CATIA V5 Training Basic

CATIA V5

October 2006

CATIA V5 Basic Training Presentation

CATIA V5 Basic - Presentation

|

V5 14

|

Issue: Draft A6

|

Date: 29. October 06

Contents

CATIA V5 Basic Training

© AIRBUS DEUTSCHLAND GmbH. Alle Rechte vorbehalten. Vertrauliches und geschütztes Dokument.

Functionalities and AIRBUS methodologies

• • • • • • • • •

Introduction Catia V5 Sketcher Part Design Generative Shape Design Introduction Q-Checker Assembly Design Generative Drafting DMU Introduction Settings


|

V5 14

|

Issue: Draft A6

|


Page 2 of 312

Introduction


V5 Basics • • • • • • • • • • • • • • •

Philosophy of CATIA V5 Product Structures Solutions and Workbenches Using the Mouse Desktop User Interface Toolbars Starting the Part Design Workbench Online Documentation Select Objects and Geometry Delete Objects and Geometry General Toolbars Options and Settings Naming and Numbering Layer Filter


|

V5 14

|

Issue: Draft A6

|


Page 3 of 312

Introduction Philosophy of CATIA V5


CATIA Version 5 is an integrated suite of (CAD) Computer Aided Design, (CAM) Computer Aided Manufacturing, (CAE) Computer Aided Engineering applications for digital product definition and simulation.

• • • • • • • • • • •

Interoperability between all CATIA V5 modules (Workbenches) Consistency of data Support of process chains Build up and working in Product structures Parametric design with links inside a Part as well as between the Parts inside an Assembly Individual degree of parameterisation Knowledge based technology Specification-driven modelling for part design, assembly design and integrated drafting Associative feature based modelling Multi window desktop environment Platform independent (UNIX, NT)


|

V5 14

|

Issue: Draft A6

|


Page 4 of 312

Introduction Solutions and Workbenches Solutions

Workbenches


E.g. Part Design Workbench

Catia V5 is divided into different solutions, which contain workbenches that are dedicated to specific tasks


|

V5 14

|

Issue: Draft A6

|


Page 5 of 312

Introduction Solutions and Workbenches


During the design process you can switch between the workbenches to change the available functions for different tasks. Changing the workbench Start With the workbench icon, which is normally located in the right top corner, you have access to your most favourite workbenches

Configure the favourites workbenches Tools

Configure

Available workbenches

Favourites

Note: If you choose the same workbench, which is still open, a new part, product or drawing will be started CATIA V5 Basic - Presentation

|

V5 14

|

Issue: Draft A6

|


Page 6 of 312

Introduction


Using the Mouse Right handed users

Left handed users

Selecting

Click MB1

Click MB3

Zooming

Hold down MB2 and click MB1 once

Hold down MB2 and click MB3 once

Rotating

Hold down MB2 and then MB1

Hold down MB2 and then MB3

Rotation Centre

Click MB2 once

Click MB2 once

Panning

Hold down MB2

Hold down MB2

Contextual menu

Click MB3

Click MB1

Right Button (MB3)

Middle Button (MB2) Left Button (MB1) The following pages refer to right handed users CATIA V5 Basic - Presentation

|

V5 14

|

Issue: Draft A6

|


Page 7 of 312

Introduction Catia V5 Desktop User Interface Pull Down Menus

Compass

Windows Manipulations Help Menu Workbench icon


Specification Tree Workbench Toolbars / Icons General Toolbars / Icons

Dialogue area

Document window Standard Toolbar


|

V5 14

|

Issue: Draft A6

View Toolbar / Manipulation Icons |


Command Input Box Page 8 of 312

Introduction Toolbars (1/3)


All workbenches are driven by the use of icons to issue commands, which are grouped together in toolbars.

Click with the MB1 on the icon to activate the command. The icon will be highlighted in orange. Note: By double clicking on some of the icons the command will stay active. To deselect the command, click on the Icon again or press the Esc key.

Some icons have a subtoolbar, which is indicated by a small black arrow in the right corner at the bottom of the icon.

Note: It is also possible to activate the commands by using the pull down menus.


|

V5 14

|

Issue: Draft A6

|


Page 9 of 312

Introduction Toolbars (2/3)


Use View > Toolbars to know which toolbars should be displayed. You can also click with MB3 on an visible toolbar

The tick indicates that the toolbar is visible in the activated workbench

Note: If a toolbar with the tick is missing in the workbench, it may be outside of the visible desktop area. This will be indicated with chevrons. With MB1 on the chevrons drag the hidden toolbar into the desktop. CATIA V5 Basic - Presentation

|

V5 14

|

Issue: Draft A6

|


Page 10 of 312

Introduction Toolbars (3/3) Resetting Toolbars CATIA V5 memorizes the last toolbar positions.


To reset the toolbars and reach an initial state select View > Toolbars > Customize > Restore position


|

V5 14

|

Issue: Draft A6

|


Page 11 of 312

Introduction Starting the Part Design Workbench Start CATIA V5 from VPM too build up the connection between this two programs A new part can be creates of two different ways:

• Use the Start > Mechanical Design > Part Design pull down menu for starting the Part Design Workbench. • Use the File > New pull down menu to create a new CATPart.


Note: It is not necessary to enter a part name, since the naming and numbering mandatory has to be done by the use of the create & save functionality in VPM.


|

V5 14

|

Issue: Draft A6

|


Page 12 of 312

Introduction Catia V5 Online Documentation (1/3) F1

Use the keyboard key F1 to start the Online Documentation either with Netscape or with Mozilla and get more detailed Information about a functionality

CATIA Documentation Home Page


Full-Text Search

Workbench Indexes

Automation Documentation Home Page CATIA V5 Basic - Presentation

|

V5 14

|

Issue: Draft A6

|


Page 13 of 312

Introduction Catia V5 Online Documentation (2/3) Full-Text Search

2


1 3


|

V5 14

|

Issue: Draft A6

|


Page 14 of 312

Introduction Catia V5 Online Documentation (3/3) Workbench Indexes

2 © AIRBUS DEUTSCHLAND GmbH. Alle Rechte vorbehalten. Vertrauliches und geschütztes Dokument.

1

3


|

V5 14

|

Issue: Draft A6

|


Page 15 of 312

Introduction Selecting Elements Selecting Elements can be done in the geometry area or in the specification tree.

Geometry area In the geometry area you normally select a sub element of the geometry. For a Solid the sub elements are:

• Vertex • Edge • Face

Vertex Edge


Face During a modification this sub elements will be new calculated by CATIA and in some cases the references will be lost!

Specification tree In the specification tree you can select only whole features.

When ever possible use the specification tree for select elements. Because, these kind of selection is a more stable solution for modifications and updates! CATIA V5 Basic - Presentation

|

V5 14

|

Issue: Draft A6

|


Page 16 of 312

Introduction Selecting Objects and Geometry (1/4)

By pointing it to an object’ s element (e.g. lines, edges, vertices, faces, planes) the arrow will be replace by a hand, and by clicking with the MB1 on the element, the object name will be highlighted in the specification tree.

Select


Multi-selection is possible by using the Ctrl-Key

Only the objects located entirely inside the trap will be selected

Selection Trap

Note: It is also possible to drag a bounding outline using the select icon.


|

V5 14

|

Issue: Draft A6

|


Page 17 of 312


Any objects partly or entirely inside the trap will be selected


Intersecting Trap

Drag to create the polygon around the objects to be selected. Close the polygon with a double-click. Only the objects located entirely inside the trap will be selected


|

V5 14

|

Issue: Draft A6

Polygonal Trap

|


Page 18 of 312



Any objects crossed by the paint will be selected

Paint Stroke Trap


|

V5 14

|

Issue: Draft A6

|


Page 19 of 312


Only the objects located entirely outside the trap will be selected


Outside Trap Selection

Any objects partly or entirely inside the trap will be selected

Intersecting Outside Trap Selection


|

V5 14

|

Issue: Draft A6

|


Page 20 of 312

Introduction Preselection Navigator (1/1) With the preselection navigator hidden or coincident elements, or elements located elsewhere in the specification tree can be selected The Preselection Navigator can by activated by: • Any keyboard arrow (left, right, up, down) • ALT + MB1 • CTRL+F11 • Time function


The following Options are available (see Options and Settings)

Activate timer

Display element list Display additional Window (Auxiliary Viewer) Highlight behavior of elements


|

V5 14

|

Issue: Draft A6

|


Page 21 of 312

Introduction Preselection Navigator (2/2) Additional Display window

Arrows for navigating Black arrow indicates the last element in this direction Cross display the selected location


List of stacked elements

Depth selection arrow controls for hidden and coincident elements (up / down) Arrow controls for navigating in the specification tree (top / bottom) MB1 Click on an element or in the circle to select it

In the Dialog area the identification of the pre selected element is displayed:


|

V5 14

|

Issue: Draft A6

|


Page 22 of 312

Introduction Delete Objects and Geometry To delete objects or geometry:

• select the element with the MB1 and use the Del (Entf) key on the keyboard or

• move the cursor to the element and click the MB3 to open the © AIRBUS DEUTSCHLAND GmbH. Alle Rechte vorbehalten. Vertrauliches und geschütztes Dokument.

contextual menu. Select the Delete option.


|

V5 14

|

Issue: Draft A6

|


Page 23 of 312

Introduction General Toolbars Standard Toolbar Open


New

Quick Print

Save

Undo Selection

Copy

Cut

Paste

What‘s this?

Redo Selection

Note: Do not use the Cut function to delete objects or geometry (Memory effect)

Undo last Action

Redo last Action

Undo with History

Redo with History

Change the numbers of steps to Undo in: Tools > Options > General > Performance Note: By increasing the Stack size, the Computer’ s performance will decrease!!


|

V5 14

|

Issue: Draft A6

|


Page 24 of 312

Introduction General Toolbars View Toolbar Fit All In

Fly Mode

Rotate

Pan

Zoom Out

Zoom In

View Mode

Create multi view

Normal View

Quick View

Swap Visible Space

Hide/ Show

Isometric View Shading (SHR) © AIRBUS DEUTSCHLAND GmbH. Alle Rechte vorbehalten. Vertrauliches und geschütztes Dokument.

Front View Shading with Edges

Back View

Shading with Edges without smooth Edges Left View Shading with Edges and Hidden Edges Right View Shading with Material Top View Wireframe (NHR)

Bottom View

Customized view parameters Named Views CATIA V5 Basic - Presentation

|

V5 14

|

Issue: Draft A6

|


Page 25 of 312

Introduction Multi view Divide the screen in several views of the 3D model. The views can be customized in the Menu View

Navigation Mode

Multi-View Customization


Choose a Layout

Viewpoint definition for each view

Define Options for each view


|

V5 14

|

Issue: Draft A6

|


Page 26 of 312

Introduction Named Views / Compass Additional Viewpoints can be saved. 1. 2.

Define the viewpoint by rotate, translate an zoom Create a new view

Add the new view to the selection list Modify the View parameters


Rename the view

Activate the standard views using the compass. Click on the X, Y or Z letter Click on Z axis


|

V5 14

|

Issue: Draft A6

|


Click on Z axis again to reverse view direction.

Page 27 of 312

Introduction Customize View Parameters


Define the visualistaion of the 3D model


|

V5 14

|

Issue: Draft A6

|


Page 28 of 312

Introduction General Toolbars Graphic Properties

Fill colour

Line weight


Transparency

1. 2. 3.

Point type

Line type

Layer

Rendering style

Wizard

Painter (copy graphic Properties)

Select the element of which the graphic properties will be changed Select the icon Select the element with the reference graphic properties

With the Wizard the graphic properties of an element and its parents can be analysed


|

V5 14

|

Issue: Draft A6

|


Page 29 of 312

Introduction Colours (1/3) With colours a hole part or sub elements of a part can be marked.

See AM2232 Module 1 Layers and Colours within CATIA V5

Colours can be defined for different elements:


CATPart • Face (Solid) • Feature • Body • Wireframe and Surface Inside a CATPart the priority of the element colour is from bottom up which can be analyzed with the graphic wizard (CATIA V5 R14):


|

V5 14

|

Issue: Draft A6

|


Page 30 of 312

Introduction Colours (2/3) CATProduct • Product / Sub product • Instance

See AM2232 Module 1 Layers and Colours within CATIA V5


Inside a CATProcuct the priority of the element colour is top down up which can be analyzed with the graphic wizard (CATIA V5 R14):


|

V5 14

|

Issue: Draft A6

|


Page 31 of 312

Introduction Colours (3/3) See AM2232 Module 1 Layers and Colours within CATIA V5

Regulations for Colours • Do not use the colours red and orange, because this are system


• • •

colours of CATIA V5 and define a special model status. Do not use colours on Product level A CATPart should have only one colour. For A-UK set all colourdefinitions back to colour by layer. (see NATCO Add-on)


|

V5 14

|

Issue: Draft A6

|


Page 32 of 312

Introduction Layer (1/2)


CATIA V5 functionality enables See AM2232 Module 2 CAD Layers Organisation designers to manage their own design See AM2232 Module 1 Layers and colours within CATIA V5 and data organisation without layering use. Nevertheless, the use of layers is necessary for Master Model identification, DMU Visualization, Data transfer and Manufacturing processes CATPart • In case of solid definition, only the Part-body has to be on a layer • In case of wire-frame or surface definition (MG, DP, FM), the Open-body grouping some elements might be on the appropriate layer and elements inside the Openbody may be on layer none • Use of layers forbidden for Part Number property level CATProduct Use of layers forbidden for CATProduct and CATPart Part Number property levels. CATDrawing No mandatory layers CATIA V5 Basic - Presentation

|

V5 14

|

Issue: Draft A6

|


Page 33 of 312

Introduction Layer (2/2) Select View > Toolbars > Graphic Properties in the pull down menu

Layer box Catia V5 provides several layers. All layers will be visible in the layer box

•

"None" in the Layer box indicates that there is no current layer for the selected object. If an object is selected, the name of the layer on which the object is located is displayed in the box. To find out which layer an object is assigned to, select the object and look at the Layer box. When no objects are selected, the layer is displayed in the Layer box as “None” Any new objects will be created on the current layer To move from the current layer, make sure that no object is selected, then enter the new layer number in the box.


•

• • •

To change the layer of an object • •

Note: It is not allowed to modify or add a layer name

select the object select a layer in the Layer box CATIA V5 Basic - Presentation

|

V5 14

|

Issue: Draft A6

|


Page 34 of 312

Introduction Filter After assigning objects to layers, create some filters which allow you to display only the objects which are located in specific layers. Select Tools > Visualization Filters... To create a new filter click on New

Define the new filter

Select a filter and click ok


New

To use one of the default filters select the filter and click ok


|

V5 14

To rename the filter select it, (MB1) and once more, a bounding box appears round it. You can now change its name.

|

Issue: Draft A6

|


Page 35 of 312

Introduction Options and Settings To modify the CATIA V5 options use the pull down menu Tools > Options. There are several general options and special options for each Workbench.


For example Tools > Options > General > Display > Tree to show the “display of the specification tree” options

If an option is locked (a red symbol) the user can’t modify it.


|

V5 14

|

Issue: Draft A6

|


Page 36 of 312


Sketcher • • • • • • • • • • • • •

Basics Sketcher Rules Accessing the Sketcher Toolbars and Icons Overview Toolbar Profile Creation Toolbar Operations Toolbar Constraints Toolbar Sketch Tools Constraints Formula Parameter Sketch Analysis Hints and Tips

Constraints Dimensioning Sketch positioning Multi domain Projection and Intersection Create Circle


|

V5 14

|

Issue: Draft A6

|


Page 37 of 312

Sketcher Basics • A Sketch is a geometric elements which contains one or several contour created in the Sketcher workbench.

• The sketcher workbench provides a set of functions for creating and


modifying sketched elements.

• A sketch contour may include profiles, construction lines and points • It is possible to apply constraints to the sketched elements. • In the Sketcher it is possible to work with an individual degree of parameterisation. This is not allowed at AIRBUS.


|

V5 14

|

Issue: Draft A6

|


Page 38 of 312

Sketcher Sketcher Rules


• Keep sketches as simple as possible to make modifications easily. • Don’t create geometry which can be created as a feature • • •

(e.g. fillets, chamfers, holes) Use the mirror function in the Part Design, not in the Sketcher. The sketch has to be fully constrained. Auxiliary elements have to be created as construction elements


|

V5 14

|

Issue: Draft A6

|


Page 39 of 312

Sketcher Sketcher Rules There are some restrictions for sketches to create solid features: Allowed Sketch Contours

One closed contour

Several contours

Several contours


Sketch Contours with restrictions for some solid features

Open contour

Intersecting open contour

Point (In standard mode)

Not Allowed Sketch Contours

Intersecting closed contours CATIA V5 Basic - Presentation

|

V5 14

|

Self intersecting contour Issue: Draft A6

|


Page 40 of 312

Sketcher Accessing the Sketcher (1/4) There are different possibilities to start the sketcher:

• Inside e.g. the Part Design or Wireframe and Surface Design Workbench click the


Sketcher Icons

Sketcher

Sketch with Absolute Axis definition

• From any Workbench double-click an existing sketch • Alternatively : Start > Mechanical Design > Sketcher from the pull down menu. Note: If there is no CATPart open, Start > Mechanical Design > Sketcher will create a new CATPart inside the Part Design Workbench


|

V5 14

|

Issue: Draft A6

|


Page 41 of 312

Sketcher Accessing the Sketcher (2/4) Sketcher To define the Sketch Support, select a plane or a planar face or surface (either in the geometry area or in the specification tree).


Sketcher The normal of the working support is the same as the principal normal of the selected plane. Eg. If you choose a plane parallel to the xy plane, the principal normal is z. The origin of the Absolute Axis system of the sketch is automatically positioned on the origin of the CATPart.

Note: A sketch used to create a Part Design element (e.g. a pad) should be created directly in the body that will contain this element and not in an open body. Otherwise it will be duplicated and its management will be trickier. (See AM2259)


|

V5 14

|

Issue: Draft A6

|


Page 42 of 312

Sketcher Accessing the Sketcher (3/4) Sketch with Absolute Axis definition This command enables to create a logical sketch origin. This will give better control and easier constraining of the sketch.


Origin (e.g. intersection between the axis and the face of the shaft) Sketch Support (e.g. face of the shaft)

Sketch with Absolute Axis definition

Note: You can use the contextual menu (MB3 > Sketch object > Change Sketch Support ...) to change the Sketch Positioning at any time. CATIA V5 Basic - Presentation

|

V5 14

|

Issue: Draft A6

|

Orientation (e.g. horizontal direction (H) parallel to an edge of the pocket) Date: 29. October 06

Page 43 of 312

Sketcher Accessing the Sketcher (4/4) Sketch with Absolute Axis definition

Origin: Define the Origin of the sketch


Origin:

Part origin Projection point Intersection 2 lines Curve intersection Middle point Barycentre

Project a point on the sketch plane Intersection Point of two lines Intersection point of a curve with the sketch plane Middle point of a curve / line Centre of gravity of a surface

Orientation: Define the orientation of the h and v axis Orientation: X, Y, Z-Axis Components Through point Parallel to line Intersection plane


|

V5 14

|

define a vector by its components Line between the origin and a point Parallel to a line intersection between a plane an the sketch plane

Issue: Draft A6

|


Page 44 of 312

Sketcher Toolbars and Icons Overview (1/9) Toolbar Profile Creation (1/2)

Rectangle


Profile

Spline

Circle

Line

Ellipse

Rectangle

Circle

Oriented Rectangle

Three Point Circle

Parallelogram

Circle using Coordinates

Elongated Hole

Tri-Tangent Circle

Cylindrical Elongated Hole

Three Point Arc

Point

Axis

Spline Connect

Three Point Arc Starting With Limits

Keyhole Profile

Arc Hexagon Centered Rectangle Centered Parallelogram CATIA V5 Basic - Presentation

|

V5 14

|

Issue: Draft A6

|


Page 45 of 312

Sketcher Toolbars and Icons Overview (2/9) Toolbar Profile Creation (2/2) Rectangle


Profile

Spline

Circle

Line

Ellipse

Point

Axis

Ellipse

Line

Point

Parabola by Focus

Infinite Line

Point Using Coordinates

Hyperbola by Focus

Bi-Tangent Line

Equidistant Points

Creates a Conic

Bisecting Line

Intersection Point Projection Point Line Normal to Curve


|

V5 14

|

Issue: Draft A6

|


Page 46 of 312

Sketcher Toolbars and Icons Overview (3/9) Toolbar Operation Chamfer


Corner

Symmetry

Trim

Trim

Symmetry

Break

Translate

Quick Trim

Rotate

Close

Scale

Complement

Offset


|

V5 14

|

Issue: Draft A6

|


Project 3D-Elements

Project 3D Elements Intersect 3D Elements Project 3D Silhouette Edges

Page 47 of 312

Sketcher Toolbars and Icons Overview (4/9) Toolbar Constraints


Constraint

Constraints Defined in Dialog Box

Auto Constraint

Contact Constraint

|

V5 14

|

Issue: Draft A6

Edit Multi Constraint

Fix together

Constraint


Animate Constraint

|


Page 48 of 312

Sketcher Toolbars and Icons Overview (5/9) Toolbar Sketch tools (Standard)

Snap to Point on Grid


Construction/Standard Element

Geometrical Constraints

Dimensional Constraints


|

V5 14

|

Issue: Draft A6

|


Page 49 of 312

Sketcher Toolbars and Icons Overview (6/9) Toolbar Sketch tools (Extended)

Further tools belonging to the selected function (e.g. Profile)

Standard tools

Options


Function:

Option:

Function:

Option: Select a Curve before

Symmetrical Extension Line normal to a curve

Line

Infinite Line

Profile Tangent Arc

Line through two Points Vertical Line

Line (Standard)

Horizontal Line

Three Point Arc


Fields for entering constraints value manually

|

V5 14

|

Issue: Draft A6

|


Page 50 of 312

Sketcher Toolbars and Icons Overview (7/9) Toolbar Sketch tools (Extended) Funktion:

Option:

Funktion:

Nearest Endpoint

Connect with an Arc


Connect

Conic Connect with a Spline

Two Points

Continuity in Point

Four Points

Continuity in Tangent

Five Points

Continuity in Curvature

Start and End Tangent

Tension of the tangency


|

Option:

V5 14

|

Issue: Draft A6

|


Tangent Intersection Point

Page 51 of 312

Sketcher Toolbars and Icons Overview (8/9) Toolbar Sketch tools (Extended) Function:

Function:

Option:

Trim all Elements


Corner


Trim all Elements Chamfer

Trim first Element

|

Option:

Trim first Element

No Trim

No Trim

Standard Lines Trim

Standard Lines Trim

Construction Lines Trim

Construction Lines Trim

Construction Lines No Trim

Construction Lines No Trim

V5 14

|

Issue: Draft A6

|


Page 52 of 312

Sketcher Toolbars and Icons Overview (9/9) Toolbar Sketch tools (Extended) Funktion:

Option:

Funktion:

Quick Trim

Trim

Break and keep Break and rubber out Break and rubber in

Trim first Element © AIRBUS DEUTSCHLAND GmbH. Alle Rechte vorbehalten. Vertrauliches und geschütztes Dokument.

Option:

Trim all Elements

Both Side Offset Offset

Point Propagation

Along a Direction Projection Point

Orthogonal Projection

Tangent Propagation No Propagation


|

V5 14

|

Issue: Draft A6

|


Page 53 of 312

Sketcher SmartPick (1/3) Using SmartPick, you will easily specify a location:

• all over a curve • at the intersection point of two curves • aligned at a vertical/horizontal position • on the fictitious perpendicular line through a line end point • any of the above cases possibly combined together,

• somewhere on the grid • using coordinates • on a point • at the extremity point of a curve • at the midpoint of a line • at the centre of a circle or an ellipse

whenever possible.


There are four ways to use the SmartPick: 1. 3D graphic window and SmartPick cursor:

2. Contextual menu:

3. Sketch tools toolbar (Coordinates and parameters): 4. Ctrl and Shift key


|

V5 14

|

Issue: Draft A6

|


Page 54 of 312

Sketcher SmartPick (2/3) Symbols for the SmartPick cursor horizontal Vertical Point, Curve Extremity Point, Midpoint of a Line All over a Curve, Intersection Point Tangent


Parallel Perpendicular Selection not possible

Note: To create a geometrical constraint from the SmartPick detection the „Geometrical Constraint“ icon must be activated (orange). To create a dimensional constraint from the parameter values in the Sketch Tools Toolbar the „Dimensional Constraint“ icon must be activated (orange). CATIA V5 Basic - Presentation

|

V5 14

|

Issue: Draft A6

|


Page 55 of 312

Sketcher SmartPick (3/3) Control the activity of the constraint detection Shift Key: Dynamic deactivation of the auto-detection (SmartPick)


Press and Keep Hold of the Shift Key

In this example the horizontal and coincidence constraints are not longer detected

Ctrl Key: Lock the current detected constraint to reduce the degree of freedom Press and Keep Hold of the Ctrl Key

In this example the tangency constraint is locked CATIA V5 Basic - Presentation

|

V5 14

|

Issue: Draft A6

|


Page 56 of 312

Sketcher Toolbar Profile Creation (1/6) Create an open or closed shape including arcs and lines. You can create either by clicking or using the Sketch tools toolbar. When you create a profile by using the Sketch tools toolbar, constraints are similarly assigned to this profile. Profile Create a rectangle by clicking or using the Sketch tools toolbar. The orientation of the lines will be horizontal or vertical.


Rectangle Create a rectangle in the direction of your choice by clicking or using the Sketch tools toolbar. Define the direction of the first side with a line, and then the height of the rectangle with a point. Oriented Rectangle Create a parallelogram by clicking or using the Sketch tools toolbar.

Parallelogram Create an elongated hole by clicking or using the Sketch tools toolbar. Define the first and the second point of the symmetry axis, and then the elongated hole radius. Elongated Hole


|

V5 14

|

Issue: Draft A6

|


Page 57 of 312

Sketcher Toolbar Profile Creation (2/6) Create an cylindrical elongated hole by clicking or using the Sketch tools toolbar. Define the circle centre, the arc extremities and the radius of the cylindrical elongated hole. Cylindrical Elongated Hole Create a keyhole profile by clicking or using the Sketch tools toolbar. Define the first and the second point of the symmetry axis, the first radius and then the second radius.


Keyhole Profile Create an hexagon inside a construction circle by clicking or using the Sketch tools toolbar. Define the hexagon centre and then either a point on this hexagon or the hexagon dimension and angle Hexagon Create a circle by clicking or using the Sketch tools toolbar. Define the circle centre and the radius. Circle Create a circle by clicking or using the Sketch tools toolbar. Define the circle start point, second point and end point one after the other. Three point Circle


|

V5 14

|

Issue: Draft A6

|


Page 58 of 312

Sketcher Toolbar Profile Creation (3/6) Create a circle by using the Circle Definition dialog box. Define the centre point coordinates and the Radius. If you select a point before clicking the icon, this point will be used as reference point. Else the reference point is the origin of the sketcher axis system. Circle using Coordinates Create a circle by clicking. Define three elements (point, line, circle, spline) one after the other to create a circle made of three tangent constraints (line, circle, spline) or coincidence constraints (point). Tri-Tangent Circle


Create an arc by clicking or using the Sketch tools toolbar. Define the arc start point, second point and end point one after the other. Three Point Arc Create a circle by clicking or using the Sketch tools toolbar. Define the arc start point, end point and second point one after the other. Three Point Arc Starting With Limits Create a circle by clicking or using the Sketch tools toolbar. Define the arc centre and then the arc start point and end point. Arc


|

V5 14

|

Issue: Draft A6

|


Page 59 of 312

Sketcher Toolbar Profile Creation (4/6)

Spline


Connect

Create a spline by clicking or using the Sketch tools toolbar. Indicate the points through which the spline goes. Double-click to end the spline. To edit a control point (position, tangency, curvature radius) double-click on this. Create a connection between two curves. Select the connect option in the Sketch tools toolbar: With an Arc or With a Spline. Select the first element and then the second element. The connection is tangent to both selected elements. Create an ellipse by clicking or using the Sketch tools toolbar. Define the ellipse centre, major semi-axis and minor semi-axis endpoints one after the other.

Ellipse Create a parabola by clicking or using the Sketch tools toolbar. Define the focus, apex and then the parabola two extremity points. Parabola by Focus Create a hyperbola by clicking or using the Sketch tools toolbar. Define the focus, centre and apex, and then the hyperbola two extremity points. Hyperbola by Focus


|

V5 14

|

Issue: Draft A6

|


Page 60 of 312

Sketcher Toolbar Profile Creation (5/6) Create a conic type element (circle, ellipse, parabola, hyperbola) by clicking or using the Sketch tools toolbar. Define the desired points and if needed, use tangents or enter the excentricity Creates a conic


Line

Create a line by clicking or using the Sketch tools toolbar. Define the startpoint and the endpoint of the line. Use the contextual menu to copy the length of an existing line or to take an existing line as angle reference. Create an infinite line either horizontal, vertical or through two points by clicking and using the Sketch tools toolbar. Select an option in the toolbar and then indicate one or two points.

Infinite Line Create a line by clicking. Define two elements (point, line, circle, spline) one after the other to create a line made of two tangent constraints (line, circle, spline) or coincidence constraints (point). Bi-Tangent Line Create an infinite bisecting line by clicking or using the Sketch tools toolbar. Select two existing lines. If both selected lines are parallel to each others, a new line will be created between these lines. Bisecting Line


|

V5 14

|

Issue: Draft A6

|


Page 61 of 312

Sketcher Toolbar Profile Creation (6/6)

Point

Create a point by clicking or using the Sketch tools toolbar. Define the horizontal and vertical coordinates of the point. To get the centre of gravity between existing points (isobarycenter), select this points before clicking the point’s icon. NOTE: All the points must be converted into construction elements, before using a sketch for creating a solid feature (e.g. a pad).


Create a point by using the Point Definition dialog box. Define the point coordinates. If you select a point before clicking the icon, this point will be used as reference point. Else the reference point is the origin of the sketcher axis system. Point Using Coordinates Create a point by using the Equidistant Point Definition dialog box. Select a line or a curve-type element. Define the number and spacing of the points. Equidistant Points Create one or more points by intersecting curve type elements. Multi-select the elements to be used for intersecting, then click the Intersection Point icon and then select the element which intersect with the first selected. Intersection Point

Projection Point

Create one or more points by projecting points perpendicular onto curve type elements. Select the points to be used for projection, then click the Projection Point icon and then select an element on which the points will be projected.


|

V5 14

|

Issue: Draft A6

|


Page 62 of 312

Sketcher Create a profile (1/2) 1. Click with MB1 to define the start point of the profile

2. Move the mouse to define the end point of the first segment. Click with MB1 to define the end point. This is the start point for the next line.


The parameters for the segments can also defined in the Sketch tool bar.

3. Finish a closed profile by select the start point. Pay attention for the SmartPick icon.

4. Finish a open profile by double click.


|

V5 14

|

Issue: Draft A6

|


Page 63 of 312

Sketcher Create a profile (2/2) 5. To create an tangent arc, hold down the MB1 and move the mouse away from the last endpoint. The parameters for the segments can also defined in the Sketch tool bar.


6. To create an non tangent arc or start the profile with an arc, you have to use the “Three point arc” icon.


|

V5 14

|

Issue: Draft A6

|


Page 64 of 312

Sketcher Toolbar Operation (1/3)

Corner


Chamfer

Trim

Create a rounded corner between two lines or curve type elements using trimming operation. The arc will be tangent to the two lines or curves. To modify the trim option (Trim All Elements, Trim First Element, No Trim) use the Sketch tools toolbar. You can create several corners by multi-selecting Create a chamfer between two lines or curve type elements using trimming operation. To modify the trim option (Trim All Elements, Trim First Element, No Trim) or the chamfer definitions (Angle/Hypotenuse, Length1/Length2, Length1/Angle) use the Sketch tools toolbar. You can create several chamfers by multi-selecting Trim lines or curve type elements. If an element does not intersect with another element an extrapolation is done. To modify the trim option (Trim All Elements, Trim First Element) use the Sketch tools toolbar. You can multi-select the elements to be trimmed Break a line or a curve type element. First select the line to be broken and then the element which is used for breaking. By using the break icon, you can also isolate points.

Break Quickly breaking, trimming and/or deleting (rubber) elements intersected by other Sketcher elements. To modify the trim option (Break And Rubber In, Break And Rubber Out, Break And Keep) use the Quick Trim Sketch tools toolbar.


|

V5 14

|

Issue: Draft A6

|


Page 65 of 312

Sketcher Toolbar Operation (2/3) Close circles or ellipses. Set splines which was relimited by using the trim icon to its original limitation again. Close Complement an arc (circle or ellipse)


Complement Create the symmetry of existing Sketcher elements by using a line, a construction line or an axis. The geometry will be duplicated. If the Dimensional Constraint option in the Sketch tools toolbar is activated a Symmetry symmetry constraint is created. Create a translation by using the Translation Definition dialog box. Enter the number of copies, (multi-)select the element to be translated, select the start and endpoint of the translation vector and define the value for the translation length. The duplicate mode is activated by default. Internal and Translate external constraints (geometrical and dimensional) can be preserved.

Rotate

Create a rotation by using the Rotation Definition dialog box. Enter the number of copies, (multi-)select the element to be rotated, select the rotation centre point, click a point to define the reference line, define the value for the rotation angle. The duplicate mode is activated by default. Internal constraints can be preserved. External geometrical constraints are deleted. External dimensional constraints are modified.


|

V5 14

|

Issue: Draft A6

|


Page 66 of 312

Sketcher


Toolbar Operation (3/3)

Scale

Scale a profile. The distance values will be resized, the angle values will not be modified. (Multi-)select the element to be scaled, define the centre point on the geometry, enter the scale value. The duplicate mode is activated by default. Internal constraints can be preserved. External geometrical constraints are killed. External dimensional constraints are modified.

Offset

Create an offset of 2D geometry (lines and curves). Create an associative offset of 3D geometry (edge, face and geometrical features). To modify the offset options (No Propagation, Tangent Propagation, Point Propagation and Both Side Offset) use the Sketch tools toolbar. Constraints are not created. No propagation on 3D edges.

Project 3D elements (e.g. edges or faces) onto the sketch plane. If you select a face, the edges are projected. These projections (marks) are yellow and associative to the 3D part. If needed, use the contextual menu to isolate the marks. Project 3D Elements Intersect 3D elements (e.g. edges, faces, pads) onto the sketch plane. If you select a face or pad, the edges are projected. These projections (marks) are yellow and associative to the 3D part. If needed, use the contextual menu to isolate the marks. Intersect 3D Elements Project silhouette edges from a canonical surface onto the sketch plane. The axis of the canonical surface must be parallel to the sketch plane. These projections (marks) are yellow and associative to the 3D part. If needed, use the contextual menu to isolate the marks. Project 3D Silhouette Edges CATIA V5 Basic - Presentation

|

V5 14

|

Issue: Draft A6

|


Page 67 of 312

Sketcher Toolbar Constraints Define one or several constraints simultaneously using the Constraint Definition dialog box. Select or multi-select the elements to be constrained and then the Constraints Defined in Dialog Box Icon. Constraints Defined in Dialog Box Set dimensional or geometrical constraints between one or several elements. The constraints are in priority dimensional. Use the contextual menu to get other types of constraints and to position this constraint as desired. Constraint


Apply a constraint with a relative positioning that can be compared to contact: Concentricity, coincidence or tangency Contact Constraint Automatic detection and creation of possible constraints between selected elements. It is possible to define reference elements and symmetry lines. Automatic Constraint Examine how the whole sketch is reacting when one constraint is varied between a maximum and a minimum value. Animate Constraint


|

V5 14

|

Issue: Draft A6

|


Page 68 of 312

Sketcher Toolbar Constraints Join geometry to a rigid set. If one element is moved, the hole group move together. Fix together

All the dimensional constraints of a sketch can be edit in a dialog box at the same time


Edit Multi-Constraint


|

V5 14

|

Issue: Draft A6

|


Page 69 of 312

Sketcher Toolbar Sketch Tools

If activated, this option makes your sketch begin or end on the points of the grid. As you are sketching the points are snapped to the intersection points of the grid. Snap to Point Create standard elements when the icon is inactivated and construction elements when the icon is activated. Construction elements are not taken into account when creating features, and they do not appear outside the Sketcher


Construction/Standard Element

Geometrical Constraints will automatically be created while creating the sketch. Geometrical Constraints Dimensional Constraints will automatically be created while creating the sketch.

Dimensional Constraints


|

V5 14

|

Issue: Draft A6

|


Page 70 of 312

Sketcher Tools If the Icon is activated Projections, Intersections and Silhouettes from 3D are not associative. Create Datum With the output feature construction elements and single elements can be used outside the sketch. Output features have a special update behaviour. Output feature


Several Profiles inside a complex sketch can be defined. In the specification tree each profile can be selected separate Output Profil Analyse if the sketch is fully, under or over constraint

Sketch Solving Status Analysis sketches for inconsistence

Sketch Analysis


|

V5 14

|

Issue: Draft A6

|


Page 71 of 312

Sketcher Visualisation Cut the 3D Solid geometry temporary on the sketch plane to see the inside the volume. Cut Part by Sketch plane The Usual mode is the default option. When activated, the 3D geometry is visible in the Sketcher.


Usual In the Low Light mode all geometrical elements and features appear as graycolored, except for the current sketch. You cannot select the 3D geometry, you can just handle Sketcher elements. Low Light

The No 3D Background mode hides all geometrical elements and features (products, parts, etc.) except for the current sketch. No 3D Background


|

V5 14

|

Issue: Draft A6

|


Page 72 of 312

Sketcher Visualisation Show / Hide the diagnostic colours of the sketch

Diagnostic Show / Hide all dimensional Constraints of the sketch

Dimensional constraint


Show / Hide all geometrical Constraints of the sketch

Geometrical Constraint


|

V5 14

|

Issue: Draft A6

|


Page 73 of 312

Sketcher Constraints (1/4) Constraints are used to control the size and the position of an element and its relationship to other elements.


Geometric Constraints control the • relationship between the elements (e.g. coincidence, parallel) or • the orientation of an element (e.g. horizontal, vertical). Dimensional Constraints control the • size of an element (e.g. length, radius) or • the distance and angle between elements.


|

V5 14

|

Issue: Draft A6

|


Page 74 of 312

Sketcher Constraints (2/4)


Visualization of Geometric Constraints

Fix

Concentricity

Coincidence

Symmetry

Horizontal

Midpoint

Vertical

Equidistant point

Tangency Perpendicular Parallelism


|

V5 14

|

Issue: Draft A6

|


Page 75 of 312

Sketcher Constraints (3/4) Visualization of Dimensional Constraints

Length / Distance Radius Diameter © AIRBUS DEUTSCHLAND GmbH. Alle Rechte vorbehalten. Vertrauliches und geschütztes Dokument.

Angle Semiminor axis

Note: You can obtain a radius constraint by editing a diameter constraint. You just need to double-click the diameter constraint and choose the radius option in the displayed dialog box.

Semimajor axis


|

V5 14

|

Issue: Draft A6

|


Page 76 of 312

Sketcher Constraints (4/4)


Constraint Colors Select another element or the background

Orange

Selected

Green

Fixed

All relevant dimensions are created. The whole geometry has been fixed using the fix constraint

Sketch can be used

Green

Iso-constrained

The element is fixed and cannot be moved from its geometrical support. (E.g. if you fix a line it is still possible to move the endpoints)

Sketch can be used

White

Under-constrained

Still some degrees of freedom remaining

Sketch can be used but is not allowed at AIRBUS

Purple

Over-constrained

Too many dimensions have been applied to the geometry

Remove one or more dimensional constraints

Red

Inconsistent

The system is unable to find a consistent solution for the dimension system

At least one dimension value needs to be changed

Brown

Geometry not changed

No recalculation because some geometrical elements are over-defined or inconsistent

Remove one or more constraints

Protected

E.g. marks which were created via projection or intersection with associativity to external 3D elements

Sketch can be used. Isolate the marks to get rid of the associativity

Yellow


|

V5 14

|

Issue: Draft A6

|


Page 77 of 312

Sketcher Formula (1/3)


Adding a Formula

Select the Edit formula option to open the Formula Editor

Double-clicking on the desired constraints to modify the related data in the displayed Constraint Definition dialog box move the cursor to the value and click the MB3 to open the contextual menu


|

V5 14

|

Issue: Draft A6

|


Page 78 of 312

Sketcher Formula (2/3) Adding a Formula

In the upper field you will find the selected constraints, the field below is for the formula.


In the sketch the value of the constraint is modified and the formula symbol is shown.

Define the formula

In the Constraint Definition dialog box the Value is dimmed and the formula symbol appears.


|

V5 14

|

Issue: Draft A6

|


Page 79 of 312

Sketcher Formula (3/3) Show the name of a dimension


For a better overview, it is possible to display the name of a dimension in the sketch.

Move the cursor to the value and click the MB3 to open the contextual menu

Note: Use formulas only for real master elements and not for creation comfort reasons (See AM2259) CATIA V5 Basic - Presentation

|

V5 14

|

Issue: Draft A6

|


Page 80 of 312

Sketcher Parameter (1/4) Creating a user Parameter


It is possible to create additional parameters which can be used e.g. in a formula.

The parameter will automatically get a name (e.g. Length.1). Replace the name and assign the value to this parameter

3

Click New Parameter of type

2 1 Select e.g. the Length item with Single Value in the New Parameter of type list


|

V5 14

|

Issue: Draft A6

|


Page 81 of 312

Sketcher Parameter (2/4) Displaying a user Parameter


The user parameters are displayed in the Parameters box of the specification tree

Note: To display the parameter use Tools > Options > Infrastructure > Part Infrastructure > Display > Display in Specification Tree To display the parameter with their provided values, use Tools > Options > General > Parameters and Measure > Knowledge > Parameter Tree View


|

V5 14

|

Issue: Draft A6

|


Page 82 of 312

Sketcher Parameter (3/4) Using a user Parameter


The new parameter can be used to define a formula. To display the new and renamed parameter select Renamed parameters in the field Members of Parameter

Double-click the parameter in the field Members of Renamed parameters to insert the parameter in the formula.


|

V5 14

|

Issue: Draft A6

|


Page 83 of 312

Sketcher Parameter (4/4) Lock Parameter With this functions parameters can be looked and unlooked. The value of a looked parameter can not be changed. Select the parameter and the icon for lock and unlock.

Lock Unlock


A special icon identify the locked status of a parameter.

Alternatively the MB3 can be used to lock and unlock parameters.


|

V5 14

|

Issue: Draft A6

|


Page 84 of 312

Sketcher Equivalent Parameters (1/4) Equivalent Parameters With this function several (Length and Angle) Parameters can be set to the same value. When one of the equivalent parameters will be changed all the other will became the same value.


Menu to choose the parameters


|

V5 14

|

Issue: Draft A6

|


Page 85 of 312

Sketcher Equivalent Parameters (2/4)


Select the parameters in the sketch or in the left column of the dialog window.

Add the parameter to the list of equivalent dimensions.


|

V5 14

|

Issue: Draft A6

|


Page 86 of 312


List of the parameters with the same values

Change the parameter value


Finish the function by clicking OK

In the specification tree the equivalent dimensions is positioned under the relations


|

V5 14

|

Issue: Draft A6

|


Page 87 of 312



Equivalent Dimensions can be edit by double click the specification tree or one of the values


|

V5 14

|

Issue: Draft A6

|


Page 88 of 312

Sketcher Sketch Analysis (1/3)


Inside the Sketcher Workbench use the Tools > Sketch Analysis pull down menu to start the Sketch Analysis


|

V5 14

|

Issue: Draft A6

|


Page 89 of 312

Sketcher Sketch Analysis (2/3) A general status of all geometrical elements will be shown After the selection of an element in the Geometry list (e.g. Point.22) or in the Projections/Intersections list, it is possible to use some corrective actions if the geometry is not correct. Projections / Intersections


Geometry turn this element into a construction element

isolate geometry

close an open profile

activate/deactivate a constraint

erase a disturbing element

erase geometry

Hide constraints

replace 3D geometry

Hide Construction Geometries

Hide constraints Hide Construction Geometries


|

V5 14

|

Issue: Draft A6

|


Page 90 of 312

Sketcher Sketch Analysis (3/3)


The Diagnostic tab provides information about under-constraint elements


|

V5 14

|

Issue: Draft A6

|


Page 91 of 312

Sketcher Hints and Tips – Constraints (1/3) Starting the Sketch in the origin of the sketch absolute axis


If the origin of the sketch absolute axis (yellow axis) has been selected as the starting point of the sketch (e.g. the centre point of a circle), the system will automatically create a coincidence constraint between the origin and the starting point. Note: This constraint won’ t be displayed, therefore it won’ t be possible to select the constraint directly to delete it.

Hint: By using the Break icon, you can isolate points: If you select a point with a coincident constraint, this point will become independent of the coincidence constraint. CATIA V5 Basic - Presentation

|

V5 14

|

Issue: Draft A6

|

Select the Break icon and then the point


Page 92 of 312

Sketcher Hints and Tips – Constraints (2/3) Control the activity of the constraint detection (3/3) SmartPick switch button: Permanent deactivation of the auto-detection (SmartPick).


As you create more and more elements, SmartPick detects multiple directions and positions, and more and more relationships with existing elements. This may lead to confusion due to the rapid highlighting of several different detection possibilities as you point the cursor at different elements in rapid succession. Consequently, you can decide to filter out undesired detections. Use the Tools > Options > Mechanical Design > Sketcher > Sketcher > Constraints menu and select the SmartPick Icon to modify the SmartPick options.

Alternatively you can

press the Shift key to deactivate all smart pick options.


|

V5 14

|

Issue: Draft A6

|


Page 93 of 312

Sketcher Hints and Tips – Constraints (3/3) Modify the Constraint Type 1. 2. 3.

Activate the Constraint command or the Contact Constraint command Click with the MB3 the constraint to be modified. Select the option corresponding to the desired operation, from the contextual menu.


Coincidence constraint type.

1

Distance constraint type.

2

3 CATIA V5 Basic - Presentation

|

V5 14

|

Issue: Draft A6

|


.

Page 94 of 312

Sketcher Hints and Tips – Dimensioning (1/2) Manage the orientation and type of the current dimension


Constraint Icon activated + MB3 (Contextual menu): • Change length or distance to horizontal or vertical dimension

• Change the type of the dimension (e.g. from Angle to Perpendicular)


|

V5 14

|

Issue: Draft A6

|


Page 95 of 312

Sketcher Hints and Tips – Dimensioning (2/2) Modify geometry


Edit dimensional constraint values just by dragging constrained geometry

Press and Keep Hold of the Shift Key while dragging the geometry

The constraint is temporary a reference


|

V5 14

|

Issue: Draft A6

|


Page 96 of 312

Sketcher Hints and Tips - Multi domain Sketch Multi domain


A sketch can contain several contours with functional links.


|

V5 14

|

Issue: Draft A6

|


Page 97 of 312

Sketcher Hints and Tips - Projection and Intersection (1/2) Projection and Intersection of 3D Elements Note that the order of the selection (Action-Object or Object-Action) can change the result 1. Action-Object Select the Surface of a cylinder


Select the Intersection Icon

The axis will be highlighted

The result is a point

2. Object-Action Select the Surface of a cylinder


|

Select the Intersection Icon

V5 14

|

Issue: Draft A6

|


The result is a circle

Page 98 of 312

Sketcher Hints and Tips - Projection and Intersection (2/2) Projection and Intersection of 3D Elements Projection and intersection of 3D elements directly to sketches •


•

Marks created via projection, intersection or silhouette edges are associative to their parent 3D elements To break this associativity use the MB3 > Sketch.object > Isolate. The marks are isolated and each trace is replaced by an equivalent geometrical element

Note if working in an assembly: If the option “Keep link with selected object” is active, an object created from the selection will keep the link with it. A selection between two different CATParts (selection in context) will create and keep a link (external reference) between these. To avoid undesired links, make sure that at least the option Tool > Option > Infrastructure > Part Infrastructure > General > “Confirm when creating a link with selected object” is activated. CATIA V5 Basic - Presentation

|

V5 14

|

Issue: Draft A6

|


Page 99 of 312

Sketcher Hints and Tips - Create Circle Switch between radius and diameter


double-click the radius value > Constraint Definition

Copy radius to the next circle Select the circle Icon and move the cursor over the existing circle, now MB3.


MB3 > Parameters > Copy Radius

|

V5 14

|

Issue: Draft A6

|


Page 100 of 312

Sketcher Hints and Tips - Dimension of an Ellipse For a iso constraint ellipse you need the following five constraints:

Semiminor axis

Position of the centre


Semimajor Axis: Select the ellipse

Angle

Semimajor axis

Semiminor Axis: Select the ellipse and select Semiminor axis in the context menu

Angle: select the ellipse and a reference element.


|

V5 14

|

Issue: Draft A6

|


Page 101 of 312

Part Design

• Basics

• Hints and Tips


• The Specification Tree • PartBody, Body and Open body • Features

• • •

• • • • • • • • • •

Toolbars and Icons Overview Sketch-Based Features Dress-Up Features Transformation Features Reference Elements Surface based Operations Boolean Operations Using Boolean Operations Using Fillets and Drafts Link management • Sketch • Publication • Material


|

V5 14

|

Issue: Draft A6

• • • • • •

Pattern Searching Elements Change the Sketch Support To stack Actions Hide Elements Behaviour of Show/Hide Hole positioning Variable Edge Fillet Using multi domain Sketch

• Basic Methods • General Modelling Rules

|


Page 102 of 312

Part Design Basics – The Specification Tree (1/3)


Structure of the Specification Tree The specification tree shows the hierarchy of the part defined by the operations during the design process. The structure of each operation created by the designer will be kept in the tree. Thus, at the beginning you start with a very small tree which will grow up during the design. At the end you might have a very long and complex tree, but nevertheless all your design steps are included in it. A new part starts with these objects: • the 3 main planes xy, yz and zx • the absolute axis system • the PartBody A good structure of the tree is profitable for: • a clean construction • updates with no problems • good overview of the part design Before starting the construction, take time to create a strategy. Investigate: • the aproach • the logical structure of the part • the expected result • the down stream processes and their interfaces. CATIA V5 Basic - Presentation

|

V5 14

|

Issue: Draft A6

|


Note: You may require more time to produce a good concept, you will gain this by spending less time during the design. Starting without a concept can lead in extreme cases in having to start again.

Page 103 of 312

Part Design Basics – The Specification Tree (2/3) Structure of the Specification Tree

Note: The elements will automatically get names which are built out of strings defined by the element type and a running number (e.g. Pad.1). By using only this automatic naming you can easily loose the overview and orientation in the tree. It is difficult to remember what e.g. Assemble.278 connects with Body.9. A good practice will be to rename the features to help you to navigate through the tree. You can rename by selecting the feature and using MB3 on that Feature> Properties > Feature Properties Short cut = ALT-ENTER.


Starting point for the solid generation is the PartBody.

Below the PartBody all the different elements (like features, sketches etc.) will be automatically implemented corresponding to their chronological creation.

To have a clean structure in complex parts, you should implement additional Bodies. CATIA V5 Basic - Presentation

|

V5 14

|

Issue: Draft A6

|


Page 104 of 312

Part Design Basics – The Specification Tree (3/3) Structure of the Specification Tree You can reorder the positions of the features in the tree afterwards. But remember, this can have an influence on the geometry of the part. Sometimes the result will totally change or some geometry won’ t be calculated. On the other hand, the reordering of the tree can sometimes help to get the desired result.


MB3 > ….Object > Reorder


|

V5 14

|

Issue: Draft A6

|


Page 105 of 312

Part Design Basics – PartBody, Body and Geometrical Sets (1/7) PartBody The PartBody has a special role in the specification tree. Its use and influence on the construction has to be known. The finished designed part has to be completed within the PartBody (at AIRBUS this is mandatory!). Only by this way, a clean connection to down stream processes (e.g. calculations or automatic bill of material) is guaranteed. Important:


• The PartBody cannot be deleted • Boolean operations which will use the PartBody (e.g. Remove-, Add- or Assemble-body) are not possible. The PartBody cannot be added to or subtracted from other bodies, but it is possible to add (subtract) other bodies to (from) it.


|

V5 14

|

Issue: Draft A6

|


Page 106 of 312

Part Design Basics – PartBody, Body and Geometrical Sets (2/7) PartBody


It is possible to move all or part of the content of the PartBody into a new body

The new body is automatically assembled to the PartBody It is also possible to let an existing body becomes the PartBody

MB3 The body becomes the PartBody


|

V5 14

|

Issue: Draft A6

|


Page 107 of 312

Part Design Basics – PartBody, Body and Geometrical Sets (3/7) Body Additional bodies can be inserted. They will help to generate a better structure of the tree in cases of complex parts. These bodies can be connected by Boolean operations. E.g. using separate bodies for the inner areas, outer areas, the raw casting and/or machining helps to divide the different operation steps and make a clearer structure.


Remember: The finished designed part has to be completed within the PartBody

Use the Insert > Body pull down menu for creating an additional Body.


|

V5 14

|

Issue: Draft A6

|


Page 108 of 312

Part Design Basics – PartBody, Body and Geometrical Sets (4/7) Geometrical Set


During the work in PartDesign, by creating reference elements (point, line or plane), a “Geometrical Set” will be automatically inserted in the tree as a store for the elements. By default, the wireframe and surface geometry is created in an Geometrical Set in parallel with the PartBody. There will be no chronological trace of the design if the tree remains as such.


|

V5 14

|

Issue: Draft A6

|


Page 109 of 312

Part Design Basics – PartBody, Body and Geometrical Sets (5/7) Ordered Geometrical Set

The ordered geometrical Set (OGS) contains wireframe and surface geometry like the normal geometrical Set. The OSG works like an Solid Body. The elements will created and ordered in a linear way and a chronological order.


Properties of an OSG:

• OSG is fully linear • The order of the appararation of features in the specification tree is consistent with the chronological creation

• Modification features will absorb there parents which are not longer accessible for users

• An OSG must created by the user • Every element in an OSG can be defined as in work object, all elements located behind the work object are not accessible.

• An OSG can be scanned by the “Scan” function CATIA V5 Basic - Presentation

|

V5 14

|

Issue: Draft A6

|


Page 110 of 312

Part Design Basics – PartBody, Body and Geometrical Sets (6/7) Geometrical Set To keep the overview in the tree, it is good to add one or several Geometrical Sets to the tree and name them with corresponding names. By that you can group the wireframe objects. Change into the Wireframe and Surface Design Workbench > Insert > Geometrical Set


The sequence of the various bodies in the specification tree must be ordered logically. To obtain a more logical tree, insert the Geometrical Set where the wireframe or surface geometry is needed. Insert > Geometrical Set…


|

V5 14

|

Issue: Draft A6

|


Page 111 of 312

Part Design Basics – PartBody, Body and Geometrical Sets (7/7) Geometrical Set

The function „Change Geometrical Set…“ allows you to move the Geometrical sets within the specification tree. They can also be moved directly under a given body.


MB3 > ….Object > Geometrical Set…


|

V5 14

|

Issue: Draft A6

|


Page 112 of 312

Part Design Basics – Features (1/3) Feature-based design


Features are entities that should be combined to make up a part. They include the generating of geometry, an operation or a combination of both. Some operations consist in adding material (e.g. rib), others in removing material (e.g. hole and pocket) There are several groups of Features: • Sketch-based Features • Dress-Up Features • Surface Based Features • Transformation Features


|

V5 14

|

Issue: Draft A6

|


Page 113 of 312

Part Design Basics – Features (2/3) Handling of Features Features can be duplicated, copied, translated, deleted, deactivated, or modified in the structure position.

• With the context menu of the right mouse button you can delete, deactivate, or translate the features.

• You can also use the buffer for the cut, copy, and translate functions to modify the © AIRBUS DEUTSCHLAND GmbH. Alle Rechte vorbehalten. Vertrauliches und geschütztes Dokument.

Features in the structure.

Note: It is not allowed to use the Drag&Drop functionality at Airbus.


|

V5 14

|

Issue: Draft A6

|


Page 114 of 312

Part Design Basics – Features (3/3) Parameters and References of Features


The parameter values and the references of a Feature can be modified at any time. • Double click on the Feature in the structure tree and the corresponding panel will appear. • The same is true for the sketches. A double click on it to open it, then constraints, dimensions or geometry can be modified, added, or deleted.

New references which lead to new dependencies will be created during, • the dimensioning, • the defining of geometrical constraints (like tangency, symmetry ..) • and the defining of Dress-Up-Features Deleting a used reference implies that the related dimensioning parameters, constraints, or features will also be deleted automatically. Attention: The deletion of a reference can happen during the design process. If e.g. an edge which had been used for a fillet doesn’t exist any more after a change during the design, the fillet will be deleted automatically. CATIA V5 Basic - Presentation

|

V5 14

|

Issue: Draft A6

|


Page 115 of 312

Part Design Toolbars and Icons Overview (1/4) Toolbar Sketch - Based Features Pocket


Pad

Groove

Shaft

Rib

Hole

Stiffener

Slot

Removed Loft

Loft

Pad

Pocket

Stiffener

Drafted Filleted Pad

Drafted Filleted Pocket

Solid Combine

Multi Pad

Multi Pocket


|

V5 14

|

Issue: Draft A6

|


Page 116 of 312

Part Design Toolbars and Icons Overview (2/4) Toolbar Dress – Up Features Champfer


Fillet

Shell

Thread/Tap

Thickness

Draft

Remove Face

Edge Fillet

Draft Angle

Remove Face

Variable Fillet

Draft Reflect Line

Replace Face

Face – Face Fillet

Variable Draft

Tritangent Fillet


|

V5 14

|

Issue: Draft A6

|


Page 117 of 312

Part Design Toolbars and Icons Overview (3/4) Toolbar Transformation Feature

Toolbar Surface Based Feature

Mirror

Scaling

Surface


Translation

Pattern

Split Translation

Rectanggular Pattern

Rotation

Circular Pattern

Symmetry

User Pattern

Thick Surface

Close Surface

Sew Surface


|

V5 14

|

Issue: Draft A6

|


Page 118 of 312

Part Design Toolbars and Icons Overview (4/4) Toolbar Boolean Operations Add

Remove Lump


Assemble

Union Trim

Add

Remove

Intersect


|

V5 14

|

Issue: Draft A6

|


Page 119 of 312

Part Design Sketch-Based Features (1/2) Create a pad means extrude a profile in one or two directions. You can choose the limits of creation as well as the direction of extrusion. Pad Create a pocket consists in extruding a profile and removing the material resulting from the extrusion. You can choose the limits of creation as well as the direction of the extrusion. Pocket


Create a shaft by revolve a open or closed profile in one or two directions. Shaft

Grooves are revolved features that remove material from existing features Groove

Create a hole consists in removing material from a body. Various shapes of standard holes can be created. Hole


|

V5 14

|

Issue: Draft A6

|


Page 120 of 312

Part Design


Sketch-Based Features (2/2)

Rib

Create a rib by using a centre curve, a planar profile and possibly reference element or a pulling direction. Ribs can also be created from sketches including several profiles. These profiles must be closed and must not intersect.

Slot

To define a slot, you need a centre curve, a planar profile, a reference element and possibly a pulling direction. Slots can also be created from sketches including several profiles. These profiles must be closed and must not intersect. To define a stiffener you need an open profile. Make sure that the material can limit the extrusion of this profile.

Stiffener Define a Solid with an intersection of two sketches in different planes

Solid Combine


|

V5 14

|

Issue: Draft A6

|


Page 121 of 312

Part Design Pad /Pocket A pad /pocket is a prismatic volume based on a sketch, planar curve or surface / face


Closed sketch or closed planar curve

Face or Surface

A pad / pocket can be limited by parameters or geometric elements

Dimension

Up to next

Up to last

Plane

Surface

Note: The limits for „Up to next“ / „Up to last“ must be in the same Body! CATIA V5 Basic - Presentation

|

V5 14

|

Issue: Draft A6

|


Page 122 of 312

Part Design Pad /Pocket The extrusion direction of a pad / pocket normally is normal to the sketch plane. You can define the direction by select a linear curve.


Reference for direction

With the Thick option a wall thickness on the sketch contour can be created.

Closed contour


|

Open contour

V5 14

|

Issue: Draft A6

|


Page 123 of 312

Part Design Pad /Pocket Special cases


If another solid feature in the body exists, an open contour can be trimmed on this geometry

Pad Open contour

Pocket Open contour

Open contour Options: Thick, Merge Ends Note: The limits for „Merge Ends“ must be found on both ends of the contour in the current body! CATIA V5 Basic - Presentation

|

V5 14

|

Issue: Draft A6

|


Page 124 of 312

Part Design Shaft / Groove A shaft / groove is a rotational volume based on a sketch, planar curve or surface / face The rotation axis can be: • A sketch axis (preferred solution) • A cylindrical face • A linear curve (line) The contour does not intersect the rotation axis:


9

8

Closed Contour

Open Contour


|

V5 14

|

Issue: Draft A6

|


Page 125 of 312

Part Design Shaft / Groove Rotation Angle


Rotation Axis Recognized by CATIA, if the sketch contains an axis

Shaft

Sketch for shaft CATIA V5 Basic - Presentation

|

V5 14

|

Issue: Draft A6

|


Page 126 of 312

Part Design Hole (1/5) The sketch of a hole must not defined in advance, the sketch will be created automatically an contain one point in standard mode. Select a face (or plane)

Extension


Hole dimensions Direction of the hole axis

Bottom shape


|

V5 14

Modify the position of the hole center by edit the positioning sketch

|

Issue: Draft A6

|


Page 127 of 312

Part Design Hole (2/5)


Hole Types

Simple

Tapered

Counterbored

Countersunk

Counterdrilled

For the countersunk hole type are three parameter combinations available: Depth & Angle Depth & Diameter Angle & Diameter CATIA V5 Basic - Presentation

|

V5 14

|

Issue: Draft A6

|


Page 128 of 312

Part Design Hole (3/5) Thread Activate Thread Select Thread standard


Select Thread size

Thread Analysis

Numeric Value Symbolic geometry Define Filters

Start Thread analysis with Apply CATIA V5 Basic - Presentation

|

V5 14

|

Issue: Draft A6

|


Page 129 of 312

Part Design Hole positioning (4/5) It is possible to constraint a hole during the creation


Available selections: • Circular edge + support = concentricity

• 1 edge + support = 1 dimension • 2 edge + support = 2 dimension • Point + support = coincidence to point CATIA V5 Basic - Presentation

|

V5 14

|

Issue: Draft A6

|


Page 130 of 312

Part Design Hole positioning (5/5) To control the hole direction on a non planar face you can use an line for steering the hole direction


• Line + support = hole direction and center point

The center point is the intersection between the face and the line


|

V5 14

|

Issue: Draft A6

|


Page 131 of 312

Part Design


Rib / Slot

Merge rib’s ends If there exist an other solid feature in the body, the rib/slot can be trimmed on this geometry

Note: The limits for „Merge rib’s ends“ must be found on both ends of the rib/slot in the current body! CATIA V5 Basic - Presentation

|

V5 14

|

Issue: Draft A6

|


Page 132 of 312

Part Design Rib / Slot


Profile Control Keep Angle

Pulling Direction

Reference Surface

The angle between the profile plane and center curve is constant

The angle between the profile plane and the reference element is constant

The angle between the profile and the normal to the surface is constant


|

V5 14

|

Issue: Draft A6

|


Page 133 of 312

Part Design Stiffener Mode: From Side Sketch the Side view of the Stiffener An open sketch is limited by intersect or extrapolation on the solid geometry of the current body. A limitation in all directions is necessary.

Direction of the wall thickness

NF

NF


Direction of search material for Intersect / extrapolate

Remark: The sketch plane define the Neutral Fiber


|

V5 14

|

Issue: Draft A6

|


Page 134 of 312

Part Design Stiffener Mode: From Top Sketch the Top view of the Stiffener An open sketch is limited by intersect or extrapolation on the solid geometry of the current body. A limitation in all directions is necessary.

Direction of the wall thickness

NF

NF


Direction of search material for Intersect / extrapolate

Remark: The sketch contours define the Neutral Fiber CATIA V5 Basic - Presentation

|

V5 14

|

Issue: Draft A6

|


Page 135 of 312

Part Design Combine Define a Solid with an intersection of two pads with extrusion directions in one step.


+

=

The profiles can be a sketch, a planar contour or a surface / face. (See pad feature for details) The extrusion direction of a pad / pocket normally is normal to the sketch plane. You can define the direction by select a linear curve. (See pad feature for details) CATIA V5 Basic - Presentation

|

V5 14

|

Issue: Draft A6

|


Page 136 of 312

Part Design Dress-Up Features A fillet is a curved face of constant or variable radius. It is tangent to two surfaces. These three surfaces form either an inside or an outside corner. You obtain a fillet by propagation along one or several edges. Edge Fillet Variable radius fillets are curved surfaces created to a variable radius. That means that at least two different constant radii are applied to two entire edges. Variable Radius Fillet


The fillet can be created between two faces without intersection or when there are more than two sharp edges between the faces. Face-Face Fillet You can create a fillet between three surfaces. One of the three surfaces is replaced by a fillet. This fillet is tangent to the three selected surfaces. Tritangent Fillet A chamfer consists in removing or adding a flat section from a selected edge to create a bevelled surface between the two original faces common to the edge. You obtain a chamfer by propagation along one or several edges. Chamfer


|

V5 14

|

Issue: Draft A6

|


Page 137 of 312

Part Design Fillets The fillet operation create a curved face with a constant radius. The fillet need an edge or a faces for support.

Limits Radius


Object to fillet

Support

Support

Support: Faces on which rolling a sphere. The fillet is tangent to the supports. Limits: Define the end of the supports Object to fillet: Edge: Edge which will be filleted Face: All non tangent boundaries of the face will be filleted Radius: Radius of the sphere CATIA V5 Basic - Presentation

|

V5 14

|

Issue: Draft A6

|


Page 138 of 312

Part Design Fillets Trim ribbons With the option „Trim ribbons“ overlapping fillets will be trimmed by CATIA.


Without Trim ribbons

With Trim ribbons


|

V5 14

|

Issue: Draft A6

|


Page 139 of 312

Part Design Fillets Edge(s) to Keep


With The Option „Edge(s) to Keep“ one or several Edges can be selected on which the sphere is rolling instead of one support face.

Edge(s) to keep: In this case the fillet is tangent to one Support face and goes through a curve (kept edge).

Examples

Edge to keep CATIA V5 Basic - Presentation

|

V5 14

|

Issue: Draft A6

|


Page 140 of 312

Part Design Fillets Blend Corner(s) With the option „Blend corner(s)“ the connection point of several edges in one fillet operation becomes smoother.

With Blend corner


Without Blend corner

1. Select the edges to be fillet

2. Select the „Blend corners“ button

3. The corners are recognized automatically by the system.


|

V5 14

|

4. Edit the „Setback distance“ global in the dialog box or individual by double click on the value in the 3D window. Issue: Draft A6

|


Page 141 of 312

Part Design Variable Fillet


The fillet operation create a curved face with a variable radius. The fillet need an edge or a faces for support.

A radius value can be defined on a vertex, a point, a plane ore somewhere on the edge(s) to fillet

Edit the list to Remove or replace the elements of the radius values


|

V5 14

|

Issue: Draft A6

|


Page 142 of 312

Part Design


Variable Fillet

Planes or Points can be used to define intermediary radius values (In the variable Edge Fillet creation window in the point field) By moving these planes, Catia will compute the intersections again and modify the fillet


|

V5 14

|

Issue: Draft A6

|


Page 143 of 312

Part Design Variable Fillet Variation


The kind of the run between the points can be defined with the variation option:

Cubic


|

V5 14

Linear

|

Issue: Draft A6

|


Page 144 of 312

Part Design Face-Face Fillet / Tritangent Fillet Face-Face Fillet


A Face-Face Fillet is normally used if two support faces have no common edge.

Tritangent Fillet A Tritangent Fillet connect two surfaces which are separated by a third surface. The third surface will be replaced by the fillet.


|

V5 14

|

Issue: Draft A6

|


Page 145 of 312

Part Design Dress-Up Features Drafts are defined on moulded to make them easier to remove from moulds. The characteristic elements are pulling direction, draft angle, parting element and neutral element Draft Angle Shelling a feature means emptying it, while keeping a given thickness on its sides. Shelling may also consist in adding thickness to the outside.


Shell The function Thickness add or remove materiel on the faces which are selected. Thickness The Thread capability removes material surrounding the hole. To define a thread, you can enter the values of your choice, but you can use standard values or personal values available in files too. Thread


|

V5 14

|

Issue: Draft A6

|


Page 146 of 312

Part Design Dress-Up Features

Simplify a part by removing some of its faces e.g. for finite element analysis Remove Face

Replace a face or a set of tangent faces with a surface


Replace Face


|

V5 14

|

Issue: Draft A6

|


Page 147 of 312

Part Design Draft Angle Create conical faces on a prismatic geometry


Neutral element

Draft angle

Pulling Direction

Faces to draft

Angle: Cones for mould in degree Faces to draft: Faces with cones. Selecting the faces or Select the neutral element first, the faces to draft will be selected automatically by CATIA (Option: Selection by neutral face) Neutral element: On the neutral element the dimension of the geometry will not be modified. Pulling direction: The direction for remove the moulds from the part.


|

V5 14

|

Issue: Draft A6

|


Page 148 of 312

Part Design Draft Angle Neutral and Parting Element

Neutral Pulling Direction


On the parting element the draft is limited along the pulling direction. The parting element can be equal to the neutral element. A plane, a surface or a join can be used for the parting element

Neutral

Parting

Neutral Parting

Neutral


|

V5 14

|

Issue: Draft A6

|


Page 149 of 312

Part Design Draft Angle Draft in two directions

Note:

Pulling Direction


For a draft in two directions the parting element must be equal to the neutral plane.

The neutral and parting element must not be a planar element.

Neutral Parting


|

V5 14

|

Issue: Draft A6

|


Page 150 of 312

Part Design Shell

Faces to remove and default Inside and outside thickness

Outside thickness

Inside and Outside thickness

Initial geometry

Initial geometry

Initial geometry


Inside thickness

Face with other thickness CATIA V5 Basic - Presentation

|

V5 14

|

Issue: Draft A6

|


Page 151 of 312

Part Design Transformation Features Create a translation of the current body. Select a line, edge or plane (to take its normal) as the translation direction. The original element is no longer visible but remains in the specification tree. No duplicate available. Translation

Rotation

Create a rotation of the current body around an axis. Select a line or edge as the rotation axis. The original element is no longer visible but remains in the specification tree. No duplicate available.


Create a symmetry operation of the current bodies. Select a point, line or plane as reference element. The original element is no longer visible but remains in the specification tree. No duplicate available. Symmetry

Mirror

Mirroring a body or a list of features consists in duplicating these elements using a symmetry. You can select a face or a plane to define the mirror reference. If you modify the original object, the mirrored one will also change .

Create a scale operation of the current body. Select a point or plane as reference element. The original element is no longer visible but remains in the specification tree. No duplicate available. Scaling


|

V5 14

|

Issue: Draft A6

|


Page 152 of 312

Part Design Translation / Rotation Note: Do not use the translation and rotation for position the parts in an assembly!

Translation Move the current body by a rotation

Direction (Linear curve) and distance Point to Point: Select the start and end point of the translation Coordinates: Define the translation between the origin and a point defined by x, y and z value


Rotation Move the current body by a rotation

Axis: Linear curve

Note: The original elements are no longer visible but remains in the specification tree. No duplication available. CATIA V5 Basic - Presentation

|

V5 14

|

Issue: Draft A6

|


Page 153 of 312

Part Design Symmetry Create a symmetry operation of the current body by selecting a point, line or plane as reference element. Plane


Line

Point

Note: The symmetry operation must be used for opposite handed parts CATIA V5 Basic - Presentation

|

V5 14

|

Issue: Draft A6

|


Page 154 of 312

Part Design Mirror Mirroring a body or a list of features consists in duplicating these elements using a symmetry. Current Solid

Select the operation Mirror and the mirroring plane


Feature List

Select the features by multi select, the Operation Mirror and the mirroring plane. Not all features can by mirrored by a feature list. The feature list cannot be edited. The mirror done by a feature list can be exploded into single features.


|

V5 14

|

Issue: Draft A6

|


Page 155 of 312

Part Design Transformation Features

Duplicate geometry of one or more features at the location of a rectangular pattern. Rectangular Pattern Duplicate geometry of one or more features right away at the location of a circular pattern.


Circular Pattern Duplicate geometry of one or more features right away at the location of a pattern defined by user. User Pattern

Note: In the assembly workbench it is possible to reuse pattern for positioning. To benefit from this possibility, use pattern as standard practice.


|

V5 14

|

Issue: Draft A6

|


Page 156 of 312

Part Design Rectangular Pattern Length

Spacing


Object to pattern

Reference directions Instances: Number of Copies including the object to pattern Spacing: Distance between to Copies Length: Distance between the first and last copy With the Option „Keep Specifications“ the limitation options e.g. „Up to Last“ of the initial element is used for all pattern instances .


|

V5 14

|

Issue: Draft A6

|


Page 157 of 312

Part Design Circular Pattern Angular Spacing


Reference Element

Circle Spacing

Object to pattern

Instances: Number of Copies including the object to pattern Angular spacing: Angle between two Copies Total Angle: Angle between the first and last copy Circles: Number of Circles Circle Spacing: Distance between two Circles Crown Thickness: Distance between the inner and outer circle Reference Element: Rotation Axis CATIA V5 Basic - Presentation

|

V5 14

|

Issue: Draft A6

|


Page 158 of 312

Part Design Circular Pattern


It is possible to use a cylindrical face as a reference element of a circular Pattern

Select cylindrical face as a reference element

pattern origin

Activate Radial alignment CATIA V5 Basic - Presentation

|

V5 14

|

Issue: Draft A6

|


Deactivate Radial alignment Page 159 of 312

Part Design Circular Pattern


With the option “Instance(s) &unequal angular spacing” an individual angel between all instances can be defined.

Edit each angel by double click


|

V5 14

|

Issue: Draft A6

|


Page 160 of 312

Part Design User Pattern In case of „User Defined Pattern“, only points which are defined in one sketch can be selected. Single 3D Points can’t be used, even if they are all on the same plane.

Object to pattern (Hole) Anchor: The Centre of the object to pattern is positioned of the sketch points. If you need an other point of the initial geometry you must define an anchor.


Anchor

|

V5 14

|

Issue: Draft A6

With Anchor

Without Anchor

Initial Situation


Each Point in standard mode in the sketch define the position of a pattern instance.

|


Page 161 of 312

Part Design Pattern – Hints and Tips • Deleting an instance of the pattern, the whole pattern will be deleted • Suppress an Instance of the pattern by clicking the small orange dot • If no feature is selected, the current Solid will be pattered. Pattern based on a feature list It is possible to pattern a list of Part Design features. These features must belong to the same body. The body must be set as “Define in Work Object”.


You can only get a feature list while the creation of the pattern. You have to multi-select at least two objects before you click the Pattern Icon. Note that adding a feature to a pattern is only possible if your pattern is already based on a feature list. It is not possible to add any feature to a basic pattern created using a single feature.


|

V5 14

|

Issue: Draft A6

|


Page 162 of 312

Part Design Reference Elements Define a point by coordinates, on a curve, on a plane, on a surface, at a circle centre, tangent point on a curve, and between two elements. Point


Create lines by following methods: point to point, point and direction, angle/normal to curve, tangent to curve, normal to surface, and bisecting. Line

Plane

Create planes by various methods: Offset from a plane, parallel through point, at an angle to a plane, through three points, through two lines, through a point and a line, through a planar curve, normal to a curve, tangent to a surface, from its equation, mean through points.


|

V5 14

|

Issue: Draft A6

|


Page 163 of 312

Part Design Surface Based Operations

Split a body with a plane or surface.

Split Add material to a surface in two opposite directions by using the thick surface capability.


Thick Surface Define a body by closing a surface. The sites to be close must be planar. Close Surface Add or remove material by computing the intersection between a given surface and a body. The surface must completely intersect the body. Sew Surface


|

V5 14

|

Issue: Draft A6

|


Page 164 of 312

Part Design Split Split the current body on a plane or surface. Split on a surface


The surfcae must intersect the whole solid

The arrow indicate the side to keep. Select the arrow to invert. Split on a plane


|

V5 14

|

Issue: Draft A6

|


Page 165 of 312

Part Design Thick surface

Negative Second Offset

Positive Second Offset


The arrows indicate the direction of the first offset. Click on an arrow or the “Reverse Direction” button to invert the direction.

Is the Offset value greater then the smallest concave curvature radius of the surface, this face cannot be on the borders of the surface


|

V5 14

|

Issue: Draft A6

|


Page 166 of 312

Part Design Sew Surface The Sew Surface operation integrate a surface in the current body an combine them.


Remove material

Add material

Without the option „Intersect body“ the surface boundaray have to lay down complitly on the triming body

With the option „Intersect body“ the sew Operation is combined with a split operation.


|

V5 14

|

Issue: Draft A6

|


Page 167 of 312

Part Design Boolean Operations Assemble a body to another body. The second body will be attached to the first one. Assemble Add a body to another body. Adding a body to another one means uniting them.


Add

Remove a body from another body. Removing a body from another one means subtracting them. Remove The material resulting from an intersection operation between two bodies is the material shared by these bodies. Intersect Assemble two bodies by defining the elements to be kept or removed while performing the union operation. Union and Trim


|

V5 14

|

Issue: Draft A6

|


Page 168 of 312

Part Design Using Boolean Operations (1/4) Using Boolean Operations


Add A fusion of a body to the existing geometry which doesn’t define a NC-operation like pocket or drilling hole. Most common operation, also often used to make a better structure in the tree. Don’t use it for pockets and holes. Remove Removes a body from the existing geometry. Only use it for non NC-operations. Note: If the Remove is the highest part in the sub-tree, it automatically changes to an Add and leads to undesired results!


|

V5 14

|

Issue: Draft A6

|


Page 169 of 312

Part Design Using Boolean Operations (2/4) Using Boolean Operations

Assemble Assemble of positive or negative bodies for operations. Before the Assemble the raw part has a positive volume.


Holes and NC pockets in parts should not be created by Boolean volumes in the raw part, since these cannot be recognized later as NC relevant operations. It is also wrong to create the holes as normal pads, you get geometrically the same result, but the logical structure would be incorrect, since it should be a hole and not a dummy subtraction body. Assemble means:

• Remove material, if the body consists of pocket volumes. • Add material, if the body consists of pads. Note: NC pockets should be created using the Pocket feature. CATIA V5 Basic - Presentation

|

V5 14

|

Issue: Draft A6

|


Page 170 of 312

Part Design Using Boolean Operations (3/4) • Structure Parts with different bodies Bodies Tree


Feature Tree

• Used for simple parts up to ~20 features • Only one body (PartBody) is used • The first feature must be positive, up from the second feature positive and negative features can be used CATIA V5 Basic - Presentation

|

V5 14

|

Issue: Draft A6

|


• Used for complex parts with more then ~20 • •

features The geometry is divided into several geometrical areas The bodies must be connected by Boolean operations Page 171 of 312

Part Design


Using Boolean Operations (4/4)


|

V5 14

|

Issue: Draft A6

|


Page 172 of 312

Part Design Using Fillets and Drafts Fillet and Draft Rules Draft before Fillet Fillets should always be added to a part after drafts, since the value of the fillet will be changed and a kind of “variable fillet” with different radii will show up. (Exception: draft on reflect line.) Large Fillets before small Fillets If the rule is not take into account, it can lead to incorrect geometry and even in special cases to error messages, since the geometrical creation is impossible.


Vertical Fillets before horizontal Fillets Order of the Fillets in the Specification Tree To get a higher update performance and improve modification possibilities, the Dress- up features (fillet, chamfer, draft and shell) should be used in a special order. E.g. fillet should be one of the last features. On the other hand, by waiting with the fillets to the total end of the design, the creation of the fillets might be more complex or even impossible. So, use the fillet function quite early, but take the later design into account. Only group together edges which mandatory will have the same radius value (See AM2259)


|

V5 14

|

Issue: Draft A6

|


Page 173 of 312

Part Design Link management – Sketch (1/5) Using Sketch from Geometrical Sets (1/2) … and create through it a Pad (Pad.1) in a new Body (Body.2) …


Create a sketch in a Geometrical Set (Sketch.1) …

…the sketch appears twice in the structure tree, under the Geometrical Set body and under the pad. For modification just click on one of them. Note: If the sketch is deleted in the Geometrical Set, the pad will also be deleted.

Note: To avoid this “duplication” of the sketch, create it directly in the body which will contain the element bearing on the sketch, or cut and paste into that body. CATIA V5 Basic - Presentation

|

V5 14

|

Issue: Draft A6

|


Page 174 of 312

Part Design Link management – Sketch (2/5) Using Sketch from Geometrical Set (2/2)


In this case Sketch.1 from Geometrical Set.1 is used to create Pad.1 and Pad.2. Changing the Sketch.1, will modify both Pads.


In order to independently modify the Sketch of Pad.2, create a new sketch first. Use “copy and paste” to create a copy of the original sketch.

|

V5 14

|

Issue: Draft A6

|

Then edit the pad definition of Pad.2. Double-click on Pad.2 or use MB3 on Pad.2 > Pad.2 object > Definition.


Under Profile > Selection, replace the Sketch.1 by Sketch 2 (Copy of Sketch.1).

Page 175 of 312

Part Design Link management – Sketch (3/5) Copy and paste a sketch from Geometrical Set

Create a sketch in a Geometrical Set (Sketch.1) …


… and copy this one by “copy and paste” in a Body (Body.2), ...


|

V5 14

|

Issue: Draft A6

|


… there won’ t be any link created between the sketches . The new sketch is independent (Sketch.2)

Page 176 of 312

Part Design Link management – Sketch (4/5) Copy and Paste a Body

… The result will be a new Body (Body.3) and an independent sketch (Sketch.4).


Create a sketch (Sketch.3) in a body (Body.2) …

… copy and Paste this body in the Part (Part1), …


|

V5 14

|

Issue: Draft A6

|


Page 177 of 312

Part Design Link management – Sketch (5/5) Copy and paste special a sketch from Geometrical Set or Body


Create a sketch in a Geometrical Set or a Body (Sketch.1) …

… and then copy it with “copy and paste special” > AsResultWithLink into another body (Body.2), …

Caution: … the new sketch (Sketch.2) has a link to the original sketch and it can’t be modified.

The link can be deleted afterwards by MB3 on the new sketch > Sketch.2 object > Isolate. By this operation the Icon of the sketch in the SpecificationTree will change. CATIA V5 Basic - Presentation

|

V5 14

|

Issue: Draft A6

|


Page 178 of 312

Part Design Link management – Publication (1/2) Published Geometry Publication is the process of naming elements (geometric features or parameters) with specific tags. Published elements can be used in one CATPart or for maintaining multi-model links. Published geometry is similar to that of linked geometry but published elements have a greater level of associativity.


The Publication command is available in the workbenches Assembly Design, Part Design and Generative Shape Design and lets you: • • • •

publish one or several geometric element/s edit the default name given to the published element replace the geometric element associated with a name delete a published element.

Note: To create Symmetrical Parts or Assembly-Cut Parts it is necessary to publish the PartBody


|

V5 14

|

Issue: Draft A6

|


Page 179 of 312

Part Design Link management – Publication (2/2) Published Geometry Tools > Publication


Select the element to be published (e.g. plane.2)

Select the Name (plane.2) twice and Rename it (e.g. Main Plain)


The plane is published under a new name, but the geometric element Part1/Geometrical Set.1/Plane.2 has not been renamed.

|

V5 14

|

Issue: Draft A6

|


Page 180 of 312

Part Design Material Apply Material

Select a material on the list

Set the properties


Apply Material

Show Material Applies customized view parameters

The window can also be opened with View > Render Style > Customize View


|

V5 14

|

Issue: Draft A6

|


Page 181 of 312

Part Design Hints and Tips – Searching Elements To find the graphic representation of an element, select this element in the tree and then MB3 > Reframe on. The element will be centred inside the document window. It is also possible to search for constraints.


Reframe on

To find out where a visible graphic element is located in the specification tree, select the element and then MB3 > Center Graph. The element will be highlighted in the tree.

Center Graph


|

V5 14

|

Issue: Draft A6

|


Page 182 of 312

Part Design Hints and Tips – Working with the specification tree Show / Noshow the Specification tree With the F3 key the Specification tree can be noshow an show

Collaps and Expand the Specification tree The specification tree ca be collapsed and expanded by View >Tree Expansion . In the menu Expand Selection you can choose the expansion level


Move and zoom the Specification tree After clicking on a branch (white line) in the specification tree you can zoom and pan the tree instead of the geometry. To pan, zoom and rotate the geometry, you have to click on the branch again or on the axis system in the bottom right corner of the window.

Opening Sub-Trees For a better visualization of the tree, a part of it can be opened in a separate window. Select the item, click with MB3 and choose the contextual command Open Sub-Tree.


|

V5 14

|

Issue: Draft A6

|


Page 183 of 312

Part Design Hints and Tips – Change the Sketch Support To define a new support for a sketch, use the contextual menu. Select the sketch and then MB3 > Sketch.x object > Change Sketch Support and then the new sketch plane.

Select the new sketch plane and define the origin and the orientation of the sketch


MB3

Select the sketch

Sketch.x object > Change Sketch Support CATIA V5 Basic - Presentation

|

V5 14

|

Issue: Draft A6

|


Page 184 of 312

Part Design Hints and Tips – To stack Actions If an additional geometry is needed to create an element (e.g. a reference to create a line), it is not necessary to close the definition panel. By using the contextual menu (MB3) in the field where the geometry is needed, it’s possible to create it (e.g. a boundary) directly.


MB3

MB3


|

V5 14

|

Issue: Draft A6

|


Page 185 of 312

Part Design Hints and Tips – Hide Elements Design geometry (e.g. sketches and planes) must be in the non visible area (hide) before finishing a part.


An easy way to hide all elements of one type is to use Tools > Hide in the pull down menu.


|

V5 14

|

Issue: Draft A6

|


Page 186 of 312

Part Design Hints and Tips – Behavior of Show/Hide

Show/Hide


There is a hierarchical display status in Catia V5. By hiding a PartBody, all elements below (e.g. Sketches, Geometrical sets) will be hidden too. Note. The status Show/hide of these elements can be changed, but they won’t be displayed as long as the PartBody is hidden.


|

V5 14

|

Issue: Draft A6

|


Page 187 of 312

Part Design Hints and Tips – Using multi domain Sketch (1/2) Using Multi domain Sketch to create e.g. Pockets


If a sketch that contains e.g. 4 contours is used for the pocket definition, the result will be 4 pockets with the same height. To manage modifications correctly, initially create 4 pockets bearing on 4 contours. The 4 contours can be either in 4 different sketches or in the same sketch. For dimensioning contours, it can be suitable to group them in the same sketch.


|

V5 14

|

Issue: Draft A6

|


Page 188 of 312

Part Design Hints and Tips – Using multi domain Sketch (2/2) Using Multi domain Sketch to create e.g. Pockets However it is possible to access a single contour inside the sketch while creating pockets. By selecting the profile in the pocket definition panel, use the contextual menu (MB3) to get the Go to profile definition panel. This panel allows a selection of a single contour inside the sketch.


Remove first


|

V5 14

|

Issue: Draft A6

|


Page 189 of 312

Part Design Hints and Tips – Delete unnecessary elements In a CATIA V5 Model unnecessary elements (Reference, Wireframe and Surface elements without children) should be deleted when the design process is finished.


Delete Unnecessary elements is in the Workspaces Part Design and Generative Shape Design (GSD) available:

Keep, Solid: Solids are always be kept Keep, used by Solid: Non solids will be kept, when there are parents of a solids Delete: Non solids will be deleted, if there are not necessary for the Solid design.

The delete Status can be changed by the Context menu:


|

V5 14

|

Issue: Draft A6

|


Page 190 of 312

Part Design Basic Methods – General Modelling Rules (1/2) Starting the Design Process


Elementary part axis system used to design the part • If no more information are given to the designer by ACMT, CDBT, … the default method is Local (Axis inside or near the solid). The positioning will be done within the assembly (See AM5012).


|

V5 14

|

Issue: Draft A6

|


Page 191 of 312

Part Design Basic Methods – General Modelling Rules (2/2) Finishing the Design Process • Delete all unnecessary elements • Do not use red colours for solids • Every Sketch has to be fully defined by parameters (only if possible) • Rename the Part Body with the Partnumber and publish them.


• Publish reference elements To be able to use the elements in a context, publish the geometry that will be used as reference for the modelling of other parts

• Activate the button "fit all in“ before saving • Update the part before saving • Design geometry must be in NOSHOW (e.g.: Sketches, Planes) • Every part must have only one body (PartBody) (rule: one part one model) To allow use of detail part file in CAM, model one part per CATPart file

• The PartBody has to be set as “Define in Work Object“ • Use QCHECKER V5 tools for CATPart CATIA V5 Basic - Presentation

|

V5 14

|

Issue: Draft A6

|


Page 192 of 312

Generative Shape Design Introduction


• • • • •

Philosophy and Meaning of Surfaces and Wireframe Toolbars and Icons Overview Toolbar Wireframe Toolbar Surfaces Toolbar Operations


|

V5 14

|

Issue: Draft A6

|


Page 193 of 312

Generative Shape Design Introduction Philosophy and Meaning of Surfaces and Wireframe The Wireframe and Surface product allows the creation of wireframe construction elements during the preliminary design and enriches the existing 3D mechanical part design with wireframe and basic surface features.


The Generative Shape Design workbench allows you to quickly model both simple and complex shapes using wireframe and surface features. It provides a large set of tools for creating and editing shape designs.

When combined with other products such as Part Design, both Wireframe and Surface Design and Generative Shape Design meets the requirements of solid-based hybrid modeling.


|

V5 14

|

Issue: Draft A6

|


Page 194 of 312

Generative Shape Design Introduction Toolbars and Icons Overview (1/3) Toolbar Wireframe

Line

Point

Projektion

Intersection

Plane

Point Points and Planes Repetition © AIRBUS DEUTSCHLAND GmbH. Alle Rechte vorbehalten. Vertrauliches und geschütztes Dokument.

Parallel Curve

Spline

Circle

Projection

Circle

Combine

Corner

Reflect Line

Connect Curve

Extremum ExtremumPolar

Conic Line

Parallel Curve

Spline

Axis

3D Curve Offset

Helix Spiral

Polyline

Spine CATIA V5 Basic - Presentation

|

V5 14

|

Issue: Draft A6

|


Page 195 of 312

Generative Shape Design Introduction Toolbars and Icons Overview (2/3) Toolbar Surfaces


Extrude

Offset

Sweep

Fill

Loft

Blend

Extrude

Offset

Sweep

Revolve

Variable Offset

Adaptive Sweep

Sphere

Line

Rough Offset

Conic

Cylinder Explicit CATIA V5 Basic - Presentation

|

V5 14

|

Issue: Draft A6

|


Circle Page 196 of 312

Generative Shape Design Introduction Toolbars and Icons Overview (3/3) Toolbar Operations

Translate

Join

Split

Boundary

Shape Fillet

Extrapolate

Rotate

Symmetry Translate


Join

Scaling

Shape Fillet

Split Boundary

Affinity

Edge Fillet

Healing

Axis To Axis Trim Extract

Variable Radius Fillet

Curve Smooth Face-Face Fillet Multiple Edge Extract

Untrim

Tritangent Fillet

Disassemble


|

V5 14

|

Issue: Draft A6

|


Page 197 of 312

Generative Shape Design Introduction Toolbar Wireframe

Create a curve resulting from the intersection of the extrusion of two planar curves. The extrusions may be normal to the curves or along a direction Combine Create a geometry by projecting one or more elements onto a support. The projection may be normal to the support element or along a direction


Projection Create a wireframe geometry by intersecting wireframe elements, surfaces or solids Intersection Create a curve parallel to a reference curve

Parallel Curve


|

V5 14

|

Issue: Draft A6

|


Page 198 of 312

Generative Shape Design Introduction Toolbar Surfaces Create a surface by extruding a profile along a given direction Extrude Create a surface by rotating a planar profile around an axis Revolve Create a a full or a partly spherical surface


Sphere

Create a cylindrical Surface Cylinder Create one or several surface by offsetting an existing surface or a set of surfaces Offset Create fill surfaces between a number of boundary segments Fill CATIA V5 Basic - Presentation

|

V5 14

|

Issue: Draft A6

|


Page 199 of 312

Generative Shape Design Introduction Toolbar Operations Join at least two adjacent surfaces or two adjacent curves. Join Split a surface, a wireframe element or a solid with a cutting element. Note: If you split a solid, the result will be a split-surface. Split Trim two surfaces or wireframe geometry. Both elements will be modified. © AIRBUS DEUTSCHLAND GmbH. Alle Rechte vorbehalten. Vertrauliches und geschütztes Dokument.

Trim Performing an extract from elements (e.g. curves, points, solids) Extract

Create boundary curves of one or several surfaces Boundary

Extrapolate a curve or a surface boundary Extrapolation CATIA V5 Basic - Presentation

|

V5 14

|

Issue: Draft A6

|


Page 200 of 312

Generative Shape Design Introduction Hints and Tips - Managing Multi-Result Operations (1/2) If the result of an operation is not a single element, you can choose, which part of the result should be used .


Example: Intersection between a Circle and a plane. The Operation contain to points which can normally not used for the next operation (e.g. line from Point to Point)

The Multi-Result Dialog box appears


|

V5 14

|

Issue: Draft A6

|


Page 201 of 312

Generative Shape Design Introduction Hints and Tips - Managing Multi-Result Operations (2/2) Using the „Near“-Function to keep only one Sub-element

Only this element which is nearest to the reference element will be kept.


The Near- Function can also used by the menu Insert

Using the „Extract“-Function to keep only one Sub-element


|

V5 14

|

Issue: Draft A6

|


Page 202 of 312

Q-Checker


• General • Quality Control of Catia V5 Data • Quality Control of Catia V5 Data in a Batch Process


|

V5 14

|

Issue: Draft A6

|


Page 203 of 312

Q-Checker General


The Q-Checker controls the data quality of CATProducts, CATParts and CATDrawings. It checks the compliance with Airbus standards, the structure and the geometry, and provides automatic correction functionalities. The results of the analysis will be displayed in an interactive panel. Good data quality avoids a lot of workload in following process steps (DEX, CNC). To assure, that errors are detected early so that only a small workload for model correction will be needed: • Use the Q-Checker from an early stage • Repeat the check regularly, at least daily before storing. It is advised to check the data only with the AIRBUS administrator profiles Note: Only the check performed with the administrator profiles will automatically be taken into account before • storing in the vault • data exchange • release process CATIA V5 Basic - Presentation

|

V5 14

|

Issue: Draft A6

|


Page 204 of 312

Q-Checker Quality Control of Catia V5 Data (1/4)


Accessing Q-Checker from Catia V5

Available profiles for Long Range: AIRBUS_LONGRANGE (default) AIRBUS_LONGRANGE_FLX (for FLX and CUT parts)

Q-Checker start without healing

Select a check profile Note: As the Catia model is considered to be under the responsibility of its author, the automatic function will not be used

Prepare batch run

Start Q-Checker

In this mode it is possible to analyse numerous models at the same time


|

V5 14

|

Issue: Draft A6

|


Page 205 of 312

Q-Checker Quality Control of Catia V5 Data (2/4)


The active Catia model is checked automatically

Representation And Description

Healing and close Analysis Window

Error Categories Error

Prevents the execution of certain steps. Not possible to check in into Primes.

Model is rejected in release and data exchange process. Correction is mandatory

Blue

Warning

Results normally in disadvantages, but cannot be avoided in certain situations

Correction by user is recommended but not mandatory

Green

Error-free

The element is ok

Red


|

V5 14

|

Issue: Draft A6

|


Page 206 of 312

Q-Checker Quality Control of Catia V5 Data (3/4) Representation and Description Zoom automatically


Graphic Fine Analysis

Criterion Help


|

V5 14

|

The incorrect element is shown centred and enlarged

Getting of additional graphic information for some violated criteria.

This help includes illustrating pictures, the problem description, a suggested solution, and an application tip.

Issue: Draft A6

|


Page 207 of 312

Q-Checker Quality Control of Catia V5 Data (4/4) Healing and close Analysis Window


Heal

Automatic healing of errors according to the settings in the profile.

Close panel and restore

The analysis panel will be closed and the original Catia settings will be restored

Close panel and keep current

The analysis panel will be closed and the current Catia settings (the modifications done during the healing) will be used


|

V5 14

Note: The automatic healing is not to be used for transfer to first permitted layer

|

Issue: Draft A6

|


If the automatic healing isn’t available in the analysis panel, the correction must be done by using the Catia function.

Note: To do the modifications, you have to exit the Q-Checker Page 208 of 312

Q-Checker Quality Control of Catia V5 Data in a Batch Process (1/2) Q-Checker provides the ability to check more than one model in a batch process.

1

4


1

2 3

2


3

|

V5 14

|

Issue: Draft A6

|


4

Pre-selection of CATIA models (Filetree, CATIA Declaration Files, Current Session) Selection of directory Selection of models – only the marked model will be checked Possibilities to filter the models for a better selection

Page 209 of 312

Q-Checker Quality Control of Catia V5 Data in a Batch Process (2/2)

1

2

1

3 4

2


3 4

Declaration of the control (*.in) file Path and name of the output file Selection of check profile Declaration of the name of the report files

After the performing of the batch mode check, the output file will be generated in the specified directory. The output file contains information about the check run and the model assessments.


|

V5 14

|

Issue: Draft A6

|


Page 210 of 312


Assembly Design • • • • • • • • • • •

Structure and Components Document Modes Toolbars and Icons Overview Product Structure Tools Moving Tools Assembly Constraints Tools Creating Assembly Constraints Save Management Linkmanagement Standard Parts Hints and Tips Hide Elements / Search • Positioning of Components •


|

V5 14

|

Issue: Draft A6

|


Page 211 of 312

Assembly Design Structure and Components The CATProduct structure is a hierarchical tree composed of items (or nodes). A CAD model (wireframe, solid, etc.) can be assigned to each item. This model can be positioned in space within the Assembly Design Workbench. A positioning matrix may be assigned to the link between the component and the higher sub-assembly. Repetitive parts are instantiated several times and are therefore assigned several positioning matrices. Structures are represented in a CATIA V5 specification tree composed of nodes, and managed by a "parent/child" link system. Component (Components are internal sub-assemblies within a product structure and are not saved as external CATProduct files)


Root Node (CATProduct) M1

Referenced Assembly (CATProduct)

M2

Link between items M3 M4

Sub-Assembly (CATProduct)

M5 M6

CATPart

M7 M8

Part instantiated twice


|

V5 14

|

Issue: Draft A6

|


Page 212 of 312

Assembly Design Document Modes Document Modes


There are two different document modes available when a product is opened •

Visualisation Mode Visualisation mode opens a significantly lighter model than its true geometrical form, and can increase the performance. The visualisation mode uses a geometrical format .cgr (Catia Graphical Representation) that represents only the external appearance of the component. No Specification Tree available.

•

Design Mode Design mode is the original editable format, making all geometrical data available. Exact geometry is loaded. If the Option “Work with the Cache System” is activated (default at AIRBUS) all parts are loaded in Visualisation mode. When modification is required on a part it can be converted from visualisation to design mode by: • MB3 over the part icon > Representations > Design Mode or • double-click MB1 on the part icon CATIA V5 Basic - Presentation

|

V5 14

|

Issue: Draft A6

|


Page 213 of 312

Assembly Design Toolbars and Icons Overview (1/2) Toolbar Product Structure Tools


New Component

New Product

New Part

Replace Component

Existing Component

Toolbar Move Generate Numbering

Graph Tree Reordering

Manage Representations

Selective Load

Multi Instantiation

Snap

Manipulation

Stop manipulate on clash

Explode

Snap

Fast Multi Instantiation

Smart Move

Define Multi Instantiation


|

V5 14

|

Issue: Draft A6

|


Page 214 of 312

Assembly Design Toolbars and Icons Overview (2/2) Toolbar Constraints

Contact

Toolbar Assembly

Not allowed at AIRBUS Flexible/ Rigid Sub – Assembly

Fix Together

Angle

Create symmetry Reuse Pattern


Assembly Features Coincidence

Offset

Fix

Quick Constraint

Change Constraint

Split Hole

Caution: Do not use the Flexible / Rigid Sub Assembly command in the Assembly Design workbench as this causes problems when assembly trees created with CATIA V5 are converted to Product structure format (See AM5012) CATIA V5 Basic - Presentation

|

V5 14

|

Issue: Draft A6

|


Pocket

Not allowed at AIRBUS

Add Remove

Page 215 of 312

Assembly Design Product Structure Tools (1/2) Insert a component into an existing assembly. Components are internal sub-products within a product structure and are not saved as external .CATProduct files New Component

Insert a product into an existing assembly. New Product


Insert a part into an existing assembly. New Part Insert an existing component (e.g. part or assembly) into an existing assembly. Multiple Components can be selected using the Control and Shift Keys Existing Component Components, Products and Parts can be reordered inside the main Product and Sub-Products. To reorder the tree: select the reorder icon and then the product to be changed Graph Tree Reordering


|

V5 14

|

Issue: Draft A6

|


Page 216 of 312

Assembly Design Product Structures Tools (2/2) Number the components of an assembly. You can find these instance numbers in the properties panel of the components. Generate Numbering

Selective Load

Load partially some components in an assembly. Can be applied only when the option Load referenced documents, in Tools > Options > General is deactivated


Managing context-specific representation of Parts (e.g. shape or .cgr) in the assembly structure. Manage Representations Quickly repeat the insert of a component Fast Multi Instantiation Quickly repeat the insert of a component as many times as you wish in the direction of your choice Define Multi Instantiation


|

V5 14

|

Issue: Draft A6

|


Page 217 of 312

Assembly Design Moving Tools Move a component freehand (translate or rotate) with the mouse by using the Manipulation Parameters dialog box. The move can be done with respect to existing constraints. Manipulation


Snap

Project the geometric element of a component onto another geometric element . The element selected first is always the element that will move. No constraints will be created. It is necessary to work in the Design mode. Combines the constraint creation and snap capabilities. The smart move panel contains a list of the constraints that can be set. This list displays these constraints in a hierarchical order.

Smart Move Exploding an assembly takes into account the assembly constraints. This Explode type is applicable when coincidence, constraints axis/axis or plane/plane are assigned to the assembly Explode

Compass

Manipulate the assembly by checking if the components react in the expected way, i.e. according to the constraints. Select the red square at the centre of the compass and drag it onto a component to snap it to this component. Press and hold down the Shift key while moving.


|

V5 14

|

Issue: Draft A6

|


Page 218 of 312

Assembly Design Assembly Constraints Tools (1/2)

Coincidence Constraint


Contact Constraint

Is used to align elements. You may obtain concentricity, coaxiality or coplanarity, depending on the selected elements. Points, Lines, Planes, Planar Faces, Cylinder’s Axis, Sphere’s Point are elements which can be selected. Their orientation can be defined by choosing 3 options: Same, Opposite, Undefined (with it, the Application will find the best solution) Create a contact between two planar Faces. The contact area between the Faces could be a point, a line or a plane. Planar Faces, Sphere, Cylinder, Cone and Circle are elements which can be selected. The contact’s Orientation can be external or internal

Set an Offset constraint between two components. Points, Lines, Planes, Planar Faces can be selected. The Faces orientation should be specified when defining an Offset Constraint. Offset Constraint Set an angle Value as constraint between elements of 2 different components. Lines, Planes, Planar Faces can be selected as Elements. Angle Constraint


|

V5 14

|

Issue: Draft A6

|


Page 219 of 312

Assembly Design Assembly Constraints Tools (2/2) Does not allow a component to move from its Position during the update operation. There are two ways of fixing a component: According to the Assembly geometrical origin (absolute position) and according to the other components (relative position). Fix Component


Flexible/Rigide Sub-Assembly

Instead of moving a whole Sub-Assembly, this Function gives the opportunity to move only one component of a sub-Assembly within the main Assembly. Before the moving, the Sub-Assembly must be defined as Flexible.

Not allowed at AIRBUS

Repeat automatically a Component in an assembly by using a Pattern created in Part Design. There are two work modes: - Using associativity with the geometry: the option "Keep link with the pattern" is on Reuse Pattern - Using no associativity: the option is off


|

V5 14

|

Issue: Draft A6

|


Page 220 of 312

Assembly Design Creating Assembly Constraints Creating Assembly Constraints Note: The active component is blue framed (default colour) and underlined. It is activated by double-clicking. Product A

Sub-Product B Sub-Product C Part instance 1.1


Part instance 2.1

You cannot apply a constraint between two components belonging to the same subassembly if this subassembly is not the active component

Part instance 3.1 Part instance 4.1

You can apply constraints only between the child components of the active component

Sub-Product D

Part instance 5.1

Part instance 6.1

You cannot define constraints between two geometric elements belonging to the same component

Constraints


|

V5 14

|

Issue: Draft A6

|


Page 221 of 312

Assembly Design Save Management


The Save Management command lets you save all or several of your new or modified documents (CATParts and CATProducts). In the Save Management panel the state (e.g. opened, modified, new) is displayed.


|

V5 14

|

Issue: Draft A6

|


Page 222 of 312

Assembly Design Link management See AM2252 CATIA V5 Multi Model Links


The option “Keep link with selected object” is deactivated by default


|

V5 14

|

Issue: Draft A6

|


Page 223 of 312

Assembly Design Standard Parts (1/2) Using a Standard Part contained in a Standard Part Catalog

See AM5012 CATIA V5 Assembly Rules

Standard parts are elements defined by a standard document. They are delivered in a CATIA V5 catalog named “AIRBUS CATALOG”. 1.

Access the Catalog Browser


Select the Catalog Browser Icon or Tools > Catalog Browser to access the Catalog Browser directly, and then browse to find the needed catalog

Key in or select the AIRBUS catalog directory

Catalog Browser

Browse another Catalog


|

V5 14

|

Issue: Draft A6

|


Page 224 of 312

Assembly Design Standard Parts (2/2) 2. 3. 4. 5. 6.

Navigate through the chosen catalog Select the desired family and within this family the part you need Right-click to select the Copy contextual command Select the base of your assembly Right-click to select the Paste contextual command


The part is copied into your assembly. Note that this part is no longer linked to the catalog.

Note: If you select Tools > Mechanical Standard Parts > xxx catalogs you will access a catalog delivered with CATIA V5 (EN, ISO …). This are not AIRBUS standard catalogs!


|

V5 14

|

Issue: Draft A6

|


Page 225 of 312

Assembly Design Hints and Tips – Hide Elements / Search The functionality Tools > Hide is not available in the Assembly Design. To hide the same type of elements, use the Edit > Search function from the pull down menu to find the elements and then click the Hide icon.


E.g. search all planes


|

V5 14

|

Issue: Draft A6

|


Page 226 of 312

Assembly Design Hints and Tips – Positioning of Items (1/4) The example shows how to position one Part (A) in a specific angle (45 degree) to another cylindrical Part (B). 1.

Fix Part B

2.

Create a contact constraint between Part A and Part B • Select the face of Part A to be constrained • Select the circular face of Part B • Click the Contact Constraint icon, select External Orientation and then ok


Part B

Part A

Contact Constraint


|

V5 14

|

Issue: Draft A6

|


Page 227 of 312

Assembly Design


Hints and Tips – Positioning of Items (2/4) 3.

Position the compass to get a rotation axis • Select the red square at the centre of the compass and drag it onto Part B to snap it to the cylinder axis

4.

Select the Part A

5.

Double click one of the green compass axis to open the Compass Manipulation panel


|

V5 14

|

Issue: Draft A6

|


Page 228 of 312

Assembly Design



Rotate the Part A • Define the angle value (45 deg) in the Rotation increment field • Click the rotation icon

7.

Close the Compass Manipulation panel


|

V5 14

|

Issue: Draft A6

|


Page 229 of 312

Assembly Design



Put the compass back to the default position • Drag the compass away from the selected part and drop it on the axis system in the lower right corner of the document window

9.

Fix the Part A • Select the Part A • Click the Fix Component icon

Fix Component


|

V5 14

|

Issue: Draft A6

|


Page 230 of 312


Generative Drafting • • • • • • • • • • • • •

Starting the Drafting Workbench General Drafting Rules Quality Rules Toolbars and Icons Overview Generating Views Generating Dimensions Generating Instantiations Generating Drawings from 3D Changing the Drawing Scale Replacing the Drawing Sheet Overload Properties Plot / Print Hints and Tips •

View Properties


|

V5 14

|

Issue: Draft A6

|


Page 231 of 312

Generative Drafting Starting the Drafting Workbench (1/3)


Use the Start > Mechanical Design > Drafting pull down menu for starting the Generative Drafting Workbench. A new CATDrawing will be activated with an empty sheet.

See AM2264 Main Module Drafting with CATIA V5

Also use File > Page Setup to modify the format

To check that the correct ISO file (AIRBUS_ISO) is used, proceed to File > Page Setup within the CATDrawing CATIA V5 Basic - Presentation

|

V5 14

|

Issue: Draft A6

|


Page 232 of 312

Generative Drafting Starting the Drafting Workbench (2/3) If the 3D geometry already is open in V5 when using the Start > Mechanical Design > Drafting it is possible to select between an empty sheet or the automatic layout.


OK

Use Modify... to select the correct ISO file (AIRBUS_ISO) and to do the page setup


|

V5 14

|

Issue: Draft A6

|


Page 233 of 312

Generative Drafting Starting the Drafting Workbench (3/3) Drawing frames and title blocks must be stored within the Background of the CATDrawing file


The geometry will be created in the Working Views

When any work needs to be done on the views, select Edit > Working Views.

When any work needs to be done on the title block, select Edit > Background. CATIA V5 Basic - Presentation

|

V5 14

|

Issue: Draft A6

|


Page 234 of 312

Generative Drafting Titelblock Work arround (1/5)


1.

Change from Working Views in Background

2. Select Button Catalog Browser Select Button Browse another catalog : /CADLIB/std/CATIAV5-Drafting/A-D open the catalog: FramesGeneralEng.catalog


|

V5 14

|

Issue: Draft A6

|


Page 235 of 312

Generative Drafting Titelblock Work arround (2/5) 3. Open the chapter „Frames“.

4. Select a frame format with double click or with the contextual menu „Instantiate © AIRBUS DEUTSCHLAND GmbH. Alle Rechte vorbehalten. Vertrauliches und geschütztes Dokument.

component“. For the exact positioning the smart pick can be used.


|

V5 14

|

Issue: Draft A6

|


Page 236 of 312

Generative Drafting Titelblock Work arround (3/5) 5. Break the links to the Catalog document.


Select the componenets insert from the catalogs Catalog objects and use the function „xy Object / Expose 2D Component“ in the context menu from the right mouse button.

6. Is no detailsheet in the drawing a new one will be created..


|

V5 14

|

Issue: Draft A6

|


Page 237 of 312

Generative Drafting Titelblock Work arround (4/5) 7. Check if all links to the catalog document are broken by the function Edit / Links. Only


the link type ViewLink and no MML may be shown in the link list.

8. Change back to the Working Views


|

V5 14

|

Issue: Draft A6

|


Page 238 of 312

Generative Drafting Titelblock Work arround (5/5)


9. To insert a Text in the title block you have to change to the detailsheet and edit the text

Do not delete unused text (xxxx) replace this text by a dash ( - ).


|

V5 14

|

Issue: Draft A6

|


Page 239 of 312

Generative Drafting General Drafting Rules • • • • •


•

Only one sheet per file (CATDrawing) shall be produced Many detail sheets can be produced per CATDrawing If a drawing will contain more than one sheet a separate CATDrawing file needs to be created (xxx-01.CATDrawing, xxx-02.CATDrawing, …) All title blocks will be inserted within the Background of the CATDrawing When creating a drawing with CATIA V5 the naming of the CAD files shall conform to AP2610 and ABD0004 The sheet sizes shall conform to ABD0004 Part1


|

V5 14

|

Issue: Draft A6

|


Page 240 of 312

Generative Drafting Quality Rules To assure the overall usage (PDM-System and Release Management) of the drawings there some rules to follow: • • •


•

• • • • • • • •

The Magnitude Length shall be mm. View Frames shall be invisible, otherwise they would occur in TIFF files The first 9 characters of the CATDrawing file name and the CATPart/CATProduct file name, which is linked by the views, shall be identical. This is needed to assure the consistency between the part/product and its representation in a drawing There shall be no activated View in Sheet / no activated Detail View in Detail Sheet. Plot problems are possible, if one of the views / detail views etc. is activated instead of the sheet. A View should always linked to Part/Product. View with broken link to part/product shall be avoided Non-associative Dimensions and Non Up-to-date Dimensions shall be avoided Fake Dimensions should be avoided Elements in a 2D view, which have been created by hand and have no association to 3D should be avoided Empty sheets, views, detail views should be deleted Look the views Use the QCHECKER for drawings CATIA V5 Basic - Presentation

|

V5 14

|

Issue: Draft A6

|


Page 241 of 312

Generative Drafting Toolbars and Icons Overview (1/9) Sections

Toolbar Views (1/2)

Projections


Unfolded View

Front View

Projection View

View from 3D

Aligned Section View


|

V5 14

Details

Break view

Detail View Profile

Quick Detail View Profile

Advanced Front View

Aligned Section Cut

Offset Section Cut

|

Wizard

Isometric View

Auxiliary View

Offset Section View

Clippings

Issue: Draft A6

|

Detail View


Quick Detail View

Page 242 of 312

Generative Drafting Toolbars and Icons Overview (2/9) Sections

Toolbar Views (2/2)

Projections

Clippings

Details

Wizard

Break view

Clipping View Profile


Clipping View

Breakout View

Broken View Views via the Wizard


|

V5 14

|

Issue: Draft A6

|


Page 243 of 312

Generative Drafting Toolbars and Icons Overview (3/9) New View

Toolbar Drawing (Working Views activated)

New Sheet

Instantiate 2D Component


New Sheet Selected Edit > Working Views or Edit > Background in the Pull Down Menu to switch between the Views and the Background

Toolbar Drawing (Background activated)


|

V5 14

New Detail Sheet

Bill of Material

Frame Creation

|

Issue: Draft A6

|


Instantiate 2D Component

Page 244 of 312

Generative Drafting Toolbars and Icons Overview (4/9) Toolbar Dimension Generating

Generating Dimensions Step by Step


Generate Dimensions

Generate Dimensions


|

V5 14

|

Issue: Draft A6

|


Generate Balloons

Page 245 of 312

Generative Drafting Toolbars and Icons Overview (5/9) Technological Features Dimensions (TFD)

Toolbar Dimensioning TFD

Length TFD

Details

Radius Diameter TFD TFD

Dimensions

Re-route Dimensions

Create Interruption(s)

Geometrical Tolerance


Angle TFD Remove Interruption(s)

Re-route Dimensions Cumulated Dimensions

Dimension

Length/ Distance Dimensions

Stacked Dimensions


|

Radius Dimensions

Angle Dimensions V5 14

|

Issue: Draft A6

Chamfer Dimensions

Diameter Dimensions |


Datum Feature

Coordinate Dimensions

Thread Dimension

Coordinate Dimension Table

Hole Dimension Table Page 246 of 312

Generative Drafting Toolbars and Icons Overview (6/9) Toolbar Tools Palette


Projected dimension Force dimension on element Force horizontal dimension in view Force vertical dimension in view Force dimension along a direction True length dimension Intersection point detection

Force dimension along a direction Dimension perpendicular to a direction Dimension along a fixed angle in view


|

V5 14

|

Issue: Draft A6

|


Page 247 of 312

Generative Drafting Toolbars and Icons Overview (7/9) Toolbar Annotations

Symbols

Table From CSV Text

Table


Table

Text

Text Replicate

Datum Target Welding Symbol

Text with Leader


Ballon

|

V5 14

|

Text Template Placement

Issue: Draft A6

|


Roughness Symbol

Weld

Page 248 of 312

Generative Drafting Toolbars and Icons Overview (8/9) Area Fill

Toolbar Dress Up

Arrow


Axis and Threads

Centre Line with Reference

Center Line


|

V5 14

|

Issue: Draft A6

|


Thread with Reference

Thread

Axis Line and Centre Line

Axis Line

Page 249 of 312

Generative Drafting Toolbars and Icons Overview (9/9) Toolbar Tools Analysis Display Mode

Sketcher grid


Snap to point

Create Detected Constraints

Show Constraints

Dimension sytem selection Mode

Filter Generated Elements

F1 For the Toolbars Positioning, Analyse, Multi-View, Dimension generation, Dimension Properties, Profile, Background and General Tools see the Catia V5 Online Documentation: Workbench Indexes > Generative Drafting > Workbench Description > Command Board CATIA V5 Basic - Presentation

|

V5 14

|

Issue: Draft A6

|


Page 250 of 312

Generative Drafting Generating Views (1/2)

Create predefined Views about the assistant. It is possible to use default predefine Views or to create new configurations of views. View Creation Wizard Create associative Views from 3D.


Front View

Create an offset/aligned section view, or an offset/aligned section cut Offset Section View

Create a detail by defining a circle or sketched profile. Detail View


|

V5 14

|

Issue: Draft A6

|


Page 251 of 312

Generative Drafting Generating Views (2/2)

Create clippings by definition of a circle or a sketched profile. Clipping View Create a broken view by modification of an available view.


Broken View Create a breakout view by modification of an available view. Breakout View


|

V5 14

|

Issue: Draft A6

|


Page 252 of 312

Generative Drafting Generating Dimensions (1/2)

Generate Dimensions such as Distance, Length, Angle, Radius, Diameter and so on. Dimensions

Create Datum Features and Geometrical Tolerance.


Datum Feature

Create Text such as Text with Leader, Balloon and Datum Target. 5

A

Text

Create Roughness Symbols, Welding Symbols and Welds. Roughness Symbol


|

V5 14

|

Issue: Draft A6

|


Page 253 of 312

Generative Drafting Generating Dimensions (2/2) Generate all Dimensions from 3D in one Shot or Step by Step.

Generating Dimensions Analysis of dimensions that were generated and possibly re-positioned on the active view. Dimensions Analysis shows the dimension interferences. Dimensions Analysis


Dimensions are automatically re-positioned. Dimension Positioning...


|

V5 14

|

Issue: Draft A6

|


Page 254 of 312

Generative Drafting Generating Instantiations

Create a new Detail Sheet. The geometries created in this sheet can be inserted in the Drawing sheet. New Detail Sheet Insertion of geometries from Detail Sheet.


Instantiate 2d Component Insertion of Standard Details with Catalog Browser. Catalog Browser


|

V5 14

|

Issue: Draft A6

|


Page 255 of 312

Generative Drafting Generating Drawings from 3D (1/2) 1.


2. 3. 4. 5. 6.

Use the Start > Mechanical Design > Drafting pull down menu for starting the Generative Drafting Workbench. A new CATDrawing will be activated with an empty sheet. Insert the drawing frame and the title block in the Background Select Edit > Working Views In the same session open an existing part or product (if not already opened) Use Window > Tile ... to show both the 3D geometry and the drawing For View creation use either • the normal Projection panel

•

or the View Creation Wizard


|

V5 14

|

Issue: Draft A6

|


Page 256 of 312

Generative Drafting


Generating Drawings from 3D (2/2) 6.

Select a reference plane on the 3D geometry to define the front view

7.

Specify the final view direction with the view manipulator

Note: Drawing views generated are fully associative with the 3D model so therefore when a CATPart/CATProduct requires a modification, the CATDrawing will subsequently require an update to take into account the changes. The drawing can be checked at any time to make sure the links are maintained with the 3D model. This is done using Edit > Links. CATIA V5 Basic - Presentation

|

V5 14

|

Issue: Draft A6

|


Page 257 of 312

Generative Drafting Changing the Drawing Scale In order to avoid the loose of associativity, the views scale must be changed only in the Properties window and not by overwriting in the Text field of the view.


• Move the cursor to the view frame and click the MB3 to open the contextual menu • Select the Properties option • Modify the scale of the view

Only the scale of the geometry will be modified, not the value of the dimensions. CATIA V5 Basic - Presentation

|

V5 14

|

Issue: Draft A6

|


Page 258 of 312

Generative Drafting Modify the View Projection Plane After creation of the Front, Projection and Detail Views the projection plane of the Front View can be changed:


Select the Front View and click MB3 to open the context menu:

Choose a new projection plane in the 3D-Window and start the creation of the front view again.


|

V5 14

|

Issue: Draft A6

|


Update the views

Page 259 of 312

Generative Drafting Overload Properties In the Overload Properties can be set, how a Part should be represented in the section or in the projection view . • Move the cursor to the view frame and click the MB3 to open the contextual menu • Select Front view object > Overload Properties option • Select an element in the Characteristic list • Click on Edit to open the Editor


• Modify the properties and click ok

Note: The Overload Properties are only available when at least two Parts exist in the extracted view.


|

V5 14

|

Issue: Draft A6

|


Page 260 of 312

Replace a 3D Document (1)

View-Link

Vi e


Erzeugen einer Neuen Version

w-

Li

nk

Erzeugen einer Neuen Version

View-Link Replace 3D Document


|

V5 14

|

Issue: Draft A6

|


Page 261 of 312

Replace a 3D Document (2) Replace a 3D document of a drawing Requirement: The UUID of the old and new 3D document must be the same.


1. 2.

Open the new drawing and the new 3D document Replace the link to the 3D document by Edit/Links

3.


|

V5 14

Select the option „Loaded Document and select the new Dawing in the list

|

Issue: Draft A6

|


Page 262 of 312

Generative Drafting Plot / Print (1/2) To print or to plot the drawings, click on the function 'Print' from the 'File' menu. It is possible to print/plot the drawings in the actual or in a modified sizes. The choice of the printer and the settings to Page Size and Page Position take place in the 'Print' menu.


1

2 3 Use Tools > Image > Capture to capture a selected region! CATIA V5 Basic - Presentation

|

V5 14

|

Issue: Draft A6

|


Page 263 of 312

Generative Drafting Plot / Print (2/2) Choose of Printer

Print Preview


1

3

Settings of Page Size

2


|

V5 14

|

Issue: Draft A6

|


Page 264 of 312

Generative Drafting Hints and Tips - View Properties The generation of the geometry is predefined in Tools > Options > Mechanical Design > Drafting > Generation.


To modify the visualisation and dress-up of a single view, use the View Properties MB3 on the View > Properties > View…


|

V5 14

|

Issue: Draft A6

|


Page 265 of 312

DMU Introduction • Basics • • • • • • •

• DMU Space Analysis

General Design Review Document Modes Cache Management Memory Allocation Activate / Deactivate Load / Unload

• • • • •

Toolbar Overview Toolbar Measure Toolbar Analyse Measure Clash Computation


• DMU Navigator • • • • • • • •

Toolbar Overview Toolbar View Toolbar DMU Viewing Toolbar Navigation Tools Toolbar Data Navigation Toolbar DMU Move Toolbar DMU Generic Animation Fly Mode


|

V5 14

|

Issue: Draft A6

|


Page 266 of 312

DMU Introduction Basics – General


•

The CATIA V5 DMU solution includes the Workbenches DMU Navigator, DMU Space Analysis, DMU Fitting, DMU Kinematics and DMU 2D Viewer. This documentation will give an introduction into the DMU Navigator and the DMU Space Analysis.

See AP2264 Management of the digital mock-up See AP2266 Digital Mock-Up General Process

•

The DMU Workbenches are integrated into Catia V5, the application must not be changed.

•

A CATProduct is needed to work with the DMU Tools.

•

Within the DMU Workbenches you will worked mainly in the visualization mode. Original geometries can be used by switching from the visualization mode in the design mode.

•

All results calculated in the DMU Workbenches (Distance, Measure, Group, Sectioning, …) are filed in the CATProduct under the entry "Applications" in the tree. They are assigned to the highest node and are stored in the CATProduct.


|

V5 14

|

Issue: Draft A6

|


Page 267 of 312

DMU Introduction Basics – Design Review DMU Navigator

General Process

• • • •

Find and load necessary geometries

•

Visualize geometries


•

2D/3D Annotation Group Spatial Query Create one or more ‚Scene‘ for comparing the different Assemblies Exact positioning ‚Snap‘ of Parts by taking the geometrical elements into account (lines, points, planes, ...) Generating of animation (*.avi)

Analyse geometries DMU Analysis • • • •

Mark of problem areas

Documentation and storage of the results


|

V5 14

|

Issue: Draft A6

|

• • •


Interactive clash detection Sectioning Performing of measurement Compare products, visualisation of removed or added geometry Distance and Band Analysis Publish of clash detection (*.xml) Show clash detection as 2D section

Page 268 of 312

DMU Introduction Basics - Document Modes Document Modes


There are two different document modes available when a product is opened •

Visualisation Mode Visualisation mode opens a significantly lighter model than its true geometrical form, and can increase the performance. The visualisation mode uses a geometrical format .cgr (Catia Graphical Representation) that represents only the external appearance of the component. No Specification Tree available. No axis and wireframe geometry is visible. No plus sign is visible in front of the components in the tree.

•

Design Mode Design mode is the original editable format, making all geometrical data available. Exact geometry is loaded. If the Option “Work with the Cache System” is activated (default at AIRBUS) all parts are loaded in Visualisation mode. When modification is required on a part it can be converted from visualisation to design mode by: • MB3 over the part icon > Representations > Design Mode or • double-click MB1 over the part icon CATIA V5 Basic - Presentation

|

V5 14

|

Issue: Draft A6

|


Page 269 of 312

DMU Introduction Basics – Cache Management (1/3) Working with the Cache System

CATProduct


Insert an Existing Component (e.g. Part1.CATPart) or Open a CATProduct which includes at least one Part

Catia V5

Part1 loaded in visualisation mode

Tessellation

Local Cache Part1.CATPart.”timestamp”.cgr

The first time a Part is inserted, it is tessellated. It means that the corresponding .cgr file is computed and saved in the local cache as well as displayed in the document window. The .cgr file is described by the name of the CATPart and a timestamp

It is possible to work with a released cache. A released cache is a read-only cache that can be located anywhere on the network and several directories can be defined for this cache.


|

V5 14

|

Issue: Draft A6

|


Page 270 of 312

DMU Introduction Basics – Cache Management (2/3) When this component will be required again, the .cgr file which already exists (and not the original document) is automatically loaded from the local cache. Before the loading of the .cgr file, its timestamp will be checked to verify that no modifications have been made to the CATPart since the generation of the .cgr file. If the timestamp is out of date, the CATPart will be re-tessellated. Insert an Existing Component (e.g. Part1.CATPart) or Open a CATProduct which includes at least one Part

Check if .cgr exist in the local cache (e.g. usr/tmp/CATCache) Yes


No

Check if timestamp ok Yes

No Check if .cgr exist in the released cache (e.g. fc/d21w1 in the ROA) Yes

No

Check if timestamp ok No

Yes

Create a new .cgr in the local cache

Load the .cgr CATIA V5 Basic - Presentation

|

V5 14

|

Issue: Draft A6

|


Page 271 of 312

DMU Introduction Basics – Cache Management (3/3)


To view the contents of the cache use Tools > Cache Content in the DMU Navigator Workbench


|

V5 14

|

Issue: Draft A6

|


Page 272 of 312

DMU Introduction Basics – Memory Allocation


Impact of available Functionalities

Icon

Function

Impact

Edit/ Delete

delete

Model and structure element will be unloaded completely

load

Model will be loaded in RAM

only *.CATPart and *.CATProduct

unload

Model will be unloaded from the RAM

only *.CATPart and *.CATProduct

activate

Model is loaded in the RAM, structure element must exist

deactivate

Model will be unloaded from the RAM, structure element survives

design mode

Native Geometry will be loaded

visualisation mode

Only tessellated Geometry will be loaded, native Geometry will be unloaded from RAM

hide

Models will be transferred in the no-show area, no RAM is released

show

Models will be transferred from the no-show area in the show area, no additional RAM is covered


|

V5 14

|

Issue: Draft A6

Comment

|


Strong utilization of RAM!

Page 273 of 312

DMU Introduction Basics – Activate / Deactivate


MB3 > Representation > …

Grey axis: Deactivated Red axis: Activated

Note: If Tools > Options > Infrastructure > Product Structure > Product Visualization > Representation: Do not activate default shapes on open is selected, all geometry will be deactivated while loading. CATIA V5 Basic - Presentation

|

V5 14

|

Issue: Draft A6

|


Page 274 of 312

DMU Introduction Basics – Load / Unload

Unloaded


MB3 > Components > …

Loaded

Note: If Tools > Options > General > Referenced Documents: Load referenced documents is selected, only the structure will be loaded. CATIA V5 Basic - Presentation

|

V5 14

|

Issue: Draft A6

|


Page 275 of 312

DMU Introduction Navigator – Toolbar Overview 1/4 Toolbar View (Examine mode)


Fly Mode

Toolbar View (Fly mode) Fly

Examine Mode


Turn Head

|

V5 14

|

Decelerate

Accelerate

Issue: Draft A6

|


Page 276 of 312

DMU Introduction Navigator – Toolbar Overview 2/4 Toolbar DMU Viewing

Previous View


Look At

Manage Annotated Views

Create an Annotated View CATIA V5 Basic - Presentation

|

V5 14

Magnifier

Next View

Toolbar Navigation Tools

|

Issue: Draft A6

Depth Effects

Lighting

3D Annotation Create Scene

Add Hyperlinks

|

Horizontal Ground


Group

Sectioning

Page 277 of 312

DMU Introduction Navigator – Toolbar Overview 3/4 Toolbar Data Navigation

Spatial Query

Search


Go to Hyperlinks

Current Selection Panel

Applicative Entities Reordering

Start Publish

Toolbar DMU Move Cumulative Snap

Translation or Rotation


|

V5 14

|

Issue: Draft A6

|

Reset Position s

Symmetry


Page 278 of 312

DMU Introduction Navigator – Toolbar Overview 4/4 Toolbar DMU Generic Animation

Clash Detection (Off)

Track


Play a Simulation


|

V5 14

|

Edit Sequence

Record Viewpoint Animation

Track

Clash Detection (Off)

Colour Action

Clash Detection (On)

Visibility Action

Clash Detection (Stop)

Issue: Draft A6

|


Page 279 of 312

DMU Introduction Navigator – View Navigating in examine mode is the default mode. Documents can be examined from the outside by moving around the perimeters, or from the inside by turning the head to view or moving closer to different objects. Examine Mode In Fly mode, you can move upwards or downwards on any horizontal view plane. You can also move forwards or backwards. Fly Mode


In Walk mode, you can walk forwards and backwards as well as turning right or turning left. You can also walk along the horizontal plane Walk Mode In Walk mode or Fly mode it is possible to use the ‚Turn Head‘ function.

Turn Head


|

V5 14

|

Issue: Draft A6

|


Page 280 of 312

DMU Introduction Navigator – DMU Viewing Visualisation of an On-Screen detail by using the button.

Look At Create a separate window where the enlarged details of a document will be displayed. The complete environment is permanently visible.


Magnifier Achieve 3D depth effects by clipping geometry on a plane parallel to the screen and creating fog effects. After closing the function the clipping planes are still active. Only in deactivating the clipping planes will the components be complete again. Depth Effects Visualise a plane at the ground level of the document, this enables to recognise if the document is positioned in the right direction. Horizontal Ground Variation of ambient lighting effects. It is possible to change the lighting direction, brightness, contrast and highlights. Lighting


|

V5 14

|

Issue: Draft A6

|


Page 281 of 312

DMU Introduction Navigator – Navigation Tools Generate text fields and marker in a stored view. When moving the view the texts disappear. The function is usable within a section. Annotated View Create a comment to describe a problem or to document a message. The comment is permanently visible. 3D Annotation


Define a group of Objects by individual selection. Groups can be stored in the document.

Group Enable: To work on the evolution of an assembly in a separate window from the actual assembly, Or to save a copy of an assembly in a separate window, work on the development directly on the assembly. Create Scene


|

V5 14

|

Issue: Draft A6

|


Page 282 of 312

DMU Introduction Navigator – Data Navigation Search for an object with a specific name, or with a specific type or colour. Search for product properties or objects created using a specific workbench, in a current document or throughout the whole product structure. Search


Spatial Query

Simplify a complex assembly by displaying only those products you want to work with. It is based on cubic representation of each part. The size of the cubes is designated by the accuracy parameter. Zone Query: The Ability to search all products is included in a rectangular box Preparation of html reports so that you can publish it on the enterprise intranet. You can insert a snapshot of a clash conflict, add appropriate comments or annotations and even select parts to insert as a VRML link.

Start Publish


|

V5 14

|

Issue: Draft A6

|


Page 283 of 312

DMU Introduction Navigator – DMU Move Move a set of components by using the parameters in the Move dialog box.

Translation or Rotation This allows the definition of an environment with additional constraints a component’s reducing degree of freedom Cumulative Snap


Create a symmetrical component by mirroring, or a new instance by rotation and translation, or the same instance by rotation. Create symmetry on Component This resets the position of selected products or of all products if none are selected. The position of products corresponds to the last stored position. Reset the position of Products


|

V5 14

|

Issue: Draft A6

|


Page 284 of 312

DMU Introduction Navigator – DMU Generic Animation The simulation player is available every time you create a track, a sequence or when you simulate your track. Simulation Player Recording of viewpoint animations either using the fly/walk command or direct manipulation of the geometry. A replay is automatically created for each new viewpoint recording. Record Viewpoint Animation


Deactivate interference detection while replaying a simulation.

Clash Detection (Off) Activate interference detection while replaying a simulation.

Clash Detection (On) Activate automatic clash detection stop mode for simulation.

Clash Detection (Stop)


|

V5 14

|

Issue: Draft A6

|


Page 285 of 312

DMU Introduction Navigator – Fly mode

• Select the button „Fly“ • Change to perspective projection by confirmation of the counter „Yes“ • Start the fly: Hold MB2 and click MB1 once


• Beginning of the fly phase. In the middle of the screen a target point appears. On lower screen border there is a green arrow which shows the fly direction. Under the arrow the current airspeed is indicated. • The fly direction can be steered with the mouse. The deflection depends on the distance between mouse pointer and target point. • Button ‚Screen up / Screen down‘ – makes possible to adjust the speed. • Click MB1 again to change the direction of the flight (Change from forward to backward) • To finish the flight mode switch back into the "Examine“ mode • Use View > Render Style > Parallel to exit the perspective projection


|

V5 14

|

Issue: Draft A6

|


Page 286 of 312

DMU Introduction Space Analysis – Toolbar Overview 1/2 Toolbar DMU Space Analysis

Compare Products


Sectioning

Clash

Distance and Band Analysis

Measure Item

Measure between

Measure Three Points

Measure Inertia

Create an Annotated View

3D Annotation

Group

Manage Annotated Views

See next page


|

V5 14

|

Issue: Draft A6

|


Page 287 of 312

DMU Introduction Space Analysis - Measure Measure the minimum distances and angles between geometrical entities (surfaces, edges, vertices and entire products) or between points. Measuring within a section is possible. Measure between Measure the properties associated to a selected item (points, edges surfaces and entire products).


Measure Item Measure the length, radius and angles of an arc drawn through three points. Measure Three Points

Measure the inertia properties of an object. To store the results in a text file click the export icon. Measure Inertia Measure a minimum distance, distances along x,y,z, or run a band analysis by defining the band and setting the accuracy. Distance and Band Analysis CATIA V5 Basic - Presentation

|

V5 14

|

Issue: Draft A6

|


Page 288 of 312

DMU Introduction Space Analysis – Analyse Detect interferences between two or more products. It is possible to read or compare clash command results in the Check Clash dialog box. The interferences will be shown in a preview window. Clash Define a sectioning of one or more products by creating a section plane, a section slide or a section box. Sectioning


Compare two parts or two products to detect differences between them and identify where material has been added and/or removed. Compare Products


|

V5 14

|

Issue: Draft A6

|


Page 289 of 312

DMU Introduction Space Analysis – Toolbar Overview 2/2 Sectioning Definition Panel Sectioning tools

Edit Geometrical Invert Position Target Normal And Positioning by Dimension 2/3 Selections

Reset Position


Volume Cut Section Plane Section Slice

Export As

Edit Grid

Results Window

Section Fill

Clash Grid Detection

Section Box


|

V5 14

|

Issue: Draft A6

|


Page 290 of 312

DMU Introduction Space Analysis - Measure Measurements can be executed in tessellated and native geometry. If native geometry (design mode) is measured, the exact values are calculated. With the tessellated geometry the value is approximated. This is made recognisable by a tilde (~).


Tessellated files (cgr) allow no selection of corners, edges and surfaces. To be able to use also this functional character, the mode must be switched from the visualization in the design mode. This must take place before the beginning of the measurement procedure. To avoid unnecessary post loading times, only the geometry which will be measured native should be loaded. Note: The results of the functions Clash, Distance, Band Analysis and Section are always based on the approximate representation. By working with cgrs it is the SAG value, by working without Cache or in the design mode it is the 3D Accuracy. Only the function ‘Measure Between’ guaranteed exactly measured values. The Value of 3D accuracy will be used for the transformation of data in tessellated shape automatically. The value can be changed later. If there is a difference between the SAG of the tessellated Part and the 3D accuracy, the SAG will be used for viewing. CATIA V5 Basic - Presentation

|

V5 14

|

Issue: Draft A6

|


Page 291 of 312

DMU Introduction Space Analysis – Clash computation • Contact+Clash • Clearance+Contact+Clash • Allow negative Penetration depth, e.g. for flexible Parts

Clash


Apply

• Inside one selection • Selection against all • Between all components (Only

recommend for smaller circumferences) • Between two selections

•Clash: Red •Contact: Yellow •Clearance: Green CATIA V5 Basic - Presentation

|

V5 14

|

Issue: Draft A6

|


Page 292 of 312

CATIA V5 System settings


System settings • Tools - Options • Document search • Display Accuracy • Display of Geometry • Part Update • Assembly Update • Cache Management • Part Number • External References • Product Visualization • Tree Customization • Display in Specification Tree • UNDO Steps


|

V5 14

|

Issue: Draft A6

|


Page 293 of 312

CATIA V5 Tools - Options

Tools - Options Settings (Tools - Options)


In this chapter often needed settings are explained for better understanding, user control and system performance. General information A “red closed padlock setting” is created by the administrator and cannot be modified by the user. An “grey open padlock setting” can be activated or deactivated (hook, input command or path and so on).

User setting activated User setting deactivated System administrator setting


|

V5 14

|

Issue: Draft A6

|


Page 294 of 312

CATIA V5 Document search

Document search General - CATIA document search


This defines the possible paths to look for documents single CAD models or linked in products (“Load referenced documents”).

Allowed or not allowed paths, the “Current” marked is the default path to search and save CAD data. TOP to BOTTOM search order and with “Active = Yes” allowance to look in this paths for linked CATIA objects.


|

V5 14

|

Issue: Draft A6

|


Page 295 of 312

CATIA V5 Display Accuracy

Display Accuracy General – Display performance


The “Accuracy” has a great influence in the time needed for rendering your geometry. Therefore keep the standard value or switch back to this value after temporary use of better display e.g. for screen shots.


|

V5 14

|

Issue: Draft A6

|


Page 296 of 312

CATIA V5 Display of Geometry

Display of Geometry General – Display - Navigation - Selection


This defines the way the geometry is shown before or after selecting.

(Face boundary dashed)


|

V5 14

|

Issue: Draft A6

|


Page 297 of 312

CATIA V5 Part Update

Part Update


Updating Parts Infrastructure – Part Infrastructure – General – Update These options define the system update for Parts (Solids and Surface Design). An automatic update works suddenly on every modification. If You want to make more modifications at once You should change the setting to manual update to save time.

Synchronization of Links from part to part e.g. mirrored parts (left / right part) If activated: The modification is recognised – but must manually be updated in “red coloured part”


|

V5 14

|

Issue: Draft A6

|


Page 298 of 312

CATIA V5 Assembly Update

Assembly Update Updating Assemblies Mechanical Design – Assembly Design – General - Update


These options define the system update for Assemblies. Time save on several modifications like above Î Manual.


|

V5 14

|

Issue: Draft A6

|


Page 299 of 312

CATIA V5 Cache Management

Cache Management Cache Management Infrastructure – Product Structure – Cache Management


For large assemblies it is necessary to work with the cache system. So normally it is activated.


|

V5 14

|

Issue: Draft A6

|


Page 300 of 312

CATIA V5 Part Number

Part Number Correct naming for new parts Infrastructure – Product Structure – Product Structure – Part Number


It is recommended to use the correct part name from the very first beginning of a new designed part. So this activated option will help you to avoid mistakes in naming and saving your CATIA model. On opening a New Part … … Naming is first step Î

Saving with correct predefined name:

Otherwise: Inconsistency Î CATIA V5 Basic - Presentation

|

V5 14

|

Issue: Draft A6

|


Page 301 of 312

CATIA V5 External References

External References External References and Links Infrastructure – Part Infrastructure – General – External References


Here the creation of “external Links” between parts is controlled. It is not allowed to create such external Links at AIRBUS today. The activated “Confirm when creating a link…” is an additional control for yourself.


|

V5 14

|

Issue: Draft A6

|


Page 302 of 312

CATIA V5 Product Visualization (1/2)

Product Visualization (1/2) Display models in products Infrastructure – Product Structure – Product Visualization – Representation (1/2)


If you are loading large assemblies, you can save time on “not activating shapes on open”. This means, that the product structure is shown in the specification tree – but no geometry is loaded.


|

V5 14

|

Issue: Draft A6

|


Page 303 of 312

CATIA V5 Product Visualization (2/2)

Product Visualization (2/2) Display models in products Infrastructure – Product Structure – Product Visualization – Representation (2/2)


In this case you can decide to show only a few needed geometry models by activating them in the tree:

MB3 – Representations – Activate Node


|

V5 14

|

Issue: Draft A6

|


Page 304 of 312

CATIA V5 Tree Customization (1/2)

Tree Customization (1/2)


Display in specification tree Infrastructure – Product Structure – Tree Customization – Specification tree order

This panel is used to manage the display of Product Structure nodes in the specification tree. But only nodes belonging to products are affected: Constraints, relations, applications defined under a product. The display within Part structure nodes is not affected!


|

V5 14

|

Issue: Draft A6

|


1 2

1. 2.

Position in tree Displayed or not

Page 305 of 312

CATIA V5 Tree Customization (2/2)

Tree Customization (2/2) Display in specification tree Infrastructure – Product Structure – Tree Customization – Specification tree order


Example:


|

V5 14

|

Issue: Draft A6

|


Page 306 of 312

CATIA V5 Display in Specification Tree

Display in Specification Tree Displayed information in specification tree Infrastructure – Part Infrastructure – Display


To activate the options to be displayed in specification tree set the hooks. Most important informations are: External References (Links outside the model) Formula defined: •Parameters (direct access only in tree) •Relations


|

V5 14

|

Issue: Draft A6

|


Page 307 of 312

CATIA V5 UNDO Steps

UNDO Steps General - UNDO steps Here the possible number of “UNDO” steps is defined.


Increasing this number will influence your system performance especially on big assemblies and part modifications.


|

V5 14

|

Issue: Draft A6

|


Page 308 of 312

This document and all information contained herein is the sole property of AIRBUS DEUTSCHLAND GmbH. No intellectual property rights are granted by the delivery of this document or the disclosure of its content. This document shall not be reproduced or disclosed to a third party without the express written consent of AIRBUS DEUTSCHLAND GmbH. This document and its content shall not be used for any purpose other than that for which it is supplied.


The statements made herein do not constitute an offer. They are based on the mentioned assumptions and are expressed in good faith. Where the supporting grounds for these statements are not shown, AIRBUS DEUTSCHLAND GmbH will be pleased to explain the basis thereof.


|

V5 14

|

Issue: Draft A6

|


Page 309 of 312


Document Control

Issue

Date

Summary and Reasons for change

Writer(s)

Draft A1

21 Sep 2004

Initial Issue

Michael Schwartz ACE Academy

Draft A2

03 Jan 2005

Incorporation of information about System settings

Michael Schwartz ACE Academy

Draft A3

10 Oct 2005

Release update CATIA V5 R12

Marcus Bendel ACE Academy

Draft A4

26 Oct 2005

Release update CATIA V5 R14


Draft A5

29 Oct 2006

Enhanced function description


Draft A6

29 Mar 2007

Deleted all German Specific informations

Volker Kowald ACE Academy


|

V5 14

|

Issue: Draft A6

|


Page 310 of 312

CATIA V5 Training Basic

Recommend Documents