Emilian Popa
Mastercam Mill 2008
-1-
Emilian Popa
Mastercam Mill 2008
Introduction to Mastercam Wire Welcome to Mastercam Wire Version 9. This product creates wirepaths for wire EDM machines, offering advanced tapering in both 2-axis and 4-axis wirepaths, automatic corner filleting and skim cut definition, advanced synchcronization, and efficient tab creation and management. Version 9 provides graphic land programming, supports multiple tabs with click-and-drag positioning, and lets you translate wirepaths for repetition without creating new geometry. To help you learn Mastercam Wire, this tutorial and extensive online help accompany the product. -
Use this tutorial as a self-training aid to orient yourself to the Wire program and interface. The projects included in the tutorial are designed to show you efficient ways to use Wire on realworld parts. The tutorial does not try cover every Wire feature.
If you need more help Online Help Online help contains the latest and most up-to-date information about Mastercam. The following pictures show how to use the online help.
-2-
Emilian Popa
Mastercam Mill 2008
Creating Single Contour Wirepaths A contour wirepath is used to cut out part boundaries, such as punches and dies, from a piece of stock. Contour wirepaths result in parts that have the same basic size and shape at the top and bottom of the part, depending on whether taper and special corner definitions are applied. In this chapter, you will create a contour wirepath for a punching die. The part consists of a vertical land and a tapered relief and will be programmed in an upside-down orientation for easy slug removal. The following picture shows a side view of this type of part.
In this chapter, you will perform the following tasks: -
Starting Mastercam Wire Opening a part file Setting up the part Chaining the wirepath geometry Setting contour wirepath parameters Backplotting the wirepath Saving the part and exiting Mastercam
Starting Mastercam Wire 1. Double-click the Mastercam Wire icon on your Windows desktop.
The following picture shows you some of the main features of the Mastercam work space.
-3-
Emilian Popa
Mastercam Mill 2008
Learning about the HASP and NetHASP Mastercam uses two types of licensing: single-user licensing and network licensing. If you are using single-user licensing, you need to have a special piece of hardware called a HASP (sometimes called a dongle or SIM) attached to your parallel port or USB port. If you get an error message like the following:
the HASP component is either missing or not configured properly. Refer to your installation instructions (included in a separate document) or contact your dealer for assistance. If you are using network licensing, then a NetHASP must be installed on a compter on your network. If you see any of the following messages, see your network administrator:
-4-
Emilian Popa
Mastercam Mill 2008
For more information on NetHASP installation, see Mastercam Network Licensing.doc in your main Mastercam folder.
Controlling part display in the graphics window Mastercam provides several different ways to control how jobs display in the graphics window. In the toolbar, the buttons below let you control the display scale of the part in the graphics window:
To the right of these buttons in the toolbar are buttons that control the graphics view (Gview), which is how you view the part in the graphics window:
-5-
Emilian Popa
Mastercam Mill 2008
Note: The graphics view does not affect the plane in which the part geometry exists. In Mastercam, this is called the “construction plane” or “Cplane” . Please refer to Mastercam’s online Help for more information on Cplanes and Gviews. When you right-click in the graphics window, a menu appears that lets you control the display in a similar way to the toolbar buttons and also provides some additional controls:
You will use these controls throughout this tutorial. Opening a part file In order to program a contour wirepath, you need a file containing geometry that defines the contour to be machined. In Mastercam, you have several options for obtaining part geometry. You can import the file from another file format, create a geometry file using Mastercam’s design capabilities, or open an existing Mastercam file. For this exercise, you will open an existing part file. 1. From the Main Menu, choose File, Get. Mastercam opens the Specify File Name to Read dialog box to the default folder (C:\Mcam9\Wire\Mc9) Tip: You can navigate quickly through Mastercam menus by typing the underlined character of each menu option. (In this case, type F,G instead of choosing File,Get with the mouse). You can also press [Esc] to back up one menu level instead of choosing the Backup button from the menu.
2. Select the Preview button in the top-right corner. This options lets you preview a file before opening it. The Specify File Name to Read dialog box should look similar to the following picture, although there may be more files in the white area.
-6-
Emilian Popa
Mastercam Mill 2008
Notes: If you are running Microsoft Windows, you will not have the Preview option. If you are running Microsoft Window and do not see the preview option, you probably need to run the CNCRegEdit program, which should be in the Mcam9 folder. Double-click CNCRed.exe, select the Wire version you are using from the Installed product list, then choose Mastercam for the File, Get dialog. Do not make any other changes. Choose OK to exit the program. The Preview window may display a different icon, depending on which Mastercam products you have installed on your system. 3.Navigate to the folder with the tutorial parts. The parts for all of the exercises in this tutorial are located in the C:\Mcam9\Tutorials\Wire Tutorial\Inch folder. 4. Select Wire Tutor Contour.mc9. The Preview window shows a picture of the geometry contained in the file.
-7-
Emilian Popa
Mastercam Mill 2008
5. Choose Open. The part geometry displays in the graphics window.
6. If the image doesn’t fit entirely within the graphics window, choose the Screen-Fit button from the Mastercam toolbar, or right-click in the graphics window and choose Fit screen from the menu. -8-
Emilian Popa
Mastercam Mill 2008
The green outline represents the part profile. The following symbols represent the default start, thread, cut, and work origin (STCW) positions:
Setting up the part Before you define the wirepath, you will prepare the start of the contour, where the wire begins cutting the part boundary, and move the default start, thread, and cut (STC) positions to a location suitable for machining this part. Turning on the AutoCursor and AutoHighlight features The AutoCursor feature aids the process of entering points in Mastercam by automatically detecting entity positions, such as midpoint and endpoints. AutoHighlight makes it easier to identify entities by automatically highlighting an entity when the cursor is over it. 1. Right-click in the graphics window. Mastercam displays the following menu.
2. If the AutoCursor and AutoHighlight options do not have check marks next to them, choose each option to enable it. Mastercam closes the menu after each choice, so right-click again if necessary. If the option already has a check mark next to it, the feature is already turned on. Click in the graphics window to close the menu.
Manually breaking the geometry -9-
Emilian Popa
Mastercam Mill 2008
To set up the start of contour, you will break the geometry at the point where the contour will start. The best location for the break point is along a flat section of the part boundary. Placing the start of contour on a flat part of the geometry makes it easier to grind down any burrs that result from the wire entering the material at this position. 1. Choose Main Menu, Modify, Break, 2 pieces 2. Click on the line indicated in the following picture to select it.
3. Position the cursor halfway along the line that you selected in step 2. When the cursor changes to an open square and Mastercam highlights the Midpoint option on the Point Entry menu (as shown in the following pictures), click to select this position. Mastercam breaks the entity at the midpoint of the selected line.
4. To verify that Mastercam broke the entity, move the cursor up and down over the line. Mastercam lighlights the line on either side of the break point, indicating that there are now two separate entities. You could continue to break other entities but that won’t be necessary for this exercise. Creating a point
- 10 -
Emilian Popa
Mastercam Mill 2008
Next, you will create a point entity that will be used to define new start, thread, and cut (STC) positions. There are many ways to create points in Mastercam. For this exercise, you will create a point perpendicular to the start of the contour at a specified distance. You will create the point inside the contour boundary because you are cutting a die. Note: You will create the point perpendicular to the start of the contour because many wire EDM machines require a perpendicular move into the part in order to compensate correctly for the wire diameter. 1. Choose Main Menu, Create, Point, Perp/dist 2. Select either of the lines that resulted from the previous break operation, as shown in the following picture.
3. Position the cursor at the break point. When the cursor changes to an open square and Mastercam highlights the Endpoint option on the Point Entry menu (as shown in the following pictures), click to select this position. Note: Every line has two endpoints and a midpoint. Make sure you select the endpoint to create the correct point.
- 11 -
Emilian Popa
Mastercam Mill 2008
4. In the prompt area at the bottom of the screen, type a distance value of 0.25 and press [Enter]. Mastercam temporarily creates a point at the break point and two 0.25-inch lines perpendicular to point on the line you selected. Each temporary line starts at the break point and ends 0.25 inch away in a horizontal direction. 5. Select the line that lies inside the contour boundary (to the left of the vertical line you have been working width), as shown in the following picture.
Mastercam creates a point at the endpoint of the temporary line that lies inside the boundary. You part should look like the following picture. ( The temporary lines and point disappear as soon as the screen refreshes.)
- 12 -
Emilian Popa
Mastercam Mill 2008
Moving the STC positions Now that you have created a point that is perpendicular to where you will start the contour, you will move the start, thread, and cut (STC) positions to this point. 1. Choose the STCW button on the Secondary Menu. Mastercam opens the STCW Parameters dialog box. The SCTW positions are all currently set to the default position (0,0).
2. You can enter coordinates for each of the positions if you want, but for this exercise you will use the point you created. Choose the Select Start/Thread/Cut button so you can select the point from the graphics window. 3. Position the cursor over the point that you just created. When the cursor changes to an open square and Mastercam highlights the Point option on the Point Entry menu, click to select this position.
- 13 -
Emilian Popa
Mastercam Mill 2008
Mastercan reopens the STCW Parameters dialog box. The STC position coordinates have changed and are now set to the location of the point that you selected. The work origin (W) remains at 0,0.
4. Choose OK to close the dialog box. Your part should now look like the following picture.
- 14 -
Emilian Popa
Mastercam Mill 2008
Chaining the wirepath geometry Now that you have defined the STCW positions, you’ve ready to create the wirepath. The first step is to chain the wirepath geometry. Chaining is the process of linking geometric entities (lines, arc, points, etc) in a specific order and direction, which determines the initial direction the wire will take. In this exercise, you will start the chain with point you created for the STC position, then chain a contour for the part boundary. You don’t have to start a wirepath by chaining a point. However, if you don’t start with a point, Mastercam uses the default STC position for the thread and cut positions, which may not be the best position for all parts. In addition, wirepaths can consist of more than one chain or contour, each of which must start with a point entity and have more than one STC position, as you will see in subsequent chapters. Setting chaining options Mastercam provides a number of options that simplify chaining geometry for wirepaths. Before you chain the entities for this wirepath, you will set the chaining options. 1. Choose Main Menu, Wirepaths, Contour, Chain, Options. Mastercam displays the Chaining Options dialog box. 2. If necessary, choose the Set start of chain from point entities check box to clear it. When this option is selected, Mastercam begins the chain at a point entity regardless of where you start the chain. In this exercise, you want the chain to start at the break you created, not a point. The chaining options should match the following picture.
- 15 -
Emilian Popa
Mastercam Mill 2008
3. Choose OK to close the dialog box. Notice that the chaining options are displayed in the prompt area at the bottom of the screen. Chaining the thread point The first entity that you will chain is the thread position (T). By chaining this point entity, Mastercam will associate it to the contour wirepath. Select the point that you created in the previous exercise, as shown in the following picture. Note. Do not choose Done.
Chaining the contour The second chain that you select will define the contour, or part boundary. You will start this chain at the break point that you created in the previous exercise. The chain start point marks the start of contour, where the wire begins cutting the part. 1. Select the line close to the break point as shown in the following picture.
- 16 -
Emilian Popa
Mastercam Mill 2008
Mastercam displays a direction arrow on the selected line. The base of the arrow should be located at the break point. If it is not choose Chg strt, the choose Move fwd or Move back from the menu to reposition the base of the arrow at the break point. If you make changes using this menu, choose Done to return to the contour chaining menu. 2. Check the direction arrow, which reflects the chaining (cutting) direction. For this exercise, it should point along the contour in a clockwise direction (down) as shown in the following picture. If it does not, choose Reverse from the menu.
3. Choose Done to end chaining. The Wire Contour dialog box opens. Setting contour wirepath parameters The Wire Contour dialog box has five tabs, or pages, of parameters. You will set parameters on each tab to define different aspects of the wirepath, such as power settings, taper, and compensation.
Selecting a wire power settings library
- 17 -
Emilian Popa
Mastercam Mill 2008
The first tab of the Wire Contour dialog box allows you to select a power settings library. A power settings library contains information that describes the wire, including wire offset, condition, diameter, overburn, stock to leave. Each power setting library contains different values for up to 24 passes of the wire through the wirepath. Mastercam provides many defined wire libraries, and you can also define you own wire libraries. For this exercise, you will select one of Mastercam’s predefined wire libraries. 1. On the Wire Parameters dialog box tab, choose Select Library. 2. Navigate to the C:\Mcam9\Wire\Power\Mits folder. The power settings in this library are for a Mitsubishi wire EDM. 3. Continue navigating to English\010 Dia Brass Wire, select ST_1250_3_RA32.wp9, then choose Open. Note. The power settings library file name identifies the type of material to be cut, its thickness, and the number of passes fro which is information is stored. The library you selected provides settings for 0.010” diameter brass wire to cut steel (ST) 1.250” thick and contains different settings for three passes. RA32 is a machine-dependent finish designation. 4. Clear the Associate to library check box. Notice that the settings are no longer grayed, which means that you can now change the power settings. For this exercise, you will do this only to make the settings easier to read. Note: When the Associate to library check box. Notice that the settings are no longer grayed, which means that you can now change the power settings. For this exercise, you will do this only to make the settings easier to read. Note: When the Associate to library check box is checked, Mastercam maintains an association between the wirepath and selected library. If settings in the library are changed at any time, all wirepaths associated to it are marked for regeneration the next time the part is opened. The power settings are grayed to prevent unintentional mofication of associated wirepaths in other jobs. When the Associate to library check box is not checked, you can make changes that will apply just to this part. 5. Select the Pass number field up arrow twice. The power settings change according to the different passes (1 through 3). Note: The Total Offset field is grayed because it is calculated from the wire radius, overburn, and stock to leave. You cannot enter it directly.
- 18 -
Emilian Popa
Mastercam Mill 2008
6. Return the Pass number to 1, and check to be sure your settings match the following picture.
7. Check the Associate to library check box again. Setting contour parameters The Contour dialog box tab contains parameters that describe how the top (UV) and bottom (XY) contours of the part will be cut, whether to cut a land, where compensation will occur, and more. It also identifies which contour the geometry defines – the XY contour, the UV contour, or the land, if there is one.
- 19 -
Emilian Popa
Mastercam Mill 2008
Note: All of the values you enter here will be expressed as absolute values relative to the system origin. 1. Choose the Contour dialog box tab at the top of the dialog box.
2. Choose the land down taper style by clicking on the radio button. 3.Type 2.0 for the taper in the Initial value field. Because you chose outside taper and chained the contour in a clockwise direction, Mastercam sets the taper to the left. You can override this direction, but for this exercise you will not. 4. Choose Cancel taper after pass from the pull-down menu, then select pass 1. This will cut the taper with the first pass, then cancel the taper for the subsequent passes to cut the land. 5. Choose the Chain height radio button that is at the XY height level. This setting indicates that the part geometry represents the XY contour.
6. Type 1.3 in the Rapid Height field and select Absolute. This value determines the location of the upper guide during rapid moves and should be higher than the UV Trim Plane to be sure to clear clamps and other fixtures. Note: If you select a button such as Rapid Height, the dialog box closes temporarily to allow you to select an entity in the graphics window to define the height dimension. You will not do this in this exercise. 7. Type 1.25 in the UV Trim Plane field and select Absolute. This value determines the location of the upper guide on the wire machine. It is usually set at the machine. 8. Type 1.25 in the UV Height field and select Absolute. This value determines in the top of the stock. 9. Type 0.20 in the Land Height field and select Absolute. This value determines the top of the land and the start of the taper. 10. Type 0.00 in the XY Height field and select Absolute. This value determines the bottom of the stock.
- 20 -
Emilian Popa
Mastercam Mill 2008
11. Type 0.00 in the XY Height field and select Absolute. This value determined the location of the lower guide on the wire machine. It is usually set at the machine. 12. If necessary, set Compensation type (in the upper right corner of the dialog box) to Control. This allows the wire EDM machine control to calculate compensation. 13. Set the Compensation direction to Auto. This allows the machine control to calculate whether to compensate to the left or right based on the location of the thread point inside or outside the contour. Leave the remaining parameters parameters set to their default values. Check to be sure your settings match the following picture. Make any necessary adjustments.
Setting lead in/out parameters The Lead in/out dialog box tab contains parameters that determine the wire movement upon entering and exiting the part. In this exercise, you will program the wire to enter the contour by moving into the part from the thread point, first in a linear move and then in an arc move tangent to the start of contour. For the exit move, you will program the wire to go past (overlap) the start of contour by a specified distance before exiting the contour. It will lead out of the contour using a tangent arc move followed by a linear move to the cut point. You will cut the wire before it returns to the thread point by specifying a maximum lead out.
- 21 -
Emilian Popa
Mastercam Mill 2008
The following picture illustrates lead in and lead out in a wirepath without a tab.
You can also program lead in/out moves for tabs. In this exercise, however, you will allow Mastercam to calculate the tab lead in and out in a way that prevents dropout. This is called the “no dropout method.” 1. 2. 3. 4.
Choose the Lead in/out dialog box tab at the top of the dialog box. For Lead in, choose Line and radius. For Lead out, choose Radius and line. Allow the Arc radius to remain at 0.012. This value determines the size of the arc used in the lead in/out moves.
Note: When you use the no dropout method, the lead in/out arc radius should be less than or equal to the smaller wire diameter plus twice the overburn defined in the selected power settings library to avoid dropout. However, when the compensation calculated in the control, as it will be in this part, the arc radius must be slightly larger than the wire diameter plus twice the overburn to prevent a fault at the control. This may permit dropout even though the No dropout method is activated. 5. Type 90.0 in the Arc sweep field. This values determines the total angle in degrees from the beginning to the end of the arc move. 6. Type 0.075 in the Overlap field. This value determines how far past the start of contour to begin the lead out move. Note: Setting an overlap distance results in the wire exiting the part at a different location from then entry point, thus preventing the formation of a burr or overburn. However, setting tool large a value may result in an error and an incorrect wirepath. 7. Select the Max lead out check box and type 0.05. This value determines how far the wire travels along the lead out move. Note: By setting this option, you save machining time by preventing the wire from traveling the entire distance of the lead out move. 8. Select the Also trim final leadout check box. After the lead out move, the wire will be cut while still in the taper position and will then return to a vertical position before being threaded for the next pass. - 22 -
Emilian Popa
Mastercam Mill 2008
Note: Some machines force the wire into a vertical position when they execute a cut commond. On such machines, trimming the final lead out might cause gouging on some tapered parts because the wire will be forced into a vertical position. In this situation, clear the Also trim final leadout check box. 9. Select Tab Cuts (no dropout method) to allow Mastercam to calculate tab lead in and lead out. 10. Leave the remaining parameters set to their default values. Check to be sure your settings match the following picture. Make any necessary adjustments.
Setting the number and type of cuts The Cuts dialog box tab determines how many of each type of cut (rough, tab, and skim) the wire makes on the part. The library that you selected for this part contains power settings for three passes, and you will program the wirepath to use three different settings – a rough cut (pass 1) and a skim cut before the tab cut (pass 2). You will also program a tab cut using the rough cut (pass 1) power settings, and a skim cut after the tab (pass 3). 1. Choose the Cuts dialog box tab at the top of the dialog box. 2. Select the Perform rough cut check box to activate it. 3. Enter 1 for Additional skim cuts (before tab). 4. Select the Tab check box and for the Tab width enter 0.1. Note: The tab width is calculated from the start of contour in a backward direction along the boundary.
- 23 -
Emilian Popa
Mastercam Mill 2008
5. Type 1 in the Number of tab cuts field. 6. Choose the Automatic radio button and enter 1, if necessary. Mastercam will create one tab perpendicular to the STC position. 7. Choose Skim cuts after tab and enter 1 in the Together field. This setting programs a finish cut after the tab cut but before the wire is cut to perform the next operation. 8. Check Reset pass number on tab cuts. This setting programs the wire to use the power setting for the first pass (rough cut) because the tab is usually made in raw stock. Note: If this option is not checked, Mastercam uses the next pass setting. If the next pass is not defined, no power setting will be output, so be sure to define sufficient passes in the power settings library to accommodate all passes. 9. Leave the remaining parameters set to their default values. Check to be sure your settings match the following picture. Make any necessary adjustments.
Note: Notice the list of cuts on the lower right of the dialog box. You have programmed four cuts even though the power settings library you selected contains settings for three passes. The rough cut uses pass 1 settings and the first skim cut uses pass 2 settings. Because you checked Reset pass number on tab cuts, the tab cut also uses pass 1 power settings. The third skim cut uses pass 3 settings. Setting the general parameters 1. Choose the General dialog box tab. - 24 -
Emilian Popa
Mastercam Mill 2008
2. Choose One way cutting method if it is not already selected. This setting programs the wire to cut in the same direction every pass. 3. Leave the remaining parameters set to their default values. Check to be sure your settings match the following picture. Make any necessary adjustments.
4. Choose OK.
Completing the wirepath Mastercam enters the Change at Point editing function, highlights the contour, and marks the entity endpoints with yellow points as shown in the following picture. The Change at Point function is used to vary wirepath conditions, such as taper and corner types, at defined points along the wirepath. You will learn more about Change at Point in Chapter 3 and 5.
- 25 -
Emilian Popa
Mastercam Mill 2008
1. Choose Done from the menu. 2. Choose OK to close this message. Mastercam generates the wirepath as shown in the following picture.
In the next exercise, you will examine the wirepath in greater detail. Backplotting the wirepath Now that you’ve programmed the part, you can check if for errors before you machine it. To do so, you will use the Backplot feature, which simulates the wire cutting motion on the part in the graphics window. In this exercise, you will backplot the current Mastercam job. You can also backplot any Mastercam job or NCI file (intermediate NC file) you have saved. - 26 -
Emilian Popa
Mastercam Mill 2008
Setting backplot parameters 1. Choose Operations from the Wirepaths menu. The Operations Manager lists all operations in the current job, allows you to modify them, and gives you tools to manage them. Tip: You can also press [Alt + O] to open the Operations Manager. 2. Choose the Backplot button on the right side of the dialog box. Mastercam closes the Operations Manager and displays the Backplot menu. 3. Make sure the Backplot menu Yes/No options match the following picture. If necessary, select an option to change its Y/N toggle.
Note: These settings will produce a wireframe representation of the wirepath, which will show the UV contour and wire itself. The Verify option, which creates a shaded representation of the contour, if off. 4. Choose Display from the Backplot menu. Mastercam opens the Backplot Wire Display Parameters dialog box, which allows you to control how Backplot displays the wirepath. 5. Select Color Loop to clear the check box, if necessary. The Color loop option displays every pass of the wire in a different color. You will disable it for this exercise to simplify the wirepath display. 6. Check to be sure your settings match the following picture.
- 27 -
Emilian Popa
Mastercam Mill 2008
7. Choose OK to close the dialog box.
8. Choose the Gview – Isometric toolbar button to change the orientation of the part in the graphics window.
9. Choose the Screen-Fit toolbar button to fit withing the graphics window. 10. Choose Run in the Backplot menu. Mastercam displays the wirepath. Tip: If the wirepath display does not fit entirely within the graphics window, press [Page Down] to zoom out, or press [Up arrow] to move the image down in the graphics window. Choose Run to display the wirepath again.
- 28 -
Emilian Popa
Mastercam Mill 2008
The light blue line represents the part geometry, the XY contour and the bottom of the land. The vertical gray lines represent the wire. Where they diverge indicates the start of the taper and the top of the land. The purple lines represent the UV contour (top of part), including both passes.Yellow lines represent rapid wire motion. 11. To zoom in and examine the tab, right-click in the graphics window and choose Top, then rightclick again and choose Zoom window. 12. Draw a window around the STC position and the nearby contour, where the tab exists. 13. Choose Run. The tab should look like the following picture.
- 29 -
Emilian Popa
Mastercam Mill 2008
If the part doesn’t look like the precending pictures, open the Operations Manager by choosing Backup, select the Parameters icon, and double-check the parameter settings.
Backplotting in step mode The Step option on the Backplot menu simulates the wire cutting motion by moving from point to point in the wirepath, one step at a time. You advance the movement from step to step by repeatly choosing the Step option (or pressing [S]). This mode is useful for examining the wirepath slowly at different stages. 1. Right-click in the graphics window and choose Fit screen. 2. In the Backplot menu, choose Step. The prompt area provides information regarding the step that is currently being performed, as shown in the following picture. This information will be updated continually during the backplot.
3. Continue to choose Step. The simulation displays, one step at a time. 4. Choose Step repeatedly (or press [S] until the wirepath is complete. The wire moves around the part boundary three times, once for each pass that you programmed. You will know it’s finished when the following message displays. Tip: You can right-click and choose Repaint at any time to erase the wirepath already displayed. You can also choose Run at any time to complete the wirepath, or press [Esc] to terminate it.
5. Choose OK. 6. Choose the Backup button on the left-hand side of the Mastercam screen to return to Operations Manager. 7. Choose OK to close the Operations Manager. Saving the part and exiting Mastercam Now that you’ve completed the wirepath, it’s ready for machining. At this point, it’s a good idea to save the work that you’ve done.
- 30 -
Emilian Popa
Mastercam Mill 2008
1. Choose Main Menu, File, Save. Mastercam opens the Specify File Name to Write dialog box. 2. Enter a new name for the file name so that you don’t write over the original file. 3. Choose the Save button in the lower-right corner. Mastercam saves the file with the new name. You’ve now ready to move on to the next chapter where you’ll learn about creating multiple contour wirepaths. Note: If you need to exit Mastercam and come back to the tutorial later, choose Main Menu, File, Next menu, Exit or press [Alt + F4]. Choose Yes to confirm that you want to close the program. Creating Multiple Contour Wirepaths In Chapter 2, you learned about contour wirepaths and created a wirepath for a punching die that consisted of a single wirepath. In this chapter, you will build on what you learned to create a punching die containing multiple contour wirepaths cut from a single piece of stock in a single operation. You will set up the job to cut the punches in five passes, including a separate pass to cut the tabs. You will also learn how to modify the wirepath after creation to add a glue stop on a specific contour. The following picture shows the part.
Like the part in Chapter 2, this will be programmed with the relief taper on top for easy slug removal. The following picture shows a side view of the part.
- 31 -
Emilian Popa
Mastercam Mill 2008
In this chapter you will perform the following tasks: - Creating a new configuration file - Opening the part file - Converting thread holes to thread points - Using AutoSave to save your work - Chaining the wirepath geometry - Setting wirepath parameters - Changing and previewing the wirepath - Backplotting the wirepath - Changing contour cutting order - Saving a wirepath as geometry.
Note: If you exited Mastercam Wire at the end of Chapter 2, restart it by double-clicking the Mastercam Wire icon on your desktop or by clicking the Windows Start button and choosing Programs, Mastercam 9, Wire 9. Creating a new configuration file The configuration file contains defaults for many Mastercam settings – memory allocations, tolerances, file locations, screen settings, and much more. Mastercam provides two standard configuration files, one for English units (wire9.cfg) and one for metric units (wire9m.cfg). You can also create your own. In this exercise, you will activate the wirepath preview system configuration feature, which simulates the wirepath as you define it and allows you to accept or reject it immediately. You will create a new configuration file with this feature activated. Whenever the new configuration file is current, wirepath preview will be activated. 1. Choose Main Menu, Screen, Configure. Mastercam opens the System Configuration dialog box.
- 32 -
Emilian Popa
Mastercam Mill 2008
2. Select the NC Settings dialog box tab, which defines many settings that control the display and creation of NC programs. 3. Select the Preview all wirepaths check box, if it is not already checked. 4. Choose Save As to save the change to a configuration file.
5. The Specify File Name to Write dialog box opens. Type myconfing in the File name field and choose Save, myconfig.cfg becomes the current configuration file. 6. Select OK. Note: You will learn more about the configuration file in the next chapter. You can also refer to Mastercam’s online Help for more information. Opening the part file 1. Choose Main Menu, File, Get 2. Navigate to the folder with the English tutorial parts. 3. Select Wire Tutor Multicontour.mc9 then choose Open.
- 33 -
Emilian Popa
Mastercam Mill 2008
Mastercam opens the part in the graphics window. Tip: If the part does not display completely, right-click in the graphics window and choose Fit screen or press [Alt + F1]. The punch die is approximately 5.7 “ by 8.7” in size overall and contains 14 small contours that represent the die openings. The four circles in the corners are mounting holes: you will not program them.
- 34 -
Emilian Popa
Mastercam Mill 2008
Converting thread holes to points When you open the, notice that each contour has a small circle in the center, which will become the thread and cut point for the contour. This part was created using a CAD software package that uses small circles to denote thread points. Mastercam, however, uses point entities to denote thread and cut positions. Before beginning the wirepath definition, you will replace the small circles with point entities. Analyzing the size of a thread circle This part contains many arcs of different sizes and radius values. Some of the arcs are less than 360 degree; others are full circles. To change only the circles designated as thread circles to point entities, you will first analyze the size of a thread circle to make selection of the circles easier. 1. Choose Main Menu, Analyze 2. Position the cursor over one of the small green circles in the graphics window. Mastercam highlights each entity when the cursor is over it, although it may be hard to see because the circles are small. Click to select a circle. 3. On the Analyze Entity menu, make sure the Edit option is set to N. If not, select it to toggle it to N. Mastercam display data for the analyzed arc in the prompt area at the bottom of the screen. Note the size of the arc (circle). Its radius is 0.03000. Note: Some of the information displayed may differ from the picture below. For this exercise, only the radius is important.
Note: If the Edit option were set to Y, Mastercam would open a dialog box that would allow you to change various attributes of the arc. Replacing the 0.03-radius thread circles with point entities. In this part, all the thread circles have the same radius. You will create points to replace all small arcs (circles). 1. Choose Main Menu, Create, Point, Next menu, Small arcs. Mastercam displays the Entity Selection menu.
- 35 -
Emilian Popa
Mastercam Mill 2008
Note: The Entity Selection menu displays whenever you must select entities. If offers various ways to select entities (area, only specific entities, all entities, etc.). It also allows you to unselect a selected entity. 2. Choose All, Arcs, Done. Mastercam selects all arcs in the part (not just the small circles) and displays the From Small Arcs/Circles menu, which lets you further define the arcs you want to replace. Note: Notice that Mastercam displays information about the selection you just made in the prompt area at the bottom of the screen. 3. Choose Max radius, which allows you to limit the selection to arcs with a maximum radius. 4. Type 0.03 in the prompt area, then press [Enter]. This value is the radius of the thread circle that you just analyzed, and of the other thread circles. By setting the maximum radius to this value, Mastercam will not create points for the larger arcs in the part. Tip: You can also type R, press [Enter], then select one of the thread circles to enter the radius. 5. Toggle the From Small Arcs/Circles menu Y/N (Yes/No) options to match the following picture. In addition to the radius limit that you set in the previous step, these settings will cause Mastercam to create points only for full circles and to delete the small circles where points are created.
6. Choose Do it to delete the small circles and create the point entities (indicated by cross hairs) in their place. The resulting part should look like the following picture.
- 36 -
Emilian Popa
Mastercam Mill 2008
7. Choose Main Menu, File, Save 8. Make sure the Save thumbnail image with geometry and Prompt for descriptor check boxes are checked. 9. Enter a new name in the File name field so that you don’t write over the original file.
Note: If you are running Microsoft Windows or if you have not configurated your Registry to use the Mastercam File Get/Save dialog, this dialog box will look different. 10. Choose Save.
- 37 -
Emilian Popa
Mastercam Mill 2008
11. Type a descriptor and choose OK. Whenever you select files in Mastercam, you can right-click on the file name to see the file information (dates created and modified, size) and descriptor. You can modify it whenever you save the file. Using AutoSave to save your work The next step is to chain the geometry, but before beginning chaining, you will learn how to use the AutoSave feature to save parts automatically at a regular time interval. You will save the part to a different file. This will allow you to keep a backup file and prevent accidental data loss, and still allow you to decide when you want to save the part. 1. 2. 3. 4.
Press [Alt + A]. The AutoSave dialog box opens. Select the Active check box to activate automatic file saves. For the interval, enter 10 to save the file automatically every ten minutes. Select Save using active Mastercam file name to clear the check box. This setting allows you to enter a different file name for the automatic file saves. If checked, AutoSave would use the current file name. 5. Enter a new file name, such as multicontour backup, in the File name box. 6. Clear the Prompt before saving file check box so that AutoSave operates in the background. When checked, Mastercam asks each time it saves if you want to delete the old file.
7. Choose OK. Every 10 minutes, Mastercam will save a copy of the file in mcam9\wire\mc9 folder. Tip: You can save your file at any time and also reduce keystrokes by pressing [Alt + A] and [Enter]. Chaining the wirepath geometry In this exercise, you will quickly chain (connect) 14 contours so they can be cut in a single operation. To do this, you will use a window chaining option, which lets you draw a window around all geometry you want to include in the wirepath. Mastercam then chains all the contours within the window. It also chains the point inside each contour to be the thread and cut point for the contour and breaks each contour at a point perpendicular to the thread point. (Remember that when you created the singlecontour wirepath in the preceding chapter, you broke the contour manually.) - 38 -
Emilian Popa
Mastercam Mill 2008
Setting chaining options 1. Choose Main Menu, Wirepaths, Contour, Window, Options The Chaining Options dialog box opens. 2. Select the Color mask and Set start of chain from point entities check boxes to clear them, if necessary, then select the Break closest entity to thread point check box. This automatically breaks the entity in each contour that is closest and perpendicular to the thread point and starts the contour there. Doing this permits the wire to lead into and out of the wirepath perpendicular to the wirepath, which many wire machines require to compensate correctly for the width of the wire. 3. Make sure the remaining options match the following picture, the choose OK to return to the Chain window menu.
Chaining the geometry 1. Toggle the Rectangle and Inside menu options to +. The menu options should match the following picture.
- 39 -
Emilian Popa
Mastercam Mill 2008
2. Draw a rectangle surrounding all the contours in the part (excluding the mounting holes) by clicking in opposite corners (for example, upper left and lower right).
3. The prompt area instructs you to enter a search point for Mastercam to search for entities to chain. Click anywhere on the lower rightmost contour as shown in the following picture. Note: The contour you select first becomes the first chain, which determines where Mastercam starts the multi-contour wirepath.
- 40 -
Emilian Popa
Mastercam Mill 2008
Mastercam highlights all contours and points inside the rectangle.
4. Choose Done. The Wire Contour dialog box opens. Setting wirepath parameters Next, you will set contour wirepath parameters. Like the single contour parameters, these include the power settings, lead in and lead out configuration, number of rough and finish passes, tabs, and more. The parameters will be applied to all contours in the operation. Selecting a power settings library 1. Choose the Wire Parameters dialog box tab, then choose Select library. 2. Navigate to:
- 41 -
Emilian Popa
Mastercam Mill 2008
C:\Mcam9\Wire\Power\Mits\English\010 Dia Brass Wire\ST_1000_5_RA12.wp9 This library contains settings for five passes through 1-inch steel. Setting the contour parameters 1. Choose the Contour dialog box tab at the top of the dialog box.
2. Select the land down style, which will taper the sides toward the outside of the part starting at the land and extending to the top of the part. 3.For the taper, enter an Initial value of 5.0 (degrees) Note: The chain direction of the first chain in a multicontour wirepath determines whether the taper leans left or right to create an outside taper. In this part, the chain direction of all contours is counterclockwise (the default direction for closed chains set in the Chaining Options dialog box). Mastercam sets the taper to the right. You can override this settings, but you will not for this exercise. 4.From the pull-down menu, select Apply taper after pass and scroll the pass number to 2. The taper settings should match the following picture.
5. Enter a Rapid Height of 1.3 (absolute) to clear the top of the one-inch stock and any clamps. 6. Enter a UV Trim Plane of 1.0 (absolute). 7. Enter a UV Height of 1.0 (absolute), which represents the top of the stock. 8. Enter an Land Height of 0.3 (absolute). 9. Enter an XY Height of (absolute), which represents the bottom of the stock. 10. Enter an XY Trim Plane of 0.0 (absolute) Make sure the Contour dialog box tab values match the following picture.
- 42 -
Emilian Popa
Mastercam Mill 2008
Setting the lead in/out parameters 1. Choose the Lead in/out dialog box tab. 2. Select Line and radius for the lead in, and Radius and line for the lead out. 3. If necessary, enter 0.012 for the Arc radius. When compensation is applied in the control, this radius should be larger that the smallest wire diameter plus twice the overburn to avoid a fault at the control. Make sure the remaining values match the following picture.
- 43 -
Emilian Popa
Mastercam Mill 2008
Setting the cuts parameters 1. 2. 3. 4. 5.
Choose the Cuts dialog box tab. Make sure Perform rough cut is selected. For Additional skim cuts (before tab), enter 2. Select Tab to activate it, then enter 0.05 for the Tab width. Choose All cuts together from the pull-down menu. This programs Mastercam to cut all passes on a single contour before proceeding to the next contour. 6. Select Skim cuts after tab and enter 1 in the Together field. Leave the remaining settings at their defaults. Make sure the Cuts dialog box values match the following picture.
- 44 -
Emilian Popa
Mastercam Mill 2008
Note: In the lower right corner of the Cuts dialog box (precending picture), Mastercam lists each chain in the contour and the cuts programmed for it. It also shows the total cuts for each chain. You have programmed each chain (contour) to have five cuts, and all cuts are performed on one chain before proceeding to the next. This list is provided for information only and cannot be modified. To change the order and grouping of cuts, change the parameters to the left. Setting the general parameters 1. Choose the General dialog box tab. 2. For this exercise, use the default settings. Make sure the settings match the following picture.
- 45 -
Emilian Popa
Mastercam Mill 2008
3. Choose OK. Changing and previewing the wirepath After you define the multi-contour wirepath. Mastercam lets you preview the wirepath for examination and possible modification by displaying the points on every contour, as shown in the following picture.
- 46 -
Emilian Popa
Mastercam Mill 2008
In this exercise, you will add a glue stop ( a position where the wire pauses in the wirepath) on one of the contours in pass 2. This change will be associative, which means that Mastercam can regenerate the wirepath to incorporate the change without requiring you to redefine the wirepath. You will also learn how to zoom in on details of the wirepath. 1. In the Wirepaths: Entity endpoint to change menu, toggle Multi Sel to Y. This allows you to select more than one endpoint to change, although for this exercise you will make a change on only one endpoint. 2. Choose Next chain until the chain identified in the following picture is highlighted.
- 47 -
Emilian Popa
Mastercam Mill 2008
3. To get a closer view of the contour, choose the Screen-Zoom toolbar button, then click and drag a rectangle around the contour circled in the previous picture. 4. Select the line identified in the following picture by clicking near the point above it as shown. Mastercam highlights the point and the associated line segment.
- 48 -
Emilian Popa
Mastercam Mill 2008
5. Choose Done Sel (not Done) from the menu. Mastercam opens the Change At Point dialog box, where you can change contour parameters for specific points in the contour. Note: If you chose Done accidentally, right-click the Geometry icon in the Operations Manager, choose Next chain until the correct chain is highlighted, and repeat the selection. Adding a glue stop Change at Point allows you to make changes to contour wirepath parameters at specific points on the geometry. You can change taper, corner type, compensation, feed rate and other settings. Some of the changes can be applied only during a specific pass. Change a Point can only be used on contour wirepaths. The changes you make are associative, so they remain in effect even if you change the geometry. If you rechain the geometry, however, Mastercam erases the point changes. 1. Scroll the pass number to 2 so that the additional stop is applied during the second pass. 2. Select the Control Flags check box located in the lower right, then choose the Control Flags button.
3. The Control Flags dialog box opens. Select the Stop/Glue check box, select Glue, then choose OK to return to the Change At Point dialog box.
- 49 -
Emilian Popa
Mastercam Mill 2008
4. Choose OK. Mastercam changes the highlight on the selected point and segment to red. 5. Right-click in the graphics window and choose Isometric to change to isometric view, then right-click again and choose Fit screen to fit the geometry. Although you could choose Next chain or Prev chain and make changes to other points in the wirepath, for the exercise you will choose Done. 6. Mastercam previews the wirepath in shaded (verify) view. Choose Accept to accept the multiple contour wirepath. The wirepath displays.
Backplotting the wirepath As you learned in past, backplotting simulates wire cutting motion. But backplotting can show more than just the path the wire takes. It can:
- 50 -
Emilian Popa -
Mastercam Mill 2008
Plot the wirepath as wireframe Simulate the cutting operation in three dimensions by shading surfaces, which is called verify mode. Save the entire wirepath as geometry, which allows you to print or plot a hard copy of the wirepath. Backplotting with shaded surfaces and as wireframe
1. Press [Alt + O] to open the Operations Manager. 2. Choose Backplot. Toggle the Backplot menu options so that they match the menu shown in the following picture.
3. Choose Run. Mastercam plots the wirepath with shaded surfaces.
4. In the Backplot menu, toggle Verify to N, then choose Run again. Mastercam plots the wirepath with wireframe geometry.
- 51 -
Emilian Popa
Mastercam Mill 2008
5. Right-click in the graphics window and choose Top. The display should remain zoomed in on the contour you changed. If not, zoom in on it now. 6. Choose Run again. Notice the stop you added to the contour in the previous exercise (indicated by the stop symbol).
Tip: To find out what the other backplot symbols mean, press [Alt + H] to open Mastercam Help, then choose the Backplot symbols topic. Changing Backplot display parameters To make it easier to understand the display, you can reset the Backplot display parameters to display each pass in a different color (color loop) and simulate compensation in control. 1. In the Backplot menu, choose Display. The Backplot Wire Display Parameters dialog box opens. 2. Select the Color Loop check box, which will display each pass in a different color.
- 52 -
Emilian Popa
Mastercam Mill 2008
3. Select the Simulate Cutter Compensation check box, which will simulate the actual cutter path including offset.
4. Choose OK. 5. Right-click in the graphics window and choose Isometric, then choose Fit screen, if necessary.
6. Choose Screen-Zoom from the toolbar and draw a window around the contours shown in the following picture.
- 53 -
Emilian Popa
Mastercam Mill 2008
7. Toggle Show wire to N to disable display of the wire. 8. Press [S] repeatedly to step through the backplot. Mastercam enters the first contour and cuts the first pass, simulating it with different colors for the XY and UV contours.
9. Continue pressing [S] to continue the backplot. Mastercam simulates the remaining passes, applying the taper in the third pass. At the end of the backplot, the contour should look like the following picture. Tip: You can switch from Step to Run mode at any time by pressing [R]. You can stop a backplot at any time by pressing [Esc].
- 54 -
Emilian Popa
Mastercam Mill 2008
Tip: To examine each pass individually, release [S] at the end of the pass, repaint the screen, the resume the backplot by again pressing [S]. Examining compensation simulation When you program the wirepath so that the control applies cutter compensation, backplot must simulate the compensation. 1. Stop the backplot if necessary by pressing [Esc] then choose OK. 2. Zoom in on the area indicated in the following picture.
3. Choose Run. The backplot shows cutter compensation in control as a gray line next to the cutter path.
- 55 -
Emilian Popa
Mastercam Mill 2008
4. Choose Display and clear the Simulate Cutter Compensation check box. The dialog box should look like the following picture.
5. Choose OK. 6. Choose Run to backplot the wirepath. The display should look like the following picture.
- 56 -
Emilian Popa
Mastercam Mill 2008
Turning off symbols To make it easier to understand the display, you can turn off the shop, register, thread, and cut symbols. 1. 2. 3. 4.
Stop the backplot if necessary by pressing [Esc], then select OK Choose Backup to return to the Operations Manager, then select OK to close it. Choose Main Menu, Screen, Configure. The System Configuration dialog box opens. Choose the Screen dialog box tab, and clear the Draw stop/info/regs and Draw thread/cut symbols check boxes. This simplifies the backplot display by eliminating these symbols.
5. 6. 7. 8.
Choose OK, but do not save these changes to the configuration file. Choose Main Menu, NC utils, Backplot. This is an alternate way to acess the Backplot feature. Right-click in the graphics window and choose Top view, then choose Fit screen, if necessary. Choose Run. Notice that the wirepath symbols are not displayed.
- 57 -
Emilian Popa
Mastercam Mill 2008
Changing contour cutting order Mastercam’s associativity feature allows you to change a wirepath without having to reprogram it. In this exercise, you will change the order in which the contours are cut. 1. Press [Alt + O] to open the Operations Manager. 2. Left-click on the Geometry icon in the operations list.
3. The Chain Manager opens, Right-click in the with chain list area, the choose the Sort Chains option from the menu.
- 58 -
Emilian Popa
Mastercam Mill 2008
4. The Point Sorting dialog box displays. Choose the 2D sort method identified in the following picture.
5. Choose OK to close the Point Sorting dialog box.
- 59 -
Emilian Popa
Mastercam Mill 2008
6. Choose OK to close the Chain Manager and return to the Operations Manager. The Operation Manager marks the operation for regeneration. The Operation Manager marks the operation for regeneration. Wirepath marked with the regen symbol are sometimes referred to as “dirty”.
7. Choose Regen Path to regenerate the wirepath using the new sort order. Mastercam regenerates and previews the wirepath. 8. Choose Accept. 9. Choose Backplot and Run to see the regenerated wirepath and new cutting order.
- 60 -
Emilian Popa
Mastercam Mill 2008
Saving a wirepath as geometry Wirepaths remain displayed in the graphics window only while you are working on them, for example, during backplotting or while you are performing functions in the Operations Manager. If you want to print or plot the wirepath or use it in other ways, you must save the wirepath as geometry. Backplot allows you to do this. When you save a wirepath as geometry and save it to a level. Mastercam stores the geometry on data level 255, unless you specify a different level. In Mastercam, levels provide a way to organize data and control display. By turning off level 255 (or the level where you saved the wirepath), you can view (and print) the original geometry without the wirepath. 1. From the Backplot menu, choose Display then select Save as geometry and Session. This setting continues to save the wirepath every time you run a backplot until the end of the session (when you exit Mastercam). The dialog box should look like the following picture. 2. Select Save to a Level to activate the feature and enter 255, if necessary.
Notes: If you select Now, Mastercam saves the wirepath once only when you next run the backplot. If you select Always, Save as Geometry remains active, continues to save until you exit Mastercam, and is active when you run Mastercam again. Save as Geometry is not active by default. Caution: Save as Geometry does not replace existing data; it adds to it. If you save the same backplot multiple times, you will get duplicate entities. 3. Choose OK, then choose Run to backplot the wirepath. 4. Choose Backup to return to the Operations Manager, then choose OK to close it.
- 61 -
Emilian Popa
Mastercam Mill 2008
5. To turn off wirepath display (that is, the wirepath geometry that you saved, not the actual wirepath), choose Level from the Secondary Menu.
6. The Level Manager opens. Similar to the Operations Manager, the Level Manager provides center control for levels. In the List levels group, choose Used to display only the levels that are used in the part. These should be three levels and all should have checks in Visible column, indicating that they are currently visible. 7. Select the check mark next to level 255 to clear it. This setting will display all data except than on level 255 (the wirepath data). The dialog box should look like the following picture.
8. Select OK 9. Right-click and choose Repaint. The part displays without the wirepath. 10. Choose Level from the Secondary Menu, and select level 255 in the Visible column to make it visible. 11. Choose OK to close the dialog box. The wirepath again displays. - 62 -
Emilian Popa
Mastercam Mill 2008
12. To cancel the Save as Geometry option, choose NC utils, Backplot, Display and select Save as Geometry to clear the check box. 13. Choose OK to close the dialog box. In this chapter, you programmed a wirepath containing multiple contours and explored modifying a wirepath by adding a glue stop and changing the order of machining. In the next chapter, you will program another wirepath type the no core wirepath. Creating No Core Wirepaths In past, you learned about contour wirepaths, which cut an outline. In past you saw that Mastercam helps you simplify programming by allowing you to combine multiple wirepaths into a single operation with a single set of parameters. In this chapter, you will examine no core wirepaths, which pocket out areas of material by removing all the material within a boundary without producing sliver or slugs. A no core wirepath typically starts at a pre-drilled hole in the material and zigzags or spirals outward until all material within the chained geometry is removed. Mastercam provides several different no core wirepath patterns to accommodate a wide variety of geometry. A no core wirepath may be defined by both an inner and an outer boundary, and the inner boundary may form an island within the no core area. It is important to realize that the island represents material that is removed in a separate machining operation. It is usually a pre-existing void, not material to be retained. For this reason, a no core wirepath can pass across this area which, in other wirepaths or machine toolpaths, would be considered an error.
- 63 -
Emilian Popa
Mastercam Mill 2008
In this chapter, you will learn how to perform the following tasks: - Preselecting a configuration file - Chaining a part for a no core wirepath - Setting no core wirepath parameters - Checking for and correcting slivers and slugs - Modifying the wire power setting library The part you will use is a small die with small openings (0.036 inch channels and a 0.14 inch cavity). The thread, cut, and start points have been predefined.
Preselecting a configuration file The configuration file contains defaults for many Mastercam settings, including memory allocations, tolerances, file locations, and screen settings. When you start Wire, Mastercam selects one of the two standard files as the current configuration file- either wire9.cfg for English (inch) units or wire9m.cfg for metric units. You can also preselect a specific configuration file. When you preselect a configuration file, it becomes the current configuration file when Wire starts, and it controls configuration settings. To do this, you will alter the command used to launch Mastercam. 1. If you did not exit Mastercam at the end of the last chapter, exit now.
2. Right-click the Mastercam Wire icon on the desktop. Tip: You can also choose Start, Programs, Mastercam 9 and right-click Wire 9. 3.Choose Properties from the menu.
- 64 -
Emilian Popa
Mastercam Mill 2008
4.Choose the Shortcut tab in the Properties dialog box. 5. In the Target field, position the cursor at the end of the path name and type [space] followed by the configuration file name. For example: C:\Mcam9\Wire9.exe myconfig.cfg
- 65 -
Emilian Popa
Mastercam Mill 2008
6.Choose OK 7. Double-click the Wire icon to start Wire 8.Choose Screen, Configure. Msconfig.cfg is the current configuration file and will be whenever you start Mastercam. 9. Choose OK to close the dialog box. Note: You can change the current configuration file at any time by choosing Main Menu, Screen, Configuration and choosing a configuration file from the Current configuration file pull-down menu.
Chainin a part for a no core wirepath In this exercise, you will program the no core wirepath to have a finish contour operation that Mastercam automatically generates without requiring you to rechain geometry. Getting the part file 1. Choose Main Menu, File, Get 2. Navigate to the directory with the English tutorial parts. 3. Select Wire Tutor NoCore.mc9 then choose Open. Mastercam opens the part in the graphics window. - 66 -
Emilian Popa
Mastercam Mill 2008
Controlling wirepath display Before chaining the geometry, you will set some system configuration values that control wirepath display. 1. Choose Main Menu, Screen, Configure and choose the NC Settings dialog box tab. 2. Select the Preview all wirepaths check box to clear it, if necessary. As you saw in the precending chapter, the Preview wirepath option gives you the opportunity to review and accept or reject each operation as you generate it. Disable it will speed this exercise.
- 67 -
Emilian Popa
Mastercam Mill 2008
3. Choose the Screen dialog box tab. 4. Select the Draw stop/info/regs and Draw thread/cut symbols check boxes to activate them, if necessary.
5. Choose OK 6. Choose Yes to save the settings to the configuration file. Chaining the geometry 1. Choose Main Menu, Wirepaths, No core. The Pocket: Select chain 1 menu displays. 2. Select the contour near the thread point as shown in the following picture. Note: When you program a no core wirepath to have an automatically generated finish contour, as yo will in this exerciser, you must select the boundary chain at a point close to the thread and cut points because the finish contour will start at this point. If you do not program an automatically generated finish contour, you can select the no core boundary chain anywhere.
- 68 -
Emilian Popa
Mastercam Mill 2008
Mastercam highlights the entire contour, indicates the chain direction, and allows you to select a second boundary. You will not chain a second boundary for this operation.
3. Choose Done. The Wire No Core dialog box opens. Setting no core wirepath parameters In this exercise, you will program the o core wirepath to thread and cut at a pre-drilled hole, lead out with a radius, and automatically generate a fimish contour. Setting the Wire parameters 1. Choose the Wire Parameters dialog box tab, choose Select Library, and navigate to - 69 -
Emilian Popa
Mastercam Mill 2008
Mcam9\Wire\Power\Mits\English\010 DiaBrass Wire 2. Select ST_0500_3_RA32.wp9 and choose Open. 3. Select Associate to library to clear the check box. The wire parameters become available for editing. 4. For Stock to leave, enter 0.004. This setting will leave some stock after the no core operation for the final skim contour operation. Note:This change will be applied only to this part. To make the change part of the power settings library and available to other parts, you would choose Save library. You will not save the change for this exercise. The Wire Parameters dialog box should look like the following picture.
Setting the No Core parameters 1. Choose the No Core dialog box tab. 2. Enter a Rapid Height of 0.53 (absolute) to clear the top of the stock and any clamps during rapid moves. 3. For the UV Trim Plane, enter 0.50 (absolute) for the height of the upper wire guides. 4. For the UV Height, enter 0.50 (absolute), which represents the stock thickness. 5. For the XY Height, enter (absolute), which represents the bottom of the stock. 6. For the XY Trim Plane, enter (absolute) for the position of the lower wire guides. - 70 -
Emilian Popa
Mastercam Mill 2008
7. Make sure Auto entry at the bottom left pg the dialog box is selected, which causes Mastercam to start cutting at the thread point. 8. Make sure Auto exit is selected, which cause Mastercam to cut the wire at the cut point. Note: If you clear the Auto entry exit check boxes, Mastercam calculates start and exit points for the no core wirepath, which may be different from the thread and cut points. The No Core dialog box should look like the following picture:
Setting the Lead in/out parameters 1. Choose the Lead in/out dialog box tab. Notice that there are no settings for tab lead in and lead out because no core wirepaths do not use tabs. 2. For Lead in, select Line and radius. 3. For Lead out, select Radius and line. 4. If necessary, select Auto position cut point to activate it. This allows Mastercam to determine the best cut point for the contour. In this operation, Mastercam uses the previously defined cut point because you select Auto exit and No core dialog box tab. 5. If necessary, select Auto start position to activate it. This moves the job start to the thread point. 6. Use the default values for the remaining settings. The dialog box should look like the following picture. - 71 -
Emilian Popa
Mastercam Mill 2008
Setting the Roughing/Finishing parameters 1. Choose the Roughing/Finishing dialog box tab. This dialog box contains parameters that control the cutting method and finish cuts for no core wirepaths. 2. Select the Parallel Spiral cutting method icon, which cuts pockets by spiraling outward within the boundary, offsetting each pass by a specified stepover amount. 3. Enter a Stepover percentage of 50 to eliminate slivers. 4. Make sure the Optimize path check box is selected. (You will learn more about this option in the next exercise.) 5. Select Add finish contour operation to automatically add a finish pass a separate operation. Note: Mastercam can add the automatically generated finish contour operation only when you first define the no core wirepath. You cannot automatically generate it later; the check box will be disabled. 6. The Roughing/Finishing dialog box should look like the following picture.
- 72 -
Emilian Popa
Mastercam Mill 2008
7. Choose OK. The Wire Contour (No Core Finish) parameters dialog box opens to allow you to program the automatically generated finish contour. Setting the finish contour wirepath parameters The automatically generated finish contour is a separate contour wirepath that can have different parameters and will be listed as separate operation in the Operations Manager. 1. On the Wire Parameters dialog box tab, choose Select Library 2. Navigate to: Mcam9\Wire\Power\Mits\English\010 Dia Brass Wire\ST_0500_3_RA32.wp9 3. Choose Open. This is the same library that you used for the no core operation. Notice that there is no stock to leave amount because you did not save the change you made in the no core operation to the llibrary. 4. Because this is a finishing operation consisting of a single pass, you will program a lower setting appropriate for a skim cut. To do this, set the Starting pass # to 2. 5. Choose the Contour tab. Mastercam automatically inserts the values from the no core operation. Use the default values for the remaining parameters. The dialog box should look like the following picture.
- 73 -
Emilian Popa
Mastercam Mill 2008
6. Choose the Lead in/out dialog box tab, then select Line and radius for Lead in and Radius and line for Lead out. The dialog box should look like the following picture. Make any necessary adjustments.
- 74 -
Emilian Popa
Mastercam Mill 2008
7. Choose the Cuts dialog box tab. 8. The Perform rough cut check box should be selected. Remember that you set this contour operation to start with the Pass 2, so it will not use the rough cut power setting. You should have an operation consisting of a single rough cut as shown in the following picture.
9. Choose the General dialog box tab. Use the default settings. The dialog box should look like the following picture.
- 75 -
Emilian Popa
Mastercam Mill 2008
10. Select OK. Mastercam displays the wirepath.
11. Save your file. Be sure to use a fillerent name. Tip: Using AutoSave ([Alt +A]) is a quick way to save automatically. Checking for and correcting slivers Mastercam makes it easy to check for and minimize slivers of material than can drop out of the part. Use the Backplot function with the Verify option turned on to display the no core wirepath so that you can see slivers. The Optimize part feature on the Roughing/Finishing wirepath parameters tab checks for and adjusts the wirepath to eliminate dropouts. This feature is enabled by default and should be enabled in most cases. In this exercise, you will disable it to investigate its function. Note: The Optimize feature cannot be used with the Morph or True Spiral wirepaths. Backplotting the wirepath 1. Press [Alt + O] to open the Operations Manager. You will see two operations – the no core operation and the contour operation. 2. Select the Wire No Core operation, then choose Backplot.
- 76 -
Emilian Popa
Mastercam Mill 2008
3. The Backplot menu displays, Toggle Verify to Y. Press and hold [S] to step through the backplot while watching for slivers, which would appear as black areas in the gray wirepath. The following picture illustrates the backplot and shows on sliver formation.
4. Choose OK when the backplot is complete. Examining the wirepath without optimization 1. Choose Backup to open the Operations Manager. 2. Select the Parameters icon of the Wire No Core operation.
- 77 -
Emilian Popa
Mastercam Mill 2008
3. Select the Roughing/Finishing dialog box tab. 4. Clear the Optimize path check box.
5. You will change the library to lower the power setting so that you can see a sliver. Choose the Wire Parameters dialog box tab, then choose Select Library. 6. Choose No in response to the Edit Power Settings warning message. Mastercam displays this warning because you deactivated the Associate to library option and entered a Stock to leave value. 7. Navigate to: Mits\English\006 Dia Brass Wire\ST_0050_3_RA16.wp9 8. Make sure the Associate to library check box is not checked, then enter a Stock to leave of 0.004. Regening and displaying the wirepath
- 78 -
Emilian Popa
Mastercam Mill 2008
1. Choose OK. Mastercam opens the Operations Manager and marks the operation for regeneration. 2. Choose Regen Path, then choose Backplot. 3. Press and hold [S] while watching for slivers. 4. Release it when you see a sliver appear. The un-optimized wirepath may contain other slivers. The following picture shows an example of a sliver. (The colors have been inverted to make it easy to see the sliver.)
5. Choose Backup to stop the backplot, then choose OK in the Backplot complete message. Re-enabling the Optimize feature 1. Choose Backup to open the Operations Manager 2. Select the Parameters icon of the Wire No Core operation. The Wire parameters dialog box opens. 3. On the Roughing/Finishing dialog box, select the Optimize path check box to activate it. Note: The No Core Optimize path option should normally remain active to reduce the possibility to creating slivers. The Optimize path option was turned off in this example only to show that slivers are much more likely to occur when Optimize path is off. Please check your part carefully for slivers, since they can cause damage to the wire EDM machine tool.
- 79 -
Emilian Popa
Mastercam Mill 2008
4. Choose OK. The Operations Manager dialog box opens. 5. Choose Regen Path. Mastercam regenerates the wirepath. Simulating machining with wirepath verification Now that you have created and checked the no core wirepath, you will examine the wirepath in the stock using the Verify function in the Operations Manager. The Verify utility is different from the Verify option in the Backplot menu. The Verify utility simulates the machining operation in three dimensions and provides features that allow you to examine the machining operation in various ways (such as stock cross section). Backplot verify provides a quick machining simulation for 2D parts. Configuring the simulation 1. Choose Select All to select both operations 2. Choose Verify. The Verify toolbar opens. 3. Choose the Configure toolbar button to set the parameters that control the appearance of the Verify display.
- 80 -
Emilian Popa
Mastercam Mill 2008
4. The Verify Configuration dialog box opens. For Stock Shape, select Box. 5. For Boundaries, select the Scan toolpath(s) button to scan the no core toolpath to calculate appropriate stock size. 6. For the X Margin and Y Margin, enter 0.1 which provides a margin around the part in the stock. Without a margin, the edge of the part will lie on the edge of the stock. 7. Select the Translucent stock check box, which will leave the stock transparent after Mastercam completes the machining simulation. 8. Drag the Display Control Speed/Quality slider all the way to the right to maximize the display quality. The Verify Configuration dialog box should look like the following picture.
9. Choose OK. The Verify toolbar reopens. Running the simulation
1. Choose the Machine (play) button. Mastercam animates the machining operation in three dimensions.
- 81 -
Emilian Popa
Mastercam Mill 2008
2. To examine a cross section of the part, choose the Stock section button.
3.The prompt area tells you to select a section reference point, which is the position on the stock where you want to slice it. Try to select the stock in the approximate position shown in the following picture. 4. Select a point on the stock on the side that you want to keep.
Mastercam displays the cross section. Your part should look similar to the following picture depending on the positions you selected.
- 82 -
Emilian Popa
Mastercam Mill 2008
5. Close the Verify toolbar. 6. Close the Operations Manager Tip: Use the following buttons control simulation: To pause the machining simulation ay any time, choose the Pause button. To continue simulation uninterrupted, choose the Machine button. To continue simulation one step at a time, choose the Step button. Modify the power settings library In this exercise, you will modify the power settings library you used for the finish contour. Because you associated the wirepath operation in the contour operation (not the no core operation) to the power settings library on the wire parameters dialog box, shown in the following picture, changes to the library will be reflected in all operations associated to it. Be sure to use this feature carefully.
- 83 -
Emilian Popa
Mastercam Mill 2008
Mastercam will alert you to change and allow you to update the wirepath after you modify the library. Editing the power settings library 1. Choose OK to close the Operations Manager. 2. Choose Main Menu, NC utils, Power set. The Edit Library dialog box opens. 3. Choose Select Library, navigate to: Mcam9\Wire\Power\Mits\English\010 Dia Brass WireST_0500_3)RA32.wp9 and choose Open. 4. For the Pass 1 Feedrate, enter 0.1. The dialog box should look like the following picture.
Tip: If you wanted to change the wire power settings for other passes, press [Page Up] or [Page Down] to change the pass number. 5. Select OK. The Specify Power Setting Library to Write dialog box opens. 6. Select Save. Mastercam warns you that the library already exists as shown in the following picture.
7. Select Yes. Mastercam warns you that operations using this library will require regeneration.
- 84 -
Emilian Popa
Mastercam Mill 2008
8. Select OK. Regenerating the wirepaths 1. Press [Alt + O] to open the Operations Manager. The contour operation has been marked for regeneration because the library changed, even though the change is to a pass that is not currently used in this operation. The no core operation has not be marked because it was not associated. 2. Select the Wire Contour operation.
3. Choose Regen Path to regenerate the wirepath. 4. Choose OK to close the Operations Manager. 5. Save the file. Note: Unless you want the feed rate for the power setting library to remain 0.1, repeat the steps in the section titled “Editing the power settings library”. For Pass 1, enter 0.16 for the feed rate and save the library. In this chapter, you programmed a wirepath to pocket out a small part, included an automatically generated finish pass, and saw how the Optimize path feature can eliminate slivers. You also demonstrated how associativity can allow a part program to accommodate changes to a wire power settings library. In the next chapter, you will learn how to create multiple tabs on a contour and to change wirepath parameters such as taper angle and corner type in sections of the wirepath
- 85 -
Emilian Popa
Mastercam Mill 2008
- 86 -
