroded on both the inner and outer surfaces. The properties for PZT4 in a cylindrical system are: Elasticity Matrix: 2

115:4 6 74:28 6 6 74:28 6 6 0 4 0 0

74:28 139:0 77:84 0 0 0

74:28 77:84 139:0 0 0 0

0 0 0 25:64 0 0

0 0 0 0 25:64 0

3 0 0 7 7 0 7 7 0 7 5 0 25:64

GPa

Piezoelectric Coupling Matrix (Stress Coefficients): 2

15:08 6 ¡5:207 6 6 ¡5:207 6 6 0 4 0 0

0 0 0 12:710 0 0

3 0 0 7 7 0 7 7 0 7 5 12:710 0

Coulomb/m2

Dielectric Matrix: 2

5:872 4 0 0

0 6:752 0

3 0 0 5 10¡9 6:752

farad/m

The 1-direction is radial, the 2-direction is axial, and the 3-direction is tangential. From these matrices

5-1016

Electrical Analyses

it is seen that the poling direction is radially outwards from the axis of symmetry. (The order of the stresses in ABAQUS may differ from those typically used in electrical applications. ABAQUS uses the standard mechanical convention, where the stress components are ordered as f¾11 ¾22 ¾33 ¿12 ¿13 ¿23 g. See ``Piezoelectric behavior,'' Section 12.6.2 of the ABAQUS/Standard User's Manual.) The brass is elastic and isotropic with a Young's modulus of 104 GPa and a Poisson's ratio of 0.37.

Models The transducer is modeled with a variety of elements. It is modeled as an axisymmetric structure utilizing both the planar, axisymmetric elements and the three-dimensional elements. For the axisymmetric elements, five meshes employing 4-node, 6-node, and 8-node elements are used in the finite element discretization. The first two meshes use 4-node elements with two levels of refinement, the third mesh uses 6-node elements, and the last two meshes use the 8-node elements with two levels of refinement. Lumped mass matrices are used for the lower-order elements. Consistent mass matrices are used in the higher-order elements. The meshes used for the 4-node and 6-node axisymmetric elements are shown in Figure 5.1.1-2. The meshes used for the 8-node axisymmetric elements are shown in Figure 5.1.1-3. The three-dimensional model uses a slice of the structure and applies axisymmetric boundary conditions; 8-node and 20-node brick elements are used. The discretization used for each model is shown in Figure 5.1.1-3. These models use the *ORIENTATION option to maintain the proper definitions of the material properties. Also, in order to prescribe the axisymmetric boundary conditions, the nodal degrees of freedom are transformed into a cylindrical coordinate system. All the models are considered to be open-circuited. The potentials on the inside surface are restrained to zero. The frequencies correspond to those for anti-resonance.

Results and discussion The solutions obtained with the various ABAQUS models are shown in Table 5.1.1-1. Even for these coarse models, the results are quite close to the experimental results. In addition, the results from ABAQUS for the lower-order axisymmetric elements with lumped mass and the higher-order axisymmetric elements with consistent mass matrices in the computation of both the resonant and antiresonant frequencies match well with the numerical results reported in Mercer et al. The first four mode shapes for the more refined model with CAX8RE elements are shown in Figure 5.1.1-4. Similar analyses have been performed considering the problem to be closed-circuited to obtain the resonant frequencies. For this situation, the potentials on both the inner and outer surfaces are set to zero. The results also compare well with those given in Mercer et al.

Input files eigenpiezotrans_cax4e_coarse.inp Coarse mesh with 4-node axisymmetric elements. eigenpiezotrans_cax4e_fine.inp

5-1017

Electrical Analyses

Refined mesh with 4-node axisymmetric elements. eigenpiezotrans_cax6e.inp Mesh with 6-node axisymmetric elements. eigenpiezotrans_cax8re_coarse.inp Coarse mesh with 8-node axisymmetric elements. eigenpiezotrans_cax8re_fine.inp Refined mesh with 8-node axisymmetric elements. eigenpiezotrans_c3d8e.inp Mesh with 8-node three-dimensional elements. eigenpiezotrans_c3d8e.f User subroutine ORIENT used in eigenpiezotrans_c3d8e.inp. eigenpiezotrans_c3d20e.inp Mesh with 20-node three-dimensional elements. eigenpiezotrans_c3d20e.f User subroutine ORIENT used in eigenpiezotrans_c3d20e.f. eigenpiezotrans_elmatrixout.inp Data that test the use of *ELEMENT MATRIX OUTPUT with piezoelectric elements. eigenpiezotrans_usr_element.inp Data for a job that reads in the matrices output in eigenpiezotrans_elmatrixout.inp and performs an eigenvalue analysis.

Reference · Mercer, C. D., B. D. Reddy, and R. A. Eve, "Finite Element Method for Piezoelectric Media," University of Cape Town/CSIR Applied Mechanics Research Unit Technical Report No. 92, April 1987.

Table Table 5.1.1-1 Piezoelectric transducer eigenvalue estimates. Model Frequencies (kHz) for mode number Type # of Elements 1 2 3 4 5 CAX4E 13 14.1 39.1 56.2 66.1 79.3 CAX4E 320 18.6 40.3 57.8 64.2 88.1 CAX6E 10 20.0 43.2 63.2 70.4 98.8 CAX8RE 5 19.6 42.8 61.0 66.9 96.3

5-1018

Electrical Analyses

CAX8RE 80 18.6 40.3 57.6 64.2 C3D8E 16 19.8 41.8 62.0 68.7 C3D20E 16 19.7 42.9 60.4 66.5 18.6 35.4 54.2 63.3 Experimental(1) (1): Experimental results obtained from Mercer et al. (1987).

87.6 95.2 91.7 88.8

Figures Figure 5.1.1-1 Piezoelectric transducer.

Figure 5.1.1-2 Meshes used with 4-node and 6-node axisymmetric elements.

5-1019

Electrical Analyses

Figure 5.1.1-3 Meshes used with 8-node axisymmetric and 8-node and 20-node three-dimensional elements.

5-1020

Electrical Analyses

Figure 5.1.1-4 Mode shapes for 8-node axisymmetric elements.

Sample listings

5-1021

Electrical Analyses

Listing 5.1.1-1 *HEADING EIGENVALUE ANALYSIS OF CYLINDRICAL TRANSDUCER PIEZOELECTRIC CERAMIC AND BRASS END CAPS, COARSE MODEL WITH FOUR-NODE AXISYMMETRIC PIEZOELECTRIC ELEMENTS *NODE 1, .0110,.0 2, .01175, 0.0 3, .0125, 0.0 13, .0110, .0125 14, .01175,.0125 15, .0125,.0125 16, .0110, .0155 17, .01175,.0155 18, .0125,.0155 19, 0.0,.0125 21,.0073333,.0125 22, 0.0,.0155 24,.0073333,.0155 *NGEN 1,13,3 2,14,3 3,15,3 19,21 22,24 *ELEMENT,TYPE=CAX4E 1, 1,2,5,4 *ELEMENT,TYPE=CAX4,ELSET=BRASS 9, 13,14,17,16 10, 14,15,18,17 11, 19,20,23,22 12, 20,21,24,23 13, 21,13,16,24 *ELGEN,ELSET=PZT4 1,2,1,1,4,3,2 **local orientation matching global system *ORIENTATION,NAME=RECT 1.0, 0.0, 0.0, 0.0, 1.0, 0.0 1, 0.0 *SOLID SECTION,MATERIAL=PZT4,ELSET=PZT4,ORIENT=RECT *SOLID SECTION,MATERIAL=BRASS,ELSET=BRASS *MATERIAL,NAME=PZT4

5-1022

Electrical Analyses

*ELASTIC,TYPE=ORTHOTROPIC 11.54E10,7.428E10,13.90E10,7.428E10,7.784E10,13.90E10,2.564E10,2.564E10 2.564E10, *PIEZOELECTRIC,TYPE=S 15.08,-5.207,-5.207,0.,0.,0.,0.,0. 0.,12.710,0.,0.,0.,0.,0.,0., 12.710,0. *DIELECTRIC,TYPE=ANISO 5.872E-9,0.,6.752E-9,0.,0.,6.752E-9 *DENSITY 7500., *MATERIAL,NAME=BRASS *ELASTIC,TYPE=ISOTROPIC 10.4E10,0.37 *DENSITY 8500., *NSET,NSET=IN,GENERATE 1,13,3 *NSET,NSET=SYM 1,2,3 *NSET,NSET=ASYM 19,22 *BOUNDARY SYM,2 ASYM,1 IN,9 *RESTART,WRITE ** *STEP,PERTURBATION *FREQUENCY 5,100000.,10. *EL PRINT S,E EFLX,EPG *NODE PRINT U,EPOT RF,RCHG *ELSET,ELSET=OUTPUT 1,9 *EL FILE,ELSET=OUTPUT S,E,EFLX,EPG *NSET,NSET=OUTPUT1 5,8

5-1023

Electrical Analyses

*NODE FILE,NSET=OUTPUT1 U,EPOT *NSET,NSET=OUTPUT2 1,19 *NODE FILE,NSET=OUTPUT2 RF,RCHG *OUTPUT,FIELD *ELEMENT OUTPUT,ELSET=OUTPUT S,E,EFLX,EPG *OUTPUT,FIELD *NODE OUTPUT U, *NODE OUTPUT,NSET=OUTPUT1 EPOT, *OUTPUT,FIELD *NODE OUTPUT,NSET=OUTPUT2 RF,RCHG *END STEP

5.2 Joule heating analyses 5.2.1 Thermal-electrical modeling of an automotive fuse Product: ABAQUS/Standard Joule heating arises when the energy dissipated by electrical current flowing through a conductor is converted into thermal energy. ABAQUS provides a fully coupled thermal-electrical procedure for analyzing this type of problem. An overview of the capability is provided in ``Coupled thermal-electrical analysis,'' Section 6.6.2 of the ABAQUS/Standard User's Manual. This example illustrates the use of the capability to model the heating of an automotive electrical fuse due to a steady 30 A electrical current. Fuses are the primary circuit protection devices in automobiles. They are available in a range of different current ratings and are designed so that, when the operating current exceeds the design current for a period of time, heating due to electrical conduction causes the metal conductor to melt and--hence--the circuit to disconnect. A description of the original problem, as well as experimental measurements, can be found in Wang and Hilali (1995). The experimental data and some of the material properties were refined subsequent to this publication. These properties are used here, and the finite element results are compared with the refined measurements (Hilali, July 1995).

Problem description An automotive electrical fuse consists of a metal conductor, such as zinc, embedded within a transparent plastic housing. The plastic housing, which only protects and supports the thin conductor,

5-1024

Electrical Analyses

is not represented in the finite element model. Figure 5.2.1-1 shows front and top sections of the geometry of the conductor. It consists of two 0.76 mm thick blades, with an S-shaped fuse element supported between the blades. The blades fit tightly into standard electrical terminals that are built into the circuit and provide the connection between the electrical circuit and the fuse element. The fuse element is usually much thinner than the fuse blades (in this case 0.28 mm thick) and is designed to melt when the operating current exceeds the design current for a period of time. The fuse blades are 8 mm wide and 30.4 mm long. The fuse element is approximately 3.6 mm wide. The model is discretized (see Figure 5.2.1-1) with 8-node first-order brick elements (element type DC3D8E), using one element through the thickness. Two 6-node triangular prism elements (element type DC3D6E) are used to fill regions where the geometry precludes the use of brick elements. No mesh convergence studies have been performed. The electrical conductivity of zinc varies linearly between 16.75 ´ 103 1=− mm at 20°C and 12.92 ´ 1031=− mm at 100°C. The thermal conductivity varies linearly between 0.1120 W/mm°C at 20°C and 0.1103 W/mm°C at 100°C. The density is 7.14 ´ 10-6 kg/mm3, and the specific heat is 388.9 J/kg°C. The *JOULE HEAT FRACTION option is used to specify the amount of electrical energy that is converted into thermal energy. We assume that all electrical energy is converted into thermal energy. The analysis is done in two steps. In the first step heating of the conductor due to current flow is considered. Once steady-state conditions are reached, the current is switched off and the fuse is allowed to cool down to the ambient temperature in a second step. During the first part of the analysis, the coupled thermal-electrical equations are solved for both temperature and electrical potential at the nodes using the *COUPLED THERMAL-ELECTRICAL procedure. In the subsequent cool down period, since there is no longer any electric current in the fuse, an uncoupled *HEAT TRANSFER analysis (``Uncoupled heat transfer analysis,'' Section 6.5.2 of the ABAQUS/Standard User's Manual) is performed. Input files illustrating both steady-state and transient analyses are provided. Steady-state analysis is obtained by specifying the STEADY STATE parameter on the *COUPLED THERMAL-ELECTRICAL procedure. No data lines are required. Transient analysis is available by omitting the STEADY STATE parameter. In this analysis the DELTMX parameter is set to 20°C so that automatic time incrementation is used. The END parameter is set to SS so that the analysis terminates when steady-state conditions are reached. Steady state is defined here as the point at which the temperature rate change is less than 0.1° C/s. This condition is defined on the data line following the *COUPLED THERMAL-ELECTRICAL option. We specify a total analysis time of 100 s, with an initial time step size of 0.1 s. The electrical loading is a steady 30 A current. This is applied as a concentrated current on each of the nodes on the bottom edge of the left-hand-side terminal. The *CECURRENT option is used for this purpose. The *SECTION FILE option is used to output the total current and the total heat flux in a section defined through the fuse element. The electrical potential (degree of freedom 9) is constrained at the bottom edge of the right-hand-side blade by using a *BOUNDARY option (``Boundary conditions,'' Section 19.3.1 of the ABAQUS/Standard User's Manual). This option is also used to keep the bottom edges of the fuse blades at sink temperatures (degree of freedom 11) of 29.4°C and 30.2°C, respectively. It is assumed that the exposed metal surfaces lose heat through convection to an ambient temperature

5-1025

Electrical Analyses

of µ0 = 23.3°C. Heat loss from the thin edges is ignored. The film coefficient varies with temperature according to the empirical relation h = h0 (µ ¡ µ0 )1=4 ; where µ is surface temperature (°C); h is the film coefficient (W/mm2°C); and h0 is a constant that depends on the surface geometry--h0 =4.747 ´ 10-6 W/mm2 for the blade surfaces, and h0 =5.756 ´ 10-6 W/mm2 for the fuse element surfaces. This dependence is entered as a table of film property values using the *FILM PROPERTY option and is referred to on the *FILM option (see ``Thermal loads,'' Section 19.4.3 of the ABAQUS/Standard User's Manual).

Results and discussion Figure 5.2.1-2 shows a contour plot of the magnitude of the electrical current density vector at steady-state conditions. Since the dissipated electrical energy--and, hence, the thermal energy--is a function of current density, this figure represents contours of the heat generated. The figure indicates that most of the heat is generated near the inside curves of the S-shaped fuse element and near the center hole. The dissipated energy in the fuse blades is negligible compared to that in the fuse element. Figure 5.2.1-3 shows a contour plot of the temperature distribution at the end of the first analysis step. The maximum temperature is reached near the center of the S-shaped fuse element. This area is expected to fail first when the operating current exceeds the design current. Figure 5.2.1-4 compares the temperatures at the measuring positions (defined in Figure 5.2.1-1) with the experimental measurements (Hilali, July 1995). While the results show some discrepancies between the experiment and analysis, it is clear that the analysis is sufficiently representative that it provides a useful basis for studying such systems. Figure 5.2.1-5 shows the variation of temperature at measuring position 6 during the heating and subsequent cool-down periods.

Acknowledgments Mr. Hilali and Dr. Wang of Delphi Packard Electric Systems supplied the geometry of the fuse, material properties, and experimental results. Delphi Packard assumes no responsibility for the accuracy of the analysis method or data contained in the analysis.

Input files thermelectautofuse_steadystate.inp Steady-state analysis. thermelectautofuse_transient.inp Transient analysis. thermelectautofuse_node.inp Nodal coordinates for the model.

5-1026

Electrical Analyses

thermelectautofuse_element.inp Element definitions. thermelectautofuse_controls.inp Identical to thermelectautofuse_steadystate.inp, except that it uses the *CONTROLS option for control of convergence criteria.

References · Hilali, S. Y., Private communication, July 1995. · Hilali, S. Y., and B.-J. Wang, "ABAQUS Thermal Modeling for Electrical Assemblies," 1995 ABAQUS Users' Conference, Paris, May 1995, pp. 441-457. · Wang, B.-J., and S. Y. Hilali, "Electrical-Thermal Modeling Using ABAQUS," 1995 ABAQUS Users' Conference, Paris, May 1995, pp. 771-785.

Figures Figure 5.2.1-1 Geometry and finite element discretization.

Figure 5.2.1-2 Contours of the magnitude of the current density vector (A/mm 2).

5-1027

Electrical Analyses

Figure 5.2.1-3 Contours of temperature field (°C).

Figure 5.2.1-4 Temperature (°C) at measuring positions.

5-1028

Electrical Analyses

Figure 5.2.1-5 Variation of temperature (°C) at measuring position 6 with time (s).

Sample listings

5-1029

Electrical Analyses

Listing 5.2.1-1 *HEADING HEATING OF AUTOMOTIVE ELECTRICAL FUSE STEADY STATE ANALYSIS Units: mm; deg. C; Joule; sec; kg; Ampere *RESTART,WRITE,FREQUENCY=100 ** *NODE, INPUT=thermelectautofuse_node.inp *NSET, NSET=NLHS 3, 6, 9, 12, 15, 18, 21, 24, 27, 30 *NSET, NSET=NRHS 420, 423, 426, 429, 432, 435, 438, 441, 444, 447 *NSET, NSET=NOUTP 30, 51, 83, 200, 319, 335, 360, 225, 604, 500, 468, 447 *ELEMENT, TYPE=DC3D8E, ELSET=EALL, INPUT=thermelectautofuse_element.inp *ELEMENT, TYPE=DC3D6E, ELSET=EALL 135, 381, 98, 96, 382, 104, 102 138, 383, 372, 373, 384, 375, 376 *ELSET,ELSET=ELEMENT,GENERATE 77, 149 226, 227 *ELSET,ELSET=BLADES,GENERATE 1, 76 150, 225 *SOLID SECTION, ELSET=EALL, MATERIAL=ZINC *SURFACE,NAME=SIDE 88,S5 87,S5 *MATERIAL, NAME=ZINC *CONDUCTIVITY 0.1121, 20.0 0.1103, 100.0 *ELECTRICAL CONDUCTIVITY 16.75E3, 20.0 12.92E3, 100.0 *JOULE HEAT FRACTION 1.0, *FILM PROPERTY,NAME=H1 6.57E-6, 25.0 11.6E-6, 40.0

5-1030

Electrical Analyses

14.2E-6, 60.0 15.8E-6, 80.0 17.0E-6,100.0 *FILM PROPERTY,NAME=H2 5.42E-6, 25.0 9.60E-6, 40.0 11.7E-6, 60.0 13.0E-6, 80.0 14.1E-6,100.0 *STEP,INC=100 STEP 1: JOULE HEATING ANALYSIS *COUPLED THERMAL-ELECTRICAL,STEADY STATE *BOUNDARY NRHS, 9, , 0.0 NLHS, 11,, 29.4 NRHS, 11,, 30.2 *CECURRENT NLHS, 9, 3.0 *FILM ELEMENT, F1, 23.3, H1 ELEMENT, F2, 23.3, H1 BLADES, F1, 23.3, H2 BLADES, F2, 23.3, H2 *ENERGY PRINT,FREQUENCY=100 *ENERGY FILE,FREQUENCY=100 *EL PRINT,ELSET=ELEMENT,FREQUENCY=100 JENER, HFLM, ECDM, EPGM *EL FILE,ELSET=ELEMENT,FREQUENCY=100 HFL, ECD, EPG *NODE PRINT,NSET=NOUTP,FREQUENCY=100 NT,EPOT *NODE FILE,NSET=NOUTP,FREQUENCY=100 NT,EPOT *SECTION PRINT,NAME=SID88,SURFACE=SIDE SOAREA,SOH,SOE *SECTION FILE, NAME=SID88,SURFACE=SIDE SOAREA,SOH,SOE *END STEP *STEP,INC=100 STEP 2: COOL DOWN ANALYSIS *HEAT TRANSFER,STEADY STATE *END STEP

5-1031

Electrical Analyses

Listing 5.2.1-2 *HEADING HEATING OF AUTOMOTIVE ELECTRICAL FUSE TRANSIENT ANALYSIS Units: mm; deg. C; Joule; sec; kg; Ampere *RESTART,WRITE,FREQUENCY=100 *NODE, INPUT=thermelectautofuse_node.inp *NSET, NSET=NLHS 3, 6, 9, 12, 15, 18, 21, 24, 27, 30 *NSET, NSET=NRHS 420, 423, 426, 429, 432, 435, 438, 441, 444, 447 *NSET, NSET=NOUTP 30, 51, 83, 200, 319, 335, 360, 225, 604, 500, 468, 447 *ELEMENT, TYPE=DC3D8E, ELSET=EALL, INPUT=thermelectautofuse_element.inp *ELEMENT, TYPE=DC3D6E, ELSET=EALL 135, 381, 98, 96, 382, 104, 102 138, 383, 372, 373, 384, 375, 376 *ELSET,ELSET=ELEMENT,GENERATE 77, 149 226, 227 *ELSET,ELSET=BLADES,GENERATE 1, 76 150, 225 *SOLID SECTION, ELSET=EALL, MATERIAL=ZINC *MATERIAL, NAME=ZINC *CONDUCTIVITY 0.1121, 20.0 0.1103, 100.0 *ELECTRICAL CONDUCTIVITY 16.75E3, 20.0 12.92E3, 100.0 *JOULE HEAT FRACTION 1.0, *DENSITY 7.14E-6, *SPECIFIC HEAT 389.0, *FILM PROPERTY,NAME=H1 6.57E-6, 25.0 11.6E-6, 40.0

5-1032

Electrical Analyses

14.2E-6, 60.0 15.8E-6, 80.0 17.0E-6,100.0 *FILM PROPERTY,NAME=H2 5.42E-6, 25.0 9.60E-6, 40.0 11.7E-6, 60.0 13.0E-6, 80.0 14.1E-6,100.0 *SURFACE, NAME=SURF_1 ELEMENT, S1 *SURFACE, NAME=SURF_2 ELEMENT, S2 *SURFACE, NAME=SURF_3 BLADES, S1 *SURFACE, NAME=SURF_4 BLADES, S2 *STEP,INC=100 STEP 1: JOULE HEATING ANALYSIS *COUPLED THERMAL-ELECTRICAL,DELTMX=20.0,END=SS 0.1, 100.0, , ,0.1 *BOUNDARY NRHS, 9, , 0.0 NLHS, 11,, 29.4 NRHS, 11,, 30.2 *CECURRENT NLHS, 9, 3.0 *SFILM SURF_1, F, 23.3, H1 SURF_2, F, 23.3, H1 SURF_3, F, 23.3, H2 SURF_4, F, 23.3, H2 *ENERGY PRINT,FREQUENCY=100 *ENERGY PRINT,FREQUENCY=100,ELSET=BLADES *ENERGY PRINT,FREQUENCY=100,ELSET=ELEMENT *ENERGY FILE,FREQUENCY=100 *ENERGY FILE,FREQUENCY=100,ELSET=BLADES *ENERGY FILE,FREQUENCY=100,ELSET=ELEMENT *EL PRINT,ELSET=ELEMENT,FREQUENCY=100 JENER, HFLM, ECDM, EPGM *EL FILE,ELSET=ELEMENT,FREQUENCY=100 HFL, ECD, EPG *NODE PRINT,NSET=NOUTP,FREQUENCY=100

5-1033

Electrical Analyses

NT,EPOT *NODE FILE,NSET=NOUTP,FREQUENCY=100 NT,EPOT *END STEP *STEP,INC=100 STEP 2: COOL DOWN ANALYSIS *HEAT TRANSFER,DELTMX=20.0,END=SS 0.1, 100.0, , ,0.1 *END STEP

5-1034

Mass Diffusion Analyses

6. Mass Diffusion Analyses 6.1 Mass diffusion analyses 6.1.1 Hydrogen diffusion in a vessel wall section Product: ABAQUS/Standard This one-dimensional problem provides a simple verification of the mass diffusion capability in ABAQUS. The uncoupled mass diffusion formulation used in ABAQUS is described in ``Mass diffusion analysis,'' Section 6.8.1 of the ABAQUS/Standard User's Manual, and ``Mass diffusion analysis,'' Section 2.13.1 of the ABAQUS Theory Manual. The physical problem considered here is that of a pressure vessel shell wall fabricated from 2 1/4 Cr-1 Mo steel alloy base metal with an internal weld overlay of Type 347 stainless steel. These vessels are typically used at high temperatures and under high pressure conditions. Under such service conditions hydrogen dissolves into the alloys (Fujii et al., 1982) and during cool-down may cause disbonding of the weld overlay from the base metal and, possibly, crack initiation and growth in the base metal due to hydrogen embrittlement. In this example we are concerned with the hydrogen diffusion aspect of the problem.

Problem description The problem is shown in Figure 6.1.1-1 and consists of a section of the vessel wall made up of a 200-mm thick base metal and a 5-mm thick weld metal. The problem is one-dimensional, the only gradient being through the thickness of the wall. The purpose of the analysis is to predict the evolution of hydrogen concentration through the wall thickness during cooling caused by a shutdown.

Geometry and model Since the problem is one-dimensional, we use a plane mesh with only one element in the y-direction (see Figure 6.1.1-2). The mesh is graded, with more elements near the interface between the two materials because we expect very high concentration gradients in this vicinity. The material properties of the two metals given by Fujii et al. (1982) are strongly dependent on temperature and can be written as follows. Solubility in weld metal: ~

sw = 1288 e¡1078=µ

ppm mm N¡1=2

Diffusivity in weld metal: ~

Dw = 9310 e¡6767=µ

mm2 =h

Solubility in base metal:

6-1035

Mass Diffusion Analyses

~

sb = 4300 e¡3261=µ

ppm mm N¡1=2

Diffusivity in base metal: ~

Db =

274 e¡1157=µ 1 + (1:05 £

10¡3

e3573=µ~ )

mm2 =h;

where µ~ is temperature in degrees Kelvin. These temperature-dependent properties are entered in ABAQUS in tabulated form, as shown in the input listings. The wall is initially at a uniform temperature of 727.5 K (454.4° C), and during the shutdown schedule it cools down to 298.15 K (25.0° C) at a constant rate over a period of 21.5 hours. The boundary conditions are as follows. Under the initial steady-state conditions the exterior of the weld metal has a hydrogen concentration of 35.85 ppm, which corresponds to a normalized concentration of 0.1225 N 1/2mm-1. Normalized concentration is used as the primary solution variable (continuous over the discretized domain) and is given as the concentration divided by the solubility. The exterior of the base metal has a zero hydrogen concentration. As the cooling period begins, the hydrogen concentration at the exterior of the weld metal is assumed to drop to zero instantaneously.

Time stepping The problem is run in two parts. The first part consists of a step in which a single increment of *MASS DIFFUSION, STEADY STATE analysis is performed with an arbitrary time step to establish the initial steady-state hydrogen concentration distribution corresponding to the initial temperature. The hydrogen diffusion during cooling is then analyzed in four subsequent *MASS DIFFUSION transient analysis steps, using automatic time stepping. This need not be done in four separate steps. We do it here because the results given by Fujii et al. (1982), with which we compare the ABAQUS results, are presented at four specific times during the transient: 2.7 h (673.15 K, 400.0°C), 5.2 h (623.15 K, 350.0°C), 10.2 h (523.15 K, 250.0°C), and 21.5 h (298.15 K, 25.0°C). The accuracy of the time integration for the *MASS DIFFUSION transient analysis steps, during which cooling occurs, is controlled by the DCMAX parameter. This parameter specifies the allowable normalized concentration change per time step. Even in a linear problem such as this, DCMAX controls the accuracy of the solution because the time integration operator is not exact (the backward difference rule is used). In this case DCMAX is chosen as 0.01 N 1/2mm-1, which is a very tight value. This is necessary to obtain an acceptably accurate integration of the concentration because the solubility of the materials decreases significantly (by more than two orders of magnitude in the base metal) as the temperature decreases and, therefore, the changes in concentration become larger for a given change in normalized concentration. An important issue in transient diffusion problems is the choice of initial time step. As in any transient problem, the spatial element size and the time step are related to the extent that time steps smaller than a certain size may lead to spurious oscillations in the solution and, therefore, provide no useful information. This coupling of the spatial and temporal approximations is always most obvious at the 6-1036

Mass Diffusion Analyses

start of diffusion problems, immediately after prescribed changes in the boundary values. For the mass diffusion case the suggested guideline for choosing the initial time increment (see ``Mass diffusion analysis,'' Section 6.8.1 of the ABAQUS/Standard User's Manual) is ¢t ¸

1 (¢h)2 ; 6D

where ¢h is a characteristic element size near the disturbance (that is, near the weld metal surface in our case), and D is the diffusivity of the material. For the weld metal in our model we choose a typical ¢h = 0.125 mm and we have D = 0.85 mm2/h at the initial temperature, which gives ¢t ¸ 0.003 h. For the base metal in our model we choose a typical ¢h = 1.25 mm and we have D = 4.88 mm2/h at the initial temperature, which gives ¢t ¸ 0.053 h. Based on these calculations an initial time step of 0.1 h is used, which gives an initial solution with no oscillations, as expected.

Results and discussion Figure 6.1.1-3 shows hydrogen concentration distributions in the weld metal for the initial steady-state condition and four different times during the cooling period. Figure 6.1.1-4 shows corresponding hydrogen concentration distributions in the base metal. These results compare very well with those presented by Fujii et al. (1982) which are not plotted here since they would appear almost indistinguishable from the ABAQUS results. It can be observed that, although the primary solution variable (the normalized concentration) remains continuous across the material interface during the transient, the hydrogen concentration becomes increasingly discontinuous across the interface. During the cooling process the hydrogen concentration in the base metal decreases, whereas the hydrogen concentration in the weld metal increases very significantly, reaching a peak at the weld metal side of the interface.

Input files hydrodiffvesselwall_2d.inp Two-dimensional analysis. hydrodiffvesselwall_3d.inp Three-dimensional analysis. hydrodiffvesselwall_fick.inp Two-dimensional analysis using Fick's law. hydrodiffvesselwall_nonlinear.inp Nonlinear version (including concentration dependence on the material properties) of the two-dimensional analysis. hydrodiffvesselwall_heat.inp Heat transfer analysis that writes temperatures to a results file for use in hydrodiffvesselwall_massdiff.inp.

6-1037

Mass Diffusion Analyses

hydrodiffvesselwall_massdiff.inp Two-dimensional mass diffusion analysis which reads temperatures from the results file written in hydrodiffvesselwall_heat.inp.

Reference · Fujii, T., T. Nazama, H. Makajima, and R. Horita, "A Safety Analysis on Overlay Disbonding of Pressure Vessels for Hydrogen Service," Journal of the American Society for Metals, pp. 361-368, 1982.

Figures Figure 6.1.1-1 Pressure vessel shell wall section.

Figure 6.1.1-2 Finite element model of shell wall.

6-1038

Mass Diffusion Analyses

Figure 6.1.1-3 Hydrogen concentration distribution in weld metal.

Figure 6.1.1-4 Hydrogen concentration distribution in base metal.

Sample listings

6-1039

Mass Diffusion Analyses

Listing 6.1.1-1 *HEADING HYDROGEN DIFFUSION OF A SHELL SECTION *RESTART,WRITE,FREQUENCY=1000 *NODE 1, 2001,,10. 41,5., 2041,5.,10. 121,205. 2121,205.,10. *NGEN,NSET=LHEND 1,2001,1000 *NGEN,NSET=MID 41,2041,1000 *NGEN,NSET=RHEND 121,2121,1000 *NFILL,NSET=NALL,TWO STEP,BIAS=1.125 LHEND,MID,40,1 *NFILL,NSET=NALL,TWO STEP,BIAS=.875 MID,RHEND,80,1 *ELEMENT,TYPE=DC2D8 1,1,3,2003,2001,2,1003,2002,1001 *ELGEN,ELSET=WELD 1,20,2,2 *ELEMENT,TYPE=DC2D8 41,41,43,2043,2041,42,1043,2042,1041 *ELGEN,ELSET=BASE 41,40,2,2 *ELSET,ELSET=ELS1 39,41 *SOLID SECTION,MATERIAL=WELD,ELSET=WELD 1., *MATERIAL,NAME=WELD *SOLUBILITY 2.48858D+01, 2.73150D+02 3.46472D+01, 2.98150D+02 4.58298D+01, 3.23150D+02 5.82346D+01, 3.48150D+02 7.16596D+01, 3.73150D+02 8.59120D+01, 3.98150D+02 1.00815D+02, 4.23150D+02

6-1040

Mass Diffusion Analyses

1.16210D+02, 4.48150D+02 1.31960D+02, 4.73150D+02 1.47945D+02, 4.98150D+02 1.64063D+02, 5.23150D+02 1.80229D+02, 5.48150D+02 1.96372D+02, 5.73150D+02 2.12432D+02, 5.98150D+02 2.28360D+02, 6.23150D+02 2.44118D+02, 6.48150D+02 2.59672D+02, 6.73150D+02 2.74998D+02, 6.98150D+02 2.90077D+02, 7.23150D+02 2.92704D+02, 7.27550D+02 *DIFFUSIVITY 1.62094D-07,, 2.73150D+02 1.29398D-06,, 2.98150D+02 7.49035D-06,, 3.23150D+02 3.36944D-05,, 3.48150D+02 1.23910D-04,, 3.73150D+02 3.86932D-04,, 3.98150D+02 1.05615D-03,, 4.23150D+02 2.57731D-03,, 4.48150D+02 5.72350D-03,, 4.73150D+02 1.17322D-02,, 4.98150D+02 2.24546D-02,, 5.23150D+02 4.05055D-02,, 5.48150D+02 6.94021D-02,, 5.73150D+02 1.13680D-01,, 5.98150D+02 1.78977D-01,, 6.23150D+02 2.72085D-01,, 6.48150D+02 4.00960D-01,, 6.73150D+02 5.74695D-01,, 6.98150D+02 8.03461D-01,, 7.23150D+02 8.50242D-01,, 7.27550D+02 *SOLID SECTION,MATERIAL=BASE,ELSET=BASE 1., *MATERIAL,NAME=BASE *SOLUBILITY 1.78188D-01, 3.23150D+02 3.67776D-01, 3.48150D+02 6.88842D-01, 3.73150D+02 1.19243D-00, 3.98150D+02 1.93457D-00, 4.23150D+02

6-1041

Mass Diffusion Analyses

2.97365D-00, 4.48150D+02 4.36782D-00, 4.73150D+02 6.17278D-00, 4.98150D+02 8.43995D-00, 5.23150D+02 1.12152D+01, 5.48150D+02 1.45379D+01, 5.73150D+02 1.84407D+01, 5.98150D+02 2.29491D+01, 6.23150D+02 2.80820D+01, 6.48150D+02 3.38515D+01, 6.73150D+02 4.02639D+01, 6.98150D+02 4.73200D+01, 7.23150D+02 4.86282D+01, 7.27550D+02 *DIFFUSIVITY 7.85674D-03,, 2.73150D+02 3.34289D-02,, 2.98150D+02 1.13043D-01,, 3.23150D+02 3.17681D-01,, 3.48150D+02 7.65060D-01,, 3.73150D+02 1.61326D-00,, 3.98150D+02 3.02697D-00,, 4.23150D+02 5.12273D-00,, 4.48150D+02 7.92165D-00,, 4.73150D+02 1.13403D+01,, 4.98150D+02 1.52239D+01,, 5.23150D+02 1.93975D+01,, 5.48150D+02 2.37067D+01,, 5.73150D+02 2.80357D+01,, 5.98150D+02 3.23085D+01,, 6.23150D+02 3.64808D+01,, 6.48150D+02 4.05306D+01,, 6.73150D+02 4.44494D+01,, 6.98150D+02 4.82372D+01,, 7.23150D+02 4.88906D+01,, 7.27550D+02 *INITIAL CONDITIONS,TYPE=TEMPERATURE NALL,727.55 *INITIAL CONDITIONS,TYPE=CONCENTRATION NALL,.1 *AMPLITUDE,NAME=AMP1,TIME=TOTAL TIME, VALUE=ABSOLUTE 0.,727.55,1.E-5,727.55,21.5,298.15,1000.,298.15 *STEP STEADY-STATE SOLUTION UNDER OPERATING CONDITIONS

6-1042

Mass Diffusion Analyses

*MASS DIFFUSION,STEADY STATE 1.E-5,1.E-5 *BOUNDARY LHEND,11,11,.12247 RHEND,11,11,0. *EL PRINT,FREQUENCY=1000 CONC,MFL,TEMP *EL PRINT,FREQUENCY=1000 MFL1,MFL2,MFLM *EL PRINT,FREQUENCY=1000, POSITION=AVERAGED AT NODES,ELSET=WELD CONC, *EL PRINT,FREQUENCY=1000, POSITION=AVERAGED AT NODES,ELSET=BASE CONC, *EL PRINT,FREQUENCY=1000 NFLUX, *NODE PRINT,FREQUENCY=1000 NNC,NT,RFL *EL FILE,ELSET=ELS1,FREQUENCY=1000 CONC,MFL *EL FILE,ELSET=ELS1,POSITION=AVERAGED AT NODES, FREQUENCY=1000 CONC, *EL FILE,FREQUENCY=1000 NFLUX, *NODE FILE,FREQUENCY=1000 NNC,RFL *END STEP *STEP,INC=100 TRANSIENT ANALYSIS DUE TO SHUTDOWN -- PHASE 1 *MASS DIFFUSION,DCMAX=.01, END=PERIOD .1,2.7,,,.0001 *BOUNDARY LHEND,11,11,0. *TEMPERATURE,AMPLITUDE=AMP1 NALL, *END STEP *STEP,INC=100 TRANSIENT ANALYSIS DUE TO SHUTDOWN -- PHASE 2 *MASS DIFFUSION,DCMAX=.01 .1,2.5,,,.0001 *BOUNDARY

6-1043

Mass Diffusion Analyses

LHEND,11,11,0. *TEMPERATURE,AMPLITUDE=AMP1 NALL, *END STEP *STEP,INC=100 TRANSIENT ANALYSIS DUE TO SHUTDOWN -- PHASE 3 *MASS DIFFUSION,DCMAX=.01 .1,5.0,,,.0001 *BOUNDARY LHEND,11,11,0. *TEMPERATURE,AMPLITUDE=AMP1 NALL, *END STEP *STEP,INC=1000 TRANSIENT ANALYSIS DUE TO SHUTDOWN -- PHASE 4 *MASS DIFFUSION,DCMAX=.05 .1,11.3,,,.0001 *BOUNDARY LHEND,11,11,0. *TEMPERATURE,AMPLITUDE=AMP1 NALL, *END STEP

6.1.2 Diffusion toward an elastic crack tip Product: ABAQUS/Standard This simple two-dimensional problem verifies the sequentially coupled, stress-assisted mass diffusion capability in ABAQUS. The mass diffusion formulation used in ABAQUS is described in ``Mass diffusion analysis,'' Section 6.8.1 of the ABAQUS/Standard User's Manual, and ``Mass diffusion analysis,'' Section 2.13.1 of the ABAQUS Theory Manual. A center-cracked plate fabricated from 2 1/4 Cr-1 Mo steel alloy is subjected to end loading in a hydrogen-rich environment. Hydrogen is drawn to the crack-tip region by high hydrostatic stresses and may assist in crack growth resulting from hydrogen embrittlement. In this example we are concerned with the hydrogen diffusion aspect of the problem.

Geometry and model The problem geometry and boundary conditions are shown in Figure 6.1.2-1. The specimen is 10-mm thick, 20-mm wide, and 80-mm high, with a 4-mm crack at its center. The mesh near the crack is focused at the crack tip, with the element size growing as the square of the distance to the crack tip (*NFILL, SINGULAR=1). A very fine mesh (see Figure 6.1.2-2) is used to capture accurately the gradients of concentration and stress near the crack tip. Four combinations of stress and mass diffusion analyses are presented:

6-1044

Mass Diffusion Analyses

· Stress analysis with quadratic elements and quarter-point spacing at the crack tip, followed by a mass diffusion analysis with linear elements. · Stress analysis with quadratic elements and quarter-point spacing at the crack tip, followed by a mass diffusion analysis with quadratic elements and quarter-point spacing at the crack tip. · Stress analysis with quadratic elements (no quarter-point spacing), followed by a mass diffusion analysis with quadratic elements (no quarter-point spacing). · Stress analysis with linear elements, followed by a mass diffusion analysis with linear elements. p The quarter-point spacing technique is used in fracture mechanics analyses to enforce a 1= r singularity at the crack tip, where r is the distance from the crack tip. The sequentially coupled mass diffusion analysis consists of a static stress analysis, followed by a mass diffusion analysis. Equivalent pressure stresses from the static analysis are written to the results file as nodal averaged values. Subsequently, these pressures are read in during the course of the mass diffusion analysis to provide a driving force for mass diffusion. The material properties for mass diffusion given by Fujii et al. (1982) are as follows. Solubility: s = 4300 e¡3261=(µ¡µ

z

)

ppm mm N¡1=2

Diffusivity: z

7611 £ 10¡5 e¡1157=(µ¡µ ) D= 1 + (1:05 £ 10¡3 e3573=(µ¡µz ) )

mm2 =s;

where µ is the temperature in degrees Celsius and µz = -273 is the absolute zero temperature. Stress-assisted diffusion is specified by defining the pressure stress factor, ∙p ; as ∙p =

V HÁ mm N¡1=2 ; R(µ ¡ µz )

where R =8.31432 Jmol -1K-1 is the universal gas constant, V H =2.0 ´ 103mm3mol-1 is the partial molar volume of hydrogen in iron-based metals, and Á is the normalized concentration. The concentration dependence of ∙p is entered in ABAQUS in tabulated form as shown in the input listings. It is important to note that although ∙p is defined in terms of normalized concentration, Á, the tabular data must be entered in terms of concentration, c = Ás: The following properties are also used in the stress analysis: elastic modulus, E =2.0 ´ 105Nmm-2, and Poisson's ratio, º = 0.3. The specimen is maintained at a constant temperature of µ ¡ µz = 325 K throughout the analysis. Under the initial steady-state conditions the specimen has a uniform concentration of 50 ppm, which

6-1045

Mass Diffusion Analyses

corresponds to a normalized concentration of 265 N 1/2mm-1. Normalized concentration is used as the primary solution variable (continuous over the discretized domain) and is given as the concentration divided by the solubility. The exterior of the specimen has a constant hydrogen concentration equal to the initial concentration. A 1 MPa distributed pressure is applied to the ends of the specimen, ramped linearly over the length of the step, and the steady-state distribution of hydrogen is obtained.

Results and discussion The analytical solution for normalized concentration, presented by Liu (1970), has the form µ

VH p Á = Áo exp ¡ R(µ ¡ µz )

¶

;

where Áo is the normalized concentration obtained in the unstressed state and p is the equivalent pressure stress. This solution dictates that for a crack-tip problem, the concentration follows the singularity of the stresses. Figure 6.1.2-3 and Figure 6.1.2-4show the final distribution of equivalent pressure stress and concentration predicted by the ABAQUS analysis in the region around the crack tip. The results shown represent the first case described above, using a quadratic, quarter-point mesh for stresses and a linear mesh for mass diffusion. The shapes of the contours show good agreement, since contours of constant pressure stress should be contours of constant concentration, as indicated by the analytical solution above. Figure 6.1.2-5 and Figure 6.1.2-6show the pressures (in MPa) and concentrations (in ppm) ahead of the crack tip for all four combinations of stress and mass diffusion analyses. Results are presented as functions of the ratio of the distance to the crack tip, r, over the crack length, a. For the region immediately ahead of the crack, linear elastic fracture mechanics yields the analytical solution for equivalent pressure stress: p=¡

KI (1 + º ) (1 + º )¾ p ¡ ; 3 2¼r

p where KI = ¾ ¼a is the stress intensity factor for a Mode I crack of length a and ¾ is the externally applied distributed load. As can be seen from the figures, the finite element results for all four combinations of element types are identical except at the first element, where the results are not expected to be valid. The results show good agreement with the analytically predicted solutions for both equivalent pressure stress and concentration as the distance to the crack tip, r, approaches zero. Farther from the crack tip, the deviation between the analytical solution and the finite element solution increases. This deviation is consistent with the fact that the linear elastic crack-tip solution is valid only as r approaches zero. No mesh convergence studies were conducted with respect to the number of elements in the crack-tip region. For comparison with the solutions presented here, an analysis was conducted with equally spaced elements approaching the crack tip. The results (not shown here) indicate that biasing the elements toward the crack tip is necessary to capture the gradients of concentration and equivalent 6-1046

Mass Diffusion Analyses

pressure stress adequately. In addition, the equivalent pressure stress results demonstrate that the effect of using quarter-point positioning of the nodes at the crack tip is insignificant in this problem as long as the mesh is refined sufficiently. Differences between the finite element and analytically predicted concentrations are a direct result of the differences between the finite element and analytically predicted values of pressure stress. If the analytical values of equivalent pressure stress are used to drive the ABAQUS concentration solution, the resulting curve is indistinguishable from the analytical concentration shown.

Input files difftocrack_quarterpstress.inp Quadratic stress analysis with quarter-point spacing at the crack tip. This analysis writes the results file used in difftocrack_linearmassdiff1.inp and difftocrack_quarterpmassdiff.inp. difftocrack_linearmassdiff1.inp Linear mass diffusion analysis that reads results file data from difftocrack_quarterpstress.inp. difftocrack_stress.inp Stress analysis with quadratic elements (no quarter-point spacing). This analysis writes the results file used in difftocrack_massdiff.inp. difftocrack_massdiff.inp Mass diffusion analysis with quadratic elements that reads equivalent pressure stresses from the results file written in difftocrack_stress.inp. difftocrack_quarterpmassdiff.inp Mass diffusion analysis with quadratic elements and quarter-point spacing. This analysis reads equivalent pressure stresses from the results file written in difftocrack_quarterpstress.inp. difftocrack_linearstress.inp Stress analysis with linear elements. This analysis writes the results file used in difftocrack_linearmassdiff2.inp. difftocrack_linearmassdiff2.inp Mass diffusion analysis with linear elements that reads equivalent pressure stresses from the results file written in difftocrack_linearstress.inp. difftocrack_node.inp Node data for all the analyses. difftocrack_quad_elements.inp Element data for the analyses using quadratic elements. difftocrack_linear_elements.inp Element data for the analyses using linear elements.

6-1047

Mass Diffusion Analyses

References · Fujii, T., T. Nazama, H. Makajima, and R. Horita, "A Safety Analysis on Overlay Disbonding of Pressure Vessels for Hydrogen Service," Journal of the American Society for Metals, pp. 361-368, 1982. · Liu, H. W., "Stress-Corrosion Cracking and the Interaction Between Crack-Tip Stress Field and Solute Atoms," Transactions of the ASME: Journal of Basic Engineering, vol. 92, pp. 633-638, 1970.

Figures Figure 6.1.2-1 Center crack specimen geometry.

Figure 6.1.2-2 Finite element model of center crack specimen (with 1/4 symmetry) with detail of crack-tip mesh.

6-1048

Mass Diffusion Analyses

Figure 6.1.2-3 Contours of equivalent pressure stress at the crack tip.

Figure 6.1.2-4 Contours of normalized hydrogen concentration at the crack tip.

6-1049

Mass Diffusion Analyses

Figure 6.1.2-5 Distribution of pressure stress ahead of the crack tip.

Figure 6.1.2-6 Hydrogen concentration distribution ahead of the crack tip.

6-1050

Mass Diffusion Analyses

Sample listings

6-1051

Mass Diffusion Analyses

Listing 6.1.2-1 *HEADING Quadratic stress analysis, singular elements at crack tip MODEL BUILT IN mm,N,s ** *PREPRINT,ECHO=NO,MODEL=NO,HIST=NO *NODE,NSET=ALL,INPUT=difftocrack_node.inp ** ** *ELEMENT, TYPE=CPE8R, ELSET=ALL, INPUT=difftocrack_quad_elements.inp ** ** *NODE,NSET=TIP 1,2.0,0. 81,2.0,0. *NGEN,NSET=TIP 1,81,1 ** ** tipbound ** *NSET, NSET=TIPBOUND 5001, 5002, 5003, 5004, 5005, 5006, 5007, 5008, 5009, 5010, 5011, 5012, 5013, 5014, 5015, 5016, 5017, 5018, 5019, 5020, 5021, 5022, 5023, 5024, 5025, 5026, 5027, 5028, 5029, 5030, 5031, 5032, 5033, 5034, 5035, 5036, 5037, 5038, 5039, 5040, 5041, 5042, 5043, 5044, 5045, 5046, 5047, 5048, 5049, 5050, 5051, 5052, 5053, 5054, 5055, 5056, 5057, 5058, 5059, 5060, 5061, 5062, 5063, 5064, 5065, 5066, 5067, 5068, 5069, 5070, 5071, 5072, 5073, 5074, 5075, 5076, 5077, 5078, 5079, 5080, 5081, *NFILL,NSET=TIPMESH,SINGULAR=1,TWOSTEP TIP,TIPBOUND,50,100

6-1052

Mass Diffusion Analyses

*ELEMENT,TYPE=CPE8R,ELSET=ALL 2001,1,201,203,3,101,202,103,2 *ELGEN,ELSET=ALL 2001,25,200,50,40,2,1 ** ** front ** *NSET,NSET=FRONT,GEN 1,5001,100 *NSET, NSET=FRONT 5001, 5522, 5533, 5586, 5597, 5618, 5661, 5682, 5693, 5746, 5757, 5778, 5821, 6802, 6813, 6866, 6877, 6898, 6941, 6962, 6973, 7026, 7037, 7058, 7101, 7122, 7133, 7186, 7197, 7218, 7261, 7282, 7293, 7346, 7357, 7378, 7421, ** ** RIGHT ** *NSET, NSET=RIGHT 7421, 7422, 7423, 7426, 7427, 7428, 7431, 7432, 7433, 7436, 7437, 7438, 7441, 8642, 8653, 8706, 8717, 8738, 8781, 8802, 8813, 8866, 8877, 8898, 8941, 8962, 8973, 9026, 9037, 9058, 9101, 9122, 9133, 9186, 9197, 9218, 9261, 9282, 9293, 9346, 9357 ** ** left

5554, 5629, 5714, 5789, 6834, 6909, 6994, 7069, 7154, 7229, 7314, 7389,

5565, 5650, 5725, 5810, 6845, 6930, 7005, 7090, 7165, 7250, 7325, 7410,

7424, 7429, 7434, 7439, 8674, 8749, 8834, 8909, 8994, 9069, 9154, 9229, 9314,

7425, 7430, 7435, 7440, 8685, 8770, 8845, 8930, 9005, 9090, 9165, 9250, 9325,

6-1053

Mass Diffusion Analyses

** *NSET, NSET=LEFT 6481, 6782, 6786, 6787, 6791, 6792, 6796, 6797, 6801, 8051, 8111, 8131, 8191, 8201, 8261, 8281, 8341, 8351, 8411, 8431, 8491, 8501, 8561, 8581, 8641, 9387, 9417, 9422, 9452, 9462, 9492, 9497, 9527, 9537, 9567, 9572, 9602, 9612, 9642, 9647, 9677, 9687, 9691, 9692, ** ** crack ** *NSET,NSET=CRACK,GEN 81,5081,100 *NSET, NSET=CRACK 5081, 6511, 6571, 6591, 6651, 6661, 6721, 6741, 6801, ** ** top ** *NSET, NSET=TOP 9357, 9358, 9362, 9363, 9367, 9368, 9372, 9373,

6783, 6788, 6793, 6798, 8071, 8141, 8221, 8291, 8371, 8441, 8521, 8591, 9392, 9432, 9467, 9507, 9542, 9582, 9617, 9657, 9688, 9745,

6784, 6789, 6794, 6799, 8081, 8161, 8231, 8311, 8381, 8461, 8531, 8611, 9402, 9437, 9477, 9512, 9552, 9587, 9627, 9662, 9689, 9746

6785, 6790, 6795, 6800, 8101, 8171, 8251, 8321, 8401, 8471, 8551, 8621, 9407, 9447, 9482, 9522, 9557, 9597, 9632, 9672, 9690,

6531, 6601, 6681, 6751,

6541, 6621, 6691, 6771,

6561, 6631, 6711, 6781,

9359, 9364, 9369, 9374,

9360, 9365, 9370, 9375,

9361, 9366, 9371, 9376,

6-1054

Mass Diffusion Analyses

9377, 9682, 9687,

9678, 9683,

9679, 9684,

9680, 9685,

9681, 9686,

** ** top ** *ELSET, ELSET=TOP 1221, 1222, 1223, 1224, 1225, 1226, 1227, 1228, 1229, 1230, 1326, 1327, 1328, 1329, 1330 ** ** all ** *SOLID SECTION, ELSET=ALL, MATERIAL=STEEL 1., ** ** steel ** *MATERIAL, NAME=STEEL ** ** *ELASTIC, TYPE=ISO 2.E+5, 0.3 *BOUNDARY LEFT,1,1 FRONT,2,2 *STEP *STATIC 0.1,1.0 *DLOAD TOP,P2,-1 *EL PRINT,FREQ=0,position=averaged at nodes press, *NODE PRINT,FREQ=0 *NODE FILE,FREQ=0 *RESTART,WRITE,OVERLAY,FREQ=1 *EL FILE, POSITION=AVERAGED AT NODES SINV, *END STEP

6-1055

Mass Diffusion Analyses

Listing 6.1.2-2 *HEADING Mass Diffusion Analysis with Linear Elements Using Quadratic Singular Stress analysis MODEL BUILT IN mm,N,s ** *PREPRINT,ECHO=NO,MODEL=NO,HIST=NO *NODE,NSET=ALL,INPUT=difftocrack_node.inp ** ** *ELEMENT, TYPE=DC2D4, ELSET=ALL, INPUT=difftocrack_linear_elements.inp ** ** *NODE,NSET=TIP 1,2.0,0. 81,2.0,0. *NGEN,NSET=TIP 1,81,1 ** ** tipbound ** *NSET, NSET=TIPBOUND 5001, 5002, 5003, 5004, 5005, 5006, 5007, 5008, 5009, 5010, 5011, 5012, 5013, 5014, 5015, 5016, 5017, 5018, 5019, 5020, 5021, 5022, 5023, 5024, 5025, 5026, 5027, 5028, 5029, 5030, 5031, 5032, 5033, 5034, 5035, 5036, 5037, 5038, 5039, 5040, 5041, 5042, 5043, 5044, 5045, 5046, 5047, 5048, 5049, 5050, 5051, 5052, 5053, 5054, 5055, 5056, 5057, 5058, 5059, 5060, 5061, 5062, 5063, 5064, 5065, 5066, 5067, 5068, 5069, 5070, 5071, 5072, 5073, 5074, 5075, 5076, 5077, 5078, 5079, 5080, 5081, *NFILL,NSET=TIPMESH,SINGULAR=1,TWO STEP TIP,TIPBOUND,50,100

6-1056

Mass Diffusion Analyses

*ELEMENT,TYPE=DC2D4,ELSET=ALL 2001,1,201,203,3 *ELGEN,ELSET=ALL 2001,25,200,50,40,2,1 ** ** front ** *NSET,NSET=FRONT,GEN 1,5001,100 *NSET, NSET=FRONT 5001, 5522, 5533, 5586, 5597, 5618, 5661, 5682, 5693, 5746, 5757, 5778, 5821, 6802, 6813, 6866, 6877, 6898, 6941, 6962, 6973, 7026, 7037, 7058, 7101, 7122, 7133, 7186, 7197, 7218, 7261, 7282, 7293, 7346, 7357, 7378, 7421, ** ** RIGHT ** *NSET, NSET=RIGHT 7421, 7422, 7423, 7426, 7427, 7428, 7431, 7432, 7433, 7436, 7437, 7438, 7441, 8642, 8653, 8706, 8717, 8738, 8781, 8802, 8813, 8866, 8877, 8898, 8941, 8962, 8973, 9026, 9037, 9058, 9101, 9122, 9133, 9186, 9197, 9218, 9261, 9282, 9293, 9346, 9357 ** ** left

5554, 5629, 5714, 5789, 6834, 6909, 6994, 7069, 7154, 7229, 7314, 7389,

5565, 5650, 5725, 5810, 6845, 6930, 7005, 7090, 7165, 7250, 7325, 7410,

7424, 7429, 7434, 7439, 8674, 8749, 8834, 8909, 8994, 9069, 9154, 9229, 9314,

7425, 7430, 7435, 7440, 8685, 8770, 8845, 8930, 9005, 9090, 9165, 9250, 9325,

6-1057

Mass Diffusion Analyses

** *NSET, NSET=LEFT 6481, 6782, 6786, 6787, 6791, 6792, 6796, 6797, 6801, 8051, 8111, 8131, 8191, 8201, 8261, 8281, 8341, 8351, 8411, 8431, 8491, 8501, 8561, 8581, 8641, 9387, 9417, 9422, 9452, 9462, 9492, 9497, 9527, 9537, 9567, 9572, 9602, 9612, 9642, 9647, 9677, 9687, 9691, 9692, ** ** crack ** *NSET,NSET=CRACK,GEN 81,5081,100 *NSET, NSET=CRACK 5081, 6511, 6571, 6591, 6651, 6661, 6721, 6741, 6801, ** ** top ** *NSET, NSET=TOP 9357, 9358, 9362, 9363, 9367, 9368, 9372, 9373,

6783, 6788, 6793, 6798, 8071, 8141, 8221, 8291, 8371, 8441, 8521, 8591, 9392, 9432, 9467, 9507, 9542, 9582, 9617, 9657, 9688, 9745,

6784, 6789, 6794, 6799, 8081, 8161, 8231, 8311, 8381, 8461, 8531, 8611, 9402, 9437, 9477, 9512, 9552, 9587, 9627, 9662, 9689, 9746

6785, 6790, 6795, 6800, 8101, 8171, 8251, 8321, 8401, 8471, 8551, 8621, 9407, 9447, 9482, 9522, 9557, 9597, 9632, 9672, 9690,

6531, 6601, 6681, 6751,

6541, 6621, 6691, 6771,

6561, 6631, 6711, 6781,

9359, 9364, 9369, 9374,

9360, 9365, 9370, 9375,

9361, 9366, 9371, 9376,

6-1058

Mass Diffusion Analyses

9377, 9682, 9687,

9678, 9683,

9679, 9684,

9680, 9685,

9681, 9686,

** ** top ** *ELSET, ELSET=TOP 1221, 1222, 1223, 1224, 1225, 1226, 1227, 1228, 1229, 1230, 1326, 1327, 1328, 1329, 1330 ** ** all ** *SOLID SECTION, ELSET=ALL, MATERIAL=STEEL 1., ** ** steel ** *MATERIAL, NAME=STEEL ** ** *ELASTIC, TYPE=ISO 2.E+5, 0.3 *DIFFUSIVITY 34.096361E-6, *KAPPA,TYPE=PRESS 0.0,0.0 3.921890,1E3 *SOLUBILITY 0.18872283, *PHYSICAL CONS,ABS=-273 *INITIAL CONDITIONS,TYPE=PRESS ALL,0. *INITIAL CONDITIONS,TYPE=CONC ALL,264.9388 *INITIAL CONDITIONS,TYPE=TEMP ALL,52.0 *STEP,UNSYMM=YES,AMPLITUDE=STEP *MASS DIFFUSION,STEADY STATE 0.1,1.0 *BOUNDARY RIGHT,11,11,264.9388 *PRESSURE STRESS,

6-1059

Mass Diffusion Analyses

FILE=difftocrack_quarterpstress *EL PRINT,FREQ=0 *NODE PRINT,NSET=FRONT NNC11, *NODE FILE,NSET=FRONT,FREQ=2 NNC, *RESTART,WRITE,OVERLAY,FREQ=1 *EL FILE,FREQ=2 CONC, SOL, ESOL, ISOL, *END STEP

6-1060

Acoustic Analyses

7. Acoustic Analyses 7.1 Acoustic analyses 7.1.1 Coupled acoustic-structural analysis of a car Product: ABAQUS/Standard This example illustrates fully coupled acoustic-structural analysis. Such problems arise when solid-fluid interaction is fundamental to the overall vibrational behavior of the body or of the acoustic fluid. Typical examples of such problems include loudspeaker enclosures, fluid-filled tanks, muffler systems, and vehicle cabin enclosures. This particular example is a two-dimensional analysis of a car structure and interior and represents a cross-section of the car cabin cut lengthwise by a vertical plane. The model contains structural elements to model the car cabin, acoustic elements to model the air interior, and acoustic-structural interface elements to produce the coupling. All elements have an out-of-plane thickness of 1.0, so all forces can be interpreted as per unit of thickness of the cross-section. The analysis begins with natural frequency extractions for the structure alone and for the acoustic cavity alone. The remaining part of the study obtains the steady-state harmonic response of the fully coupled system, excited by a point load at one node on the floor of the car, in the range 35-65 Hz. Two models are used to obtain this response. In one the structure is represented by finite elements. In the other the structure is represented by some of its natural modes. This latter approach can be quite cost-effective in some cases (although it is not so in this small example). It is also useful in applications where the structure is so complex that its harmonic response cannot be predicted accurately with numerical modeling; instead, the modes and frequencies are obtained experimentally. This example shows how such numerically or experimentally determined modes can be used in an analysis. It also includes a study of the sensitivity of the acoustic response to damping in the structure.

Full model The models are shown in Figure 7.1.1-1. The structural model is made from beam elements of type B21, using the properties of various materials making up the structure (steel, glass, and wood). The acoustic model fills the interior of the structure with 4-node acoustic elements of type AC2D4. Acoustic interface elements (type ASI2) couple the structure and the acoustic medium. No mesh convergence study has been done since the example is intended as an illustration only. The acoustic elements that represent the seat back have a "volumetric drag coefficient" to simulate the acoustic absorbing properties of the material used in this part of the interior. The *DAMPING option is used to introduce Rayleigh stiffness proportional damping, governed by the parameter ¯, into the structural materials in the model. For a given value of ¯ applied to all materials in the structure, the damping fraction » for a mode ® with natural frequency !® (radians per unit time) is given by the formula

7-1061

Acoustic Analyses

»=

¯!® : 2

The value of ¯ in the full model was chosen to give approximately 1% critical damping for those modes of the structure whose natural frequencies are in the range of excitation. This was done by calculating ¯ to give exactly 1% critical damping at 41.51 Hz (mode 19 of the structure, !19 = 260.81 radians/time), which produces damping fractions ranging from 0.86% at mode 16 to 1.56% at mode 23.

Modal model In the modal model the structural elements are replaced with a modal representation of the structure as illustrated in Figure 7.1.1-2. In many practical cases this modal representation is based on experimental measurements. We do not have such data for this example: instead, we use the modes extracted for the structure alone. The acoustic elements are defined exactly as in the full model (including volumetric drag in the seat). Modal representation means that the physical response uN i in direction i at node N is approximated by the sum of modal amplitudes along eigenvectors of the structure uN i

=

M X

a® ÁN i® ;

®=1

where ÁN i® is the eigenvector of the structural system for mode ®, a® is the modal amplitude of the response (the "generalized coordinate"), and M is the number of modes used in the representation. This modal representation of the structure consists of the M independent single degree of freedom systems coupled to the displacements of the physical nodes through the summation equation above. Since the modes are orthogonal, the response of each mode, a® ; is that of an independent, one degree of freedom system (Figure 7.1.1-2), with mass m® , stiffness k® , and viscous damping c® . If the modes are extracted by ABAQUS, the generalized mass m® and the natural frequency !® (defining k® = m® =!®2 ) are both available from the output of the *FREQUENCY step. If the modes have been obtained experimentally, these values are provided as part of the measured response. The damping value c® for a mode ® is chosen to produce a desired fraction, »® , of the critical damping for that mode p and is given by c® = 2»® m® k® : To couple the displacements of the physical nodes to the generalized coordinates of the modes, a® , these generalized coordinates must be present as degrees of freedom in the model. For this purpose a special, nonphysical node is created for each mode. (The coordinates of these nodes do not affect the analysis, so for convenience they are all placed at the origin.) The generalized coordinate of a given mode is represented by displacement in the 1-direction (arbitrarily chosen) at its node. The generalized mass, damping, and stiffness for a given mode are incorporated as mass, dashpot, and spring elements at its node. The physical nodes are needed around the acoustic boundary where we wish to couple the structural response to the response of the acoustic fluid through ASI-type elements. The summation equation above is imposed in each direction at each such acoustic boundary node by using the *EQUATION

7-1062

Acoustic Analyses

option to tie the displacements of the physical boundary nodes to the 1-direction displacements of the nonphysical nodes. Since there are usually many such displacement components, we use a FORTRAN program to generate the *EQUATION data. acouststructcar_coupled.inp shows that program, using the ABAQUS results file from the *FREQUENCY analysis of the structure to generate the *EQUATION data. The program also extracts m® and k® from the *FREQUENCY analysis results file and calculates c® ; three files are generated and can be copied directly into an input file to define the mass, spring, and dashpot coefficients. A damping value, »® , of 1% of critical damping is used in all modes. This modal damping will not give exactly the same results as the Rayleigh damping used in the full model because in the full model the fraction of critical damping was exactly 1% at only one frequency. The fraction of critical damping can be varied in the program by changing the value of the variable FRACTD.

Results and discussion The results for each of the analyses are discussed below.

Natural frequency analysis The results of the natural frequency analysis of the structure alone are summarized in Table 7.1.1-1 and illustrated in Figure 7.1.1-3. The eight modes that occur in the frequency range of interest (35-65 Hz) are shown. The lowest of these modes, mode 16, is at 35.6 Hz when the roof of the car model vibrates in its third mode. Mode 17, at 37.1 Hz, is the third mode of the back shelf. Mode 18, at 37.7 Hz, is the fourth mode of the floor. At 47.6 Hz, mode 20, the windshield vibrates in its second mode. The rest of the modes are higher modes of the floor, the roof, and the back shelf. The frequency analysis of the acoustic cavity alone is summarized in Table 7.1.1-2 and shown (as contours of acoustic pressure) in Figure 7.1.1-4. The first nonzero mode of the acoustic cavity is at 50.2 Hz--well above the frequency range of the lowest structural modes. Only this lowest mode falls into the frequency range of interest, however. Since the acoustic cavity has no boundary conditions on acoustic pressure when it is modeled alone, there is a zero frequency mode. This requires a small frequency shift in the *FREQUENCY option to avoid the associated singularity.

Coupled analyses All of the models are run requesting analysis at 181 frequencies in the range of interest. A coarser model would result in some of the resonances being missed. A coupled acoustic-structural steady-state analysis must be performed using the *STEADY STATE DYNAMICS, DIRECT procedure in ABAQUS. The coupled analyses are performed as frequency sweeps from 35-65 Hz, with the system excited by a concentrated force at node 997 (at the location of a rear axle support point), whose magnitude is 1.0 N in phase and 0.06 N out of phase. The results of the full finite element representation of the structure are compared to the results obtained with the 25-mode model. The full model's response is illustrated by the acoustic pressure contours shown in Figure 7.1.1-5. The contours are shown at four representative frequencies within the range of interest. Figure 7.1.1-6illustrates the response of the 25-mode model for the same frequencies. The differences in the

7-1063

Acoustic Analyses

pressure contours reflect differences in the damping in the two models. The modal model, with 1% of critical damping at all frequencies, is more damped than the full model at the lower frequencies and less damped at the higher frequencies. Figure 7.1.1-7 shows the acoustic pressure at node 271 (about where the driver's head would be located) and at node 745 (low in the interior, in front of the driver's seat) plotted as a function of frequency for both the full and 25-mode models. This figure also shows the displacements at nodes 989 and 997 (both on the floor below the seat) for both models.

Effect of volumetric drag Figure 7.1.1-8 shows the acoustic pressure results for the full model, without Rayleigh damping, both with and without volumetric drag. The lack of volumetric drag allows the structural resonances at around 35 Hz and 62 Hz to excite large acoustic pressure amplitudes at these frequencies. The Rayleigh damping is excluded from the analyses of Figure 7.1.1-8to highlight the effect of volumetric drag. Comparison of this figure with Figure 7.1.1-7 shows that the Rayleigh damping dominates volumetric drag effects in this model.

Effect of Rayleigh damping Figure 7.1.1-9 shows the effect of introducing damping into the full representation of the structure. It again shows the pressures at nodes 271 and 745 as functions of frequency. As expected, damping in the structure reduces the amplitude of the resonant response substantially. The volumetric drag was included in these analyses.

Accuracy of the modal model The accuracy of the solution using a modal representation of the structure depends on using enough modes to model the structure properly in the frequency range of interest. The analysis is performed using 25 modes, then repeated using 50 modes to test the accuracy of the 25-mode solution. It would be expected that, since the frequency of any mode higher than 25 is well out of the frequency range of interest, 25 modes would be sufficient to model the structure accurately. This is indeed the case; the results from the 50-mode model are almost indistinguishable from the 25-mode model and, therefore, are not shown. The FORTRAN program can generate *EQUATION data for any number of modes by changing the variable MODES.

Input files acouststructcar_coupled.inp Fully coupled steady-state analysis of the full acoustic-structural model, including Rayleigh damping in the structure. acouststructcar_structmodes.inp Extracting the modes of the uncoupled structural model. For use with acouststructcar_equations.f, the number of modes extracted must match the number of modes desired in the modal analysis of the system.

7-1064

Acoustic Analyses

acouststructcar_acoustmodes.inp Extracting the modes of the uncoupled acoustic model. acouststructcar_equations.f FORTRAN program used to convert the structural eigenvectors from acouststructcar_structmodes.inp into *EQUATIONs for the eigenvalue (modal) representation of the structure. acouststructcar_eigen25modes.inp Fully coupled steady-state analysis, which utilizes the eigenvalue representation of the structure (25 modes), including 1% critical damping of each mode. acouststructcar_eigen50modes.inp Fully coupled steady-state analysis, which utilizes the eigenvalue representation of the structure (50 modes), including 1% critical damping of each mode.

Tables Table 7.1.1-1 Natural frequencies for the structure alone. Mode Frequenc Mode Frequenc Mode Frequenc y, Hz y, Hz y, Hz 1 1.23 11 16.91 21 47.70 2 1.87 12 17.25 22 61.52 3 2.18 13 20.10 23 64.59 4 2.88 14 21.25 24 76.92 5 4.38 15 25.38 25 76.92 6 5.18 16 35.64 7 7.34 17 37.08 8 9.73 18 37.71 9 10.18 19 41.51 10 11.16 20 47.62

Table 7.1.1-2 Natural frequencies for the acoustic cavity alone. Mode Frequenc y, Hz 1 50.2 2 95.7 3 104.7 4 141.0 5 164.5 6 190.5 7 207.2 8 228.3 9 231.9

7-1065

Acoustic Analyses

Figures Figure 7.1.1-1 Two-dimensional model of a car structure and interior.

Figure 7.1.1-2 Modal representation of structure in fully coupled acoustic-structural analysis.

Figure 7.1.1-3 Modes 16-23 of the car structure alone.

7-1066

Acoustic Analyses

Figure 7.1.1-4 Lowest 8 modes of the acoustic medium alone.

7-1067

Acoustic Analyses

Figure 7.1.1-5 Steady-state response of the full model: acoustic pressure plots.

7-1068

Acoustic Analyses

Figure 7.1.1-6 Steady-state response of the 25 mode system: acoustic pressure plots.

Figure 7.1.1-7 Steady-state response: pressure and displacement amplitudes.

7-1069

Acoustic Analyses

Figure 7.1.1-8 Steady-state response of the full model: effect of volumetric drag, without Rayleigh damping.

7-1070

Acoustic Analyses

Figure 7.1.1-9 Steady-state response of the full model: effect of Rayleigh damping.

7-1071

Acoustic Analyses

Sample listings

7-1072

Acoustic Analyses

Listing 7.1.1-1 *HEADING Car interior - coupled analysis full representation *RESTART,WRITE *NODE 101,1.000, 1.100 131,2.600, 1.100 421,0.760, 0.740 581,0.800, 0.520 741,0.600, 0.320 981,0.600,-0.020 989,1.050,-0.020 749,1.050, 0.240 755,1.440, 0.180 435,1.710, 0.730 437,1.810, 0.730 997,1.480,-0.020 1001,1.780,-0.020 921,1.860, 0.120 761,1.880, 0.300 771,2.300, 0.240 451,2.520, 0.730 737,0.250, 0.320 897,0.300, 0.080 979,0.470,-0.020 757,1.630, 0.340 93,0.350, 0.700 415,0.350, 0.700 139,3.380, 0.730 459,3.380, 0.730 *NGEN,NSET=ROOF 101,131 *NGEN,NSET=WINDOW 93,101 415,421 451,459 131,139 *NGEN,NSET=FRONT 101,421,40 421,581,40 581,741,40

7-1073

Acoustic Analyses

741,981,40 *NGEN,NSET=WINDOW 93,421,164 95,341,123 97,261,82 99,181,41 *NGEN,NSET=REAR 131,451,40 451,771,40 761,771 761,921,40 921,1001,40 *NGEN,NSET=FLOOR 979,989 749,989,40 749,755 435,755,40 435,437 437,757,40 757,997,40 997,1001 *NGEN,NSET=TORPED 737,741 737,897,40 897,979,41 *NGEN 181,211 261,291 341,371 421,435 501,515 581,595 661,675 741,749 817,829 837,841 897,909 437,451 517,531 597,611 677,691 757,761 917,921

7-1074

Acoustic Analyses

131,451,40 133,453,40 135,455,40 137,457,160 *ELEMENT,TYPE=AC2D4,ELSET=ACOUSTIC 1,257,218,95,93 2,218,179,97,95 3,179,140,99,97 4,101,99,140,101 5,421,341,218,257 6,341,261,179,218 7,261,181,140,179 8,101,140,181,101 116,213,133,131,211 156,137,135,215,137 157,297,137,215,335 158,457,297,335,455 176,139,137,297,139 177,139,297,457,139 101,183,103,101,181 181,503,423,421,501 189,519,439,437,517 259,819,739,737,817 268,839,759,757,837 *ELGEN,ELSET=ACOUSTIC 101,15,2,1,4,80,20 181, 7,2,1,4,80,20 189, 7,2,1,4,80,20 259, 6,2,1,3,80,20 268, 2,2,1,3,80,20 116, 2,2,20,4,80,1 *ELEMENT,TYPE=AC2D4,ELSET=ACOUSTIC 299,979,899,897,979 137,335,215,213,293 138,455,335,293,373 139,455,373,453,455 *ELEMENT,TYPE=AC2D4,ELSET=ABSORB 188,517,437,435,515 *ELGEN,ELSET=ABSORB 188,4,80,20 *ELEMENT,TYPE=B21 11,103,101 31,95,93

7-1075

Acoustic Analyses

41,457,459 *ELEMENT,TYPE=B21,ELSET=FLOR 81,1001,921 82,999,1001 80,989,997 84,987,989 89,897,979 90,817,897 *ELGEN,ELSET=ROOF 11,15,2 *ELGEN,ELSET=WINDOW 31,4,2 *ELGEN,ELSET=PLYWOOD 41,4,-2 *ELGEN,ELSET=FLOR 82,2,-2 84,5,-2 90,2,-80 *ELSET,ELSET=STEEL ROOF,FLOR *BEAM SECTION,SECTION=RECT,MATERIAL=STEEL, ELSET=STEEL 1,0.9E-3 *MATERIAL,NAME=STEEL *DENSITY 7850., *ELASTIC 2.1E11,0.3 *DAMPING,BETA=7.668E-5 *BEAM SECTION,SECTION=RECT,MATERIAL=WINDOW, ELSET=WINDOW 1,2.E-3 *MATERIAL,NAME=WINDOW *DENSITY 2470., *ELASTIC 0.7E11,0.23 *DAMPING,BETA=7.668E-5 *BEAM SECTION,SECTION=RECT,MATERIAL=PLYWOOD, ELSET=PLYWOOD 1,10.E-3 *MATERIAL,NAME=PLYWOOD *DENSITY

7-1076

Acoustic Analyses

300., *ELASTIC 0.001E11,0.3 *DAMPING,BETA=7.668E-5 *EQUATION 2, 459,1,1,139,1,-1 2, 459,2,1,139,2,-1 2, 459,6,1,139,6,-1 *ELEMENT,TYPE=ASI2,ELSET=INTER 1011,103,101 1031,95,93 1041,457,139 1042,455,457 1081,1001,921 1082,999,1001 1080,989,997 1084,987,989 1089,897,979 1090,817,897 *ELGEN,ELSET=INTER 1011,15,2 1031,4,2 1042,3,-2 1082,2,-2 1084,5,-2 1090,2,-80 *SOLID SECTION,MATERIAL=ACOUSTIC,ELSET=ACOUSTIC 1, *INTERFACE,ELSET=INTER 1, *MATERIAL,NAME=ACOUSTIC *DENSITY 1.293, *ACOUSTIC MEDIUM,BULK MODULUS 1.183E5, *SOLID SECTION,ELSET=ABSORB,MATERIAL=ABSORB 1, *MATERIAL,NAME=ABSORB *DENSITY 20.,

7-1077

Acoustic Analyses

*ACOUSTIC MEDIUM,BULK MODULUS 5.E6, *ACOUSTIC MEDIUM,VOLUMETRIC DRAG 30.E2, *BOUNDARY 101,ENCASTRE 131,ENCASTRE 451,ENCASTRE 737,ENCASTRE 921,ENCASTRE *NSET,NSET=OUT 271,745, 989,997 *STEP *STEADY STATE DYNAMICS, DIRECT, FREQUENCY SCALE=LINEAR 35,65,181,1 *CLOAD 997,2,1. *CLOAD, LOAD CASE=2 997,2,0.06 *EL PRINT,FREQUENCY=100 S11,PHS11,E11,PHE11 *NODE PRINT,FREQUENCY=10,NSET=OUT U2,PU2,POR,PPOR *NODE FILE,NSET=OUT U,POR,PU,PPOR *OUTPUT,FIELD *NODE OUTPUT,NSET=OUT U,POR,PU,PPOR *OUTPUT,HISTORY *NODE OUTPUT,NSET=OUT U,POR,PU,PPOR *END STEP

7.1.2 Fully and sequentially coupled structural acoustics of a muffler Product: ABAQUS/Standard This example demonstrates the solution of the acoustic field in the vicinity of a muffler in air caused by the vibrations of the muffler shell. The computations are done using both the fully coupled (``Acoustic and coupled acoustic-structural analysis, '' Section 6.9.1 of the ABAQUS/Standard User's Manual) and sequentially coupled acoustic-solid ( ``Submodeling,'' Section 7.3.1 of the ABAQUS/Standard User's Manual) interaction procedures in ABAQUS. In the fully coupled case the

7-1078

Acoustic Analyses

solid medium of the muffler is directly coupled to the enclosed and surrounding air in a single analysis. In the sequentially coupled case the muffler vibrations are considered to be independent of the loading effects of the surrounding air, while the acoustic vibrations of the surrounding air are forced by the motion of the muffler. This allows the muffler vibration and acoustic radiation problems to be solved in sequence, using the submodeling procedure in ABAQUS. The results for the sequentially coupled model are verified by comparing them to results using the fully coupled procedure.

Full modeling vs. submodeling The fully coupled model includes the effect of the acoustic pressure in the surrounding air loading the muffler body during vibration of the system. When modeling the acoustics of metal structures in air, such as in this case, such acoustic pressure loading is often negligible in comparison with other forces in the structure. The submodeling capability (*SUBMODEL) can be used in this situation. The part of the interacting system that is unaffected by the other is treated as the "global" model, while the part whose solution depends strongly on the solution of the other is treated as the "submodel." In the case of an acoustic analysis, of course, this nomenclature refers to the hierarchy of the solutions, not the geometric sizes of the models. When sequential coupling is physically appropriate, its use offers an advantage over a fully coupled solution. Two problems, each smaller than the fully coupled problem, are less computationally expensive. If the applicability of the sequentially coupled solution method is uncertain, the user should make characteristic test computations in the frequency range of interest. If these computations show little difference between the fully and sequentially coupled solutions, the less expensive sequentially coupled method can be used.

Geometry and model The system considered here consists of a cylindrical muffler and the interacting air. The muffler is a simple tube 180 mm in diameter and 1 m in length, with inlet and outlet pipes 70 mm in diameter and 100 mm in length. The muffler structure is made from stainless steel sheeting, 0.75 mm in thickness. A porous packing material, which dampens the acoustic field, surrounds the inner pipe. Although this problem is in essence axisymmetric, a narrow three-dimensional wedge (subtending an angle of 10°) of the coupled system is modeled because ABAQUS has a limitation on the use of submodeling with axisymmetric shells. Appropriate boundary conditions are applied to the three-dimensional model so that the axisymmetric solution is captured. The meshes of the surrounding air, the exterior muffler shell, and the air inside the muffler are shown in Figure 7.1.2-1, Figure 7.1.2-2, and Figure 7.1.2-3, respectively. The air inside the muffler is meshed with AC3D10 elements (second-order tetrahedra). The innermost column of fluid elements models the undamped air. The adjacent annulus models the air in the region of the packing material. These two regions are highlighted in Figure 7.1.2-3, where the annulus is shown as the darker region. The effect of the packing material is modeled using the *ACOUSTIC MEDIUM, VOLUMETRIC DRAG option. The muffler is meshed with S4R shell elements. The exterior fluid is shown in Figure 7.1.2-1. Its outer boundary is made up of spherical and cylindrical segments, on which spherical and cylindrical absorbing boundary conditions are imposed using

7-1079

Acoustic Analyses

*SIMPEDANCE, TYPE=SPHERE and *SIMPEDANCE, TYPE=CIRCULAR, respectively. The cylindrical and spherical absorbing boundary conditions can be combined in ABAQUS, allowing the external mesh to conform to the geometry of the radiating object more closely. Combinations of different boundary condition types are most effective when the boundaries are continuous in slope as well as displacement. Second-order hexahedral acoustic elements ( AC3D20) are used to fill in the volume of the exterior fluid region. In the submodeling procedure the interface between the surrounding air and the muffler is meshed with 8-node acoustic interface elements ( ASI8). The choice of mesh density (element size) is discussed in ``Acoustic and coupled acoustic-structural analysis, '' Section 6.9.1 of the ABAQUS/Standard User's Manual. In both cases the inner boundary of the exterior air mesh conforms to the muffler shell and to rigid baffles, which isolate the exterior field from the exhaust and inlet noise. These baffle pipes are the same diameter as the inlet and exhaust pipes but are modeled simply by imposing no boundary condition on the acoustic elements in this region. This is equivalent to imposing the condition that the acceleration on this boundary is zero, which is correct for a rigid baffle. We are most interested in performing a frequency sweep about the first resonant frequency of the fully coupled system. However, a direct determination of the eigenfrequencies using the *FREQUENCY procedure yields modes and frequencies associated with the decoupled fluid and solid systems (see ``Acoustic and coupled acoustic-structural analysis, '' Section 6.9.1 of the ABAQUS/Standard User's Manual, for more details). For problems involving air and metal structures, the structure usually dominates the behavior of the system. Therefore, an estimate of the first important resonance of the coupled system is found by performing a frequency sweep in the vicinity of the first eigenfrequency of the muffler shell, computed without any interaction with the interior or exterior air. This occurs at f = 172 Hz . Although the resonant frequencies of the fully coupled system do not coincide with the resonant frequencies of the muffler shell alone, they are close, especially at lower frequencies. Using the *STEADY STATE DYNAMICS, DIRECT procedure to search around 172 Hz, we find that the first resonant frequency for the fully coupled system occurs at approximately 178 Hz. A frequency sweep of both the fully coupled and the sequentially coupled models from 177.2 Hz to 179.4 Hz at 0.2 Hz increments is performed. A pressure wave of unit magnitude is applied to the muffler inlet at each frequency, and a plane wave absorbing boundary condition is applied at the muffler outlet. The material properties for the air are a bulk modulus Kf of 0:142 MPa and a density ½f of 1.2 3 kg=m , yielding a characteristic sound speed of 344 m=s. The volumetric drag, r, specified for the air in the packing material region is 1:2 N s = m. Volumetric drag values are considered "small" if they are small compared to 2 ¼ ½f f , a condition satisfied by r = 1:2 N s = m for the frequency range of interest. The muffler is made of stainless steel with Young's modulus E of 190 MPa, Poisson's ratio º of 0.3, 3 and density ½s of 7920 kg=m . Material properties affect the mesh parameters appropriate for wave problems. The characteristic wavelength of air at f = 180Hz , − = 2¼ £ 180 ¼ 1131 rad=sec , is ¸a =

q

Kf ½f −2

¼ 1:9m

, which is long compared to the overall system geometry. The internodal spacing of roughly 40 mm

7-1080

Acoustic Analyses

used in the surrounding acoustic mesh and 30 mm in the interior acoustic mesh is adequate for this frequency. The acoustic wavelength must also be considered in selecting the overall size of the exterior domain. Accuracy of the solution requires placement of the radiating boundary at least one-quarter wavelength from the acoustic sources; in this problem a standoff distance of approximately 700 mm is selected. The characteristic flexural wavelength ¸p of the steel plating can be computed using the thickness h and the formula ¸p =

2¼ Eh2 1=4 p ( ) − 12½s

¼ 190mm

. The discretization requirements of the finite element method in wave problems require at least six nodes per wavelength; here, we use an internodal distance of approximately 30 mm for the shells. The fully coupled model consists of all three meshes shown in Figure 7.1.2-1, Figure 7.1.2-2, and Figure 7.1.2-3, constrained at their abutting surfaces using the *TIE option. The sequentially coupled analysis is performed in two jobs. The "global" model job consists of the meshes shown in Figure 7.1.2-2 and Figure 7.1.2-3. Displacements and displacement phases from the shell elements are saved from this analysis and drive the second "submodel" analysis through the use of the *BOUNDARY, SUBMODEL option. The second model consists of the exterior air mesh (Figure 7.1.2-1) used in the fully coupled case, with ASI8 elements placed on the boundary that abuts the shell surface. These elements convert the displacements from the "global" analysis to the appropriate boundary conditions for acoustic elements. In this analysis the ASI8 elements conform to the acoustic submodel mesh but not to the shell mesh of the global model. The nodes of the ASI8 elements are placed in a node set, specified in the model data by the *SUBMODEL option. The GLOBAL ELSET parameter must be used in this case to ensure that only the displacements of the ASI8 elements are driven by the shell elements. Without the GLOBAL ELSET parameter, ABAQUS may attempt to drive the acoustic pressure of the ASI8 elements by the interior acoustic elements, since those elements share the shell nodes in the "global" model.

Results and discussion It is good practice to check the absorbing boundary conditions used on a particular mesh at a desired frequency by analyzing only the exterior fluid mesh with some test forcing on the boundary where acoustic excitations are expected. If the forcing is at a single point, the pressure phase angles should show a pattern of concentric circles, minimally distorted by the radiating boundary. While not a rigorous numerical test, such a result usually coincides with a properly offset radiating boundary. As shown in Figure 7.1.2-4, this criterion is met by the mesh used in this analysis. Figure 7.1.2-5 is a plot of the radial displacement of the muffler inlet as a function of frequency for both the fully coupled and the global models. The resonant peak for the fully coupled model at 178.1 Hz is clearly illustrated. In contrast, the resonant peak for the "global" model (without the acoustic medium) occurs at approximately 178.2 Hz. The difference in the two peaks can be accounted for by the fact that the exterior air on the fully coupled model adds a small amount of damping, due to radiation, as well as mass to the system, which result in a lowered natural frequency, as well as a slightly lower peak response. It is clear from Figure 7.1.2-5 that for the frequency range of interest the

7-1081

Acoustic Analyses

coupling between the exterior air and the muffler is most important at 178.1 Hz. Figure 7.1.2-6 and Figure 7.1.2-7 contain contour plots of the pressure magnitude and phase for the muffler interior at 179.4 Hz for both the "global" model and the fully coupled model. In both cases the results indicate that the modeling assumptions of the sequentially coupled analysis appear to be valid for the solutions in the muffler interior. Contour plots of the pressure magnitude and phase for the muffler exterior at 179.4 Hz are shown in Figure 7.1.2-8 and Figure 7.1.2-9. The resulting pressure magnitude in the exterior air is small in both cases. The differences in the pressure amplitudes and phase as computed by the two analyses are not considered to be significant. Two factors that account for the small differences are the different modeling methods (fully coupled vs. sequentially coupled) and the different techniques used to couple the muffler to the exterior air (*TIE vs. acoustic interface elements). Figure 7.1.2-10 and Figure 7.1.2-11 contain contour plots of the pressure magnitude and phase for the muffler interior at 178.1 Hz for both the "global" model and the fully coupled model. It is clear that at 179.4 Hz, the modeling assumptions of the sequentially coupled analysis are less valid than they are at 178.1 Hz for the solutions in the muffler interior. This result is anticipated by Figure 7.1.2-5. However, the solutions are still reasonably close to one another, indicating that the sequentially coupled analysis is still a reasonable approximation for this system even at a resonant peak. Contour plots of the pressure magnitude and phase for the muffler exterior at 178.1 Hz are shown in Figure 7.1.2-12 and Figure 7.1.2-13. Again, the resulting pressure magnitude in the exterior air is small in both cases. The differences in the pressure amplitudes and phase as computed by the two analyses is less evident in the exterior than they were in the interior. The pressure magnitudes along the muffler centerline at both 178.1 Hz and 179.4 Hz are shown in decibels in Figure 7.1.2-14. The reference pressure is chosen at one unit for convenience. The plot illustrates the variation of acoustic pressure in the muffler near resonance. Table 7.1.2-1 shows comparative solution times and memory requirements for the fully and sequentially coupled analyses. The total computational time for the sequentially coupled case is lower, and the peak memory requirements are significantly lower. These differences will be greater for larger models. Optimal speed increases occur when global and submodels have nearly equal numbers of degrees of freedom. Here, solving the fully coupled system does not impose as much of a speed penalty as might be expected, because the sparse solver used by ABAQUS exploits the extreme sparsity of the fluid-solid coupling term. When the number of system nodes involving fluid-solid coupling is a large percentage of the total number of nodes, the sparsity of the coupling term decreases, favoring the sequentially coupled procedure. Sequentially coupled analyses are even more advantageous than fully coupled analyses when many different submodels need to be analyzed, driven by a single set of global results. ABAQUS issues a series of warning messages in this example, because the narrow wedge domain results in some three-dimensional acoustic elements with bad aspect ratios. These messages can be ignored in this study, since the solutions are essentially axisymmetric and the gradient of the solution in the circumferential direction is nearly zero. Moreover, elements with scalar degrees of freedom, such as the acoustic elements used in this example, are much less sensitive to geometric distortion than

7-1082

Acoustic Analyses

elements with vector degrees of freedom, such as continuum stress/displacement elements.

Input files muffler_full.inp Three-dimensional, fully coupled model. muffler_globl.inp Muffler and internal air global model. muffler_submo.inp Exterior air submodel. muffler_shell_nodes.inp Nodal coordinates for muffler shell mesh. muffler_intair_nodes.inp Nodal coordinates for interior air mesh. muffler_extair_nodes.inp Nodal coordinates for surrounding air mesh. muffler_shell_elem.inp Element definitions for muffler shell mesh. muffler_intair_elem.inp Element definitions for interior air mesh. muffler_extair_elem.inp Element definitions for surrounding air mesh. muffler_freq.inp Natural frequency extraction for shell mesh. muffler_bctest.inp Element definitions for surrounding air mesh.

Table Table 7.1.2-1 Comparison of relative CPU times (normalized with respect to the CPU time for the sequential analysis) and approximate problem size for the frequency sweep excluding preprocessing. Memory DOF Relative CPU Time Global model 10 Mb 10030 0.325 Submodel 15 Mb 19030 0.675 7-1083

Acoustic Analyses

Fully coupled model Sequential analysis

29 Mb

29060

1.086 1.000

Figures Figure 7.1.2-1 Mesh of surrounding air.

Figure 7.1.2-2 Mesh of muffler.

Figure 7.1.2-3 Mesh of interior air.

7-1084

Acoustic Analyses

Figure 7.1.2-4 Radiating boundary condition test at 165 Hz.

Figure 7.1.2-5 Radial displacement of the muffler inlet as a function of frequency.

Figure 7.1.2-6 Muffler internal pressure magnitudes at 179.4 Hz, muffler inlet at top: fully coupled solution on left, "global" model (without the exterior acoustic medium) on right.

7-1085

Acoustic Analyses

7-1086

Acoustic Analyses

Figure 7.1.2-7 Muffler internal pressure phase at 179.4 Hz, muffler inlet at top: fully coupled solution on left, "global" model (without the exterior acoustic medium) on right.

7-1087

Acoustic Analyses

7-1088

Acoustic Analyses

Figure 7.1.2-8 Muffler external pressure magnitudes at 179.4 Hz, muffler inlet at top: fully coupled solution on left, "global" model (without the exterior acoustic medium) on right.

Figure 7.1.2-9 Muffler external pressure phase at 179.4 Hz, muffler inlet at top: fully coupled solution

7-1089

Acoustic Analyses

on left, "global" model (without the exterior acoustic medium) on right.

Figure 7.1.2-10 Muffler internal pressure magnitudes at 178.1 Hz, muffler inlet at top: fully coupled solution on left, "global" model (without the exterior acoustic medium) on right.

7-1090

Acoustic Analyses

7-1091

Acoustic Analyses

Figure 7.1.2-11 Muffler internal pressure phase at 178.1 Hz, muffler inlet at top: fully coupled solution on left, "global" model (without the exterior acoustic medium) on right.

7-1092

Acoustic Analyses

7-1093

Acoustic Analyses

Figure 7.1.2-12 Muffler external pressure magnitudes at 178.1 Hz, muffler inlet at top: fully coupled solution on left, "global" model (without the exterior acoustic medium) on right.

Figure 7.1.2-13 Muffler external pressure phase at 178.1 Hz, muffler inlet at top: fully coupled

7-1094

Acoustic Analyses

solution on left, "global" model (without the exterior acoustic medium) on right.

Figure 7.1.2-14 Muffler internal pressure magnitude at 178.1 and 179.4 Hz: dB along muffler centerline.

7-1095

Acoustic Analyses

Sample listings

7-1096

Acoustic Analyses

Listing 7.1.2-1 *HEADING FULLY COUPLED ACOUSTIC ANALYSIS OF A MUFFLER M, KG, S ** ------------------------------------------** ** PART INSTANCE: INTERIORAIR-1 ** *NODE, INPUT=muffler_intair_nodes.inp *ELEMENT, TYPE=AC3D10, INPUT=muffler_intair_elem.inp ** ------------------------------------------*ELSET, ELSET=INTERIORAIR-1_I1, GENERATE 549, 1457, 1 *SOLID SECTION, ELSET=INTERIORAIR-1_I1, MATERIAL=AIRABSORB 1., ** ------------------------------------------*ELSET, ELSET=INTERIORAIR-1_I2, GENERATE 1, 548, 1 *SOLID SECTION, ELSET=INTERIORAIR-1_I2, MATERIAL=AIR 1., ** ------------------------------------------** ** PART INSTANCE: MUFFLERSHELL-1 ** *NODE,INPUT=muffler_shell_nodes.inp *ELEMENT, TYPE=S4R, INPUT=muffler_shell_elem.inp ** ------------------------------------------*ELSET, ELSET=MUFFLERSHELL-1_I1, GENERATE 1458, 1500, 1 *SHELL SECTION, ELSET=MUFFLERSHELL-1_I1, MATERIAL=STEEL 0.00075, 5 ** ------------------------------------------** ** PART INSTANCE: OUTERAIR-1 ** *NODE,INPUT=muffler_extair_nodes.inp *ELEMENT, TYPE=AC3D20, INPUT=muffler_extair_elem.inp

7-1097

Acoustic Analyses

** ------------------------------------------*ELSET, ELSET=OUTERAIR-1_I1, GENERATE 1501, 2734, 1 *SOLID SECTION, ELSET=OUTERAIR-1_I1, MATERIAL=AIR 1., ** ------------------------------------------*NSET, NSET=SHELLSYM,UNSORTED 3301,3376,3375,3299,3373,3297,3340,3339,3338, 3337,3336,3335,3334,3333,3332,3331,3330,3329, 3328,3327,3326,3325,3324,3323,3322,3321,3320, 3319,3318,3317,3316,3315,3314,3313,3312,3311, 3310,3309,3295,3307,3292,3304,3303,3291 ** ------------------------------------------*NSET, NSET=SHELLCONSTRAINT,UNSORTED 3302,3377,3378,3300,3374,3298,3341,3342,3343, 3344,3345,3346,3347,3348,3349,3350,3351,3352, 3353,3354,3355,3356,3357,3358,3359,3360,3361, 3362,3363,3364,3365,3366,3367,3368,3369,3370, 3371,3372,3296,3308,3293,3305,3306,3294 ** ------------------------------------------*NSET, NSET=SHELLDISP 3304,3325,3375 ** ------------------------------------------*NSET, NSET=CENTERLINE 10, 11, 118, 119, 120, 121, 122, 123, 124, 125, 126, 127, 128, 129, 130, 131, 132, 133, 134, 135, 136, 137, 138, 139, 140, 141, 142, 143, 144, 145, 146, 147, 148, 149, 150, 151, 152, 153, 154, 155, 156, 157, 158, 159, 160, 161, 162, 163, 164, 165, 166, 167, 168, 169, 170, 171, 172, 173, 174, 175, 176, 831, 832, 833, 834, 835, 836, 837, 838, 839, 840, 841, 842, 843, 844, 845, 846, 847, 848, 849, 850, 851, 852, 853, 854, 855, 856, 857, 858, 859, 860, 861, 862, 863, 864, 865, 866, 867, 868, 869, 870, 871, 872, 873, 874, 875, 876, 877, 878, 879, 880, 881, 882, 883, 884, 885, 886, 887, 888, 889, 890 ** ------------------------------------------*NSET, NSET=INLETPRESSURE 11, 12, 13, 177, 186, 618, 891, 892, 893, 913, 914, 915 ** -------------------------------------------

7-1098

Acoustic Analyses

*ELSET, ELSET=INNERAIROUTLET_S4 288, 299, 367 *SURFACE, NAME=INNERAIROUTLET INNERAIROUTLET_S4, S4 ** ------------------------------------------*ELSET, ELSET=INNERAIR2SHELL_S1 367, 374, 384, 385, 386, 387, 388, 392, 393, 894, 895, 896, 1192, 1195, 1196, 1197, 1198, 1201, 1202, 1203, 1210, 1213, 1214, 1216, 1237, 1238, 1239, 1240, 1243, 1248, 1250, 1330, 1331, 1334, 1337, 1341, 1359 *ELSET, ELSET=INNERAIR2SHELL_S4 370, 373, 375, 380, 383, 391, 559, 634, 894, 895, 1193, 1194, 1200, 1204, 1206, 1208, 1211, 1212, 1215, 1217, 1235, 1242, 1244, 1246, 1247, 1249, 1251, 1276, 1298, 1320, 1321, 1322, 1323, 1326, 1329, 1335, 1336, 1338, 1340, 1343, 1347, 1349 *ELSET, ELSET=INNERAIR2SHELL_S2 379, 592, 635, 858, 917, 1199, 1205, 1209, 1236, 1241, 1252, 1253, 1254, 1325, 1339, 1344, 1345, 1346, 1348, 1350, 1351, 1352, 1353, 1354, 1355, 1356, 1357, 1358, 1360, 1361, 1362 *ELSET, ELSET=INNERAIR2SHELL_S3 377, 378, 389, 390, 557, 560, 561, 568, 683, 888, 897, 1207, 1245, 1277, 1324, 1327, 1328, 1332, 1333, 1342, 1387, 1388 *SURFACE, NAME=INNERAIR2SHELL INNERAIR2SHELL_S1, S1 INNERAIR2SHELL_S4, S4 INNERAIR2SHELL_S2, S2 INNERAIR2SHELL_S3, S3 ** ------------------------------------------*ELSET, ELSET=SHELL2INNERAIR_SNEG, GENERATE 1458, 1500, 1 *SURFACE, NAME=SHELL2INNERAIR SHELL2INNERAIR_SNEG, SNEG *ELSET, ELSET=SHELL2OUTERAIR_SPOS, GENERATE 1458, 1500, 1 *SURFACE, NAME=SHELL2OUTERAIR SHELL2OUTERAIR_SPOS, SPOS ** ------------------------------------------*ELSET, ELSET=OUTERAIR2SHELL_S6

7-1099

Acoustic Analyses

2100,2116,2420 *ELSET, ELSET=OUTERAIR2SHELL_S3 2100,2420,2421,2422 *ELSET, ELSET=OUTERAIR2SHELL_S4, GENERATE 1519, 1975, 19 *SURFACE, NAME=OUTERAIR2SHELL OUTERAIR2SHELL_S6, S6 OUTERAIR2SHELL_S3, S3 OUTERAIR2SHELL_S4, S4 ** ------------------------------------------*ELSET, ELSET=SPHERE1_S3, GENERATE 2340, 2355, 1 *ELSET, ELSET=SPHERE1_S4, GENERATE 2664, 2734, 5 *SURFACE, NAME=SPHERE1 SPHERE1_S3, S3 SPHERE1_S4, S4 ** ------------------------------------------*ELSET, ELSET=SPHERE2_S3, GENERATE 2036, 2051, 1 *ELSET, ELSET=SPHERE2_S4, GENERATE 1979, 2035, 4 *SURFACE, NAME=SPHERE2 SPHERE2_S3, S3 SPHERE2_S4, S4 ** ------------------------------------------*ELSET, ELSET=CYLINDER_S6, GENERATE 1501, 1957, 19 *SURFACE, NAME=CYLINDER CYLINDER_S6, S6 ** ------------------------------------------*ELSET, ELSET=INNERAIRABSORB_S3 382, 394, 403, 404, 405, 408, 411, 415, 417, 418, 419, 423, 429, 430, 431, 437, 438, 439, 448, 451, 452, 456, 457, 458, 459, 461, 462, 463, 464, 467, 468, 473, 477, 478, 482, 483, 484, 498, 499, 502, 503, 505, 506, 507 *ELSET, ELSET=INNERAIRABSORB_S2 407, 428, 436, 443, 471, 476, 504 *ELSET, ELSET=INNERAIRABSORB_S1 402, 410, 414, 416, 422, 426, 434, 435, 440, 441, 444, 450, 453, 455, 460, 466, 472, 475, 479, 481, 485, 486, 487, 488, 490, 491, 492, 495, 496, 497,

7-1100

Acoustic Analyses

500 *ELSET, ELSET=INNERAIRABSORB_S4 427, 432, 433, 442, 445, 446, 447, 449, 454, 465, 469, 470, 474, 480, 489, 493, 494, 501 *SURFACE, NAME=INNERAIRABSORB INNERAIRABSORB_S3, S3 INNERAIRABSORB_S2, S2 INNERAIRABSORB_S4, S4 INNERAIRABSORB_S1, S1 ** ------------------------------------------** ** MATERIALS ** *MATERIAL, NAME=AIR *ACOUSTICMEDIUM,BULKMODULUS 1.42E5, *DENSITY 1.2, *MATERIAL, NAME=AIRABSORB *ACOUSTICMEDIUM,BULKMODULUS 1.42E5, *ACOUSTICMEDIUM,VOLUMETRICDRAG 1.2, *DENSITY 1.2, *MATERIAL, NAME=STEEL *DENSITY 7920., *ELASTIC 1.9E+11, 0.3 *IMPEDANCEPROPERTY,TYPE=SPH,NAME=SPHERE 0.7 *IMPEDANCEPROPERTY,TYPE=C,NAME=CY 0.7 ** ------------------------------------------*TIE,NAME=ACOST1 INNERAIR2SHELL, SHELL2INNERAIR OUTERAIR2SHELL, SHELL2OUTERAIR ** ** BOUNDARY CONDITIONS AND CONSTRAINTS ** *BOUNDARY SHELLSYM,ZSYMM

7-1101

Acoustic Analyses

*EQUATION 2 SHELLCONSTRAINT,1,0.176326981, SHELLCONSTRAINT,3,-1. 2 SHELLCONSTRAINT,2,1., SHELLSYM,2,-1. ** ------------------------------------------** ** STEP: STEP-1 ** *STEP STEP-1: FREQUENCY RESPONSE *STEADY STATE DYNAMICS, DIRECT, FREQUENCY SCALE=LINEAR 177.21,179.41,12 *BOUNDARY INLETPRESSURE,8,8,1.0 *SIMPEDANCE CYLINDER,CY *SIMPEDANCE SPHERE1,SPHERE *SIMPEDANCE SPHERE2,SPHERE *SIMPEDANCE INNERAIROUTLET, *OUTPUT,FIELD,OP=NEW,FREQUENCY=6 *NODE OUTPUT U,PU,POR,PPOR *OUTPUT,HISTORY,OP=NEW,FREQUENCY=1 *NODE OUTPUT,NSET=CENTERLINE POR, *NODE OUTPUT,NSET=SHELLDISP U, *NODE FILE,NSET=CENTERLINE,FREQUENCY=1 COORD,POR,PPOR *NODE FILE,NSET=SHELLDISP,FREQUENCY=1 U,PU *END STEP

7-1102

Soils Analyses

8. Soils Analyses 8.1 Soils analyses 8.1.1 Plane strain consolidation Product: ABAQUS/Standard Most consolidation problems of practical interest are two- or three-dimensional, so that the one-dimensional solutions provided by Terzaghi consolidation theory (see ``The Terzaghi consolidation problem,'' Section 1.14.1 of the ABAQUS Benchmarks Manual) are useful only as indicators of settlement magnitudes and rates. This problem examines a linear, two-dimensional consolidation case: the settlement history of a partially loaded strip of soil. This particular case is chosen to illustrate two-dimensional consolidation because an exact solution is available (Gibson et al., 1970), thus providing verification of this capability in ABAQUS.

Geometry and model The discretization of the semi-infinite, partially loaded strip of soil is shown in Figure 8.1.1-1. The loaded region is half as wide as the depth of the sample. The reduced-integration plane strain element with pore pressure, CPE8RP, is used in this analysis. Reduced integration is almost always recommended when second-order elements are used because it usually gives more accurate results and is less expensive than full integration. No mesh convergence studies have been done, although the reasonable agreement between the numerical results provided by this model and the solution of Gibson et al. (1970) suggests that the model used is adequate--at least for the overall displacement response examined. In an effort to reduce analysis cost while at the same time preserve accuracy, the mesh is graded from six elements through the height, under the load, to one element through the height at the outer boundary of the model, where a single infinite element (type CINPE5R) is used to model the infinite domain. This requires the use of two kinematic constraint features provided by ABAQUS. Consider first the displacement degrees of freedom along line AC in Figure 8.1.1-1. The 8-node isoparametric elements used for the analysis allow quadratic variation of displacement along their sides, so the displacements of nodes a and b in elements x and y may be incompatible with the displacement variation along side AC of element z. To avoid this, nodes a and b must be constrained to lie on the parabola defined by the displacements of nodes A, B, and C: The QUADRATIC MPC ("multi-point constraint") is used to enforce this kinematic constraint: it must be used at each node where this constraint is required (see planestrainconsolidation.inp ). Pore pressure values are obtained by linear interpolation of values at the corner nodes of an element. When mesh gradation is used, as along line AC in this example, an incompatibility in pore pressure values may result for the same reason given for the displacement incompatibility discussed above. To avoid this, the pore pressure at node B must be constrained to be interpolated linearly from the pore pressure values at A and C: This is done by using the P LINEAR MPC. The material properties assumed for this analysis are as follows: the Young's modulus is chosen as 690 GPa (108 lb/in2); the Poisson's ratio is 0; the material's permeability is 5.08 ´ 10-7 m/day (2.0 ´ 10-5 in/day); and the specific weight of pore fluid is chosen as 272.9 kN/m 3 (1.0 lb/in 3).

8-1103

Soils Analyses

The applied load has a magnitude of 3.45 MPa (500 lb/in 2). The strip of soil is assumed to lie on a smooth, impervious base, so the vertical component of displacement is prescribed to be zero on that surface. The left-hand side of the mesh is a symmetry line (no horizontal displacement). The infinite element models the other boundary.

Time stepping As in the one-dimensional Terzaghi consolidation solution (see ``The Terzaghi consolidation problem,'' Section 1.14.1 of the ABAQUS Benchmarks Manual), the problem is run in two steps. In the first *SOILS, CONSOLIDATION step, the load is applied and no drainage is allowed across the top surface of the mesh. This one increment step establishes the initial distribution of pore pressures which will be dissipated during the second *SOILS, CONSOLIDATION step. During the second step drainage is allowed to occur through the entire surface of the strip. This is specified by prescribing the pore pressure (degree of freedom 8) at all nodes on this surface (node set TOP) to be zero. By default in a *SOILS, CONSOLIDATION step such boundary conditions are applied immediately at the start of the step and then held fixed. Thus, the pore pressures at the surface change suddenly at the start of the second step from their values with no drainage (defined by the first step) to 0.0. Consolidation is a typical diffusion process: initially the solution variables change rapidly with time, while at the later times more gradual changes in stress and pore pressure are seen. Therefore, an automatic time stepping scheme is needed for any practical analysis, since the total time of interest in consolidation is typically orders of magnitude larger than the time increments that must be used to obtain reasonable solutions during the early part of the transient. ABAQUS uses a tolerance on the maximum change in pore pressure allowed in an increment, UTOL, to control the time stepping. When the maximum change of pore pressure in the soil is consistently less than UTOL the time increment is allowed to increase. If the pore pressure changes exceed UTOL, the time increment is reduced and the increment is repeated. In this way the early part of the consolidation can be captured accurately and the later stages are analyzed with much larger time steps, thereby permitting efficient solution of the problem. For this case UTOL is chosen as 0.344 MPa (50 lb/in 2), which is 10% of the applied load. This is a fairly coarse tolerance but results in an economical and reasonable solution. The choice of initial time step is important in consolidation analysis. As discussed in ``The Terzaghi consolidation problem,'' Section 1.14.1 of the ABAQUS Benchmarks Manual, the initial solution (immediately following a change in boundary conditions) is a local, "skin effect" solution. Due to the coupling of spatial and temporal scales, it follows that no useful information is provided by solutions generated with time steps smaller than the mesh and material-dependent characteristic time. Time steps very much smaller than this characteristic time provide spurious oscillatory results (see Figure 3.1.5-2). This issue is discussed by Vermeer and Verruijt (1981), who propose the criterion ¢t ¸

°! (¢h)2 ; 6Ek

where ¢h is the distance between nodes of the finite element mesh near the boundary condition change, E is the elastic modulus of the soil skeleton, k is the soil permeability, and °! is the specific

8-1104

Soils Analyses

weight of the pore fluid. In this problem ¢h is 8.5 mm (0.33 in), so--using the material properties shown in Figure 8.1.1-1-¢tinitial = 1 £ 10¡5

days.

We actually use an initial time step of 2 ´ 10-5 days, since the immediate transient just after drainage begins is not considered important in the solution.

Results and discussion The prediction of the time history of the vertical deflection of the central point under the load (point P in Figure 8.1.1-1) is plotted in Figure 8.1.1-2, where it is compared with the exact solution of Gibson et al. (1970). There is generally good agreement between the theoretical and finite element solutions, even though the mesh used in this analysis is rather coarse. Figure 8.1.1-2 also shows the time increments selected by the automatic scheme, based on the UTOL tolerance discussed above. The figure shows the effectiveness of the scheme: the time increment changes by two orders of magnitude over the analysis.

Input file planestrainconsolidation.inp Input data for this example.

References · Gibson, R. E., R. L. Schiffman, and S. L. Pu, "Plane Strain and Axially Symmetric Consolidation of a Clay Layer on a Smooth Impervious Base," Quarterly Journal of Mechanics and Applied Mathematics, vol. 23, pt. 4, pp. 505-520, 1970. · Vermeer, P. A., and A. Verruijt, "An Accuracy Condition for Consolidation by Finite Elements," International Journal for Numerical and Analytical Methods in Geomechanics, vol. 5, pp. 1-14, 1981.

Figures Figure 8.1.1-1 Plane strain consolidation example: geometry and properties.

8-1105

Soils Analyses

Figure 8.1.1-2 Consolidation history and time step variation history.

8-1106

Soils Analyses

Sample listings

8-1107

Soils Analyses

Listing 8.1.1-1 *HEADING PLANE STRAIN CONSOLIDATION *NODE 1, 13,,2. 801,2. 813,2.,2. 1401,4. 1413,4.,2. 1506,4.5,.8333 1601,5. 1603,5.,.5 1607,5.,1. 1610,5.,1.5 1613,5.,2. 2001,9. 2007,9.,1. 2013,9.,2. 2201,17. 2213,17.,2. *NGEN,NSET=LHS 1,13 *NGEN,NSET=TOP 13,813,100 813,1413,100 1413,1613,100 1613,2013,100 *NSET,NSET=N1,GENERATE 13,813,100 *NGEN,NSET=BOT 1,801,100 801,1401,100 1401,1601,100 1601,2001,100 *NSET,NSET=BOT1,GENERATE 1,1401,100 *NSET,NSET=TOP1,GENERATE 13,1413,100 *NFILL BOT1,TOP1,12,1 *NGEN

8-1108

Soils Analyses

1607,2007,100 *NSET,NSET=ALLN,GENERATE 1,9999 ** *ELEMENT,TYPE=CPE8RP,ELSET=SOIL 1,1,201,203,3,101,202,103,2 101,801,1001,1005,805,901,1003,905,803 201,1401,1601,1607,1405,1501,1603,1506,1403 202,1405,1607,1613,1413,1506,1610,1513,1409 301,1601,1801,1813,1613,1701,1807,1713,1607 *ELGEN,ELSET=SOIL 1,6,2,1,4,200,10 101,3,4,1,3,200,10 301,2,200 *ELEMENT,TYPE=CINPE5R,ELSET=SOILIN 401,2013,2001,2201,2213,2007 *SOLID SECTION,ELSET=SOIL,MATERIAL=A1 *SOLID SECTION,ELSET=SOILIN,MATERIAL=A1IN ** *MATERIAL,NAME=A1 *ELASTIC 1.E8, *PERMEABILITY,SPECIFIC=1.0 2.E-5, *MATERIAL,NAME=A1IN *ELASTIC 1.E8, *INITIAL CONDITIONS,TYPE=RATIO ALLN,1.5 *MPC QUADRATIC,802,801,803,805 QUADRATIC,804,801,803,805 QUADRATIC,806,805,807,809 QUADRATIC,808,805,807,809 QUADRATIC,810,809,811,813 QUADRATIC,812,809,811,813 QUADRATIC,1407,1405,1409,1413 QUADRATIC,1411,1405,1409,1413 QUADRATIC,1603,1601,1607,1613 QUADRATIC,1610,1601,1607,1613 P LINEAR,803,801,805 P LINEAR,807,805,809 P LINEAR,811,809,813

8-1109

Soils Analyses

P LINEAR,1409,1405,1413 P LINEAR,1607,1601,1613 *RESTART,WRITE,FREQUENCY=3 ** *STEP SET UP INITIAL PORE PRESSURES *SOILS,CONSOLIDATION 1.E-7,1.E-7 *BOUNDARY LHS,1 BOT,2 *DLOAD 6,P3,500. 16,P3,500. *EL PRINT,FREQUENCY=0 *NODE PRINT,NSET=N1 U,POR,RVT *NODE FILE,FREQUENCY=2,NSET=N1 U, POR, *OUTPUT,FIELD,FREQ=2 *NODE OUTPUT,NSET=N1 U, POR, *END STEP ** *STEP,INC=300 *SOILS,CONSOLIDATION,UTOL=50.,END=SS 2.E-5, 1.E-1,,, 1.E-2 *BOUNDARY TOP,8 *END STEP

8.1.2 Calculation of phreatic surface in an earth dam Product: ABAQUS/Standard This example illustrates the use of ABAQUS to solve for the flow through a porous medium in which fluid flow is occurring in a gravity field and only part of the region is fully saturated, so the location of the phreatic surface is a part of the solution. Such problems are common in hydrology (an example is the well draw-down problem, where the phreatic surface of an aquifer must be located, based on pumping rates at particular well locations) and in some problems of dam design, as in this example. The basic approach takes advantage of the ABAQUS capability to perform partially and fully saturated analysis: the phreatic surface is located at the boundary of the fully saturated part of the model. This

8-1110

Soils Analyses

approach has the advantage that the capillary zone, just above the phreatic surface, is also identified.

Boundary conditions A typical dam is shown in Figure 8.1.2-1. We consider fluid flow only: deformation of the dam is ignored. Thus, although we use the fully coupled pore fluid flow-deformation elements, all displacement degrees of freedom are prescribed to be zero. A more general analysis would include stress and deformation of the dam. The upstream face of the dam (surface S1 in Figure 8.1.2-1) is exposed to water in the reservoir behind the dam. Since ABAQUS uses a total pore pressure formulation, the pore pressure on this face must be prescribed to be uw = (H1 ¡ z )g½w , where H1 is the elevation of the water surface, z is elevation, g is the gravitational acceleration, and ½w is the mass density of the water. (g½w , the weight density of the water, must be given as the value of the SPECIFIC parameter on the *PERMEABILITY option.) Likewise, on the downstream face of the dam (surface S2 in Figure 8.1.2-1), uw = (H2 ¡ z )g½w : The bottom of the dam (surface S3 ) is assumed to rest on an impermeable foundation. Since the natural boundary condition in the pore fluid flow formulation provides no flow of fluid across a surface of the model, no further specification is needed on this surface. The phreatic surface in the dam, S4 , is found as the locus of points at which the pore fluid pressure, uw , is zero. Above this surface the pore fluid pressure is negative, representing capillary tension causing the fluid to rise against the gravitational force and creating a capillary zone. The saturation associated with particular values of capillary pressure for absorption and exsorption of fluid from the porous medium is a physical property of the material and is defined in the *SORPTION option. A special boundary condition is needed if the phreatic surface reaches an open, freely draining surface, as indicated on surface S5 in Figure 8.1.2-1. In such a case the pore fluid can drain freely down the face of the dam, so uw =0 at all points on this surface below its intersection with the phreatic surface. Above this point uw <0, with its particular value depending on the solution. This example is specifically chosen to include this effect to illustrate the use of the ABAQUS drainage-only flow boundary condition. This drainage-only flow condition consists of prescribing the flow velocity on the freely draining surface in a way that approximately satisfies the requirement of zero pore pressure on the completely saturated portion of this surface (Pagano, 1997). The flow velocity is defined as a function of pore pressure, as shown in Figure 8.1.2-2. For negative pore pressures (those above the phreatic surface) the flow velocity is zero--the proper natural boundary condition. For positive pore pressures (those below the phreatic surface) the flow velocity is proportional to the pore pressure value. When this proportionality coefficient, ks , is large compared to k=°w c--where k is the permeability of the medium, °w is the specific weight of the fluid, and c is a characteristic length scale--the requirement of zero pore pressure on the free-drainage surface below the phreatic surface will be satisfied approximately. The drainage-only seepage coefficient in this model is specified as ks =10-1 m3/Nsec. This value is roughly 10 5 times larger than the characteristic value, k=°w c, based on the material properties listed below and an element length scale ¼10-1 m. This condition is prescribed using the *FLOW option with the drainage-only flow type label (QnD) as shown in phreaticsurf_cpe8rp.inp.

8-1111

Soils Analyses

Geometry and model The geometry of the particular earth dam considered is shown in Figure 8.1.2-3. This case is chosen because an analytical solution is available for comparison (Harr, 1962). The dam is filled to two-thirds of its height. Only a part of its base is impermeable. Since the dam is assumed to be long, we use CPE8RP coupled pore pressure/displacement plane strain elements (the mesh is shown in Figure 8.1.2-4). In addition, an input file containing element type CPE4P is included for verification purposes. Additional input files are included to demonstrate the use of *CONTACT PAIR and *TIE in coupled pore pressure-displacement analyses.

Material The permeability of the fully saturated earth of which the dam is made is 0.2117 ´ 10-3 m/sec. The default assumption is used for the partially saturated permeability: that it varies as a cubic function of saturation, decreasing from the fully saturated value to a value of zero at zero saturation. The specific weight of the water is 10 kN/m 3. The capillary action in the dam is defined by a single absorption/exsorption curve that varies linearly between a negative pore pressure of 10 kN/m 2 at a saturation of 0.05 and zero pore pressure at fully saturated conditions. This is not a very realistic model of physical absorption/exsorption behavior, but this will not affect the results of the steady-state analysis significantly insofar as the location of the phreatic surface is concerned. Accurate definition of this behavior would be required if definition of the capillary zone created by filling and emptying the dam at given rates is needed. The initial void ratio of the earth material is 1.0. The initial conditions for pore pressure and saturation are assumed to be those corresponding to the dam being fully saturated to the upstream water level: the initial saturation is, therefore, 1.0; and the initial pore pressures vary between zero at the water level and a maximum value of 12.19 kN/m 2 at the base of the dam.

Loading and controls The weight of the water is applied by GRAV loading, and the upstream and downstream pore pressures are prescribed as discussed above. A steady-state *SOILS analysis is performed in five increments to allow ABAQUS to resolve the high degree of nonlinearity in the problem.

Results and discussion The steady-state contours of pore pressure are shown in Figure 8.1.2-5. The upper-right part of the dam shows negative pore pressures, indicating that it is partly saturated or dry. The phreatic surface is best shown in Figure 8.1.2-6, where we have chosen to draw the contours in the vicinity of zero pore pressure. This phreatic surface compares well with the analytical phreatic surface calculated by Harr (1962), shown in Figure 8.1.2-2. Figure 8.1.2-7 shows contours of saturation that indicate a region of fully saturated material under the phreatic zone and decreasing saturation in and above the phreatic zone.

Input files

8-1112

Soils Analyses

phreaticsurf_cpe8rp.inp Phreatic surface calculation (element type CPE8RP). phreaticsurf_cpe4p.inp Element type CPE4P. phreaticsurf_cpe4p_contactpair.inp Element type CPE4P using the *CONTACT PAIR option. phreaticsurf_cpe4p_tie.inp Element type CPE4P using the *TIE option.

References · Harr, M. E., Groundwater and Seepage, McGraw-Hill, New York, 1962. · Pagano, L., "Steady State and Transient Unconfined Seepage Analyses for Earthfill Dams," ABAQUS Users' Conference, Milan, pp. 577-585, 1997.

Figures Figure 8.1.2-1 Phreatic surface problem.

Figure 8.1.2-2 Pore pressure-flow velocity relationship defined on the drainage-only surface.

8-1113

Soils Analyses

Figure 8.1.2-3 Configuration of earth dam and analytical phreatic surface.

Figure 8.1.2-4 Finite element mesh.

Figure 8.1.2-5 Pore pressure contours at steady state.

8-1114

Soils Analyses

Figure 8.1.2-6 Pore pressure contours showing phreatic surface (displayed by setting CMIN= -10, CMAX= 10).

Figure 8.1.2-7 Saturation contours at steady state (displayed by setting CMIN= -0.6, CMAX= 0.9).

Sample listings

8-1115

Soils Analyses

Listing 8.1.2-1 *HEADING EARTH DAM STEADY STATE FREE SURFACE SEEPAGE *** UNITS: M, KG, SEC, NEWTON *NODE,NSET=ALLN 1,0.,0. 39,4.8768,0. 601,1.8288,1.8288 639,3.048,1.8288 *NGEN,NSET=BOT 1,39,1 *NGEN,NSET=TOP 601,639,1 *NFILL,NSET=ALLN BOT,TOP,12,50 *NSET,NSET=PORN0,GENERATE 1,39,2 *NSET,NSET=PORN1,GENERATE 101,139,2 *NSET,NSET=PORN2,GENERATE 201,239,2 *NSET,NSET=PORN3,GENERATE 301,339,2 *NSET,NSET=PORN4,GENERATE 401,439,2 *NSET,NSET=PORN5,GENERATE 501,539,2 *NSET,NSET=PORN6,GENERATE 601,639,2 *NSET,NSET=PORN PORN0, PORN1, PORN2, PORN3 *NSET,NSET=OUTN,GENERATE 1,601,100 21,621,100 *ELEMENT,TYPE=CPE8RP,ELSET=DAM 1,1,3,103,101,2,53,102,51 *ELGEN,ELSET=DAM 1,19,2,1,6,100,20 *ELSET,ELSET=FSIDE,GENERATE 19,119,20 *ELSET,ELSET=FBOT,GENERATE

8-1116

Soils Analyses

16,19 *ELSET,ELSET=OUTE,GENERATE 11,111,20 *SOLID SECTION,ELSET=DAM,MATERIAL=FILL *MATERIAL,NAME=FILL *ELASTIC 1000., *DENSITY 2000., *PERMEABILITY,SPECIFIC=10000. 2.1167E-4, *SORPTION -100000.,.04 -10000.,.05 0.,1. *INITIAL CONDITIONS,TYPE=SATURATION ALLN,1. *INITIAL CONDITIONS,TYPE=PORE PRESSURE PORN, 12192.0, 0.0, 0.0, 1.2192 PORN4,0. PORN5,0. PORN6,0. *INITIAL CONDITIONS,TYPE=RATIO ALLN,1. *BOUNDARY ALLN,1 ALLN,2 *RESTART,WRITE,FREQUENCY=10 *STEP,INC=5 *SOILS .2,1. *DLOAD DAM,GRAV,10.,0.,-1.,0. *BOUNDARY 1,8,,12192. 101,8,,9144. 201,8,,6096. 301,8,,3048. 401,8,,0. *FLOW FSIDE,Q2D,0.1 FBOT,Q1D,0.1 *CONTROLS,ANALYSIS=DISCONTINUOUS

8-1117

Soils Analyses

*NODE PRINT,FREQUENCY=10,NSET=OUTN POR, *EL PRINT,FREQUENCY=10,ELSET=OUTE SAT,POR *NODE FILE,FREQUENCY=10,NSET=OUTN POR, *OUTPUT,FIELD,FREQ=10 *NODE OUTPUT,NSET=OUTN POR, *EL FILE,FREQUENCY=10,ELSET=OUTE SAT,POR *OUTPUT,FIELD,FREQ=10 *ELEMENT OUTPUT,ELSET=OUTE SAT,POR *END STEP

8.1.3 Axisymmetric simulation of an oil well Product: ABAQUS/Standard This example simulates the settlement of soil near an oil well. It is assumed that the oil in question is too thick for normal pumping. Therefore, steam is injected in the soil in the vicinity of the well to increase the temperature and decrease the oil's viscosity. As a result creep becomes an important component of the soil inelastic deformation and in the prediction of the effects of the oil pumping. Five years of oil pumping are simulated. This coupled displacement/diffusion analysis illustrates the use of ABAQUS to solve problems involving fluid flow through a saturated porous medium, inelastic material properties with time-dependent creep behavior, and thermal loading. No experimental data exist to compare with the numerical results of this example.

Geometry and model The example considers an axisymmetric model of an oil well and the surrounding soil, as shown in Figure 8.1.3-1. The radius of the well is 81 m (265 ft), and the well extends from a depth of 335 m (1100 ft) to 732 m (2500 ft). A depth of 1463 m (4800 ft) is modeled with 11 different soil layers. Reduced-integration axisymmetric elements with pore pressure, CAX8RP, are used to model the soil in the vicinity of the well. The far-field region is modeled with axisymmetric infinite elements, CINAX5R, to provide lateral stiffness. Reduced integration is almost always recommended when second-order elements are used, because it usually gives more accurate results and is less expensive than full integration. A coarse mesh is selected for the illustrative purpose of this example. No mesh convergence study has been performed. Soil layers designated by S1, T1, U1, and L1 are modeled using the Drucker-Prager plasticity model and are specified on the *DRUCKER PRAGER option. Both the elastic and inelastic material properties are tabulated in Table 8.1.3-1. The linear form of the Drucker-Prager model with no intermediate principal stress effect (K = 1.0) is used. The model assumes nonassociated flow;

8-1118

Soils Analyses

consequently, the material stiffness matrix is not symmetric. The use of UNSYMM=YES on the *STEP option improves the convergence of the nonlinear solution significantly. The hardening/softening behavior is specified by the *DRUCKER PRAGER HARDENING option, and the data are listed in Table 8.1.3-1. No creep data are provided for these layers since these are far removed from the loading. These layers are assumed to be saturated with water. A high permeability is assumed for the two top soil layers S1 and T1, while a low permeability is assigned to layers U1 and L1. Layers D1 through D7 are modeled with the modified Drucker-Prager Cap plasticity model. The material property data are tabulated in Table 8.1.3-2and are specified by the *CAP PLASTICITY option. As required by the creep model, no intermediate principal stress effect is included (i.e., K = 1.0), and no transition region on the yield surface is defined (i.e., ® = 0.0). The material's volumetric strain-driven hardening/softening behavior is specified with the *CAP HARDENING option, and the data are listed in Table 8.1.3-2. The initial cap yield surface position, "in vol (0) , is set to 0.02. ABAQUS automatically adjusts the position of the cap yield surface if the stress lies outside the cap surface. Consolidation creep is modeled with a Singh-Mitchell type creep model. The creep material data are specified with the *CAP CREEP option and are dependent on temperature. The following creep data are specified: A=2.2E¡7 1/day, ®=3.05 1/MPa (0.021 1/psi), t1 =1.0 day, n=1.0 at 10°C (50°F) A=3.5E¡4 1/day, ®=3.05 1/MPa (0.021 1/psi), t1 =1.0 day, n=1.0, at 100°C (212°F) These layers consist of rich organic matter and are saturated with oil. The temperature-dependent permeability data are specified by the *PERMEABILITY option. A uniform thermal expansion coefficient of 5.76E-6 1/°C (3.2E-6 1/°F) and a constant weight density 1.0 metric ton/m3 (64.6 lbs/ft 3) are assumed for all layers. For a coupled diffusion/displacement analysis care must be taken when choosing the units of the problem. The coupled equations may be numerically ill-conditioned if the choice of the units is such that the numbers generated by the equations of the two different fields differ by many orders of magnitude. The units chosen for this example are inches, pounds, and days.

Initial conditions An initial geostatic stress field is defined through the *INITIAL CONDITIONS option and is based on the soil weight density integrated over the depth. A coefficient of lateral stress of 0.85 is assumed. An initial void ratio of 1.5 is used throughout all soil layers with an initial uniform temperature field of 10°C (50°F).

Loading The problem is run in five steps. The first step of the analysis is a *GEOSTATIC step to equilibrate geostatic loading of the finite element model. This step also establishes the initial distribution of pore pressure. Since gravity loading is defined with distributed load type BZ and not with gravity load type GRAV, the pore fluid pressure reported by ABAQUS is defined as the pore pressure in excess of the hydrostatic pressure required to support the weight of pore fluid above the elevation of the material point. The second step is a *SOILS, CONSOLIDATION step to equilibrate any creep effects induced from

8-1119

Soils Analyses

the initial geostatic loading step. The choice of the initial time step is important in a consolidation analysis. Because of the coupling of spatial and temporal scales, no useful information is provided by solutions generated with time steps that are smaller than the mesh and material-dependent characteristic time. Time steps that are very much smaller than this characteristic time provide spurious oscillatory results. For further discussion on calculating the minimum time step, refer to ``Coupled pore fluid diffusion and stress analysis,'' Section 6.7.1 of the ABAQUS/Standard User's Manual. For this example a minimum initial time step of one day was selected. The third step of the analysis models the injection of steam into the well region between a depth of 366 m to 732 m (1200 ft to 2400 ft). The region is indicated by the shaded area in Figure 8.1.3-1. The nodes in this region are heated to 100°C (212°F) during a *SOILS, CONSOLIDATION analysis. The NO CREEP parameter is included; therefore, creep effects are not considered. The injection of the steam increases the permeability of the oil and increases the soil creep behavior. The fourth step simulates the pumping of oil by prescribing an excess pore pressure of -1.2 MPa (-170 psi) at nodes located at the depth of 427 m to 550 m (1400 ft to 1800 ft) below the surface. The pressure produces a pumping rate of approximately 172.5 thousand barrels per day at the end of the fifth year. The final step consists of a consolidation analysis performed over a five-year period to investigate the settlement that results from pumping and creep effects in the vicinity of the well.

Results and discussion The two initial steps show negligible deformations, indicating that the model is in geostatic equilibrium. Figure 8.1.3-2shows a contour plot of the soil settlement resulting from consolidation after the five-year period. A settlement of 0.13 m (0.4 ft) is expected at the surface. A maximum soil dislocation of 0.24 m (0.78 ft) occurs above the pump intake. Figure 8.1.3-3shows a contour plot of the excess pore pressure. The negative pore pressure represents the suction of the pump. During the five-year period, a total of 313.5 million barrels of oil are pumped (as determined from nodal output variable RVT). Figure 8.1.3-4 through Figure 8.1.3-6 show contour plots of the vertical stress components, plastic strains, and creep strains, respectively. Plastification occurs in soil layers D3 through D5. Significant creep occurs in the area in which steam is injected.

Input files axisymoilwell.inp Finite element analysis. axisymoilwell_thermalexp.inp Same as axisymoilwell.inp except that the thermal expansion of the pore fluid is also included.

Tables Table 8.1.3-1 Soil data using Drucker-Prager model.

8-1120

Soils Analyses

Soil layer S1 T1 U1

L1

Elastic

Inelastic propertie properties s E = 124 MPa ¯ = 42.0° º = 0.3 K=1.0 ' = 0.0° E = 2068 MPa ¯ = 36.0° º = 0.25 K=1.0 ' = 0.0° E = 468.8 ¯ = 38.0° MPa º = 0.22 K=1.0 ' = 0.0° E = 2482 MPa ¯ = 38.0° º = 0.29 K=1.0 ' = 0.0°

Hardening behavior 0.075 MPa, 0.0 0.083 MPa, 0.058 0.075 MPa, 0.116 0.48 MPa, 0.0 0.62 MPa, 0.058 0.48 MPa., 0.116 1.97 MPa, 0.0 3.17 MPa, 0.0037 2.47 MPa, 0.04 1.97 MPa, 0.0 3.17 MPa, 0.0037 2.47 MPa, 0.04

Table 8.1.3-2 Soil data using modified Drucker-Prager cap model. Soil layer Elastic Inelastic properties properties ® = 0.0 D1 E = 328 MPa d = 1.38 MPa º = 0.17 ¯ = 36.9° K=1.0 "in R = 0.33 vol (0) = 0.02 D2

E = 434 MPa º = 0.17

d = 1.38 MPa ¯ = 39.4° R = 0.33

® = 0.0 K=1.0 "in vol (0) = 0.02

D3

E = 546 MPa º = 0.19

d = 1.38 MPa ¯ = 42.0° R = 0.34

® = 0.0 K=1.0 "in vol (0) = 0.02

D4

E = 411 MPa º = 0.2

d = 1.2 MPa ¯ = 40.1° R = 0.3

® = 0.0 K=1.0 "in vol (0) = 0.02

D5

E = 494 MPa º = 0.17

d = 1.38 MPa ¯ = 40.4° R = 0.3

® = 0.0 K=1.0 "in vol (0) = 0.02

D6

E = 775 MPa º = 0.17

d = 17 MPa ¯ = 50.2°

® = 0.0 K=1.0

R = 0.23

"in vol (0) = 0.02

d = 1.7 MPa ¯ = 58.5°

® = 0.0 K=1.0

D7

E = 1,121 MPa º = 0.17

8-1121

Hardening behavior 2.75 MPa, 0.0 4.14 MPa, 0.02 5.51 MPa, 0.05 6.20 MPa, 0.09 1.38 MPa, 0.0 4.14 MPa, 0.02 6.89 MPa, 0.04 55.1 MPa, 0.1 1.38 MPa, 0.0 3.45 MPa, 0.02 13.8 MPa, 0.04 62.0 MPa, 0.06 1.38 MPa, 0.0 5.03 MPa, 0.02 6.90 MPa, 0.10 62.0 MPa, 0.3 2.75 MPa, 0.0 4.83 MPa, 0.02 5.15 MPa, 0.04 62.0 MPa, 0.08 2.76 MPa, 0.0 4.14 MPa, 0.005 7.58 MPa, 0.02 62.0 MPa, 0.05 3.44 MPa, 0.0 4.14 MPa, 0.006

Soils Analyses

R = 0.23

"in vol (0) = 0.02

Figures Figure 8.1.3-1 Axisymmetric model of oil well and surrounding soil.

Figure 8.1.3-2 Soil settlement after five-year period.

Figure 8.1.3-3 Contour plot of the pore pressure.

8-1122

7.58 MPa, 0.012 67.6 MPa, 0.03

Soils Analyses

Figure 8.1.3-4 Contour plot of the vertical stress components.

Figure 8.1.3-5 Contour plot of the vertical plastic strain components.

8-1123

Soils Analyses

Figure 8.1.3-6 Contour plot of the vertical creep strain components.

Sample listings

8-1124

Soils Analyses

Listing 8.1.3-1 *HEADING EXAMPLE-AXISYMMETRIC SIMULATION OF OIL WELL UNITS: F = lbs, L = in., T = days *NODE 1, 0.0, 0.0, 0.0 9, 3180.0, 0.0, 0.0 11, 9216.0, 0.0, 0.0 13, 21504.0, 0.0, 0.0 15, 46080.0, 0.0, 0.0 17, 95232.0, 0.0, 0.0 *NGEN 1, 9, 1 9, 11, 1 11, 13, 1 13, 15, 1 15, 17, 1 *NSET,NSET=CORNODES, GENERATE 1, 17, 2 *NSET,NSET=MIDNODES, GENERATE 2, 16, 2 *NSET,NSET=BASE CORNODES, MIDNODES, *NCOPY, CHANGE NUMBER=100, OLD SET=CORNODES, NEW SET=MID, SHIFT 0,7200. *NCOPY, CHANGE NUMBER=200, OLD SET=CORNODES, NEW SET=CORNER, SHIFT 0,14400. *NCOPY, CHANGE NUMBER=300, OLD SET=CORNODES, NEW SET=MID, SHIFT 0,18000. *NCOPY, CHANGE NUMBER=400, OLD SET=CORNODES, NEW SET=CORNER, SHIFT 0,21600. *NCOPY, CHANGE NUMBER=500, OLD SET=CORNODES, NEW SET=MID, SHIFT

8-1125

Soils Analyses

0,25200. *NCOPY, CHANGE NUMBER=600, OLD SET=CORNODES, NEW SET=CORNER, SHIFT 0,28800. *NCOPY, CHANGE NUMBER=700, OLD SET=CORNODES, NEW SET=MID, SHIFT 0,31200. *NCOPY, CHANGE NUMBER=800, OLD SET=CORNODES, NEW SET=CORNER, SHIFT 0,33600. *NCOPY, CHANGE NUMBER=900, OLD SET=CORNODES, NEW SET=MID, SHIFT 0,34800. *NCOPY, CHANGE NUMBER=1000, OLD SET=CORNODES, NEW SET=CORNER, SHIFT 0,36000. *NCOPY, CHANGE NUMBER=1100, OLD SET=CORNODES, NEW SET=MID, SHIFT 0,38400. *NCOPY, CHANGE NUMBER=1200, OLD SET=CORNODES, NEW SET=CORNER, SHIFT 0,40800. *NCOPY, CHANGE NUMBER=1300, OLD SET=CORNODES, NEW SET=MID, SHIFT 0,42000. *NCOPY, CHANGE NUMBER=1400, OLD SET=CORNODES, NEW SET=CORNER, SHIFT 0,43200. *NCOPY, CHANGE NUMBER=1500, OLD SET=CORNODES, NEW SET=MID, SHIFT 0,43800. *NCOPY, CHANGE NUMBER=1600, OLD SET=CORNODES,

8-1126

Soils Analyses

NEW SET=CORNER, SHIFT 0,44400. *NCOPY, CHANGE NUMBER=1700, OLD SET=CORNODES, NEW SET=MID, SHIFT 0,46800. *NCOPY, CHANGE NUMBER=1800, OLD SET=CORNODES, NEW SET=CORNER, SHIFT 0,49200. *NCOPY, CHANGE NUMBER=1900, OLD SET=CORNODES, NEW SET=MID, SHIFT 0,52500. *NCOPY, CHANGE NUMBER=2000, OLD SET=CORNODES, NEW SET=CORNER, SHIFT 0,55800. *NCOPY, CHANGE NUMBER=2100, OLD SET=CORNODES, NEW SET=MID, SHIFT 0,56700. *NCOPY, CHANGE NUMBER=2200, OLD SET=CORNODES, NEW SET=CORNER, SHIFT 0,57600. *NCOPY, CHANGE NUMBER=200, OLD SET=MIDNODES, NEW SET=MID, SHIFT 0,14400. *NCOPY, CHANGE NUMBER=400, OLD SET=MIDNODES, NEW SET=MID, SHIFT 0,21600. *NCOPY, CHANGE NUMBER=600, OLD SET=MIDNODES, NEW SET=MID, SHIFT 0,28800. *NCOPY, CHANGE NUMBER=800, OLD SET=MIDNODES, NEW SET=MID, SHIFT 0,33600.

8-1127

Soils Analyses

*NCOPY, CHANGE NUMBER=1000, OLD SET=MIDNODES, NEW SET=MID, SHIFT 0,36000. *NCOPY, CHANGE NUMBER=1200, OLD SET=MIDNODES, NEW SET=MID, SHIFT 0,40800. *NCOPY, CHANGE NUMBER=1400, OLD SET=MIDNODES, NEW SET=MID, SHIFT 0,43200. *NCOPY, CHANGE NUMBER=1600, OLD SET=MIDNODES, NEW SET=MID, SHIFT 0,44400. *NCOPY, CHANGE NUMBER=1800, OLD SET=MIDNODES, NEW SET=MID, SHIFT 0,49200. *NCOPY, CHANGE NUMBER=2000, OLD SET=MIDNODES, NEW SET=MID, SHIFT 0,55800. *NCOPY, CHANGE NUMBER=2200, OLD SET=MIDNODES, NEW SET=MID, SHIFT 0,57600. *NSET,NSET=AXIS,GENERATE 1, 2201, 100 *NSET, NSET=NALL MID, MIDNODES, CORNER, CORNODES, *NSET,NSET=FREESURF,GENERATE 2201, 2215, 2 ** ** REGION WHERE STEAM IS INJECTED ** *NSET, NSET=TARGET 601,602,603,604,605,606,607,608,609 701,702,703,704,705,706,707,708,709

8-1128

Soils Analyses

801,802,803,804,805,806,807,808,809 901,902,903,904,905,906,907,908,909 1001,1002,1003,1004,1005,1006,1007,1008,1009 1101,1102,1103,1104,1105,1106,1107,1108,1109 1201,1202,1203,1204,1205,1206,1207,1208,1209 1301,1302,1303,1304,1305,1306,1307,1308,1309 1401,1402,1403,1404,1405,1406,1407,1408,1409 1501,1502,1503,1504,1505,1506,1507,1508,1509 1601,1602,1603,1604,1605,1606,1607,1608,1609 ** ** ELEMENTS GENERATION ** *ELEMENT,TYPE=CAX8RP 1, 1,3,203,201,2,103,202,101 *ELGEN, ELSET=ESOIL 1, 7,2,1,11,200,100 *ELEMENT, TYPE=CINAX5R, ELSET=FAR 8, 215, 15, 17, 217, 115 108, 415, 215, 217, 417, 315 208, 615, 415, 417, 617, 515 308, 815, 615, 617, 817, 715 408, 1015, 815, 817, 1017, 915 508, 1215, 1015, 1017, 1217, 1115 608, 1415, 1215, 1217, 1417, 1315 708, 1615, 1415, 1417, 1617, 1515 808, 1815, 1615, 1617, 1817, 1715 908, 2015, 1815, 1817, 2017, 1915 1008, 2215, 2015, 2017, 2217, 2115 *ELSET, ELSET=L1, GENERATE 1,7,1 *ELSET, ELSET=U1, GENERATE 101,107,1 *ELSET, ELSET=D7, GENERATE 201,207,1 *ELSET, ELSET=D6, GENERATE 301,307,1 *ELSET, ELSET=D5, GENERATE 401,407,1 *ELSET, ELSET=D4, GENERATE 501,507,1 *ELSET, ELSET=D3, GENERATE 601,607,1 *ELSET, ELSET=D2, GENERATE

8-1129

Soils Analyses

701,707,1 *ELSET, ELSET=D1, GENERATE 801,807,1 *ELSET, ELSET=T1, GENERATE 901,907,1 *ELSET, ELSET=S1, GENERATE 1001,1007,1 ** ** SOIL STRATA L1 (3600 ft - 4800 ft) ** ---------------------------------*MATERIAL,NAME=L1 *ELASTIC 360000.,0.29 *DRUCKER PRAGER, SHEAR CRITERION=LINEAR 38.,1.,0. *DRUCKER PRAGER HARDENING 286.,0. 460.,0.0037 358.,0.04 *PERMEABILITY,SPECIFIC=3.61e-2 15.2, *EXPANSION 0.32E-05, ** ** SOIL STRATA U1 (3000 ft - 3600 ft) ** ---------------------------------*MATERIAL,NAME=U1 *ELASTIC 68000.,0.22 *DRUCKER PRAGER 38.,1.,0. *DRUCKER PRAGER HARDENING 286.,0. 460.,0.0037 358.,0.04 *PERMEABILITY,SPECIFIC=3.61e-2 15.2, *EXPANSION 0.32E-05, ** ** SOIL STRATA D7 (2400 ft - 3000 ft) ** ---------------------------------*MATERIAL,NAME=D7

8-1130

Soils Analyses

*ELASTIC 162600.,.17 *CAP PLASTICITY 247.,58.5,0.23,0.02,0.,1. *CAP HARDENING 500.,.0 600.,.006 1100.,.012 9800.,.03 *CAP CREEP, LAW=SINGHM, MECHANISM=CONSOLIDATION 2.2e-7, 2.1e-2, 1.0, 1.0, 50.0 3.5e-4, 2.1e-2, 1.0, 1.0, 212.0 *PERMEABILITY,SPECIFIC=3.07e-2 16.8,,0 32.0,,250 *EXPANSION 0.32E-05, ** ** SOIL STRATA D6 (2000 ft - 2400 ft) ** ----------------------------------*MATERIAL,NAME=D6 *ELASTIC 112400.,.17 *CAP PLASTICITY 247.,50.2,0.23,0.02,0.,1. *CAP HARDENING 400.,.0 600.,.005 1100.,.02 9000.,.05 *CAP CREEP, LAW=SINGHM, MECHANISM=CONSOLIDATION 2.2e-7, 2.1e-2, 1.0, 1.0, 50.0 3.5e-4, 2.1e-2, 1.0, 1.0, 212.0 *PERMEABILITY,SPECIFIC=3.07e-2 16.8,,0 32.0,,250 *EXPANSION 0.32E-05, ** ** SOIL STRATA D5 (1800 ft - 2000 ft) ** ---------------------------------*MATERIAL,NAME=D5 *ELASTIC

8-1131

Soils Analyses

71600.,.17 *CAP PLASTICITY 200.,40.4,0.30,0.02,0.,1. *CAP HARDENING 400.,.0 700.,.02 2000.,.04 9000.,.08 *CAP CREEP, LAW=SINGHM, MECHANISM=CONSOLIDATION 2.2e-7, 2.1e-2, 1.0, 1.0, 50.0 3.5e-4, 2.1e-2, 1.0, 1.0, 212.0 *PERMEABILITY,SPECIFIC=3.07e-2 16.8,,0 32.0,,250 *EXPANSION 0.32E-05, ** ** SOIL STRATA D4 (1400 ft - 1800 ft) ** ---------------------------------*MATERIAL,NAME=D4 *ELASTIC 59600.,.2 *CAP PLASTICITY 174.,40.1,0.30,0.02,0.,1. *CAP HARDENING 200.,.0 730.,.02 1000.,.04 9000.,.1 *CAP CREEP, LAW=SINGHM, MECHANISM=CONSOLIDATION 2.2e-7, 2.1e-2, 1.0, 1.0, 50.0 3.5e-4, 2.1e-2, 1.0, 1.0, 212.0 *PERMEABILITY,SPECIFIC=3.07e-2 16.8,,0 32.0,,250 *EXPANSION 0.32E-05, ** ** SOIL STRATA D3 (1200 ft - 1400 ft) ** ---------------------------------*MATERIAL,NAME=D3 *ELASTIC 79200.,.19

8-1132

Soils Analyses

*CAP PLASTICITY 200.,42.0,0.34,0.02,0.,1. *CAP HARDENING 200.,.0 500.,.02 2000.,.04 9000.,.06 *CAP CREEP, LAW=SINGHM, MECHANISM=CONSOLIDATION 2.2e-7, 2.1e-2, 1.0, 1.0, 50.0 3.5e-4, 2.1e-2, 1.0, 1.0, 212.0 *PERMEABILITY,SPECIFIC=3.07e-2 16.8,,0 32.0,,250 *EXPANSION 0.32E-05, ** ** SOIL STRATA D2 (1100 ft - 1200 ft) ** ---------------------------------*MATERIAL,NAME=D2 *ELASTIC 63000.,.17 *CAP PLASTICITY 200.,39.4,0.33,0.02,0.,1. *CAP HARDENING 200.,.0 600.,.02 1000.,.04 8000.,.1 *CAP CREEP, LAW=SINGHM, MECHANISM=CONSOLIDATION 2.2e-7, 2.1e-2, 1.0, 1.0, 50.0 3.5e-5, 2.1e-2, 1.0, 1.0, 212.0 *PERMEABILITY,SPECIFIC=3.07e-2 16.8,,0 32.0,,250 *EXPANSION 0.32E-05, ** ** SOIL STRATA D1 (700 ft - 1100 ft) ** --------------------------------*MATERIAL,NAME=D1 *ELASTIC 47700.,.17 *CAP PLASTICITY

8-1133

Soils Analyses

200.,36.9,0.33,0.02,0.,1. *CAP HARDENING 400.,.0 600.,.02 800.,.05 900.,.09 *CAP CREEP, LAW=SINGHM, MECHANISM=CONSOLIDATION 2.2e-7, 2.1e-2, 1.0, 1.0, 50.0 3.5e-5, 2.1e-2, 1.0, 1.0, 212.0 *PERMEABILITY,SPECIFIC=3.07e-2 16.8,,0 32.0,,250 *EXPANSION 0.32E-05, ** ** SOIL STRATA T1 (150 ft - 700 ft) ** -------------------------------*MATERIAL,NAME=T1 *ELASTIC 300000.,0.25 *DRUCKER PRAGER 36.,1.,0. *DRUCKER PRAGER HARDENING 70.,0. 90.,.058 70.,.116 *PERMEABILITY,SPECIFIC=3.61e-2 40, *EXPANSION 0.32E-05, ** ** SOIL STRATA S1 (0 ft - 150 ft) ** -----------------------------*MATERIAL,NAME=S1 *ELASTIC 18000.,0.3 *DRUCKER PRAGER 42.,1.,0. *DRUCKER PRAGER HARDENING 11.,0. 12.,.058 11.,.116 *PERMEABILITY,SPECIFIC=3.61e-2

8-1134

Soils Analyses

40., *EXPANSION 0.32E-05, ** FAR FIELD MATERIAL DATA ** ----------------------*MATERIAL,NAME=FAR *ELASTIC 47700.,.17 ** *SOLID SECTION, ELSET=L1, MATERIAL=L1 *SOLID SECTION, ELSET=U1, MATERIAL=U1 *SOLID SECTION, ELSET=D7, MATERIAL=D7 *SOLID SECTION, ELSET=D6, MATERIAL=D6 *SOLID SECTION, ELSET=D5, MATERIAL=D5 *SOLID SECTION, ELSET=D4, MATERIAL=D4 *SOLID SECTION, ELSET=D3, MATERIAL=D3 *SOLID SECTION, ELSET=D2, MATERIAL=D2 *SOLID SECTION, ELSET=D1, MATERIAL=D1 *SOLID SECTION, ELSET=T1, MATERIAL=T1 *SOLID SECTION, ELSET=S1, MATERIAL=S1 *SOLID SECTION, ELSET=FAR, MATERIAL=FAR ** *BOUNDARY FREESURF, 8,,0. ** *INITIAL CONDITIONS, TYPE=RATIO NALL, 1.5 ** *INITIAL CONDITIONS, TYPE=TEMPERATURE NALL, 50 *INITIAL CONDITIONS,TYPE=STRESS,GEOSTATIC L1, -2151.2, 0.,-1615.7, 14400., .85 U1, -1615.7, 14400.,-1346.4, 21600., .85 D7, -1346.4, 21600.,-1077.1, 28800., .85 D6, -1077.1, 28800., -897.6, 33600., .85 D5, -897.6, 33600., -807.8, 36000., .85 D4, -807.8, 36000., -628.3, 40800., .85 D3, -628.3, 40800., -538.6, 43200., .85 D2, -538.6, 43200., -493.7, 44400., .85 D1, -493.7, 44400., -314.2, 49200., .85 T1, -314.2, 49200., -67.3, 55800., .85 S1, -67.3, 55800. , 0.0, 57600., .85 FAR,-2151.2, 0., 0.0, 57600., .85

8-1135

, , , , , , , , , , , ,

.85 .85 .85 .85 .85 .85 .85 .85 .85 .85 .85 .85

Soils Analyses

** ** ** GEOSTATIC STEP TO BALANCE GRAVITY LOADING ** *STEP, UNSYMM=YES, NLGEOM *GEOSTATIC *MONITOR,NODE=2201,DOF=2 *BOUNDARY BASE, 2 AXIS, 1 *DLOAD S1, BZ, -0.0374 T1, BZ, -0.0374 D1, BZ, -0.0374 D2, BZ, -0.0374 D3, BZ, -0.0374 D4, BZ, -0.0374 D5, BZ, -0.0374 D6, BZ, -0.0374 D7, BZ, -0.0374 U1, BZ, -0.0374 L1, BZ, -0.0374 *END STEP ** ** CONSOLIDATION ANALYSIS (1 MONTH-BALANCE CREEP) ** *STEP,NLGEOM,INC=100,UNSYMM=YES *SOILS,CONSOLIDATION,CETOL=0.0001,UTOL=10 1.,31., *EL FILE, FREQ=0, ELSET=ESOIL S,E,PE,POR,VOIDR,CE *END STEP ** ** THERMAL LOADING - INJECTING STEAM ** *STEP, NLGEOM, INC=100, UNSYMM=YES *SOILS, CONSOLIDATION, UTOL=25, NO CREEP 1.,1. *TEMPERATURE,OP=MOD TARGET, 212. *EL FILE, FREQ=0, ELSET=ESOIL S,E,PE,POR,VOIDR,CE *END STEP

8-1136

Soils Analyses

** ** INSTALL PUMP ** *STEP, NLGEOM, INC=100, UNSYMM=YES, AMP=RAMP *SOILS, CONSOLIDATION, UTOL=25 1.,1. *BOUNDARY, OP=MOD 1001,8,8,-170 1201,8,8,-170 *EL FILE, FREQ=0, ELSET=ESOIL S,E,PE,POR,VOIDR,CE *END STEP ** ** PUMPING OIL OVER FIVE YEAR PERIOD ** *STEP,NLGEOM,INC=200,UNSYMM=YES *SOILS,CONSOLIDATION,CETOL=0.0001,UTOL=20 1.,1825., *CONTROLS, PARAMETER=FIELD, FIELD=DISPLACEMENT ,1. *CONTROLS, PARAMETER=FIELD, FIELD=PORE FLUID PRESSURE ,1. *EL FILE,FREQ=200, ELSET=ESOIL S,E,PE,CE,POR,VOIDR *EL PRINT,FREQ=0, ELSET=ESOIL S, CE, PE, *NODE PRINT,FREQ=0 U,RVF,RVT *END STEP

8.1.4 Analysis of a pipeline buried in soil Product: ABAQUS/Standard Oil and gas pipelines are usually buried in the ground to provide protection and support. Buried pipelines may experience significant loading as a result of relative displacements of the ground along their length. Such large ground movement can be caused by faulting, landslides, slope failures, and seismic activity. ABAQUS provides a library of pipe-soil interaction ( PSI) elements to model the interaction between a buried pipeline and the surrounding soil. The pipeline itself is modeled with any of the beam, pipe, or elbow elements in the ABAQUS/Standard element library. The ground behavior and soil-pipe

8-1137

Soils Analyses

interaction are modeled with the pipe-soil interaction elements. These elements have only displacement degrees of freedom at their nodes. One side or edge of the element shares nodes with the underlying beam, pipe, or elbow element that models the pipeline. The nodes on the other edge represent a far-field surface, such as the ground surface, and are used to prescribe the far-field ground motion. The elements are described in detail in ``Pipe-soil interaction elements,'' Section 18.7.1 of the ABAQUS/Standard User's Manual. The purpose of this example is to determine the stress state along the length of a infinitely long buried pipeline subjected to large fault movement of 1.52 m (5.0 ft), as shown in Figure 8.1.4-1. The pipeline intersects the fault at 90.0°. The results are compared with results from an independent analysis, as described below.

Problem description The problem consists of an infinitely long pipeline buried at a depth of 6.1 m (20.0 ft.) below the ground surface. Only a 610.0 m (2000.0 ft.) long section of the pipeline is modeled. The outside diameter of the pipe is 0.61 m (24.0 in), and the wall thickness is 0.0254 m (1.0 in). The pipeline is modeled with 50 first-order PIPE21 elements. A nonuniform mesh, with smaller elements focused near the fault, is used. The pipe-soil interaction behavior is model with PSI24 elements. The PSI elements are defined so that one edge of the element shares nodes with the underlying pipe element, and the nodes on the other edge represent a far-field surface where ground motion is prescribed. The far-field side and the side that shares nodes with the pipeline are defined by the element connectivity. A three-dimensional model that uses PIPE31 and PSI34 elements is also included for verification purposes.

Material The pipeline is made of an elastic-perfectly plastic metal, with a Young's modulus of 206.8 GPa (30 ´ 106 lb/in2), a Poisson's ratio of 0.3, and a yield stress of 413.7 MPa (60000 lb/in 2). The pipe-soil interaction behavior is elastic-perfectly plastic. The *PIPE-SOIL STIFFNESS, TYPE=NONLINEAR option is used to define the interaction model. The behavior in the vertical direction is assumed to be different from the behavior along the axial direction. It is further assumed that the pipeline is buried deep below the ground surface so that the response is symmetric about the origin. ABAQUS also allows a nonsymmetric behavior to be defined in any of the directions (this is usually the case in the vertical direction when the pipeline is not buried too deeply). The ultimate force per unit length in the axial direction is 730.0 N/m (50.0 lb/ft), and in the vertical direction it is 1460.0 N/m (100.0 lb/ft). The ultimate force is reached at 0.0304 m (0.1 ft) in both the horizontal and vertical directions. The loading occurs in a plane (axial-vertical), so the properties for the pipe-soil interaction behavior in the transverse horizontal direction are not important.

Loading

8-1138

Soils Analyses

The loading on the pipeline is caused by a relative vertical displacement 1.52 m (5.0 ft) along the fault line. It is assumed that the effect of the vertical ground motion decreases linearly over a distance of 91.4 m (300.0 ft.) from the origin of fault, as shown in Figure 8.1.4-1. This linear distribution of ground motion is prescribed as follows. Rigid ( R2D2) elements are connected to the far-field edges of the PSI to create two rigid surfaces, one on each side of the fault line. These surfaces extend a distance of 91.4 m (300.0 ft.) from the origin of the fault. The rigid body reference nodes are also placed a distance of 91.4 m (300.0 ft.) from the fault on the ground surface. The fault movement is modeled by prescribing a rotation to each of the rigid body reference nodes so that a positive vertical displacement of 0.76 m (2.5 ft) is obtained on one side of the fault and a negative vertical displacement of 0.76 m (2.5 ft) is obtained on the other side of the fault, as shown in Figure 8.1.4-2. All degrees of freedom on the remaining far-field nodes are fully fixed. In addition, the two end points of pipeline are fully fixed. Figure 8.1.4-2 does not show the PSI elements or any of the remaining nodes on the ground surface.

Reference solution The reference solution is obtained by using JOINTC elements between the pipeline and ground nodes to model the pipe-soil interaction. These elements provide an internal stiffness, which is modeled with linear or nonlinear springs; nonlinear springs are used in this example. The behavior of the nonlinear spring is elastic in the sense that reversed loading does not result in permanent deformation. This behavior is different from the behavior provided by the nonlinear PSI elements. However, this is not a limitation in this example since the loading is monotonic. Another distinct difference between JOINTC elements and PSI elements is that the spring behavior associated with JOINTC elements is defined in terms of total force, whereas the constitutive behavior for PSI elements is defined as a force/unit length. This difference requires us to define a separate stiffness for each JOINTC element or to use a uniform mesh with JOINTC elements spaced at unit length intervals along the pipeline. A unit length mesh is used in this example.

Results and discussion Figure 8.1.4-3 and Figure 8.1.4-4 show the axial and vertical forces per unit length applied to the pipeline due to relative ground motion. The figures show that permanent deformation occurs in the pipe-soil interaction model near the fault along the axial and horizontal directions, with purely elastic behavior further from the fault. Figure 8.1.4-5 compares the axial stress in the bottom wall of the pipeline with the reference solution. The figure shows that the pipeline behavior is purely elastic. The figure also shows close agreement with the reference solution. The small differences between the solutions can be accounted for by the different mesh densities. The reaction forces at the pipeline edges and the maximum pipeline displacements are also in close agreement with the reference solution.

Input files buriedpipeline_2d.inp Two-dimensional model using PSI24 elements.

8-1139

Soils Analyses

buriedpipeline_3d.inp Three-dimensional model using PSI34 elements. buriedpipeline_ref.inp Reference solution using JOINTC elements.

Reference · Audibert, J. M. E., D. J. Nyman, and T. D. O'Rourke, "Differential Ground Movement Effects on Buried Pipelines," Guidelines for the Seismic Design of Oil and Gas Pipeline Systems, ASCE publication, pp. 151-180, 1984.

Figures Figure 8.1.4-1 Pipe with fault motion.

Figure 8.1.4-2 Displaced shape (magnification factor=10.0).

Figure 8.1.4-3 Axial force/unit length applied along the pipeline.

8-1140

Soils Analyses

Figure 8.1.4-4 Vertical force/unit length applied along the pipeline.

Figure 8.1.4-5 Axial stress along the bottom of the pipeline.

8-1141

Soils Analyses

Sample listings

8-1142

Soils Analyses

Listing 8.1.4-1 *HEADING RELATIVE FAULT MOTION ACCROSS BURIED PIPELINE PSI24 elements Units: N, m *PRE PRINT,ECHO=NO,MODEL=YES,CONTACT=YES, HISTORY=YES *NODE 1, -91.4, 6.1 2, 91.4, 6.1 101, -305.0, 0.0 151, 305.0, 0.0 501, -305.0, 6.1 551, 305.0, 6.1 *NODE,NSET=NL 111, -91.4, 0.0 511, -91.4, 6.1 *NODE,NSET=NC 126, 0.0, 0.0 526, 0.0, 6.1 *NODE,NSET=NR 141, 91.4, 0.0 541, 91.4, 6.1 *NGEN,NSET=ALL 101, 111 141, 151 501, 511 541, 551 *NFILL,NSET=ALL,BIAS=1.111111 NL, NC, 15 *NFILL,NSET=ALL,BIAS=0.900000 NC, NR, 15 *NSET,NSET=PIPE,GEN 101, 151 *NSET,NSET=SURF,GEN 501, 510 526, 526 542, 551 *NSET,NSET=ENDS 101, 151 *ELEMENT,TYPE=PIPE21 101, 101, 102 *ELGEN,ELSET=PIPELINE

8-1143

Soils Analyses

101, 50 *ELSET,ELSET=PIPEPLOT,GEN 111,140 *ELEMENT,TYPE=PSI24 501, 101, 102, 502, 501 *ELGEN,ELSET=SOIL 501, 50 *ELEMENT,TYPE=R2D2 1111, 511, 512 1127, 527, 528 *ELGEN,ELSET=SURFL 1111, 14 *ELGEN,ELSET=SURFR 1127, 14 *BEAM SECTION,SECTION=PIPE,ELSET=PIPELINE, MATERIAL=STEEL 0.61, 0.0254 *MATERIAL,NAME=STEEL *ELASTIC 206.8E6, 0.3 *PLASTIC 413.7E6 *PIPE-SOIL INTERACTION,ELSET=SOIL *PIPE-SOIL STIFFNESS,TYPE=NONLINEAR,DIR=AXIAL -730.0, -0.0304 0.0, 0.0 730.0, 0.0304 *PIPE-SOIL STIFFNESS,TYPE=NONLINEAR,DIR=VERTICAL -1460.0, -0.0304 0.0, 0.0 1460.0, 0.0304 *PIPE-SOIL STIFFNESS,TYPE=NONLINEAR,DIR=HORIZONTAL -1460.0, -0.0304 0.0, 0.0 1460.0, 0.0304 *RIGID BODY,ELSET=SURFL,REFNOD=1 *RIGID BODY,ELSET=SURFR,REFNOD=2 *STEP,INC=1000,NLGEOM 1: APPLY FAULT MOTION *STATIC *BOUNDARY SURF, 1, 2 ENDS, 1, 2

8-1144

Soils Analyses

ENDS, 6 1, 1, 2 2, 1, 2 1, 6, , 0.0083368 2, 6, , 0.0083368 *NODE PRINT,FREQ=10 U, RF, *ELPRINT,FREQ=10,ELSET=SOIL S, PE COORD, *ELPRINT,FREQ=10,ELSET=PIPEPLOT 1 S, PE COORD, *EL FILE,ELSET=PIPEPLOT S *EL FILE,ELSET=SOIL S, PE, E NFORC, *OUTPUT,FIELD,FREQ=100 *ELEMENT OUTPUT,ELSET=PIPELINE S,E,EE,EP *NODE OUTPUT,NSET=ALL U, *OUTPUT,HISTORY,FREQ=1 *NODE OUTPUT,NSET=ENDS U,RF *END STEP

8-1145

ABAQUS/Aqua Analyses

9. ABAQUS/Aqua Analyses 9.1 ABAQUS/Aqua analyses 9.1.1 Jack-up foundation analyses Products: ABAQUS/Standard ABAQUS/Aqua This example simulates a jack-up rig on a sand foundation subjected to alternating wind loading.

Geometry and model The model--a simplified planar model for the analysis of a multiple leg, portal frame-type structure--is intended for the analysis of 3-leg jack-up rigs with shallow foundation supports. Figure 9.1.1-1is a schematic of a 3-leg jack-up, as represented by the model. The jack-up hull is assumed to be rigid and triangular, and the connection between the hull and the legs is also taken to be rigid. The jack-up has two windward legs and one leeward leg; the model is projected onto the vertical symmetry plane that passes through the leeward leg and between the windward legs. Elastic beam columns are used to model both the upper and lower segment of each leg. The soil model is chosen to be macro-yield sand. Three degrees of freedom--vertical, horizontal, and rotational--are assumed at each spud can at the base of each leg. Mass is assumed to be concentrated at the center of the hull. The horizontal degree of freedom at the center is assumed to represent the motion of the rig for analysis purposes. Wind loading on the rig is applied as a horizontal force below the center of gravity of the hull. The leg segments are modeled using B21 elements, and the *BEAM GENERAL SECTION option is used to define the structural properties of the beam. The interaction between the spud can and the soil is modeled through JOINT2D elements and the *JOINT ELASTICITY and *JOINT PLASTICITY options. Rigid beam elements, RB2D2, are used to model the rigid hull. The dimensions of the rig and the material properties of the sand and the spud can are as follows (force units are in kN, and length units are in meters): Leg length upper segment 49.4 Leg length lower segment 13.5 Leg EI upper segment 2.7 ´ 108 Leg EI lower segment 2.7 ´ 109 Leg AE upper segment 2.2 ´ 108 Leg AE lower segment 2.2 ´ 109 Leg GA upper segment 8.1 ´ 107 Leg GA lower segment 8.1 ´ 108 Horizontal distance from platform center of gravity to leeward leg 23.4 Horizontal distance from platform center of gravity to windward leg 11.7 Spud can diameter 10.9 Spud can cone angle 180° Foundation preload per spud can 50600 Foundation tensile capacity 0 Operational vertical load (weight) 62700

9-1146

ABAQUS/Aqua Analyses

Vertical distance from center of gravity to load application point Soil submerged unit weight Soil friction angle Soil Poisson's ratio Foundation elastic shear moduli, Gºº Ghh Grr Constant coefficient, ¤1 Constant coefficient, ¤2

5.7 10.0 33° 0.2 5.14 ´ 104 3.87 ´ 103 2.04 ´ 103 1.0 0.5

Boundary conditions and loading The base nodes of the JOINT2D elements are always fixed. The required preload is applied to each spud can using the *INITIAL CONDITIONS option. In the first step the weight loading is applied at the center of gravity of the hull. The rig is then subjected to an alternating horizontal wind loading applied at the specified location below the center of gravity of the hull. The load is applied by using the *CLOAD option. The rig is loaded from zero to 5370 kN, unloaded to zero and then to 6440 kN in the opposite direction, reloaded to 9130 kN in the initial direction, unloaded and reloaded to 9770 kN in the opposite direction, and unloaded to zero again. Each of these loadings is done in a separate step and is ramped from zero to the specified magnitude at the end of the step.

Results and discussion The estimated load path for the leeward spud can foundation is plotted in a graph of equivalent p horizontal load, R = (M=D )2 + ¤1 H 2 , versus V =Vc : The plot is shown in Figure 9.1.1-2 and is in good agreement with the load path predicted by an independent analysis, as detailed in the reference below. The moment-horizontal load response (i.e., M=D versus H) for the leeward spud can foundation, shown in Figure 9.1.1-3, compares well with the independent analysis.

Input file jackup.inp Input data for this example.

Reference · Wong, P. C. and J. D. Murff, "Dynamic Analysis of Jack-Up Rigs Using Advanced Foundation Models," Proceedings, 13th International Conference on Offshore Mechanics and Arctic Engineering (OMAE), vol. 2 - Safety and Reliability, Houston, pp. 93-109, February 1994.

Figures

9-1147

ABAQUS/Aqua Analyses

Figure 9.1.1-1 Schematic representation of jack-up rig.

Figure 9.1.1-2 Load path for leeward spud can.

Figure 9.1.1-3 Moment versus horizontal load for leeward spud can.

9-1148

ABAQUS/Aqua Analyses

Sample listings

9-1149

ABAQUS/Aqua Analyses

Listing 9.1.1-1 *HEADING 3-LEG JACK UP ON SAND --- CYLINDRICAL ** **NODE DEFINITIONS ** *NODE,NSET=BEAMS 11,0. 12,0.,13.5,0. 13,0.,62.9,0. 14,35.1,0,0. 15,35.1,13.5,0. 16,35.1,62.9,0. 17,11.7,62.9,0. 18,11.7,70.0,0. 999,11.7,75,0. *NODE,NSET=BASE 1, 0. 2, 0. 3,35.1 *NSET,NSET=EPJ BASE,11,14 ** **ELEMENT DEFINITIONS ** *ELEMENT,ELSET=BEAML,TYPE=B21 1,11,12 3,11,12 5,14,15 *ELEMENT,ELSET=BEAMU,TYPE=B21 2,12,13 4,12,13 6,15,16 *ELEMENT,ELSET=RBEAMS,TYPE=RB2D2 11,13,17 12,17,16 13,17,18 *ELEMENT,TYPE=JOINT2D, ELSET=JOINT2D 101,1,11 102,2,11 103,3,14 **

9-1150

ABAQUS/Aqua Analyses

**ORIENTATIONS AND TRANSFORMATIONS ** *ORIENTATION,NAME=ORI1 0,1,0,1,0,0 *TRANSFORM,NSET=EPJ 0,1,0,1,0,0 ** **PROPERTY DEFINITIONS ** *BEAM GENERAL SECTION,ELSET=BEAMU,SECTION=GENERAL 1.0,1.2273,0.,1.2273,2.4545, 2.2E8,8.1E7 *BEAM GENERAL SECTION,ELSET=BEAML,SECTION=GENERAL 1.0,1.2273,0.,1.2273,2.4545, 2.2E9,8.1E8 *RIGID BODY,ELSET=RBEAMS,REF NODE=999 ** *EPJOINT,ELSET=JOINT2D,ORIEN=ORI1,SECTION=SPUD 10.9,0. *JOINT ELASTIC,NDIM=2,MODULI=SPUD CAN 5.14E4, 3.87E3, 2.04E4, 0.2 *JOINT PLASTIC,TYPE=SAND 0.,1,0.5,33.0,10.0 ** *INITIAL CONDITIONS, TYPE=SPUD PRELOAD JOINT2D,50600 ** ** *STEP,INC=10000 APPLY WEIGHT *STATIC 1.0,1.0 *BOUNDARY 1,1,6,0 2,1,6,0 3,1,6,0 ** ** Apply weight ** *CLOAD 17,2,-62700

9-1151

ABAQUS/Aqua Analyses

*EL PRINT,ELSET=JOINT2D,FREQ=0 S, PE, *EL FILE,ELSET=JOINT2D,FREQ=20 S, E, PE, *NODE FILE,FREQ=20 U, RF, *OUTPUT, FIELD, FREQUENCY=10000 *NODE OUTPUT, NSET=EPJ U,RF *ELEMENT OUTPUT, ELSET=JOINT2D S,E,PE *OUTPUT, HISTORY, FREQUENCY=10 *NODE OUTPUT, NSET=EPJ U,RF *ELEMENT OUTPUT, ELSET=JOINT2D S,E,PE *END STEP *STEP,INC=10000 ALTERNATING LOADING ANALYSIS FIRST STEP *STATIC 0.001,1.0,,0.005 *BOUNDARY 1,1,6,0 2,1,6,0 3,1,6,0 *CLOAD 18,1,5370 *END STEP ** ** ** *STEP,INC=10000 UNLOADING TO ZERO *STATIC 0.001,1.0,,0.005 *BOUNDARY 1,1,6,0 2,1,6,0 3,1,6,0

9-1152

ABAQUS/Aqua Analyses

*CLOAD 18,1,0 *END STEP ** ** ** *STEP,INC=10000 LOADING IN THE OPPOSITE DIRECTION *STATIC 0.001,1.0,,0.005 *BOUNDARY 1,1,6,0 2,1,6,0 3,1,6,0 *CLOAD 18,1,-6440 *END STEP ** ** ** *STEP,INC=10000 RELOADING IN THE INITIAL DIRECTION *STATIC 0.001,1.0,,0.005 *BOUNDARY 1,1,6,0 2,1,6,0 3,1,6,0 *CLOAD 18,1,9130 *END STEP ** ** ** *STEP,INC=10000 UNLOADING TO ZERO (2) *STATIC 0.001,1.0,,0.005 *BOUNDARY 1,1,6,0 2,1,6,0 3,1,6,0 *CLOAD

9-1153

ABAQUS/Aqua Analyses

18,1,0 *END STEP ** ** ** *STEP,INC=10000 REVERSE LOADING *STATIC 0.001,1.0,,0.005 *BOUNDARY 1,1,6,0 2,1,6,0 3,1,6,0 *CLOAD 18,1,-9770 *END STEP ** ** ** *STEP,INC=10000 UNLOADING BACK TO ZERO *STATIC 0.001,1.0,,0.005 *BOUNDARY 1,1,6,0 2,1,6,0 3,1,6,0 *CLOAD 18,1,0 *END STEP

9.1.2 Riser dynamics Products: ABAQUS/Standard ABAQUS/Aqua Pipelines extending from the sea floor to the ocean surface (risers) are subject to many types of load: self-weight, buoyancy, internal and external pressure, tensile forces arising from surface moorings, current drag, and oscillatory loads resulting from wave motion. The response of a riser to these loads is complex, and the difficulty of such analysis is heightened by the relative length of such pipelines (deep water risers). In this example a riser is analyzed under conditions specified by the American Petroleum Institute for comparison of drilling riser analyses (API BULLETIN 2J, 1977), and the results are compared with the results shown in that publication.

Geometry and model

9-1154

ABAQUS/Aqua Analyses

The riser is shown in Figure 9.1.2-1. Its length is 463.3 m (1520 ft), and it stands in 448.1 m (1470 ft) of water. The outer diameter of the riser is 405 mm (1.33 ft), and it has a wall thickness of 15.88 mm (0.0521 ft). The pipeline is made of steel, with a Young's modulus of 206.8 GPa (4.32 ´ 109 lb/ft2) and a density of 11508.685 kg/m 3 (22.332 lb-s 2/ft4). The riser is modeled with 10 beam elements of type B21. No mesh convergence studies have been performed; hence, more elements may be required for accurate prediction of the stress in the riser.

Loading The riser has a weight of 2575 N/m (176.36 lb/ft) and is loaded by a top tension of 2.224 MN (5 ´ 105 lb). Drag loading is applied by a steady current flowing by the riser with a velocity distribution varying linearly from 0.257 m/s (0.844 ft/s) at the mean water level to zero at the base of the riser. The coefficients in Morison's equation are transverse drag coefficient ( CD ) 0.7, tangential drag coefficient (CT ) 0.0, and transverse inertia coefficient (CM ) 1.5. The effective outer diameter for the drag calculations is 0.66 m (2.167 ft). Waves of peak to trough height 6.1 m (20 ft) travel across the water surface with a period of 9 seconds; these are modeled with the Airy wave theory provided in the *AQUA option (``ABAQUS/Aqua analysis,'' Section 6.10.1 of the ABAQUS/Standard User's Manual). The density of the fluid is taken to be 1021 kg/m 3 (1.982 lb-s2/ft4). In ABAQUS/Aqua, user subroutine UWAVE can be used to specify user-defined wave kinematics. We illustrate this capability by repeating this analysis with a user-specified Airy wave theory that is identical to the built-in Airy wave option in ABAQUS/Aqua.

Boundary conditions The base of the riser is "gimballed," supporting no moments. The top of the riser has two motions prescribed: an initial offset of 13.716 m (45 ft) from the vertical position of the riser and a sinusoidal motion about this static configuration, representing the surge of a vessel attached to the riser, with peak-to-peak amplitude of 1.22 m (4 ft) and a period of 9 seconds. The vessel surge is 15° out of phase with the surface waves.

Analysis The analysis is done in two steps. The first is the static step, in which the top tension is applied and the riser is moved from the vertical to its offset position by specifying the necessary horizontal displacement at the top of the pipeline. The top tension is 2.224 MN (5 ´ 105 lb). In the second step, which is a dynamic step, the time increment is chosen as a fixed value of 0.125 second. The prescribed displacement at the top of the riser has a 9-second period, so this time step should provide reasonably accurate time integration once the higher modes are damped out by the fluid drag. The "half-step residual" values calculated by ABAQUS provide a measure of accuracy of the solution, and these values are typically of order 4.4 kN (1000 lb). Since these values are smaller than typical actual forces, they suggest that the time integration is reasonably accurate.

Results and discussion The initial static step, which moves the riser to its offset position and applies the static loads, is

9-1155

ABAQUS/Aqua Analyses

completed in four increments. The first increment requires more iterations than subsequent increments, which is typical of this class of problem: the riser is initially unstressed and, therefore, is highly flexible. After some loading is applied, the axial tension stabilizes the system, and convergence is more rapid. At the end of the static step the top of the riser makes an angle of 1.17° with the vertical. This value agrees well with the value of 1.20° presented in API BULLETIN 2J (1977). The angle predicted at the base of the riser is 2.48°, which compares to 2.55° reported in the API bulletin. The slight discrepancies are attributed to the relative coarseness of the model. The dynamic solution is carried out for 18 seconds of response. Typically one equilibrium iteration is required in each of the time increments. Half-step residual values for the first few increments are of order 178 MN (4.0 ´ 107 lb), and at the end of the run they are of order 4.4 kN (1000 lb). This result is typical: initially there is much high frequency content in the solution, which is reflected in the larger half-step residual values. As the analysis proceeds, the fluid drag dissipates this "noise," the solution becomes smoother, and the half-step residual values drop accordingly. The envelope of pipeline excursions during the dynamic analysis is plotted in Figure 9.1.2-2, and the envelope of bending stress is shown in Figure 9.1.2-3. These results are in basic agreement with those given in the API bulletin. As expected, the results obtained by the model with the Airy wave theory implemented in user subroutine UWAVE are identical to those due to the built-in Airy wave option.

Input files riserdynamics_airy_disp.inp Analysis with the Airy wave theory. User subroutine DISP is used to prescribe the sinusoidal surge motion. This motion could be prescribed instead through the use of the *AMPLITUDE option. User subroutine DISP is used to illustrate the use of this routine to prescribe a nonzero boundary condition value. riserdynamics_airy_disp.f User subroutine DISP used in riserdynamics_airy_disp.inp. riserdynamics_wavedata.inp Wave data for use in riserdynamics_airy_disp.inp. riserdynamics_stokes_disp.inp Analysis with the Stokes wave theory. riserdynamics_stokes_disp.f User subroutine DISP used in riserdynamics_stokes_disp.inp. riserdynamics_airy_disp_uwave.inp Analysis with the Airy wave theory implemented in user subroutine UWAVE.

9-1156

ABAQUS/Aqua Analyses

riserdynamics_airy_disp_uwave.f User subroutines UWAVE and DISP used in riserdynamics_airy_disp_uwave.inp.

Reference · American Petroleum Institute, "Comparison of Marine Drilling Riser Analyses," API Bulletin 2J, Washington, D. C., January 1977.

Figures Figure 9.1.2-1 Riser problem definition.

Figure 9.1.2-2 Horizontal displacement envelope during dynamic response.

9-1157

ABAQUS/Aqua Analyses

Figure 9.1.2-3 Bending stress envelope during dynamic response.

9-1158

ABAQUS/Aqua Analyses

Sample listings

9-1159

ABAQUS/Aqua Analyses

Listing 9.1.2-1 *HEADING RISER DYNAMIC CHECK OUT - AIRY THEORY NEEDS FILE riserdynamics_wavedata.inp FOR WAVE DATA *NODE ,NSET=ENDS 1,,1520. 11,0. *NGEN 1,11 *ELEMENT,TYPE=B21 1,1,2 *ELGEN,ELSET=PIPE 1,10 *ELSET,ELSET=PIPE1,GEN 1,5,1 *ELSET,ELSET=PIPE2,GEN 6,10,1 *BEAM GENERAL SECTION,SECTION=PIPE,DENSITY=22.332, ELSET=PIPE .6667,0.0521 ,,-1. 4.32E9,2.16E9 *AQUA 0.,1470.,32.2,1.982 0.,0.,0.,0. 0.844,0.,0.,1470. *WAVE,TYPE=AIRY,INPUT=riserdynamics_wavedata.inp *RESTART,WRITE,FREQUENCY=5 *STEP,NLGEOM INITIAL OFFSET *STATIC .25E-5,1.E-5 *DLOAD PIPE,PY,-176.36 ***** ** Aqua Normal drag load PIPE,FDD, 1., 2.167, 0.7, 1. ** ** Aqua Inertial drag load PIPE, FI, 1., 2.167, 1.5, 0.5 **

9-1160

ABAQUS/Aqua Analyses

*CLOAD 1,2,5.E5 *BOUNDARY 11,1,2 *BOUNDARY,USER 1,1 *NODE FILE,NSET=ENDS,FREQUENCY=1 U,RF *PRINT,RESIDUAL=NO *ENERGY PRINT *ENERGY FILE *ENERGY PRINT,ELSET=PIPE1 *ENERGY PRINT,ELSET=PIPE2 *ENERGY FILE,ELSET=PIPE1 *ENERGY FILE,ELSET=PIPE2 *EL PRINT,ELSET=PIPE1,TOTALS=YES ELEN, *EL PRINT,FREQUENCY=20 SF, *EL FILE,FREQUENCY=20 SF, *NODE PRINT,FREQUENCY=5 U,RF *NODE FILE,FREQUENCY=5 U,RF *END STEP *STEP,NLGEOM,INC=200 DYNAMICS *DYNAMIC .125,18. *EL PRINT,FREQUENCY=10 SF, *EL FILE,FREQUENCY=10 SF, *ENERGY PRINT,ELSET=PIPE1 *ENERGY PRINT,ELSET=PIPE2 *ENERGY FILE,ELSET=PIPE1 *ENERGY FILE,ELSET=PIPE2 *EL PRINT,ELSET=PIPE1,TOTALS=YES ELEN, *END STEP

9-1161

Underwater Shock Analyses

10. Underwater Shock Analyses 10.1 Underwater shock analyses 10.1.1 The cylinder whip problem Products: ABAQUS/Standard ABAQUS/USA An important phase of response for underwater structures is the late-time response excited by the flow field created from an explosion. The response of long underwater structures to these late-time excitations is often referred to as whipping. The capability exists within USA to analyze these late-time responses due to the flow field created by an explosion. The explosion creates a gas bubble that pulsates and (possibly) migrates toward the surface. USA will calculate the velocity potential due to the bubble, but the user must provide certain information about the explosive event. The user selects a bubble-pulse excitation by using the BUBBLE parameter on the *USA INCIDENT PRESSURE option. Once this has been selected, the user must then provide the TNT equivalent charge weight of the explosion, a bubble drag coefficient, a length scale factor ( USA bubble calculations have some embedded constants that use units of feet), a bubble cutoff time, and the elevation of the free surface. In addition, the user can indicate that the bubble is allowed to migrate toward the free surface by using the BUBBLE=MIGRATE parameter on the *USA INCIDENT PRESSURE option. Free surface corrections will not be performed unless the fluid surface information is given on the *USA FLUID PROPERTIES option. If the fluid surface data are given on the *USA FLUID PROPERTIES option, USA will use a pulsating and migrating bubble excitation regardless of whether the user specifies BUBBLE or BUBBLE=MIGRATE. For more information on bubble whip and the bubble-pulse calculations, see DeRuntz (1989) and DeRuntz et al. (1986).

Geometry and model The model consists of an open-ended cylindrical shell submerged 30.48 m (1200 in) below the surface. The origin of the coordinate system is at the cylinder's center, and only a quarter-model of the cylinder is required. For this three-dimensional analysis the fluid elevation direction must be oriented along the positive z-axis. The positive x-axis is along the axis of the cylinder. The explosive charge lies 15.24 m (600 in) directly below the cylinder's center. The charge standoff point (structural point nearest the charge) is at the lower surface of the cylinder.

Shell finite element model The cylindrical shell is modeled with S4R5 elements, using eight elements around the half-circumference and 10 along the half-length. Eighty USI4 interface elements are used to represent the fluid surface. Since both XSYMM and YSYMM are specified on the *USA FLUID PROPERTIES option, the quarter-model must be defined in the positive x-half-plane and the positive y-half-plane. The overall geometry of the problem is shown in Figure 10.1.1-1, while the quarter-shell mesh is shown in Figure 10.1.1-2. The input file for the S4R5/USI4 model is shown in ucw_usi4_p.inp. In the modeling approach with USI4 elements there is a one-to-one correspondence between USI interface and structural elements. For a given structural (or solid model) it is also possible to define a

10-1162

Underwater Shock Analyses

coarser fluid model using fluid element "overlay" interface elements. This approach is effective for reducing the size of the fluid element model in regions of small fluid pressure gradient and relatively large curvature. ABAQUS/USA supports two types of fluid element overlay elements: USI6O is a 6-node interface element for overlaying two structural elements, and USI9O is a 9-node interface element for overlaying four structural elements. Example fluid element overlay models are included with the ABAQUS release. Refer to the corresponding input files listed in the "Input files" section.

Beam element model The same problem is modeled using beam elements to discretize the structure and surface of revolution USI2SOR elements to model the fluid surface. In this case the total number of nodes is reduced to 11. Ten B31 elements are used along the half-length of the cylinder. A pipe cross-section is used for the beams, with the pipe radius and thickness given as 4.572 m (180.0 in) and 50.8 mm (2.0 in). Ten USI2SOR elements are used to model the interface to the surrounding fluid. Cosine and sine terms are selected for the SOR Fourier coefficients. Since this is a half-model (as opposed to the shell quarter-model), only XSYMM is used for the *USA FLUID PROPERTIES and *BOUNDARY specifications. All other aspects of the geometry and fluid model remain the same as above. This model requires comparatively fewer degrees of freedom and will run much faster. However, it is also limited in scope since it cannot model any local deformations (cross-sectional deformations). The input file for this model is shown in ucw_b31_p.inp. A slightly more realistic model can be generated using elbow elements in place of the beams. This allows some cross-sectional deformations of the structure to be represented. However, only nodal forces (from the fluid) are applied to the structure, and ovalization of the structure will not affect the fluid model (or its calculation of fluid pressure). Files ucw_s4_p.inp and ucw_s4_pm.inp contain elbow/SOR models.

Results and discussion The results for both models are discussed below.

Shell models The velocity history and strain history results obtained by ABAQUS/USA with the S4R5/USI4 model are compared to the USA-STAGS solution. The velocity histories of two points at the cylinder midspan (XSYMM plane) are shown in Figure 10.1.1-3. The upper plot shows the radial velocity history for the point closest to the charge, node 9 in Figure 10.1.1-2. The lower plot shows the radial velocity history for the cylinder midspan location away from the charge, node 1. The ABAQUS/USA and USA-STAGS velocity results compare very well for the low-frequency bending behavior. The difference in the high-frequency behavior is probably the result of differences in the formulations of the ABAQUS shell element (reduced integration) and the STAGS shell element (fully integrated). Experimentation with this example problem has shown that the velocity results (especially the high frequency content) change significantly with a change in the time increment size. The problem is sensitive enough to slight numerical changes that the changing word length (precision) from one machine to another may cause small differences in the velocity response.

10-1163

Underwater Shock Analyses

Strain history results at six locations along the length are shown in Figure 10.1.1-4. Strain histories (a) - (b) are taken from the "back" side of the cylinder, from the centroids of elements 1, 11, 21, 31, 41, and 51, respectively. The strain histories show very good agreement in the low-frequency range and moderate agreement in the high-frequency range. All of the USA-STAGS data shown for comparison were obtained from De Runtz (1991) and are the same data used in DeRuntz et al. (1986). In addition, results obtained for the model with 80 USI4 interface elements are compared against results obtained using a model with 20 USI9O fluid overlay interface elements and a model with 40 USI6O elements. All models employ the same structural model. For these models the velocity histories at the node closest to the charge are shown in Figure 10.1.1-5to be in good agreement, with any differences being caused by the different fluid models.

Beam/USI2SOR model The velocity history at selected nodal points from the ABAQUS/USA solution is compared against the USA-STAGS solution. The z-direction nodal velocity history of the cylinder symmetry plane (node 1) is shown in Figure 10.1.1-6. The ABAQUS/USA results compare well to the USA-STAGS results. The USA-STAGS data shown for comparison were obtained from DeRuntz (1994) and are the same data used in DeRuntz et al. (1986).

Input files Pulsating bubble excitation: ucw_b31_p.inp 10-element B31/USI2SOR model. ucw_10b31_p.inp 10-element multibranch B31/USI2SOR model. ucw_13b31_p.inp 13-element multibranch B31/USI2SOR model. ucw_usi2sor_0.inp 10-element ELBOW31/USI2SOR model, 0 ovalization modes. ucw_usi2sor_4.inp 10-element ELBOW31/USI2SOR model, 4 ovalization modes. ucw_s3r_p.inp 160-element S3R/USI3 element model. ucw_s4_p.inp 80-element S4/USI4 element model.

10-1164

Underwater Shock Analyses

ucw_s4r_p.inp 80-element S4R/USI4 element model. ucw_usi4_p.inp 80-element S4R5/USI4 model. ucw_usi90_p.inp 80 S4R5 and 20 USI9O elements. ucw_usi60_p.inp 80 S4R5 and 40 USI6O elements. ucw_stri3_p.inp 160-element STRI3/USI3 element model. ucw_mixed_ele.inp Mixed element model that uses shells and beams to model the structure and uses USI3, USI4, and USI2SOR elements to represent the fluid interface. Pulsating and migrating bubble excitation: ucw_s3r_pm.inp 160-element S3R/USI3 element model. ucw_s4_pm.inp 80-element S4/USI4 element model. ucw_s4r_pm.inp 80-element S4R/USI4 element model. ucw_usi4_pm.inp 80-element S4R5/USI4 model. ucw_stri3_pm.inp 160-element STRI3/USI3 element model. Pulsating and migrating bubble excitation with free surface corrections: ucw_s3r_pf.inp 160-element S3R/USI3 element model. ucw_s4_pf.inp 80-element S4/USI4 element model. ucw_s4r_pf.inp 80-element S4R/USI4 element model.

10-1165

Underwater Shock Analyses

ucw_usi4_pf.inp 80-element S4R5/USI4 model. ucw_stri3_pf.inp 160-element STRI3/USI3 element model.

References · DeRuntz, J. A., Jr., Private Communication, 1991. · DeRuntz, J. A., Jr., Private Communication, 1994. · DeRuntz, J. A., Jr., "The Underwater Shock Analysis Code and its Applications, " 60th Shock and Vibration Symposium Proceedings, vol. 1, pp. 89-107, 1989. · DeRuntz, J. A., Jr., C. C. Rankin, F. A. Brogan, and M. E. Reglebrugge, "Enhanced Analysis Capability in USA-STAGS," LMSC-D062084, Lockheed Palo Alto Research Laboratory, 1986.

Figures Figure 10.1.1-1 Cylinder whip overall geometry.

Figure 10.1.1-2 Cylinder whip quarter-shell model.

10-1166

Underwater Shock Analyses

Figure 10.1.1-3 Shell model velocity time histories. Solid line: ABAQUS/USA (S4R5) results. Dashed line: USA-STAGS results.

10-1167

Underwater Shock Analyses

Figure 10.1.1-4 Shell model strain time histories. Solid line: ABAQUS/USA (S4R5) results. Dashed line: USA-STAGS results.

10-1168

Underwater Shock Analyses

Figure 10.1.1-5 General and fluid overlay interface element model velocity time histories. Solid line: Reference USI4 results. Dashed line: USI9O results. Dotted line: USI6O results.

10-1169

Underwater Shock Analyses

Figure 10.1.1-6 SOR model velocity time history. Vertical velocity of the X-symmetry plane. Solid line: ABAQUS/USA results. Dashed line: USA-STAGS results.

Sample listings

10-1170

Underwater Shock Analyses

Listing 10.1.1-1 *HEADING NSWC BUBBLE-PULSE CYLINDER WHIP CYLINDER QUARTER MODEL 80 element S4R5 model all dimensions in inches Cylindrical Pipe;length=3600.0,radius=180.0, thickness = 2.0 Cylindrical Pipe Properties;E=30E6,nu=0.3, rho=1.6274 Fluid properties;rho=9.346E-5,c=60000.0 Infinite Fluid, Pulsating (Non-Migrating) Bubble Excitation *RESTART,WRITE,OVERLAY *NODE, NSET=ENDS 1, 0.0, 0.0, 180.0 9, 0.0, 0.0, -180.0 1001, 0.0, 0.0, 0.0 101, 1800.0, 0.0, 180.0 109, 1800.0, 0.0, -180.0 2001, 1800.0, 0.0, 0.0 *NGEN, LINE=C, NSET=MID 1, 9,, 1001,,,, -1.0, 0.0, 0.0 *NGEN, LINE=C, NSET=END 101, 109,, 2001,,,, -1.0, 0.0, 0.0 *NFILL, NSET=ALL MID, END, 10, 10 *NSET, NSET=EDGES, GENERATE 1, 101, 10 9, 109, 10 ** ** Structural Shell Elements ** *ELEMENT, TYPE=S4R5 1, 1, 11, 12, 2 *ELGEN, ELSET=CYL 1, 8, 1, 1, 10, 10, 10 *SHELL SECTION, ELSET=CYL, MATERIAL=STEEL 2.0, *MATERIAL, NAME=STEEL *ELASTIC 30.0E6, 0.3

10-1171

Underwater Shock Analyses

*DENSITY 4.2117E-3, ** ** USA structural interface element definitions ** *ELEMENT, TYPE=USI4 1001, 1, 11, 12, 2 *ELGEN, ELSET=FLUID 1001, 8, 1, 1, 10, 10, 10 *INTERFACE, ELSET=FLUID *USA FLUID PROPERTIES, DAA2=0.0, XSYMM, YSYMM 9.346E-5, 60000.0 ** *BOUNDARY MID, XSYMM EDGES, YSYMM ** ** Step 1 ** *STEP *USA ADDED MASS GENERATION *NODE PRINT, FREQUENCY=0 *EL PRINT, FREQUENCY=0 *END STEP ** ** Step 2 ** *STEP, INC=500 *DYNAMIC, ALPHA=0.0 0.002, 1.0 ** bubble is pulsating only (no migration, ** no free surface corrections) *USA INCIDENT PRESSURE, BUBBLE 0.0, 0.0, -600.0, 0.0, 0.0, -180.0 1000.0, 2.25, 0.083333, 0.57 1800.0, *NSET, NSET=TEMP 1, 9 *NODE FILE, NSET=TEMP, FREQUENCY=1 V, *OUTPUT,FIELD,FREQ=1 *NODE OUTPUT,NSET=TEMP V,

10-1172

Underwater Shock Analyses

*OUTPUT,HISTORY,FREQ=1 *NODE OUTPUT,NSET=TEMP V, *ELSET, ELSET=TEMP 1, 11, 21, 31, 41, 51 *EL FILE, ELSET=TEMP, FREQUENCY=1 3, E, *MONITOR, NODE=9, DOF=3, FREQUENCY=999 *END STEP

10-1173

Underwater Shock Analyses

Listing 10.1.1-2 *HEADING NSWC BUBBLE-PULSE BEAM WHIP CYLINDER HALF MODEL 10 element B31/USI2SOR model all dimensions in inches Cylindrical Pipe;length=3600.0,radius=180.0, thickness=2.0 Cylindrical Pipe Properties;E=30E6,nu=0.3, rho=1.6274 Fluid properties;rho=9.346E-5,c=60000.0 Infinite Fluid, Pulsating (Non-Migrating) Bubble Excitation *RESTART,WRITE,OVERLAY *NODE, NSET=MID 1, 0.0, 0.0, 0.0 *NODE, NSET=END 11, 1800.0, 0.0, 0.0 *NGEN, NSET=ALL 1, 11 ** ** Structural Beam Elements ** *ELEMENT, TYPE=B31, ELSET=CYL 1, 1, 2 *ELGEN, ELSET=CYL 1, 10, 1, 1 *BEAM SECTION, SECTION=PIPE, ELSET=CYL, MATERIAL=STEEL 180.0, 2.0 *MATERIAL, NAME=STEEL *ELASTIC 30.0E6, 0.3 *DENSITY 4.2117E-3, ** ** USA structural interface element definitions ** *ELEMENT, TYPE=USI2SOR, ELSET=FLUID 1001, 1, 2 1002, 2, 3 1003, 3, 4

10-1174

Underwater Shock Analyses

1004, 4, 5 1005, 5, 6 1006, 6, 7 1007, 7, 8 1008, 8, 9 1009, 9,10 1010, 10,11 *SOR PROPERTIES, ELSET=FLUID, COSINE, SINE 0, 0.0, 180.0 *USA FLUID PROPERTIES, XSYMM, DAA2=0.0 9.346E-5, 60000.0 *BOUNDARY MID, XSYMM ** ** Step 1 ** *STEP *USA ADDED MASS GENERATION *NODE PRINT, FREQUENCY=0 *EL PRINT, FREQUENCY=0 *END STEP ** ** Step 2 ** *STEP, INC=500 *DYNAMIC, ALPHA=0.0 0.002, 1.0 ** bubble is pulsating only (no migration, no ** free surface corrections) *USA INCIDENT PRESSURE, BUBBLE 0.0, 0.0, -600.0, 0.0, 0.0, -180.0 1000.0, 2.25, 0.083333, 0.57 1800.0, *NSET, NSET=TEMP 1, *NODE FILE, NSET=TEMP, FREQUENCY=1 V, *OUTPUT,FIELD,FREQ=1 *NODE OUTPUT,NSET=TEMP V, *OUTPUT,HISTORY,FREQ=1 *NODE OUTPUT,NSET=TEMP

10-1175

Underwater Shock Analyses

V, *ELSET, ELSET=TEMP 1, *EL FILE, ELSET=TEMP, FREQUENCY=1 E, *ELSET, ELSET=TEMP 1001, *OUTPUT,FIELD,FREQ=1 *ELEMENT OUTPUT,ELSET=TEMP PTOT, *OUTPUT,HISTORY,FREQ=1 *ELEMENT OUTPUT,ELSET=TEMP PTOT, *EL FILE, ELSET=TEMP, FREQUENCY=1 PTOT, *MONITOR, NODE=1, DOF=3, FREQUENCY=999 *END STEP

10-1176

Underwater Shock Analyses

Listing 10.1.1-3 *HEADING NSWC BUBBLE-PULSE CYLINDER WHIP CYLINDER QUARTER MODEL 20 (5x4) USI9O fluid element, 80 S4R5 structural element model all dimensions in inches Cylindrical Pipe;length=3600.0,radius=180.0, thickness=2.0 Cylindrical Pipe Properties;E=30E6,nu=0.3, rho=1.6274 Fluid properties;rho=9.346E-5,c=60000.0 Infinite Fluid, Pulsating (Non-Migrating) Bubble Excitation *RESTART,WRITE,OVERLAY *NODE, NSET=ENDS 1, 0.0, 0.0, 180.0 9, 0.0, 0.0, -180.0 1001, 0.0, 0.0, 0.0 101, 1800.0, 0.0, 180.0 109, 1800.0, 0.0, -180.0 2001, 1800.0, 0.0, 0.0 *NGEN, LINE=C, NSET=MID 1, 9,, 1001,,,, -1.0, 0.0, 0.0 *NGEN, LINE=C, NSET=END 101, 109,, 2001,,,, -1.0, 0.0, 0.0 *NFILL, NSET=ALL MID, END, 10, 10 *NSET, NSET=EDGES, GENERATE 1, 101, 10 9, 109, 10 ** ** Structural Shell Elements ** *ELEMENT, TYPE=S4R5 1, 1, 11, 12, 2 *ELGEN, ELSET=CYL 1, 8, 1, 1, 10, 10, 10 *SHELL SECTION, ELSET=CYL, MATERIAL=STEEL 2.0, *MATERIAL, NAME=STEEL *ELASTIC

10-1177

Underwater Shock Analyses

30.0E6, 0.3 *DENSITY 4.2117E-3, ** ** USA structural interface element definitions ** *ELEMENT, TYPE=USI9O 1001, 1, 21, 23, 3, 11, 22, 13, 2, 12 *ELGEN, ELSET=FLUID 1001, 4, 2, 1, 5, 20, 10 *INTERFACE, ELSET=FLUID *USA FLUID PROPERTIES, DAA2=0.0, XSYMM, YSYMM 9.346E-5, 60000.0 *BOUNDARY MID, XSYMM EDGES, YSYMM ** ** ** Step 1 ** *STEP *USA ADDED MASS GENERATION *NODE PRINT, FREQUENCY=0 *EL PRINT, FREQUENCY=0 *END STEP ** ** Step 2 ** *STEP, INC=500 *DYNAMIC, ALPHA=0.0 0.002, 1.0 ** bubble is pulsating only (no migration, no ** free surface corrections) *USA INCIDENT PRESSURE, BUBBLE 0.0, 0.0, -600.0, 0.0, 0.0, -180.0 1000.0, 2.25, 0.083333, 0.57 1800.0, *NSET, NSET=NOUT 1, 9 *OUTPUT,FIELD,FREQ=1 *NODE OUTPUT,NSET=NOUT V, *OUTPUT,HISTORY,FREQ=1

10-1178

Underwater Shock Analyses

*NODE OUTPUT,NSET=NOUT V, *NODE FILE, NSET=NOUT, FREQUENCY=1 V, *ELSET, ELSET=ELF 1001, 1004 *EL FILE, ELSET=ELF, FREQUENCY=1 PTOT, *OUTPUT,FIELD,FREQ=1 *ELEMENT OUTPUT,ELSET=ELF PTOT, *OUTPUT,HISTORY,FREQ=1 *ELEMENT OUTPUT,ELSET=ELF PTOT, *FILE FORMAT, ZERO INCREMENT *MONITOR, NODE=9, DOF=3, FREQUENCY=1 *END STEP

10-1179

Postprocessing of ABAQUS Results Files

11. Postprocessing of ABAQUS Results Files 11.1 Postprocessing examples 11.1.1 User postprocessing of ABAQUS results files: overview This chapter illustrates how to write and utilize postprocessing programs to manipulate data stored on the ABAQUS results file. The results file, which is identified by the file extension .fil, is created by the *CONTACT FILE, *EL FILE, *NODE FILE, *ENERGY FILE, *MODAL FILE, and *RADIATION FILE options and contains results based on user-specified output requests. The standard file format is binary, but it can be changed by user request for each run with the *FILE FORMAT, ASCII option. Alternatively, it can be set to a default ASCII format during site installation. ABAQUS uses FORTRAN unit 8 to communicate with the results file. Sample postprocessing programs that perform commonly exercised tasks are presented in separate sections in this chapter. These include merging multiple results files and converting the resulting results file from binary format to ASCII, or vice-versa; computing principal values and directions of stress and strain; and computing a perturbed mesh for a collapse analysis by incorporating a user-specified geometric imperfection in the form of the critical buckling mode shape. Each postprocessing program must be linked using the make parameter when running the ABAQUS execution procedure (see ``Execution procedure for ABAQUS/Make,'' Section 3.2.10 of the ABAQUS/Standard User's Manual). To link properly, the postprocessing program cannot contain a FORTRAN PROGRAM statement. Instead, the program must begin with a FORTRAN SUBROUTINE with the name HKSMAIN. General programming concepts, ABAQUS FORTRAN interfaces, and data processing concepts are described below. Refer to Chapter 5, "File Output Format," of the ABAQUS/Standard User's Manual for additional information. The program listings in each section provide details on the program flow, how to interface with various computer platforms that use different operating systems and FORTRAN compilers, and how to interface with ABAQUS subroutines to handle data files and records.

Initialization Details about the variables that are used in the postprocessing programs are discussed in ``Accessing the results file information,'' Section 5.1.3 of the ABAQUS/Standard User's Manual. ABAQUS uses a 512-word buffer named ARRAY for the reading and writing of data on the results file. This is dimensioned as ARRAY(513). The integer equivalent is JRRAY(513) for a 64-bit computer or JRRAY(2,513) for a 32-bit computer. The EQUIVALENCE statement is used to equivalence ARRAY and JRRAY to simplify manipulation of real and integer numbers in the data record stored in the buffer. The information concerning the FORTRAN unit number and format of the results file that is read is defined in LRUNIT(2,NRU), where NRU is the number of files to be processed. The FORTRAN unit number for the nth file is stored in LRUNIT(1,n). The information about the file format is stored in LRUNIT(2,n), which is initialized to 1 for ASCII format and to 2 for binary format. If a new results

11-1180

Postprocessing of ABAQUS Results Files

file is to be created by the postprocessing program, the file format of the output file is defined similarly via the variable LOUTF, which is also initialized to 1 for ASCII format and 2 for binary format. The root file name for both input and output results files is defined through the character variable FNAME. The root file name case will be the same as the case in which FNAME is defined; ABAQUS defines the file extensions to be lowercase letters. See ``Accessing the results file information,'' Section 5.1.3 of the ABAQUS/Standard User's Manual, for a discussion of the naming convention for the file extensions. The final initialization phase is done internally by calling the ABAQUS subroutines INITPF and DBRNU. The FORTRAN interfaces are CALL INITPF(FNAME, NRU, LRUNIT, LOUTF) CALL DBRNU (JUNIT)

where the arguments in the call to INITPF are as described above, and JUNIT is the FORTRAN unit number connecting the file. These integer variables must be defined before the subroutines are called.

Data processing Data manipulation requires knowledge of each data record. Details of these records are found in ``Results file output format,'' Section 5.1.2 of the ABAQUS/Standard User's Manual. The data organization in the results file uses a sequential format. Each record must, therefore, be retrieved in a sequential manner via a call to DBFILE using the interface CALL DBFILE(0, ARRAY, JRCD)

This call can be placed inside a DO-loop, and the loop count should exceed the number of records stored in the file. Alternatively, DBFILE can be called as long as JRCD is equal to 0. The first argument, 0, indicates that a record is to be read. Each record that is read is stored in the buffer ARRAY and returned to the calling program for manipulation. The last argument, JRCD, is a return code that is set to 0 unless an end-of-file condition or an incomplete record is processed, in which case JRCD is set to 1. If it is desirable to extract or modify certain records and save them in a new results file with the same data organization as an ABAQUS-generated results file, then the subroutine DBFILW should be called with the interface CALL DBFILW(1, ARRAY, JRCD)

The new results file will be written with the file extension .fin. Refer to ``Utility routines for accessing the results file,'' Section 5.1.4 of the ABAQUS/Standard User's Manual.

11.1.2 Joining data from multiple results files and converting file format: FJOIN Product: ABAQUS/Standard This example illustrates how to use a FORTRAN program to extract specific data from different

11-1181

Postprocessing of ABAQUS Results Files

ABAQUS results files and to join the data into a single results file. This program can also be used to convert the format of results files.

Postprocessing Sometimes it is desirable to combine a number of results files into a single file or to create a new results file by retrieving selected data from different results files. The ABAQUS/Append procedure joins two results files by stripping the header information from the second results file and appending the step information to the end of the first results file. See ``Execution procedure for joining results (.fil) files,'' Section 3.2.7 of the ABAQUS/Standard User's Manual, for more information on this utility. This example postprocessing program demonstrates how a FORTRAN program can be used to extract specific information from results files created by separate analyses of the same model. In this example the stress and strain records in three analyses will be merged to create a new results file.

Programming details The general discussion on programming concepts and ABAQUS FORTRAN interfaces in ``User postprocessing of ABAQUS results files: overview,'' Section 11.1.1, should be reviewed before running or modifying this program. Review of the results file format in Chapter 5, "File Output Format," of the ABAQUS/Standard User's Manual is also recommended. The program FJOIN (named fjoin.f on the ABAQUS release media), prompts for the values of NRU, LRUNIT(1,NRU), LRUNIT(2,NRU), and FNAME. Then subroutines INITPF and DBNRU are called to complete the necessary initializations and file connections. Data processing starts with a double DO-loop looping over all of the records to be read, one-by-one, via a call to DBFILE. A record can be skipped or written to the new results file with or without any modifications. Each record is identified by its record key, which is stored in the second entry of the record (see ``Results file output format,'' Section 5.1.2 of the ABAQUS/Standard User's Manual). Each file contains a number of header records, ( 1900-series). These records contain general information about the model. Different analyses using the same model place essentially the same information in these records. Hence, when combining results files from different analyses of the same model, all 1900-series records from the first file that is processed should be kept. Similar records in subsequent files should be skipped to avoid duplication and confusion. However, the 1910, 1911, 1922, and 1980 records should be kept. They are useful for processing superelement results, output requests, and natural frequency extraction results. The data for each increment of an analysis begins with the increment start record, which is identified by record key 2000. Record 2000 is followed by the records that correspond to the data requested through file output options specified in the ABAQUS input file. Record 1, the element header record, is automatically written to the results file when the *EL FILE option is used in the input file. It is of interest when postprocessing since it contains important information about the element data, including the location of data within an element (i.e., whether data are written at the element integration points, the centroid, nodes, etc.). For this example, records 11 and 21, the stress and strain records, respectively, are written to the results file since stress and strain were requested through the *EL FILE

11-1182

Postprocessing of ABAQUS Results Files

option. The increment end record is identified by record key 2001. When an end-of-file condition is encountered and the previously processed record is a 2001 record, a FORTRAN CLOSE is executed on the current FORTRAN unit number so that the processing of the next file can begin.

Program compilation and linking The ABAQUS/Make procedure is designed to compile and link this type of postprocessing program. It will also make the aba_param.inc file available during compilation. The ABAQUS/Make command to compile and link the FJOIN program is as follows: abaqus make job=fjoin

This command will have to be repeated if FORTRAN errors are discovered during the compilation or link. The commands used by the ABAQUS/Make procedure can be changed if necessary. The ABAQUS Site Guide lists the typical compile and link commands for each computer type.

Program execution Before program execution, the analysis jobs must be run to generate results files to be read by the program. In this example three jobs are run. The input files for these analyses are fjoin002.inp, fjoin003.inp, and fjoin004.inp. The results files from these analyses are output in binary format and are called fjoin002.fil, fjoin003.fil, and fjoin004.fil. The FJOIN program will read these files via FORTRAN units 2, 3, and 4. The name of the new file will be fjoinxxx. Before running the program, the results files must be renamed to fjoinxxx.002, fjoinxxx.003, and fjoinxxx.004. Note that the root file names are the same (defined using FNAME), and that the extensions are set to the FORTRAN unit numbers used to open the files. When the program is executed using the command abaqus fjoin, the first prompt will be Enter the number of files to be joined:

Enter 3 to set NRU=3. The second prompt will be Enter the unit number of input file # 1:

Enter 2 to define LRUNIT(1,1)=2. At the third prompt, Enter the format of input file # 1 (1-ASCII, 2-binary):

enter 2. This sets LRUNIT(2,1)=2 and means that the file being read is binary. The second and third prompts are repeated for each additional file to be processed. The program will then ask whether the new results file should be written in ASCII or binary format, Enter the format of the output file (1-ASCII, 2-binary):

Enter 2 to set LOUTF=2, which specifies that binary format has been chosen for the new results file. The format of the output file may be different from the format of the input files, so this program can also be used to convert the format of results files. Finally, when the program issues the prompt Enter the name of the input files (w/o extension):

enter fjoinxxx to define FNAME (the input files must have been given the root file name

11-1183

Postprocessing of ABAQUS Results Files

fjoinxxx; the output file will be created as fjoinxxx.fin).

As soon as the nth file has been processed, the message END OF FILE # n is written to the terminal. After all files have been processed, the program stops and the new results file is created. The new results file created by this program contains stress and strain records at all integration points in each element and at all nodal points.

Analysis description The structure is a 10 ´ 10 square plate with unit thickness. The plate lies in the X-Y plane such that its bottom edge coincides with the x-axis and the left edge coincides with the y-axis. The finite element model employs a 2 ´ 2 mesh of CPS8R elements. The material is linear elastic with Young's modulus = 30 ´ 106 and Poisson's ratio = 0.3. Three separate analyses are performed with displacement controlled load steps. In the first analysis (fjoin002.inp), the plate is subjected to biaxial tension by prescribing a vertical displacement of 0.25 along the top edge, a horizontal displacement of 0.25 along the right edge and symmetry boundary conditions on the left and bottom edges. In the second analysis (fjoin003.inp), the structure is forced to deform in simple shear by applying a horizontal displacement of 0.25 to the top edge while holding the bottom edge fixed and allowing the horizontal displacement to vary linearly with y along the left and right edges. The vertical displacement is zero everywhere. In the third analysis (fjoin004.inp), the plate is subjected to uniaxial tension by applying a displacement of 0.25 in the y-direction to the nodes along the top edge and symmetry boundary conditions to the nodes along the x- and y-axes.

Results and discussion Since the state of stress and strain is homogeneous, the integration point and nodal averaged values of stress and strain are identical everywhere. A typical record obtained at the end of each step is included below: ¾yy ¾xy ¾xx Analysis fjoin002.inp 0.0 1.07 ´ 1.07 ´ 106 106 fjoin003.inp 0.0 0.0 2.88 ´ 105 fjoin004.inp 0.0 0.0 7.50 ´ 5 10 "yy "xy " xx Analysis -2 -2 fjoin002.inp 2.50 ´ 10 0.0 2.50 ´ 10 fjoin003.inp 0.0 0.0 2.50 ´ 10-2 fjoin004.inp -7.50 ´ 10-3 2.50 ´ 10-2 0.0

Input files fjoin002.inp

11-1184

Postprocessing of ABAQUS Results Files

First analysis file. fjoin003.inp Second analysis file. fjoin004.inp Third analysis file. fjoin.f Postprocessing program.

Sample listings

11-1185

Postprocessing of ABAQUS Results Files

Listing 11.1.2-1 SUBROUTINE HKSMAIN C==================================================================== C This program must be compiled and linked with the command: C abaqus make job=fjoin C Run the program using the command: C abaqus fjoin C==================================================================== C C Purpose (this program performs two functions): C C 1. It can be used to join together a number of ABAQUS results files. C The program will prompt the user for the number of files to be C joined, the FORTRAN unit numbers associated with each file and C the file format, ASCII or binary. The user will also be prompted C for the format of the output file and the root name of the files. C C 2. It can be used to convert the format of a file from binary to C ASCII or vice-versa. This can be accomplished by reading one C file as input and giving the opposite format for the output file. C C Input File names: C C The results file to be processed should be named 'FNAME.0xx', C where xx is a 2-digit FORTRAN unit number less than 31. C Certain units within this range are used by ABAQUS internally and C by this program and cannot be used by the user. These are 01, C 05, 06, 07, 09, 11, 12, 13, 20 and 28. C C Output File name: C C 'FNAME'.fin C C==================================================================== C C Variables used by this program: C C ARRAY -- Real array containing values read from results file C (.fil). Equivalenced to JRRAY. C JRRAY -- Integer array containing values read from results file C (.fil). Equivalenced to ARRAY. C FNAME -- Root file name of input file(s) and output file.

11-1186

Postprocessing of ABAQUS Results Files

C NRU -- Number of results files (.fil) to be read. C LRUNIT -- Array containing unit number and format of results files: C LRUNIT(1,*) --> Unit number of input file. C LRUNIT(2,*) --> Format of input file. C LOUTF -- Format of output file: C 1 --> ABAQUS results file ASCII format. C 2 --> ABAQUS results file binary format. C JUNIT -- Unit number of file to be opened. C JRCD -- Error check return code: C .EQ. 0 --> No errors. C .NE. 0 --> Errors detected. C KEY -- Current record key identifier. C C==================================================================== C C The use of ABA_PARAM.INC eliminates the need to have different C versions of the code for single and double precision. C ABA_PARAM.INC defines an appropriate IMPLICIT REAL statement and C sets the value of NPRECD to 1 or 2, depending on whether the C machine uses single or double precision. C C==================================================================== C INCLUDE 'aba_param.inc' DIMENSION ARRAY(513), JRRAY(NPRECD,513) EQUIVALENCE (ARRAY(1), JRRAY(1,1)) C C==================================================================== C Set the dimensions of LRUNIT to be the maximum number of results C files to be joined. C C==================================================================== PARAMETER (MXUNIT=21) INTEGER LRUNIT(2,MXUNIT),LUNIT(10) CHARACTER FNAME*80 DATA LUNIT/1,5,6,7,9,11,12,13,20,28/ C C==================================================================== C Input the number of files to be joined and then the unit number and C format of each of the files. C C==================================================================== 5 CONTINUE

11-1187

Postprocessing of ABAQUS Results Files

WRITE(6,10) MXUNIT 10 FORMAT(1X,'Enter the number of files to be joined (MAX:',I3,'):') READ(5,'(I3)') NRU IF (NRU .GT. MXUNIT) GOTO 5 C C DO 40 INRU = 1, NRU 15 CONTINUE WRITE(6,20) INRU 20 FORMAT(1X,'Enter the unit number of input file #',I3,':') READ(5,*) LRUNIT(1,INRU) DO 41 K1=1,9 IF (LRUNIT(1,INRU) .EQ. LUNIT(K1)) THEN WRITE(6,*) 'ERROR! Unit number cannot be ',LUNIT(K1) GOTO 15 ENDIF 41 CONTINUE 42 CONTINUE WRITE(6,30) INRU 30 FORMAT(1X,'Enter the format of input file #',I3, 1 ' (1-ASCII, 2-binary):') READ(5,*) LRUNIT(2,INRU) IF (LRUNIT(2,INRU).NE. 1 .AND. LRUNIT(2,INRU) .NE. 2) THEN WRITE(6,*) 'ERROR! This number must be 1 or 2' GOTO 42 ENDIF 40 CONTINUE C C==================================================================== C Set LOUTF equal to the format of the output file. If this program C is to be used only to convert the file format from one type to C another, set NRU=1 (to read only one file) and specify a value of C LOUTF which is opposite to the value specified for LRUNIT(2,1). C C==================================================================== 45 CONTINUE WRITE(6,50) 50 FORMAT(1X,'Enter the format of the output file ', 1 '(1-ASCII, 2-binary):') READ(5,*) LOUTF IF (LOUTF .NE. 1 .AND. LOUTF .NE. 2) THEN WRITE(6,*) 'ERROR! This number must be 1 or 2' GOTO 45

11-1188

Postprocessing of ABAQUS Results Files

ENDIF C WRITE(6,60) 60 FORMAT(1X,'Enter the name of the input file(s) (w/o extension):') READ(5,'(A)') FNAME C CALL

INITPF (FNAME, NRU, LRUNIT, LOUTF)

C KEYPRV = 0 C C==================================================================== C Loop through NRU input files... C C==================================================================== DO 100 INRU = 1, NRU JUNIT = LRUNIT(1,INRU) CALL DBRNU (JUNIT) I2001 = 0 C==================================================================== C ...and cover a maximum of 10 million records in each file. C C==================================================================== DO 80 IXX2 = 1, 100 DO 80 IXX = 1, 99999 CALL DBFILE(0,ARRAY,JRCD) C WRITE(6,*) 'KEY/RECORD LENGTH = ', JRRAY(1,2),JRRAY(1,1) IF (JRCD .NE. 0 .AND. KEYPRV .EQ. 2001) THEN WRITE(6,*) 'END OF FILE #', INRU CLOSE (JUNIT) GOTO 100 ELSE IF (JRCD .NE. 0) THEN WRITE(6,*) 'ERROR READING FILE #', INRU CLOSE (JUNIT) GOTO 110 ENDIF C C==================================================================== C Initialize the flag to write a record to the file: C LWRITE=0 -- write disabled C LWRITE=1 -- write enabled C C==================================================================== LWRITE=1

11-1189

Postprocessing of ABAQUS Results Files

C C==================================================================== C For files other than the first, skip the 1900-series header records C except for the superelement path (1910; for superelement analyses), C output request (1911), heading (1922), and modal (1980; for natural C frequency extraction) records. In a merged file, the heading C record serves as a file delimiter. C C==================================================================== IF (INRU.GT.1) THEN IF (JRRAY(1,2).GE.1900 .AND. JRRAY(1,2).LE.1909) LWRITE=0 IF (JRRAY(1,2).GE.1912 .AND. JRRAY(1,2).LT.1922) LWRITE=0 C C==================================================================== C Skip the first 2001 record (this indicates the end of the header C records). C C==================================================================== IF (JRRAY(1,2) .EQ. 2001 .AND. I2001 .EQ. 0) THEN I2001 = 1 LWRITE = 0 ENDIF ENDIF C C==================================================================== C If this is the first input file, or if the write flag has not been C disabled for records in subsequent files, then write the data to C the output file. We are interested in retrieving the header C records (relevant 1900-series records), the increment start and C end records (2000 and 2001), the element header record, (1) and C the stress and strain records (11 and 21). C C==================================================================== IF (INRU .EQ. 1 .OR. LWRITE .EQ. 1) THEN KEY=JRRAY(1,2) IF((KEY.EQ.1900).OR.(KEY.EQ.1901).OR.(KEY.EQ.1902).OR. 1 (KEY.EQ.1910).OR.(KEY.EQ.1911).OR.(KEY.EQ.1921).OR. 2 (KEY.EQ.1922).OR.(KEY.EQ.1980).OR.(KEY.EQ.2000).OR. 3 (KEY.EQ.2001).OR.(KEY.EQ.1).OR.(KEY.EQ.11).OR. 4 (KEY.EQ.21)) THEN CALL DBFILW(1,ARRAY,JRCD) IF (JRCD .NE. 0) THEN WRITE(6,*) 'ERROR WRITING FILE'

11-1190

Postprocessing of ABAQUS Results Files

CLOSE (JUNIT) GOTO 110 ENDIF ENDIF ENDIF KEYPRV = JRRAY(1,2) 80 CONTINUE 100 CONTINUE 110 CONTINUE C RETURN END

11.1.3 Calculation of principal stresses and strains and their directions: FPRIN Product: ABAQUS/Standard This example illustrates the use of a FORTRAN program to read stress and strain records from an ABAQUS results file and to calculate principal stress and strain values and their directions.

General description This program shows how to retrieve integration point and nodal averaged stress and strain components from an ABAQUS results file and then compute principal values and directions using the ABAQUS subroutine SPRIND. Usage of this subroutine is documented in the program listing provided below, and further details about the interface to this subroutine are discussed in ``UMAT,'' Section 23.2.29 of the ABAQUS/Standard User's Manual. The results file created by the FJOIN program in ``Joining data from multiple results files and converting file format: FJOIN,'' Section 11.1.2, is used here to verify that the records that have been put together are retrievable. The previously generated results file was named fjoinxxx.fin. To use it as an input file for postprocessing program FPRIN, the file extension must be changed. This program will assume that the results file has the default .fil extension, which corresponds to FORTRAN unit 8.

Programming details The user should first review the general discussion on programming concepts and ABAQUS FORTRAN interfaces in ``User postprocessing of ABAQUS results files: overview,'' Section 11.1.1, and the detailed discussion of postprocessing given in Chapter 5, "File Output Format," of the ABAQUS/Standard User's Manual. When running program FPRIN (this program is named fprin.f on the ABAQUS release media), the user will be prompted for the file name that initializes FNAME. Other variables, such as LOUTF, NRU, LRUNIT(1,NRU), and LRUNIT(2,NRU), are initialized inside the program. INITPF and DBNRU are then called to complete the neccesary initializations and file connections. Data processing starts with a double DO-loop over all the records to be read, one-by-one, via a call to DBFILE. Each record

11-1191

Postprocessing of ABAQUS Results Files

is identified by its record key, which is stored in the second entry of the record. When records 1922 and 2000 are processed by program FPRIN, the heading and the current step and increment numbers are written out so as to provide a way to recognize the beginning of data in each analysis. Record type 1 is then examined to determine the output location of stress and strain, the number of direct and shear stress and strain components, and either the element number or the node number for which the records are written. The stress and strain records ( 11 and 21, respectively) will be filtered out for processing by the ABAQUS subroutine SPRIND. When a stress or strain record is passed into SPRIND, principal stresses or strains and the corresponding principal directions are calculated and returned in an unsorted order.

Program compilation and linking Before program execution, the FORTRAN program has to be compiled and linked. Both operations, as well as the inclusion of the aba_param.inc file, are performed by a single execution of the ABAQUS/Make procedure: abaqus make job=fprin

This may have to be repeated until all FORTRAN errors are corrected. After successful compilation, the program's object code is automatically linked with the ABAQUS object codes stored in the shared program library and interface library in order to build the executable program. Refer to Chapter 3, "Environment file," of the ABAQUS Site Guide to see which compile and link commands are used for a particular computer.

Program execution Before the program is executed, a results file must have been created. In this example the results file fjoinxxx.fin created by the FJOIN program discussed in ``Joining data from multiple results files and converting file format: FJOIN,'' Section 11.1.2, is used. This file must be renamed to fjoinxxx.fil since FORTRAN unit 8 (which is associated with the .fil file extension) is used in the program to read the file. When the program is executed using the command abaqus fprin, the prompt Enter the name of the input file (w/o .fil):

will appear. Enter fjoinxxx to define FNAME. The program processes the data and produces a file named pvalue.dat, which contains information about principal stresses and strains and their directions.

Results and discussion The computed principal stress and strain values and their directions are tabulated below. Analysis Principal Stress Strain Dir-1 Dir-2 Dir-3 Componen File ´ 105 ´ 10-3 t fjoin002.i 1 10.714 25.0 1.0 0.0 0.0 2 10.714 25.0 0.0 1.0 0.0 np 3 0.0 0.0 0.0 0.0 1.0 fjoin003.i 1 -2.8846 -12.5 0.707 -0.707 0.0

11-1192

Postprocessing of ABAQUS Results Files

np fjoin004.i np

2 3 1 2 3

2.8846 0.0 0.0 7.5 0.0

12.5 0.0 -7.5 25.0 0.0

0.707 0.0 1.0 0.0 0.0

Input file fprin.f Postprocessing program.

Sample listings

11-1193

0.707 0.0 0.0 1.0 0.0

0.0 1.0 0.0 0.0 1.0

Postprocessing of ABAQUS Results Files

Listing 11.1.3-1 SUBROUTINE HKSMAIN C==================================================================== C This program must be compiled and linked with the command: C abaqus make job=fprin C Run the program using the command: C abaqus fprin C==================================================================== C C Purpose: C C This program computes the principal stresses and strains and their C directions from stress and strain values stored in an ABAQUS C results file (.fil). C C Input File names: `FNAME.fil', where FNAME is the root file name of C the input file. C C Output File name: pvalue.dat C C==================================================================== C C Variables used by this program and ABAQUS subroutine SPRIND : C C NDI -- Number of direct components in stress/strain tensor. C NSHR -- Number of shear components in stress/strain tensor. C NDIP1 -- NDI + 1 C ARRAY -- Real array containing values read from results file C (.fil). Equivalenced to JRRAY. C JRRAY -- Integer array containing values read from results file C (.fil). Equivalenced to ARRAY. C FNAME -- Root file name of input file (w/o .fil extension). C NRU -- Number of results files (.fil) to be read. C LRUNIT -- Array containing unit number and format of results files: C LRUNIT(1,*) --> Unit number of input file. C LRUNIT(2,*) --> Format of input file. C LOUTF -- Format of output file: C 0 --> Standard ASCII format. C 1 --> ABAQUS results file ASCII format. C 2 --> ABAQUS results file binary format. C JUNIT -- Unit number of file to be opened. C JRCD -- Error check return code.

11-1194

Postprocessing of ABAQUS Results Files

C .EQ. 0 --> No errors. C .NE. 0 --> Errors detected. C KEY -- Current record key identifier. C JELNUM -- Current element number. C INTPN -- Integration point number. C LSTR -- Indicates type of principal value (stress/strain) and C ordering used: C For calculation of principal value (stress/strain): C 1 --> stress. C 2 --> strain. C For calculation of directions: C 1 --> stress. C 2 --> strain. C S -- Array containing stress tensor. C PS -- Array containing principal stresses. C ANPS -- Array containing directions of principal stresses. C E -- Array containing strain tensor. C PE -- Array containing principal strains. C ANPE -- Array containing directions of principal strains. C C==================================================================== C C The use of ABA_PARAM.INC eliminates the need to have different C versions of the code for single and double precision. C ABA_PARAM.INC defines an appropriate IMPLICIT REAL statement C and sets the value of NPRECD to 1 or 2, depending on whether C the machine uses single or double precision. C C==================================================================== C INCLUDE 'aba_param.inc' DIMENSION ARRAY(513), JRRAY(NPRECD,513), LRUNIT(2,1) EQUIVALENCE (ARRAY(1), JRRAY(1,1)) C C==================================================================== DIMENSION S(6), E(6), PS(3), PE(3), ANPS(3,3), ANPE(3,3) CHARACTER FNAME*80 C C==================================================================== C Get the name of the results file. C C==================================================================== WRITE(6,*) 'Enter the name of the input file (w/o .fil):'

11-1195

Postprocessing of ABAQUS Results Files

READ(5,'(A)') FNAME C C==================================================================== C Open the output file. C C==================================================================== OPEN(UNIT=9,FILE='pvalue.dat',STATUS='NEW') C NRU = 1 LOUTF = 0 LRUNIT(1,1) = 8 LRUNIT(2,1) = 2 C CALL INITPF(FNAME,NRU,LRUNIT,LOUTF) C JUNIT = 8 C CALL DBRNU(JUNIT) C C==================================================================== C Read records from the results (.fil) file and process the data. C Cover a maximum of 10 million records in the file. C C==================================================================== DO 1000 K100 = 1, 100 DO 1000 K1 = 1, 99999 CALL DBFILE(0,ARRAY,JRCD) IF (JRCD .NE. 0) GO TO 1001 KEY = JRRAY(1,2) C C==================================================================== C Get the heading (title) record. C C==================================================================== IF (KEY .EQ. 1922) THEN WRITE(9,1100) (ARRAY(IXX),IXX=3,12) 1100 FORMAT(1X,10A8) C C==================================================================== C Get the current step and increment number. C C==================================================================== ELSE IF (KEY .EQ. 2000) THEN

11-1196

Postprocessing of ABAQUS Results Files

1200

WRITE(9,1200) JRRAY(1,8), JRRAY(1,9) FORMAT(1X,'** STEP ',I2,' INCREMENT ',I3)

C C==================================================================== C Get the element and integration point numbers, JELNUM and INTPN, C and the location of INTPN (0--at int.pt., 1--at centroid, C 4--nodal average) and the number of direct and shear components C in the analysis. C C==================================================================== ELSE IF (KEY .EQ. 1) THEN JELNUM = JRRAY(1,3) INTPN = JRRAY(1,4) LOCATE = JRRAY(1,6) NDI = JRRAY(1,8) NSHR = JRRAY(1,9) NDIP1 = NDI + 1 IF(LOCATE.LE.1) THEN WRITE(9,1201) JELNUM, INTPN ,NDI,NSHR 1201 FORMAT(2X,'ELEMENT NUMBER = ',I8,5X, 1 'INT. PT. NUMBER = ',I2,5X, 2 'NDI/HSHR = ',2I2) ELSEIF(LOCATE.EQ.4) THEN WRITE(9,1191) JELNUM, NDI,NSHR 1191 FORMAT(2X,'NODE NUMBER = ',I8,5X, 1 'NDI/HSHR = ',2I2) END IF C C==================================================================== C Get the stress tensor. C C==================================================================== ELSE IF (KEY .EQ. 11) THEN WRITE(9,1202) 1202 FORMAT(3X,'STRESSES:') C DO 10 IXX = 1, NDI S(IXX) = ARRAY(IXX+2) 10 CONTINUE WRITE(9,1203) (S(IZZ), IZZ = 1, NDI) 1203 FORMAT(4X,'S11 = ',E12.5,' S22 = ',E12.5,' S33 = ',E12.5) DO 20 IYY = NDI + 1, NSHR + NDI S(IYY) = ARRAY(IYY+2)

11-1197

Postprocessing of ABAQUS Results Files

20 1204

CONTINUE WRITE(9,1204) (S(IZZ), IZZ = NDI + 1, NSHR + NDI) FORMAT(4X,'S12 = ',E12.5,' S13 = ',E12.5,' S23 = ',E12.5)

C C C==================================================================== C Calculate the principal stresses and corresponding principal C directions in unsorted order. C==================================================================== LSTR = 1 CALL SPRIND(S,PS,ANPS,LSTR,NDI,NSHR) WRITE(9,1205) PS(1), ANPS(1,1), ANPS(1,2), ANPS(1,3) 1205 FORMAT(4X,'PS1 = ',E12.5,/, 1 5X,'PD11 =',F8.3,2X,'PD12 =',F8.3,2X,'PD13 =',F8.3) WRITE(9,1206) PS(2), ANPS(2,1), ANPS(2,2), ANPS(2,3) 1206 FORMAT(4X,'PS2 = ',E12.5,/, 1 5X,'PD21 =',F8.3,2X,'PD22 =',F8.3,2X,'PD23 =',F8.3) WRITE(9,1207) PS(3), ANPS(3,1), ANPS(3,2), ANPS(3,3) 1207 FORMAT(4X,'PS3 = ',E12.5,/, 1 5X,'PD31 =',F8.3,2X,'PD32 =',F8.3,2X,'PD33 =',F8.3) C C C==================================================================== C Get the strain tensor. C C==================================================================== ELSE IF (KEY .EQ. 21) THEN WRITE(9,2202) 2202 FORMAT(3X,'STRAINS:') C DO 30 IXX = 1, NDI E(IXX) = ARRAY(IXX+2) 30 CONTINUE WRITE(9,2203) (E(IZZ), IZZ = 1, NDI) 2203 FORMAT(4X,'E11 = ',E12.5,' E22 = ',E12.5,' E33 = ',E12.5) DO 40 IYY = NDI + 1, NSHR + NDI E(IYY) = ARRAY(IYY+2) 40 CONTINUE WRITE(9,2204) (E(IZZ), IZZ = NDI + 1, NSHR + NDI) 2204 FORMAT(4X,'E12 = ',E12.5,' E13 = ',E12.5,' E23 = ',E12.5) C C C====================================================================

11-1198

Postprocessing of ABAQUS Results Files

C Calculate the principal strains and corresponding principal C directions in unsorted order. C==================================================================== LSTR = 2 CALL SPRIND(E,PE,ANPE,LSTR,NDI,NSHR) WRITE(9,2205) PE(1), ANPE(1,1), ANPE(1,2), ANPE(1,3) 2205 FORMAT(4X,'PE1 = ',E12.5,/, 1 5X,'PD11 =',F8.3,2X,'PD12 =',F8.3,2X,'PD13 =',F8.3) WRITE(9,2206) PE(2), ANPE(2,1), ANPE(2,2), ANPE(2,3) 2206 FORMAT(4X,'PE2 = ',E12.5,/, 1 5X,'PD21 =',F8.3,2X,'PD22 =',F8.3,2X,'PD23 =',F8.3) WRITE(9,2207) PE(3), ANPE(3,1), ANPE(3,2), ANPE(3,3) 2207 FORMAT(4X,'PE3 = ',E12.5,/, 1 5X,'PD31 =',F8.3,2X,'PD32 =',F8.3,2X,'PD33 =',F8.3) C END IF C 1000 CONTINUE 1001 CONTINUE C CLOSE (UNIT=9) C RETURN END

11.1.4 Creation of a perturbed mesh from original coordinate data and eigenvectors: FPERT Product: ABAQUS/Standard This example illustrates the use of a FORTRAN program to create a perturbed mesh by superimposing a small imperfection in the form of the weighted sum of several buckling modes on the initial geometry. The program retrieves the original nodal coordinates and the desired eigenvectors from an ABAQUS results file, then calculates new nodal coordinates for the perturbed mesh.

General description Collapse studies of a structure's postbuckling load-displacement (Riks) behavior are often conducted to verify that the critical buckling load and mode predicted by an eigenvalue buckling analysis are accurate. They are also done to investigate the effect of an initial geometric imperfection on the load-displacement response. A typical assumption is that an imperfection made up of a combination of the eigenmodes associated with the lowest eigenvalues will be the most critical. One method of PM introducing an imperfection of this type into the model is by adding i=1 ®i ui to the original mesh coordinates. In this case ui is the ith eigenmode, ®i is a scaling factor of the ith eigenmode, and M is

11-1199

Postprocessing of ABAQUS Results Files

the total number of eigenmodes extracted in the buckling analysis. Since the eigenvector is typically normalized to a maximum absolute value of one, ®i is usually some fraction of a geometric parameter, such as the shell thickness. The postprocessing program described below can be used to introduce an imperfection of this type into a model. The perturbation procedure is illustrated in ``Buckling of a cylindrical shell under uniform axial pressure,'' Section 1.2.3 of the ABAQUS Benchmarks Manual. An eigenvalue buckling analysis, fpert001, is run first. This analysis creates the results file, fpert001.fil, which contains the original nodal coordinates and the eigenvectors for the buckling modes. This results file is then used to generate a perturbed mesh for the postbuckling load-displacement analysis. The postprocessing program perturbs the original mesh using the relation 0

X =X+

M X

®i ui ;

i=1

where X0 is the vector containing the new global coordinates; X is the vector of original coordinates; M is the number of buckling modes; and ®i is the imperfection factor for the ith eigenvector, ui . The new coordinates are written to the file fpert002.015, which is read by the load-displacement analysis fpert002.

Programming details The general discussion on programming concepts and ABAQUS FORTRAN interfaces in ``User postprocessing of ABAQUS results files: overview,'' Section 11.1.1, should be reviewed before running or modifying this program. Review of the results file format in Chapter 5, "File Output Format," of the ABAQUS/Standard User's Manual is also recommended. The FPERT program (this program is named fpert.f on the ABAQUS release media) makes some assumptions concerning the type of results file it will be reading. Variables NRU, LRUNIT(1,NRU), and LRUNIT(2,NRU) are initialized within the program to 1, 8, and 2. These values indicate that one file will be read, the FORTRAN unit used will be 8, and the file type will be binary. See ``Accessing the results file information,'' Section 5.1.3 of the ABAQUS/Standard User's Manual, for more information on opening and initializing postprocessing files. Once the file specification parameters are set, the INITPF and DBNRU subroutines are called to open and ready the file, whose name is stored in FNAME, for reading. The file to which the perturbed coordinates are to be written can be directly opened using a FORTRAN OPEN statement. The ABAQUS file utilities are not necessary since the file is a plain text file. The records with the original nodal coordinates are read using the DBFILE routine and stored in the local array COORDS(3,8000). The first index of the COORDS array indicates the x-, y-, and z-coordinate of the node. The second index indicates the node number. The second dimension should be increased if there are more than 8000 nodes in a model. Components of the eigenvector are stored in the local array DISP(6,8000). This array holds up to 6 displacement terms for each node. The second dimension should be increased if there are more than 8000 nodes in a model. Subroutine NODEGEN, a subroutine local to this postprocessing program, is 11-1200

Postprocessing of ABAQUS Results Files

then called to compute the new nodal coordinates. Once all the requested mode shapes are computed, the new nodal coordinates are written to the plain text file opened earlier.

Program compilation and linking The ABAQUS/Make procedure is designed to compile and link this type of postprocessing program. It will also make the aba_param.inc file available during compilation. The ABAQUS/Make command to compile and link the FPERT program is as follows: abaqus make job=fpert

This command will have to be repeated if FORTRAN errors are discovered during the compilation or link. The commands used by the ABAQUS/Make procedure can be changed if necessary. The ABAQUS Site Guide lists the typical compile and link commands for each computer type.

Program execution Before the program is executed, an eigenvalue buckling job must have been run with ABAQUS. In this example the input file fpert001.inp is used to generate the results file fpert001.fil. When the FPERT program is executed using the command abaqus fpert, the first prompt will be Enter the name of the results file (w/o .fil):

Enter fpert001 to define FNAME. The second prompt will be Enter the mode shape(s) to be used in calculating the perturbed mesh (zero when finished):

Enter 1 followed by 0, since this is the only eigenvector available in the results file for this example. At the third prompt, Enter the imperfection factor to be introduced into the geometry for this eigenmode:

enter 0.25. This sets ® = 0.25, the shell thickness for this model. The program then processes the data and writes the nodal coordinates for the new mesh to fpert002.015.

Analysis description For a full discussion of the analysis, refer to ``Buckling of a cylindrical shell under uniform axial pressure,'' Section 1.2.3 of the ABAQUS Benchmarks Manual. The input file fpert001.inp (same file as bucklecylshell_s9r5_n3.inp) contains a 2 ´ 20 mesh of S9R5 elements and data lines for a buckling analysis. The input file fpert002.inp contains data lines for a Riks analysis using a perturbed mesh. The source code for the FPERT program is in fpert.f.

Results and discussion Plots produced by these analyses are shown in Figure 11.1.4-1 and Figure 11.1.4-2. Figure 11.1.4-1 is obtained from the eigenvalue buckling analysis and shows the original (cylindrical) mesh and the critical buckling mode. Figure 11.1.4-2 is generated when the load level has reached a local maximum (increment 8) in the Riks analysis using the perturbed mesh.

11-1201

Postprocessing of ABAQUS Results Files

Input files fpert001.inp Eigenvalue buckling analysis. fpert002.inp Riks analysis using a perturbed mesh. fpert.f Postprocessing program.

Figures Figure 11.1.4-1 Undeformed shape and eigenvalue buckling mode.

Figure 11.1.4-2 Deformed shape at first peak load in Riks analysis.

11-1202

Postprocessing of ABAQUS Results Files

Sample listings

11-1203

Postprocessing of ABAQUS Results Files

Listing 11.1.4-1 SUBROUTINE HKSMAIN C==================================================================== C This program must be compiled and linked with the command: C abaqus make job=fpert C Run the program using the command: C abaqus fpert C==================================================================== C C PURPOSE: C This program computes a perturbed mesh based on a user-specified C perturbation factor. The original coordinate data and C eigenvectors are read from an ABAQUS results (.fil) file. C C PROMPTS: C 1. `Enter the name of the results file (w/o .fil):' C 2. `Enter the mode shape(s) to be used in calculating the C perturbed mesh (zero when finished):' C 3. `Enter the imperfection factor to be introduced into the C geometry for this eigenmode:' C C==================================================================== C C INPUT FILE -- `FNAME'.fil C C OUTPUT FILE -- fpert002.015 C C==================================================================== C C The use of ABA_PARAM.INC eliminates the need to have different C versions of the code for single and double precision. C ABA_PARAM.INC defines an appropriate IMPLICIT REAL statement and C sets the value of NPRECD to 1 or 2, depending on whether the C machine uses single or double precision. C C==================================================================== C ARRAY = Described in Section 7.0.0 of the Verification manual C JRRAY = Described in Section 7.0.0 of the Verification manual C LRUNIT = Described in Section 7.0.0 of the Verification manual C DISP = Contains the eigenvector for a particular eigenmode C COORD = Original coordinate data C INODE = Original node label

11-1204

Postprocessing of ABAQUS Results Files

C IDOF = DOF for the element C JEIGNO = Array of mode shapes used for calculating the perturbed C mesh C FNAME = Name of the results file C NODEMAX = Number of nodes in the model C IELMAX = Number of elements in the model C==================================================================== INCLUDE 'aba_param.inc' DIMENSION ARRAY(513), JRRAY(NPRECD,513), LRUNIT(2,1) EQUIVALENCE (ARRAY(1), JRRAY(1,1)) C=================================================================== C ITOTAL must be greater than or equal to the number of nodes in the C model C=================================================================== PARAMETER (ITOTAL = 8000) C C==================================================================== C DIMENSION DISP(6,ITOTAL), COORD(3,ITOTAL) DIMENSION INODE(ITOTAL), IDOF(30), JEIGNO(10) CHARACTER FNAME*80,OUTFILE*(*) PARAMETER (OUTFILE = 'fpert002.015') C C==================================================================== C Define flags and counters. C C==================================================================== ICYCLE = 0 I1901 = 0 I101 = 0 I = 1 K = 1 C C==================================================================== C Define file access variables. C C==================================================================== NRU = 1 LRUNIT(1,NRU) = 8 LRUNIT(2,NRU) = 2 LOUTF = 0 C C====================================================================

11-1205

Postprocessing of ABAQUS Results Files

C Open output file. C C==================================================================== OPEN(UNIT=15,FILE=OUTFILE,STATUS='UNKNOWN',IOSTAT = J) IF (J .NE. 0) THEN WRITE(*,900) OUTFILE GOTO 950 ENDIF C C==================================================================== C Get the name of the results (.fil) file. C C==================================================================== WRITE(*,2000) WRITE(6,*) ' Enter the name of the results file (w/o .fil):' READ(5,'(A)', IOSTAT = J ) FNAME IF (J .NE. 0) GOTO 950 C C==================================================================== C Access ABAQUS libraries to set up input file. C C==================================================================== CALL INITPF (FNAME, NRU, LRUNIT, LOUTF) C JUNIT = LRUNIT(1,NRU) C CALL DBRNU (JUNIT) C C==================================================================== C Read a record from the input file. C On the first pass through the file obtain the number of nodes for C a diagnostic check. C==================================================================== CALL DBFILE (0, ARRAY, JRCD) DO WHILE (JRCD .EQ. 0) IF (JRRAY(1,2) .EQ. 1980) IEIGNO = JRRAY(1,3) IF (JRRAY(1,2) .EQ. 1921 ) THEN NODEMAX = JRRAY(1,8) IELMAX = JRRAY(1,7) ICYCLE = ICYCLE +1 ENDIF CALL DBFILE (0, ARRAY, JRCD) ENDDO

11-1206

Postprocessing of ABAQUS Results Files

C CALL DBFILE (2, ARRAY, JRCD) C=================================================================== C User is given a choice of eigenmodes for calculating the perturbed C mesh. C C=================================================================== WRITE(*,2010) NODEMAX, IELMAX WRITE(*,2015) IEIGNO 5 READ(5,*,ERR = 950) JEIGNO(I) IF (JEIGNO(I) .EQ. 0) GOTO 10 I=I+1 GOTO 5 C 10 CONTINUE CALL DBFILE (0, ARRAY, JRCD) C DO WHILE (JRCD .EQ. 0) C C==================================================================== C If this is the first pass through the file and the current record C is the nodal coordinate record, then read the original nodal C coordinates and the node numbers. Make sure that the third C coordinate exists before saving it. C C==================================================================== IF (JRRAY(1,2) .EQ. 1901 .AND. ICYCLE .LE. 1) THEN I1901 = I1901 + 1 INODE(I1901) = JRRAY(1,3) COORD(1,I1901) = ARRAY(4) COORD(2,I1901) = ARRAY(5) COORD(3,I1901) = 0.0D0 IF (JRRAY(1,1) .GE. 6) COORD(3,I1901) = ARRAY(6) C C==================================================================== C If this is the first pass through the file and the current record C is the active degree of freedom record, save the active d.o.f. C If the d.o.f. is active in the model, IDOF(XX) equals the C position of d.o.f. XX in the output arrays. If the d.o.f. is not C active, IDOF(XX) is zero for d.o.f. XX (i.e., for planar models C IDOF(1) = 1, IDOF(2) = 2, IDOF(3) = 0, IDOF(4) = 0, IDOF(5) = 0, C IDOF(6) = 3, etc.). ITRANS equals the number of translational C d.o.f.'s in the model.

11-1207

Postprocessing of ABAQUS Results Files

C C==================================================================== ELSE IF (JRRAY(1,2) .EQ. 1902) THEN DO 15 IXX = 1, JRRAY(1,1)-2 IDOF(IXX) = JRRAY(1,IXX+2) 15 CONTINUE ITRANS = 3 IF (IDOF(3) .EQ. 0) ITRANS = 2 C C==================================================================== C If the current record is the modal record, save the current C eigenvalue number. C C==================================================================== C ELSE IF (JRRAY(1,2) .EQ. 1980) THEN IEIGNO = JRRAY(1,3) DO J = 1, I-1 IF (JEIGNO(J) .EQ. IEIGNO) K = J ENDDO C C==================================================================== C If the current record is the displacement record and the current C eigenvalue was requested, read the displacement data. The data C will be in the coordinate system specified in the C `*NODE FILE,GLOBAL=' option. If nodal transformations were C performed and GLOBAL=NO was used, the displacements will be in C the local system. If nodal transformations were used and C GLOBAL=YES, the results will be in the global system. In all C other cases the results will be in the global system. Also, C make sure that degrees of freedom are active in the model before C saving them in the appropriate array location. C C==================================================================== C ELSE IF (JRRAY(1,2) .EQ. 101 .AND. IEIGNO .EQ. JEIGNO(K)) THEN I101 = I101 + 1 DISP(1,I101) = ARRAY(4) DISP(2,I101) = ARRAY(5) IF (IDOF(3) .NE. 0) DISP(3,I101) = ARRAY(IDOF(3)+3) IF (IDOF(4) .NE. 0) DISP(4,I101) = ARRAY(IDOF(4)+3) IF (IDOF(5) .NE. 0) DISP(5,I101) = ARRAY(IDOF(5)+3) IF (IDOF(6) .NE. 0) DISP(6,I101) = ARRAY(IDOF(6)+3)

11-1208

Postprocessing of ABAQUS Results Files

16 1

IF (INODE(I101) .EQ. 0) INODE(I101) = JRRAY(1,3) IF( I101 .EQ. NODEMAX ) THEN WRITE(6,16) JEIGNO(K) FORMAT(/,2X,'Nodal coordinate data being computed for', ' eigenvalue . . .',I5)

C C==================================================================== C FACTOR should be entered as a perturbation factor in terms of a C percentage value multiplied by a geometric parameter C (e.g., shell thickness) C==================================================================== C WRITE(6,2020) READ(5,*,IOSTAT = J) FACTOR IF (J .NE. 0) GOTO 950 ICYCLE = ICYCLE + 1 I101 = 0 C C==================================================================== C Compute the perturbed mesh. This section assumes that nodal C displacements are in the GLOBAL coordinate system. If they are C not, the correct transformations should be applied prior to C perturbing the mesh. The user should supply this coding. Also, C only the translational degrees of freedom should be used for the C perturbation (X = Xo + u). C==================================================================== C==================================================================== C Subroutine NODEGEN is the actual mesh generator. C==================================================================== CALL NODEGEN(COORD,DISP,I1901,FACTOR) ENDIF ENDIF C CALL DBFILE(0, ARRAY, JRCD) ENDDO C C==================================================================== C Next line is added for diagnostics C C==================================================================== IF (NODEMAX .NE. I1901) THEN WRITE(*,2025) NODEMAX,I1901 GOTO 950

11-1209

Postprocessing of ABAQUS Results Files

ENDIF C

30

IF (ICYCLE .LE. 1) THEN WRITE(*,30) FORMAT(2X,'. . . NO EIGENVECTORS WERE FOUND . . .',/ 1 2X,'The input file for the buckling analysis must contain:', 2 /,2X,'--> *NODE FILE <--', 3 /,2X,'--> U <--') GOTO 950 ENDIF

C C=================================================================== C Output the coordinates of the perturbed mesh and close the file. C=================================================================== WRITE(*,100) OUTFILE 100 FORMAT(//,2X,'The perturbed mesh data are being written to:', 1 1X,A,//) C DO K = 1, NODEMAX WRITE(15,110) INODE(K), (COORD(J,K),J = 1, ITRANS) 110 FORMAT(I6,3(',',1PE14.6)) ENDDO CLOSE (15) C C==================================================================== C 900 FORMAT(//, 1 /,2X,'TROUBLE OPENING FILE',1X,A) 950 WRITE(*,1000) 1000 FORMAT(//, 1 /,2X,' . . . TROUBLE READING DATA . . . ', 2 /,2X,' . . . PROGRAM STOPPED . . . ',/) 2000 FORMAT(//, 1 /,' +----------------------------------------------+', 2 /,' | |', 3 /,' | P R O G R A M --- F P E R T |', 4 /,' | P E R T U R B E D M E S H |', 5 /,' | G E N E R A T O R |', 6 /,' | |', 7 /,' +----------------------------------------------+',//) 2010 FORMAT(//, 1 /,2X,'Number of nodes in model . . . . . . . ',I5, 2 /,2X,'Number of elements in model . . . . . . . ',I5)

11-1210

Postprocessing of ABAQUS Results Files

2015 FORMAT(//, 1 /,2X,'Number of mode shapes available . . . . . . .',I5, 2 //,2X,'Enter the mode shape(s) to be used in calculating', 3 /,2x,'the perturbed mesh (zero when finished):') 2020 FORMAT(//, 1 /,2X,'Enter the imperfection factor to be introduced ', 2 /,2X,'into the geometry for this eigenmode: ') 2025 FORMAT(//, 1 /,2X,'. . . TROUBLE READING COORDINATE DATA . . . ', 2 /,2X,'Number of coordinates in model . . . . . .',I5, 3 /,2X,'Number of coordinates read . . . . . . . .',I5) RETURN C==================================================================== C SUBROUTINE NODEGEN(COORD,DISP,I1901,FACTOR) C C==================================================================== C PURPOSE: Defines new coordinate data based upon a fraction of the C eigenvector obtained in a buckling analysis C C INPUT: C C COORD = Original coordinate data C DISP = Displacement data (eigenvector) C I1901 = Total number of nodes C FACTOR = Imperfection factor (e.g., percentage of shell C thickness) C==================================================================== C INCLUDE 'aba_param.inc' DIMENSION COORD(3,*),DISP(6,*) C DO I = 1, I1901 COORD(1,I) = COORD(1,I) + FACTOR*DISP(1,I) COORD(2,I) = COORD(2,I) + FACTOR*DISP(2,I) COORD(3,I) = COORD(3,I) + FACTOR*DISP(3,I) ENDDO RETURN END

11.1.5 Output radiation viewfactors and facet areas: FRAD Product: ABAQUS/Standard

11-1211

Postprocessing of ABAQUS Results Files

This example illustrates the use of a FORTRAN program to read the radiation viewfactors and the facet areas from the results file.

General description The program shows how to retrieve the viewfactors and the facet areas from the results file. The results file created from the benchmark problem detailed in ``Axisymmetric elemental cavity radiation viewfactor calculations,'' Section 1.6.6 of the ABAQUS Benchmarks Manual, is used to verify that the output records have been read and output correctly. This program will assume that the results file has the default file extension, .fil, which corresponds to FORTRAN unit 8.

Programming details Before proceeding, review the general discussion on programming concepts and ABAQUS FORTRAN interfaces in ``User postprocessing of ABAQUS results files: overview,'' Section 11.1.1, and the detailed discussion of postprocessing given in Chapter 5, "File Output Format," of the ABAQUS/Standard User's Manual. When running the program FRAD (this program is named frad.f on the ABAQUS release media), the user will be prompted for the file name that initializes FNAME. Other variables, such as LOUTF, NRU, LRUNIT(1,NRU), and LRUNIT(2,NRU), are initialized inside the program. INITPF and DBNRU are then called to complete the necessary initializations and file connections. By default, the results file is processed for all steps and increments in the results file. The user can restrict the output by setting LSTEPA and LINCA to the required step and increment and uncommenting the simple IF - END IF block. Data processing starts with a DO-loop over all the records to be read, one-by-one, by means of a call to DBFILE. Each record is identified by its record key, which is stored in the second entry of the record. When records 1922 and 2000 are processed by FRAD, the heading and the current step and increment numbers are written out so as to provide a way to recognize the beginning of data in each analysis. Record types 1605, 1606, 1607, and 1609 are then read; and the desired output is written to the output file vfout.

Program compilation and linking Before it can be executed, the FORTRAN program must be compiled and linked. Both operations, as well as the inclusion of the aba_param.inc file, are performed by a single execution of the ABAQUS/Make procedure: abaqus make job=frad

This procedure may have to be repeated until all FORTRAN errors are corrected. After successful compilation, the program's object code is linked automatically with the ABAQUS object codes stored in the shared program library and the interface library to build the executable program. Refer to the ABAQUS Site Guide for information about the compile and link commands for a particular computer.

Program execution Before the program is executed, a results file must have been created with the desired output being written to that file. In this example the results file xrvda4n1.fil created by running the input file

11-1212

Postprocessing of ABAQUS Results Files

xrvda4n1.inp discussed in ``Axisymmetric elemental cavity radiation viewfactor calculations,'' Section 1.6.6 of the ABAQUS Benchmarks Manual, is used. When the program is executed using the command abaqus frad, the prompt Enter the name of the input file (w/o .fil):

will appear. Enter xrvda4n1 to define FNAME. The program processes the data and produces a file named vfout, which contains the required information.

Results and discussion The radiation viewfactors and facet areas are read and output to vfout. The output agrees with the expected results.

Input file frad.f Postprocessing program.

Sample listings

11-1213

Postprocessing of ABAQUS Results Files

Listing 11.1.5-1 SUBROUTINE HKSMAIN C==================================================================== C This program must be compiled and linked with the command: C abaqus make job=frad C Run the program using the command: C abaqus frad C==================================================================== C C PURPOSE: C This program reads the results file and outputs the radiation C viewfactors, and facet areas associated with different facets C in a cavity. C C PROMPTS: C 1. 'Enter the name of the results file (w/o .fil):' C C==================================================================== C C INPUT FILE ---- 'FNAME'.fil C OUTPUT FILE ---- vfout C C==================================================================== C INCLUDE 'aba_param.inc' DIMENSION ARRAY(513),JRRAY(NPRECD,513),LRUNIT(2,1) EQUIVALENCE (ARRAY(1),JRRAY(1,1)) DIMENSION COORD(3),TRACT(3),CLEAR(3) C CHARACTER*80 FNAME,OUTFILE,TEMP CHARACTER*8 TEMP1 CHARACTER*3 NULL LOGICAL STRNCMP PARAMETER (ZERO=0.0D0,ONE=1.0D0,TWO=2.0D0,NULL=' ') C-----------------------------------------------------------C NRU Number of results files (*.fil) to be read C LRUNIT(1,*) Unit number of results file C LRUNIT(2,*) Format of input file (1 = ASCII, 2 = BINARY) C LOUTF Format of output file (not needed here) C COORD(*) Stores the nodal coordinates C IXX Record length C KEY Record key

11-1214

Postprocessing of ABAQUS Results Files

C LSTEPA Step Number C LINCA Increment Number C-----------------------------------------------------------C C--- Initialize File --------------------------------------NRU = 1 LRUNIT(1,NRU) = 8 LRUNIT(2,NRU) = 2 LOUTF = 0 OUTFILE = 'vfout' FNAME = NULL C--- Change below to set to desired step and increment when C--- requesting restricted output; Default is for all steps C--- and increments available in the results file LSTEPA LINCA

= 1 = 1

C--C C Get the name of the results (.fil) file C C-----------------------------------------------------------WRITE(6,*) ' Enter the name of the results file (w/o .fil): ' READ (5,'(A)', IOSTAT=J) FNAME IF (J .NE. 0) WRITE(*,*) 'ERROR IN READING INPUT DATA' C C C Access ABAQUS libaries and open input file C-----------------------------------------------------------CALL INITPF(FNAME, NRU, LRUNIT, LOUTF) OPEN(UNIT=15,FILE=OUTFILE,STATUS='UNKNOWN') JUNIT = LRUNIT(1,NRU) CALL DBRNU(JUNIT) C-----------------------------------------------------------C End access C CALL DBFILE(0, ARRAY, JRCD) if (jrcd .ne. 0) write(15,*) 'ERROR IN FILE-ACCESS' DO WHILE (JRCD .EQ. 0) C C IXX = Record length C

11-1215

Postprocessing of ABAQUS Results Files

IXX = JRRAY(1,1) C C KEY = Record type key C KEY = JRRAY(1,2) C C Output Request Definition C IF(KEY .EQ. 2000) THEN LINC = JRRAY(1,9) LSTEP= JRRAY(1,8) END IF C Output desired quantities to the output file C C----------------------------------------------------------C Uncomment below to get output for specific increment/step. C Default output is for all increments available in the file. C----------------------------------------------------------C IF((LINC .EQ. LINCA) .AND. (LSTEP .EQ. LSTEPA)) THEN

1 1

30 1

40

IF (KEY .EQ. 2000) THEN WRITE(15,'(/,1X,A,1X,I6,1X,A,I6)')'STEP NUMBER', LSTEP, 'INCREMENT',LINC WRITE(*,'(/,1X,A,1X,I6,1X,A,I6)') 'WRITING OUTPUT FOR STEP', LSTEP, 'INCREMENT', LINC END IF IF(KEY .EQ. 1605)THEN NUMFACETS = JRRAY(1,3) WRITE(TEMP,'(A)') ARRAY(4) WRITE(15,30)TEMP,NUMFACETS FORMAT(//,1X,'CAVITY NAME:',1X,A,/, 1X,'NUMBER OF FACETS:',1X,I6) ELSEIF(KEY .EQ. 1609) THEN MVFLEN = JRRAY(1,3) MATRIXSIZE = INT(SQRT(REAL(MVFLEN))) ELSEIF( KEY .EQ. 1606 ) THEN WRITE(15,'(/,1X,A)')'VIEWFACTOR MATRIX (ROW - COLUMN)' WRITE(15,40) (ARRAY(I),I=3,JRRAY(1,1)) FORMAT(1X,1PE14.6,', ') ELSEIF(KEY .EQ. 1607) THEN

11-1216

Postprocessing of ABAQUS Results Files

50

C

WRITE(15,'(/,1X,A)') 'FACET AREA' WRITE(15,50)(ARRAY(I),I=3,JRRAY(1,1)) FORMAT(1X,1PE14.6,', ') ENDIF ENDIF CALL DBFILE(0, ARRAY, JRCD) ENDDO RETURN END

11.1.6 Creation of a data file to facilitate the postprocessing of elbow element results: FELBOW Product: ABAQUS/Standard This example illustrates the use of a FORTRAN program to read selected element integration point records from an ABAQUS results file to facilitate the postprocessing of elbow element results. X-Y data are created that are suitable for use with the X-Y plotting capability in ABAQUS/Viewer.

General description This program shows how to retrieve integration point data for elbow elements from an ABAQUS results file to visualize one of the following: 1. Variation of a variable along a line of elbow elements, 2. Variation of a variable around the circumference of a given elbow element, or 3. Ovalization of a given elbow element. An ASCII file containing X-Y data is created that can be read into ABAQUS/Viewer for visualization purposes. To execute option 1, the elbow elements must be numbered such that they increase monotonically within the range of elements considered; all elements in the desired range must be elbow elements. X-Y data will be created with the X-data being the distance along the line of elbow elements, measured along the elbow centerline and the Y -data being the variable value. The user must ensure that the integration point coordinates (COORD) are written to the results file if either option 2 or 3 is needed. For option 2 X-data are the distance around the circumference of the elbow element, measured along the middle surface, and Y -data are the variable value. For option 3 the X-Y data are the current

11-1217

Postprocessing of ABAQUS Results Files

coordinates of the middle-surface integration points around the circumference of the elbow element, projected to a local coordinate system in the plane of the deformed cross-section. The origin of the local system coincides with the center of the cross-section; the plane of the deformed cross-section is defined as the plane that contains the center of the cross-section and integration points 1 and 2.

Programming details The user is prompted for the name of the results file (assumed to be binary) and the postprocessing option (1, 2, or 3). The user is then prompted for additional information depending on the option that was chosen; this information includes · The range of element numbers (options 2 and 3 require only a single element number), · The section point number (options 1 and 2 only), · The integration point number (option 1 only), · The element variable (options 1 and 2 only), · The component of the variable (as defined in ``Results file output format,'' Section 5.1.2 of the ABAQUS/Standard User's Manual, options 1 and 2 only), · The step number, and · The increment number. The data are processed in a double DO-loop over all records, via a call to DBFILE. The desired data are stored in variable VAR; the integration point coordinates are stored in COORDS. The program checks to make sure the requested data are available in the results file. An error is issued if the user tries to process data that are not found in the results file.

Program compilation and linking Before program execution, compile and link the FORTRAN program by using the ABAQUS/Make procedure: abaqus make job=felbow

Repeat this command until all FORTRAN errors are corrected. After successful compilation, the program's object code is linked automatically with the ABAQUS object codes stored in the shared program library and interface library to build the executable program. Refer to Chapter 3, "Environment file," of the ABAQUS Site Guide to see which compile and link commands are used for a particular computer.

Program execution Before executing the program, run an analysis that creates a results file containing the appropriate output. This analysis includes, for example, output for the elements in a given range and the integration point coordinates of the elements. When the program is executed using the command abaqus felbow, the prompt

11-1218

Postprocessing of ABAQUS Results Files

Enter the name of the input file (w/o .fil):

will appear. Enter the name of the results file to define FNAME. The user is then prompted for other information, such as the desired postprocessing option, element number, etc. The program processes the data and produces a file named output.dat that contains the information required to visualize the elbow element results.

Results and discussion ``Elastic-plastic collapse of a thin-walled elbow under in-plane bending and internal pressure, '' Section 1.1.2, contains several figures created with the aid of this program. The output agrees with the expected results.

Input file felbow.f Postprocessing program.

Sample listings

11-1219

Postprocessing of ABAQUS Results Files

Listing 11.1.6-1 SUBROUTINE HKSMAIN C==================================================================== C This program must be compiled and linked with the command: C abaqus make job=felbow C Run the program using the command: C abaqus felbow C================================================================== C C PURPOSE: C C This program reads results stored in an ABAQUS results (.fil) C file and creates an input file for ABAQUS/Viewer that permits C postprocessing and visualization of elbow element results. C C C Input file names: `fname.fil', where fname is the root file name C of the input file. C C Output file name: output.dat C C================================================================== C C VARIABLES USED BY THIS PROGRAM: C C ndi -- Number of direct components in stress/strain tensor. C nshr -- Number of shear components in stress/strain tensor. C ndip1 -- ndi + 1 C array -- Real array containing values read from results file. C Equivalenced to jrray. C jrray -- Integer array containing values read from results file. C Equivalenced to array. C fname -- Root file name of input file (w/o .fil extension). C nru -- Number of results files (.fil) to be read. C lrunit -- Array containing unit number and format of results files: C lrunit(1,*) --> Unit number of input file. C lrunit(2,*) --> Format of input file. C loutf -- Format of output file: C 0 --> Standard ASCII format. C 1 --> ABAQUS results file ASCII format. C 2 --> ABAQUS results file binary format. C junit -- Unit number of file to be opened.

11-1220

Postprocessing of ABAQUS Results Files

C jrcd -- Error check return code. C .EQ. 0 --> No errors. C .NE. 0 --> Errors detected. C key -- Current record key identifier. C jelnum -- Current element number. C intpn -- Integration point number. C C================================================================== C C The use of ABA_PARAM.INC eliminates the need to have different C versions of the code for single and double precision. C ABA_PARAM.INC defines an appropriate IMPLICIT REAL statement C and sets the value of NPRECD to 1 or 2, depending on whether C the machine uses single or double precision. ABA_PARAM.INC is C referenced from the \site (for NT) or /site (for Unix) C ABAQUS release subdirectory when ABAQUS/Make is executed. C C================================================================== C include 'aba_param.inc' parameter (melem=10000,mnode=10000,mkey=3000,mintpt=360) dimension array(513),jrray(nprecd,513),lrunit(2,1) equivalence (array(1),jrray(1,1)) C C================================================================== C character fname*80 C C SOME DIMENSION STATEMENTS MAY BE NEEDED IF YOU ARE DOING ADDITIONAL C CALCULATIONS ON THE DATA C dimension var(513,melem),coords(3,mintpt) dimension iconn(3,melem),loc_el(melem) dimension naxipt(melem),iglb_nod(mnode),loc_nod(mnode) dimension islct(mkey),nintpt(melem),nodel(melem),iglb_el(melem) dimension xyz(3,mnode),xpos(mnode),tang1(3),tang2(3) dimension rot(3,3),xc(3),xpr(3,mintpt),scord(3,mintpt),xnorm(3) dimension isctchk(melem),icrdchk(melem),ivarchk(melem) C C================================================================== C C GET THE NAME OF THE RESULTS FILE.

11-1221

Postprocessing of ABAQUS Results Files

C C================================================================== C isect1 = 0 intpt1 = 0 icomp = 1 C write(6,*) 'Enter the name of the input file (w/o .fil):' read(5,'(A)') fname C 100 write(6,*) 'Enter the postprocessing option:' write(6,*) ' 1 - variation along the riser ' write(6,*) ' 2 - variation around the circumference' write(6,*) ' of the elbow' write(6,*) ' 3 - ovalization of elbow cross-section' read(5,*) ipost if (ipost .ne. 1 .and. ipost .ne. 2 .and. & ipost .ne. 3) then write(6,*)'Invalid entry - try again' go to 100 endif C write(6,*)'Enter the first element number' read(5,*) jel_1 C if (ipost .ne. 1) then jel_2 = jel_1 else write(6,*)'Enter the last element number' read(5,*) jel_2 endif if (jel_2 .lt. jel_1) then write(6,*)'last elem number must be greater than first' return endif jdiff = jel_2 - jel_1 + 1 if (jdiff .gt. melem) then write(6,*)'Too many elements - max is',melem return endif C if (ipost .lt. 3) then

11-1222

Postprocessing of ABAQUS Results Files

write(6,*)'Enter the section point number' read(5,*) isect1 endif C if (ipost .eq. 1) then write(6,*)'Enter the integration point number' read(5,*) intpt1 endif C if (ipost .lt. 3) then 998 999

write(6,999) format('Enter the key for the variable you wish to process:')

C write(6,500) 500 format(2x,'TEMP ...... 2',/, & 2x,'COORD...... 8',/, & 2x,'S.......... 11',/, & 2x,'SINV....... 12',/, & 2x,'SF......... 13',/, & 2x,'E.......... 21',/, & 2x,'PE......... 22',/, & 2x,'CE......... 23',/, & 2x,'IE......... 24',/, & 2x,'EE......... 25',/, & 2x,'THE........ 88',/, & 2x,'LE......... 89',/, & 2x,'NE......... 90',/, & 2x,'SP.........401',/, & 2x,'EP.........403',/, & 2x,'NEP........404',/, & 2x,'LEP........405',/, & 2x,'EEP........408',/, & 2x,'IEP........409',/, & 2x,'THEP.......410',/, & 2x,'PEP........411',/, & 2x,'CEP........412') C read(5,*) key C if (key .ne. 2 .and. key .ne. 8 .and. & key .ne. 11 .and. key .ne. 12 .and. & key .ne. 13 .and. key .ne. 21 .and.

11-1223

Postprocessing of ABAQUS Results Files

& & & & & & & &

key key key key key key key key

.ne. .ne. .ne. .ne. .ne. .ne. .ne. .ne.

22 .and. key .ne. 23 .and. 24 .and. key .ne. 25 .and. 88 .and. key .ne. 89 .and. 90 .and. key .ne. 401 .and. 403 .and. key .ne. 404 .and. 405 .and. key .ne. 408 .and. 409 .and. key .ne. 410 .and. 411 .and. key .ne. 412) then

C write(6,*)'Invalid key - try again' go to 998 C endif C C C C

Integration point coordinates available only at middle surface Overwrite the section point and set to the default if (key .eq. 8) isect1 = 0

C if (key .ge. 8) then write(6,*)'Enter the attribute number' read(5,*) icomp endif C if (key .eq. 13) then write(6,*)'Section force data written only once per element' if (ipost .eq. 1) then write(6,*)'Will use default integration & section point' write(6,*)' ' intpt1 = 1 isect1 = 0 elseif (ipost .gt. 1) then write(6,*)'Only use with option 1: Processing terminated' return endif endif C endif C write(6,*)' Enter the step number' read(5,*) istep1 write(6,*)' Enter the increment number' read(5,*) iinc1

11-1224

Postprocessing of ABAQUS Results Files

C C SELECT THE RECORDS TO BE PROCESSED C C IF THE ISLCT ARRAY IS SET TO 1 THE DATA WILL BE PROCESSED C IF THE ISLCT ARRAY IS SET TO 0 THE DATA WILL NOT BE PROCESSED C do ii = 1, mkey islct(ii) = 0 end do C C ELEMENT DEFINITION islct(1900)=0 C NODE DEFINITION islct(1901)=0 C INCREMENT START islct(2000)=0 C ELEMENT HEADER islct(1)=0 C COORD islct(8)=0 C if (ipost .lt. 3) islct(key) = 1 keyprv=0 C nels = 0 numnp = 0 C itimchk = 0 ielchk = 0 do i = 1, melem loc_el(i) = 0 isctchk(i) = 0 icrdchk(i) = 0 ivarchk(i) = 0 do j = 1, 513 var(j,i) = 0.0 end do end do C C================================================================== C C OPEN THE OUTPUT FILE. C

11-1225

Postprocessing of ABAQUS Results Files

C================================================================== open(unit=9,file='output.dat',status='unknown') C nru = 1 loutf = 0 lrunit(1,1) = 8 lrunit(2,1) = 2 C call initpf(fname,nru,lrunit,loutf) C junit = 8 C call dbrnu(junit) C C REWIND FILE C call dbfile(2,array,jrcd) C C C================================================================== C C Read records from the results (.fil) file and process the data. C Cover a maximum of 10 million records in the file. C C================================================================== C do 1000 k100 = 1, 100 do 1000 k1 = 1, 99999 C C READ RECORD FROM .FIL FILE AND PROCESS DATA. C call dbfile(0, array, jrcd) if (jrcd .ne. 0 .and. keyprv .eq. 2001) then write(6,*)'End of file' close(junit) go to 1001 else if (jrcd .ne. 0) then write(6,*)'Error reading input file' return endif C C LENGTH AND KEY RECORD NUMBER ARE ALWAYS NEEDED

11-1226

Postprocessing of ABAQUS Results Files

C lenf= jrray(1,1) key = jrray(1,2) C C SPECIFIC RECORD NUMBERS FOLLOW... C C================================================================== C C ELEMENT DEFINITIONS C C================================================================== if ( key .eq. 1900 ) then jelnum=jrray(1,3) if (jelnum .gt. melem) then write(6,*)'Maximum global elem number too large' write(6,*)'Increase melem' return endif ctype= array(4) if (jelnum .ge. jel_1 .and. & jelnum .le. jel_2) then ielchk = 1 nels = nels + 1 jel = nels iglb_el(jel) = jelnum loc_el(jelnum) = jel nodel(jel) = lenf - 4 naxipt(jel) = 1 if (ctype .ne. 'ELBOW31' .and. & ctype .ne. 'ELBOW31B' .and. & ctype .ne. 'ELBOW31C' .and. & ctype .ne. 'ELBOW32') then write(6,*)'Invalid element type encountered' return endif if (ctype .eq. 'ELBOW32')naxipt(jel) = 2 do kk=5,lenf ii=kk-4 iconn(ii,jel)=jrray(1,kk) end do endif keyprv = key goto 9099

11-1227

Postprocessing of ABAQUS Results Files

C C================================================================== C C NODE DEFINITIONS C C================================================================== else if ( key .eq. 1901 ) then jnod = jrray(1,3) if (jnod .gt. mnode) then write(6,*)'Maximum global node number exceeded' write(6,*)'Increase mnode' return endif numnp = numnp + 1 iglb_nod(numnp) = jnod loc_nod(jnod) = numnp xyz(1,numnp) = array(4) xyz(2,numnp) = array(5) xyz(3,numnp) = array(6) keyprv = key goto 9099 C C================================================================== C C CURRENT STEP AND INCREMENT NUMBER. C C================================================================== else if ( key .eq. 2000 ) then ttime=array(3) stime=array(4) sfreq=array(12) istep=jrray(1,8) iinc =jrray(1,9) C C SET THE FLAG ITIME IF THIS IS THE REQUESTED STEP/INC C if (istep .eq. istep1 .and. & iinc .eq. iinc1) then itime = 1 itimchk = 1 else itime = 0

11-1228

Postprocessing of ABAQUS Results Files

endif c keyprv = key goto 9099 C C================================================================== C C ELEMENT VARIABLES AT INTEGRATION POINTS WITHIN THE ELEMENT C C================================================================== C C ELEMENT DATA C else if ( key .eq. 1 ) then C C C

PROCESS THIS RECORD IF THIS IS THE CORRECT STEP/TIME if (itime .eq. 1) then jelnum = jrray(1,3) jel = loc_el(jelnum) ielem = 0

C C C

PROCESS THIS ELEMENT IF IT IS IN THE LIST OF DESIRED ELEMS if (jel .gt. 0) then ielem = 1 intpn = jrray(1,4) if (intpn .gt. mintpt) then write(6,*)'Max number of int points exceeded' write(6,*)'Increase mintpt' return endif isect = jrray(1,5) ilocn = jrray(1,6) if (ilocn .ne. 0) then write(6,*)'Element data must be at the int points' return endif crbar = array(7) ndi = jrray(1,8) nshr = jrray(1,9) ndir = jrray(1,10)

11-1229

Postprocessing of ABAQUS Results Files

&

nsfc = jrray(1,11) if (isect .eq. isect1)then isctflg = 1 isctchk(jel) = 1 else isctflg = 0 endif if ( (ipost .eq.1 .and. intpn .eq. intpt1) .or. ipost .gt. 1) then iptflg = 1 else iptflg = 0 endif endif endif keyprv = key goto 9099

C C================================================================== C C COORDINATES C C================================================================== else if ( key .eq. 8 .and. ipost .gt. 1) then C C PROCESS IF THIS IS THE CORRECT STEP/INC, ELEMENT, SECTION C POINT, AND INTEGRATION POINT C icheck = itime*ielem*iptflg if (icheck .eq. 1 ) then c if (ipost .eq. 3) nintpt(jel) = intpn icrdchk(jel) = 1 if (ipost .gt. 1) nintpt(jel) = intpn do kk=3,lenf ii=kk-2 coords(ii,intpn)=array(kk) end do C if (islct(key) .eq. 1 .and. ipost .lt. 3) then ivarchk(jel) = 1 jvar = intpn nintpt(jel) = intpn do kk=3,lenf

11-1230

Postprocessing of ABAQUS Results Files

ii=kk-2 var(ii,jvar)=array(kk) end do if (icomp .gt. ii) then write(6,*)'Invalid component' return endif endif C endif keyprv = key goto 9099 C C================================================================== C C VARIABLE RECORD C C================================================================== C PROCESS IF THIS IS THE DESIRED VARIABLE else if (islct(key) .eq. 1 .and. ipost .lt. 3) then C C C C

CONTINUE PROCESSING IF THIS IS THE CORRECT STEP/INC, ELEMENT, SECTION POINT, AND INTEGRATION POINT icheck = itime*ielem*isctflg*iptflg if (icheck .eq. 1 ) then ivarchk(jel) = 1 if (ipost .eq. 1) then jvar = jel else jvar = intpn endif nintpt(jel) = intpn do kk=3,lenf ii=kk-2 var(ii,jvar)=array(kk) end do if (icomp .gt. ii) then write(6,*)'Invalid component' return endif endif

11-1231

Postprocessing of ABAQUS Results Files

keyprv = key goto 9099 C C================================================================== C C ANYTHING ELSE C C================================================================== else c write (6,9000) key 9000 format(I5,' *** NO CODING FOR THIS RECORD ***') keyprv = key 9099 end if C C================================================================== C C END LOOPS C C================================================================== 1000 continue 1001 continue C C================================================================== C POSTPROCESS DATA HERE C================================================================== do ii = 1, nels nintpt(ii) = nintpt(ii)/naxipt(ii) end do C C================================================================== C VERIFY THAT APPROPRIATE DATA WERE WRITTEN TO RESULTS FILE C================================================================== c iquit = 0 if (ielchk .eq. 0) then write(6,*)'Desired element not found' return endif C if (itimchk .eq. 0) then write(6,*)'Desired step/increment not found' return endif C

11-1232

Postprocessing of ABAQUS Results Files

do iel = 1, nels if (isctchk(iel) .eq. 0 .and. ipost .lt. 3) then write(6,*)'Desired element and/or section point not found' return endif if (icrdchk(iel) .eq. 0 .and. ipost .gt. 1) then write(6,*)'Integration point coords not found' return endif if (ivarchk(iel) .eq. 0 .and. ipost .lt. 3) then write(6,*)'Desired element variable not found' return endif end do C C**************************************** C C PLOT VARIABLE ALONG ELBOW LENGTH C C**************************************** C if (ipost .eq. 1) then C nn_old = iconn(nodel(1),1) do iel = 1, nels nn_new = iconn(1,iel) if (iel .gt. 1 .and. nn_new .ne. nn_old) then write(6,*)'Error in element connectivity' return endif nnum_b = iconn(1,iel) nnum_b = loc_nod(nnum_b) nnum_e = iconn(nodel(iel),iel) nnum_e = loc_nod(nnum_e) if (iel .eq. 1) xpos(nnum_b) = 0.0 xlength = 0.d+0 do jj = 1, 3 delx = xyz(jj,nnum_e) - xyz(jj,nnum_b) xlength = xlength + delx*delx end do xlength = sqrt(xlength) xpos(nnum_e) = xpos(nnum_b) + xlength x_mid = 0.5*(xpos(nnum_e) + xpos(nnum_b))

11-1233

Postprocessing of ABAQUS Results Files

C C C

EXTRACT VARIABLE INFORMATION AND WRITE TO FILE

2000

data = var(icomp,iel) write(9,2000)x_mid,data format(5x,e17.9,5x,e17.9)

C nn_old=iconn(nodel(iel),iel) C end do return C C C**************************************** C C PLOT VARIABLE AROUND CIRCUMFERENCE OF ELBOW C C**************************************** C else if (ipost .eq. 2) then C xpos(1) = 0.0 C locel = loc_el(jel_1) iaxial = 1 C if (naxipt(locel) .eq. 2) then 3000 write(6,*)'Enter the axial station' read(5,*)iaxial if (iaxial .ne. 1 .and. iaxial .ne. 2) then write(6,*)'Try again - station must be 1 or 2' go to 3000 endif endif C do ipt = 1 , nintpt(locel) jpt = ipt + (iaxial - 1)*nintpt(locel) if (ipt .gt. 1) then xlength = 0.0 do jj = 1, 3 delx = coords(jj,jpt) - coords(jj,jpt-1) xlength = xlength + delx*delx end do

11-1234

Postprocessing of ABAQUS Results Files

xlength = sqrt(xlength) xpos(ipt) = xpos(ipt-1) + xlength endif C C C

EXTRACT VARIABLE INFORMATION AND WRITE TO FILE data = var(icomp,jpt) write(9,2000)xpos(ipt),data

C end do ipt = 1 jpt = ipt + (iaxial - 1)*nintpt(locel) data = var(icomp,jpt) xfinal = xpos(nintpt(locel)) + (xpos(2)- xpos(1)) write(9,2000)xfinal,data return C C**************************************** C C OVALIZATION PLOT C C**************************************** C else if (ipost .eq. 3) then C locel = loc_el(jel_1) iaxial = 1 C if (naxipt(locel) .eq. 2) then 3500 write(6,*)'Enter the axial station' read(5,*)iaxial if (iaxial .ne. 1 .and. iaxial .ne. 2) then write(6,*)'Try again - station must be 1 or 2' go to 3500 endif endif C C AVERAGE THE COORDS OF THE INTEGRATION POINTS TO GET THE CENTER C do i = 1, 3 xc(i) = 0.0

11-1235

Postprocessing of ABAQUS Results Files

end do C xnint = real(nintpt(locel)) C do ipt = 1 , nintpt(locel) jpt = ipt + (iaxial - 1)*nintpt(locel) C do i = 1, 3 xc(i) = xc(i) + coords(i,jpt)/xnint end do C end do C C C

SHIFT THE COORDINATES SO THAT CENTER OF SECTION IS AT ORIGIN do ipt = 1 , nintpt(locel) jpt = ipt + (iaxial - 1)*nintpt(locel) do i = 1, 3 scord(i,jpt) = coords(i,jpt) - xc(i) end do

C end do C C C C

DETERMINE TANGENT VECTOR 1 (FROM CENTER OF CROSS-SECTION TO INT PT 1) jpt = 1 + (iaxial - 1)*nintpt(locel) xmag = 0.0 do i = 1, 3 tang1(i) = coords(i,jpt) - xc(i) xmag = xmag + tang1(i)*tang1(i) end do xmag = sqrt(xmag) do i = 1, 3 tang1(i) = tang1(i)/xmag end do

C C C C

GUESS TANGENT VECTOR 2 (FROM CENTER OF CROSS-SECTION TO INT PT 2) jpt = 2 + (iaxial - 1)*nintpt(locel) xmag = 0.0 do i = 1, 3

11-1236

Postprocessing of ABAQUS Results Files

tang2(i) = coords(i,jpt) - xc(i) xmag = xmag + tang2(i)*tang2(i) end do xmag = sqrt(xmag) do i = 1, 3 tang2(i) = tang2(i)/xmag end do C C C

DETERMINE THE NORMAL VECTOR, TANG1 X TANG2 xnorm(1) = tang1(2)*tang2(3) - tang1(3)*tang2(2) xnorm(2) = - tang1(1)*tang2(3) + tang1(3)*tang2(1) tang1(1)*tang2(2) - tang1(2)*tang2(1) xnorm(3) = xmag = 0.0 do i = 1, 3 xmag = xmag + xnorm(i)*xnorm(i) end do xmag = sqrt(xmag) do i = 1, 3 xnorm(i) = xnorm(i)/xmag end do

C C C

REDEFINE TANGENT VECTOR 2 tang2(1) = - tang1(2)*xnorm(3) + tang1(3)*xnorm(2) tang2(2) = tang1(1)*xnorm(3) - tang1(3)*xnorm(1) tang2(3) = - tang1(1)*xnorm(2) + tang1(2)*xnorm(1)

C C C

DETERMINE THE ROTATION MATRIX do i = 1, 3 rot(1,i) = tang1(i) rot(2,i) = tang2(i) rot(3,i) = xnorm(i) end do

C C C

TRANSFORM COORDINATES INTO LOCAL SYSTEM do ipt = 1 , nintpt(locel) jpt = ipt + (iaxial - 1)*nintpt(locel) do i = 1, 3 xpr(i,ipt) = 0.0

11-1237

Postprocessing of ABAQUS Results Files

do j = 1, 3 xpr(i,ipt) = xpr(i,ipt) + rot(i,j)*scord(j,jpt) end do end do end do C C C

OUTPUT COORDS TO FILE

4000

do ipt = 1, nintpt(locel) write(9,4000)(xpr(i,ipt),i=1,2) format(5x,e17.9,5x,e17.9,5x,e17.9) end do

C ipt = 1 write(9,4000)(xpr(i,ipt),i=1,2) endif C close (unit=9) C return end

11-1238

Product Index ABAQUS/Standard Section 1.1.1

Axisymmetric analysis of bolted pipe flange connections

Section 1.1.2

Elastic-plastic collapse of a thin-walled elbow under in-plane bending and internal pressure

Section 1.1.3

Parametric study of a linear elastic pipeline under in-plane bending

Section 1.1.4

Indentation of an elastomeric foam specimen with a hemispherical punch

Section 1.1.5

Collapse of a concrete slab

Section 1.1.6

Jointed rock slope stability

Section 1.1.7

Indentation of a crushable foam specimen with a hemispherical punch

Section 1.1.8

Notched beam under cyclic loading

Section 1.1.9

Hydrostatic fluid elements: modeling an airspring

Section 1.1.10

Shell-to-solid submodeling of a pipe joint

Section 1.1.11

Stress-free element reactivation

Section 1.1.12

Symmetric results transfer for a rubber bushing

Section 1.1.13

Transient loading of a viscoelastic bushing

Section 1.1.15

Damage and failure of a laminated composite plate

Section 1.1.16

Analysis of an automotive boot seal

Section 1.1.17

Pressure penetration analysis of an air duct kiss seal

Section 1.1.18

Self-contact in rubber/foam components: jounce bumper

Section 1.1.19

Self-contact in rubber/foam components: rubber gasket

Section 1.1.20

Submodeling of a stacked sheet metal assembly

Section 1.2.1

Snap-through buckling analysis of circular arches

Section 1.2.2

Laminated composite shells: buckling of a cylindrical panel with a circular hole

Section 1.2.4

Elastic-plastic K-frame structure

Section 1.2.5

Unstable static problem: reinforced plate under compressive loads

Section 1.2.6

Buckling of an imperfection sensitive cylindrical shell

Section 1.3.1

Upsetting of a cylindrical billet in ABAQUS/Standard: quasi-static analysis with rezoning

Section 1.3.3

Superplastic forming of a rectangular box

Section 1.3.4

Stretching of a thin sheet with a hemispherical punch

Section 1.3.5

Deep drawing of a cylindrical cup

Section 1.3.6

Extrusion of a cylindrical metal bar with frictional heat generation

Section 1.3.8

Axisymmetric forming of a circular cup

Section 1.3.17

Upsetting of a cylindrical billet: coupled temperature-displacement and adiabatic analysis

Section 1.3.18

Unstable static problem: thermal forming of a metal sheet

0-1239

Section 1.4.1

A plate with a part-through crack: elastic line spring modeling

Section 1.4.2

Conical crack in a half-space with and without submodeling

Section 1.4.3

Elastic-plastic line spring modeling of a finite length cylinder with a part-through axial flaw

Section 1.4.4

Crack growth in a three-point bend specimen

Section 1.5.1

Springback of two-dimensional draw bending

Section 1.5.2

Deep drawing of a square box

Section 2.1.1

Nonlinear dynamic analysis of a structure with local inelastic collapse

Section 2.1.2

Detroit Edison pipe whip experiment

Section 2.1.5

Pressurized fuel tank with variable shell thickness

Section 2.1.6

Modeling of an automobile suspension

Section 2.1.12

Rigid multi-body mechanism

Section 2.2.1

Analysis of a rotating fan using superelements and cyclic symmetry model

Section 2.2.2

Linear analysis of the Indian Point reactor feedwater line

Section 2.2.3

Response spectra of a three-dimensional frame building

Section 3.1.1

Symmetric results transfer for a static tire analysis

Section 3.1.2

Steady-state rolling analysis of a tire

Section 3.1.3

Subspace-based steady-state dynamic tire analysis

Section 4.1.1

Thermally coupled analysis of a disc brake

Section 4.1.2

Exhaust manifold assemblage

Section 4.1.3

Coolant manifold cover gasketed joint

Section 4.1.4

Radiation analysis of a plane finned surface

Section 5.1.1

Eigenvalue analysis of a piezoelectric transducer

Section 5.2.1

Thermal-electrical modeling of an automotive fuse

Section 6.1.1

Hydrogen diffusion in a vessel wall section

Section 6.1.2

Diffusion toward an elastic crack tip

Section 7.1.1

Coupled acoustic-structural analysis of a car

Section 7.1.2

Fully and sequentially coupled structural acoustics of a muffler

Section 8.1.1

Plane strain consolidation

Section 8.1.2

Calculation of phreatic surface in an earth dam

Section 8.1.3

Axisymmetric simulation of an oil well

Section 8.1.4

Analysis of a pipeline buried in soil

Section 9.1.1

Jack-up foundation analyses

Section 9.1.2

Riser dynamics

Section 10.1.1

The cylinder whip problem

Section 11.1.2

Joining data from multiple results files and converting file format: FJOIN

Section 11.1.3

Calculation of principal stresses and strains and their directions: FPRIN

Section 11.1.4

Creation of a perturbed mesh from original coordinate data and eigenvectors: FPERT

0-1240

Section 11.1.5

Output radiation viewfactors and facet areas: FRAD

Section 11.1.6

Creation of a data file to facilitate the postprocessing of elbow element results: FELBOW

ABAQUS/Explicit Section 1.1.4

Indentation of an elastomeric foam specimen with a hemispherical punch

Section 1.1.5

Collapse of a concrete slab

Section 1.1.7

Indentation of a crushable foam specimen with a hemispherical punch

Section 1.1.9

Hydrostatic fluid elements: modeling an airspring

Section 1.1.14

Indentation of a thick plate

Section 1.2.3

Buckling of a column with spot welds

Section 1.3.2

Upsetting of a cylindrical billet in ABAQUS/Explicit

Section 1.3.4

Stretching of a thin sheet with a hemispherical punch

Section 1.3.6

Extrusion of a cylindrical metal bar with frictional heat generation

Section 1.3.7

Rolling of thick plates

Section 1.3.8

Axisymmetric forming of a circular cup

Section 1.3.9

Cup/trough forming

Section 1.3.10

Forging with sinusoidal dies

Section 1.3.11

Forging with multiple complex dies

Section 1.3.12

Flat rolling: transient and steady-state

Section 1.3.13

Section rolling

Section 1.3.14

Ring rolling

Section 1.3.15

Axisymmetric extrusion: transient and steady-state

Section 1.3.16

Two-step forming simulation

Section 1.3.17

Upsetting of a cylindrical billet: coupled temperature-displacement and adiabatic analysis

Section 1.5.1

Springback of two-dimensional draw bending

Section 1.5.2

Deep drawing of a square box

Section 2.1.3

Plate impact simulation

Section 2.1.4

Tennis racket and ball

Section 2.1.7

Explosive pipe closure

Section 2.1.8

Knee bolster impact with double-sided surface contact

Section 2.1.9

Cask drop with foam impact limiter

Section 2.1.10

Oblique impact of a copper rod

Section 2.1.11

Water sloshing in a baffled tank

Section 2.1.12

Rigid multi-body mechanism

Section 4.1.1

Thermally coupled analysis of a disc brake

ABAQUS/Design 0-1241

Section 1.1.4

Indentation of an elastomeric foam specimen with a hemispherical punch

Section 1.1.12

Symmetric results transfer for a rubber bushing

ABAQUS/Aqua Section 9.1.1

Jack-up foundation analyses

Section 9.1.2

Riser dynamics

ABAQUS/USA Section 10.1.1

The cylinder whip problem

0-1242