Brief Introduction to MasterCAM X4

Transcription

1 Brief Introduction to MasterCAM X4 Fall 2013 Meung J Kim, Ph.D., Professor Department of Mechanical Engineering College of Engineering and Engineering Technology Northern Illinois University DeKalb, IL

2 Preliminaries C-Plane: flat construction plane that can be used for sketching T-Plane: flat machinable plane MMB to rotate the model in graphics window Alt + MMB (middle mouse button) to pan Selecting WCS and changing Z level Hint appears at top of graphics window If some entities cannot be selected sometimes in graphics window (i.e., bug), use Unhide/All to show all entities and select. For Chain, the line segments in the curve must be tangent. If the curve is closed, use Loop. Settings o Configurations > see or change Units o Colors > Graphics background color > change it if needed

3 I. Sketching and Editing T/Cplane and WCS (Tool / Construction Plane and World Coordinate System) 1. Construction plane is the plane where any geometry can be constructed and Tool plane is the plane perpendicular to tool axis for machining. 2. The default level of T/Cplane is at Z=0.0 with x-y axes on the plane aligned with WCS:TOP. Any sketches are added on this plane. 3. Change the WCS and Z value to change the sketch plane. 4. Change the view to isometric view by right clicking on the graphics window and selecting it. 5. Any sketched entities can be selected and deleted. Sketching 1. Sketching menu is shown below. 2. The sketch menu of Line is shown below. 3. Starting point can be picked on the graphics window. Alternatively, entered above. 4. Further, Fast Point can be used to enter x,y,z values quickly. 5. Enter or select appropriate values and options. 6. Pick the second point and further change any values/options > Apply or OK Analyze

4 7. This menu can be used to analyze and modify properties of entities. Sketch a circle > OK 8. Analyze > Entity Properties > pick the circle > change any properties > OK Transform 1. XForm menu (XForm, Translate, Rotate, Mirror, Scale, Translate 3D, Offset, etc.) is shown below. Use ESC to cancel. 2. The following shows Dynamic Translate dialog. Pick any to move > End Selection button > use either incremental Delta or From/To to specify the distance. 3. For Dynamic Transform, pick any entities to transform > End Selection > gnomon triad appears > anchor it to a starting position > move mouse over lower end of any axis to move and click, otherwise, move over higher end of the axis to rotate and click > the attached gnomon can be move or rotated to another position > click at a new position > [user can cancel by successive ESC any time] > OK

5 Surface 1. Create > Surface > Flat boundary > pick closed boundary like a circle or polygon 2. Alt + G > check both Active and Visible grid > OK 3. Isometric (WCS) > Cplane = Front (WCS) 4. Create arc three points > pick any three points to sketch the arc > OK 5. Xform translate > pick the arc > End selection > check Join > enter a value for Z (make it long) > OK 6. Xform translate > pick either arc > End selection > check Copy > enter a value for Z and Y to copy it below in the middle > OK

6 7. Create > Surface > Net > pick all four joined lines in sequence (directions don t matter) and then the copied arc (see the second above) a. Choose Across for Style (the last arc is not included. See the third) b. Choose Average (average is used between two entities. See the last) 8. Change to 2D for sketching 9. Circle a. Sketch a circle b. Change Z-value to 10 > sketch another circle c. Change Z-value to -8 > sketch another circle > OK 10. Create/Surface > Rules/Lofted > pick three circles in sequence and make sure the directions are all same > Style = Lofted (see above middle) > Style = Ruled (see right) 11. 3D > Z = 0.0 > Sketch a closed figure as 12. Create/Surface > Revolved a. Chain > pick a point on the figure > OK b. Angle = 180 c. Select the horizontal line for the axis of rotation (see above) 13. Front (WCS) > sketch a spline > OK 14. Isometric (WCS) > sketch a circle at an end point of spline

7 15. Create/Surface > Swept a. Across contour > pick the circle > OK b. Along the curve > pick the spline > OK

8 16. Starting with 2D/3D Contours Contour 1. Machine Type > Mill / Default 2. Now, user needs toolpaths. 3. Line > sketch lines starting at (1,1,0) with horizontal length of 4 and the rest of lines have length of Stock Setup > All Entities > add a little more space for each if needed as shown below > OK. Note that Stock Origin is the position at top surface of stock and the depth is given by Z value. 5. Toolpaths > Contour > enter a name > selection dialog appears as

9 6. Select the line and choose the direction 7. Toolpath dialog appears 8. Toolpath Type = Contour. Other toolpath can be chosen here Also, see Chain geometry if needed.

10 9. Tool > enter tool diameter = 0.25 and other parameters as below, otherwise, use the tool library. 10. Holder = no holder display 11. Cut Parameters > Depth Cuts = check Depth cuts / Max rough step = Linking Parameters: Depth = -0.5 and change others as needed > OK 13. Click the tool in OM > change any parameters as needed > see Type > Parameters tab > Rough XY step (%) = 25 [this cannot be zero] and Rough Z step = 0.25 > OK 14. Right click Toolpath in OM (Operations Manager) > adjust the speed and play, see below > OK 15. Right click the graphics window > WCS:TOP > see the toolpath above right. 16. The toolpath display can be toggled on/off by 17. Observation a. Tool moves to retract plane above the approach point and plunges to feed plane, then plunge cut first and follows the toolpath.

11 b. Approach/Exit movements are along tangent arcs. c. Toolpath compensation is to left to the toolpath. 18. Click Parameters in OM > Cut Parameters > change the tool compensation direction to Right > (It can be turned off if not needed) > OK 19. Play the toolpath simulation and see it. Observe the Approach/Exit movements. 20. Back to Parameters in OM > Lead In/Out > see the approach/exit parameters as 21. Also, see Linking Parameters as

12 Pocket 1. Using same as above for most, sketch a similar pocket shape as below 2. Toolpaths > Pocket a. Choose Loop b. Pick the contour > switch the direction if necessary c. Linking Parameters > Depth = > OK Facing 1. Use same contour for face milling 2. Toolpaths > Face a. Choose Loop b. Pick the contour > switch the direction if necessary c. Linking Parameters > Depth = > OK

13 3. Note that face milling uses two opposite boundaries to cover the area between them. Also, the tool moves out of the boundary. Contour (3D) 1. Sketch as below using WCS (TOP, FRONT, RIGHT), Dynamic Transform 2. Stock Setup 3. Toolpaths > Contour a. Loop > pick the contour > switch the direction if necessary b. Toolpath Type = Contour c. Tool = ¼ Flat End Mill d. Linking Parameters > Depth = > OK

14 Tplanes (3D) 1. Create Block a. Fast Point > enter 0,0,0 > CR b. Check Solids c. Enter 5, 4, and 3 for size > OK d. Right click on graphics window > Isometric View e. Zoom Fit or scroll up/down and alt + move to position the block f. Polygon > Fast Point > enter 2.5,2,3 > CR > check Corner and enter 5 for number of sides as below > OK g. Gview (at bottom status bar) > View by Solid Face > pick the front face > accept the orientation h. Sketch a rectangle with round corners as 2. Toolpaths > Drill a. Pick all five corners of pentagon at top > OK b. Tool > Select library tool > ¼ Drill > OK c. Linking Parameters > enter as below > OK

15 3. Stock Setup > All Entities > OK 4. Play and see the drilling as 5. Gview > View by solid surface > pick the front face > OK 6. Sketch a rectangle with corner rounds 7. Toolpaths > Pocket a. Chain > pick the front rectangle > OK b. Linking Parameters > Depth = -0.5 > OK c. Play and see above right 8. Gview > View by solid face > pick the right face > OK 9. Sketch another rectangle on rightside face 10. Toolpaths > Pocket a. Chain > pick the front rectangle > OK b. Linking Parameters > Depth = 4.5 > OK 11. Select Toolpath Group-1 in OM > Verify selected operation > play and see as

16 12. See also the toolpath with point-to-point (PTP) motion in light yellow color and the machining in light blue. 13. Parameters of first Pocket in OM > Entry Motion > Off > OK > Back plot 14. Post a. Check NC file / Edit / Ask > OK b. No c. Enter a name for NC file > CR > NC file appears as below > read and understand each line. Observation: A-90 changes the Tplane with a local coordinates.

17 2D High Speed This has several toolpath type as shown below. 1. Toolpaths > 2D High Speed a. Pick the first contour > change direction if needed > pick the second contour > OK b. Toolpath Type = Blend Mill c. Tool = 0.25 flat end mill d. Cut Parameters > Cutting method = Zigzag (see also other options) > see also option of Across/Along > Max stepover = 0.1 e. Linking Parameters > Depth = > OK f. Right click Toolpath in OM > play and see g. Parameters in OM h. Change Toolpath Type = Peel Mill i. Rounding radius = 0.25, Stepover = 0.25 j. Linking Parameters > Depth = > OK k. Right click Toolpath in OM > play and see

18 l. Delete the contour and sketch two others as below (use Line, Offset, and Fillet) m. Parameters in OM n. Change Toolpath Type = Core Mill o. Geometry in OM > right click the collector > Add Chains > add first chain > Add Chains > add the second one p. Right click Toolpath in OM > play and see q. Parameters in OM r. Change Toolpath Type = Area Mill s. Right click Toolpath in OM > play and see t. Parameters in OM u. Change Toolpath Type = Dynamic Mill v. Right click Toolpath in OM > play and see

19

20 17. Starting with 3D Model Case 1. Sketch 2D shape and extrude features. 1. Alt + g for Grid > check Acitve grid and Visible grid > OK 2. Solids > Extrude a. Loop > pick a line on inner loop of outline > make sure the loop direction is CW > OK b. Cut Body > Extend by specified distance/distance = 0.25 > OK c. Repeat this for obround with depth = 0.5 > OK d. Repeat it by selecting four holes in CW with Extend thru all > OK 3. Machine Type > Mill > Default 4. Expand the Generic Mill in OM > Stock Setup a. Select corners > select two diagonal corners with some materials on sides b. Enter the depth = 1 > OK 5. Add another sketch around the workpiece 6. Toolpaths > 2D High Speed a. Pick the loop on workpiece and the loop of part outline > OK b. Tool Type = Core Mill c. Tool > select one inch tool d. Linking Parameters > Depth = -1.1 > OK e. Verify> choose Turbo 7. Toolpaths > Surface Rough > Pocket a. Pick the surface of part at top b. Select the 1/2 inch tool > OK c. Verify > choose Turbo

21 8. Toolpaths > Drill a. Pick all four holes at centers > OK b. Toolpath Type > Drill c. Tool > Filter > select the drill tool > OK > select 1/8 Drill > OK d. Break Through > check Break through > Break through amount = 0.1 e. Linking Parameters > Depth = -1 > OK 9. Select Toolpath Group-1 in OM > choose Tool > Verify Case 2. Based on a MasterCam X example, produce a revolved cut on a block by Surface High Speed (i.e., roughing), Surface Finish, Surface Finish Leftover. Then, create a word CAM by Pocket on the top surface and project it onto the bottom of the previous cut. Also, learn to correct tool handle interference by Surface Finish Pencil. Note that Surface High Speed milling can find all surfaces and machine them. However, the tool must be small enough to fit the surfaces to machine them. Otherwise, it skips any unfit surfaces. Further, if the step depth is greater than the depth of any surface, it also skips.

22 1. Alt + G for Grid > check Acitve grid and Visible grid > OK 2. Create Line End Point > sketch a vertical line from the origin with length 5 > OK 3. Create Line Parallel > pick the line > click a point on the right > enter the distance 2 > CR > pick the same first line > click a point at distance 2 to right > OK 4. Create Line End Point > sketch a horizontal line at bottom and at top, and an inclined line with angle 290 as 5. Create Arc Tangent > Tangent Point > enter radius 2, pick the inclined line 1 and the end point 2 of bottom horizontal line > click the part to keep at 3 > OK 6. Trim/Break/Extend > Trim 1 Entity > click the inclined line to trim and click the line to trim > OK 7. Delete entities > pick both vertical lines on the right > End Selection 8. Fillet > enter the radius and pick both lines at upper right corner > both lines at lower right corner > OK 9. Create > Letters > enter CAM > select True Type > Arial/Bold/12 > OK > pick a starting point > ESC (done)

23 10. Click a lower left corner, hold down LMB, drag to another corner, click to select the text just created > Xform Translate > check Move > From/To > pick starting and ending point to translate > OK (may repeat to place it at proper position) 11. Clear Colors (2 nd of toolbar) 12. Shift + pick a line in the loop > Xform Mirror > check X-axis in dialog > OK 13. Clear Colors 14. Isometric View > Fit > alt + g > uncheck both Active and Visible grid > OK 15. Create / Surface / Revolved > pick a line on right side and then the line at center (to complete a loop) > OK > enter the angle 180 > pick the line at center for rotation axis > choose correct side by > OK 16. Delete entities > pick the line at center (two of them) > Done Selection > refresh the screen > repeat this to delete another line at same position (see above right) 17. Top (WCS) 18. Create Rectangle > click Anchor to Center and Create Surface > sketch a rectangle starting from the center > OK 19. Isometric (WCS) > Fit > pan the geometry by alt + MMB 20. Create > Surface > Trim > To Curves > pick the plane > Done Selection > Loop (or Chain) > pick a point on the curve along the edge of revolved surface (it s a loop showing only an arrow on top of ending arrow) > Done Selection > pick a point on plane to keep and then pick another point > OK 21. Expand Generic Mill in Operations Manager (OM) a. Stock setup > Bounding box > increase the depth by 1 > OK > OK 22. Toolpaths > Surface High Speed

24 a. Enter a name > OK > All > OK > Done Selection > OK b. Toopath Type = Area Clearance c. Tool > Select library tool > #294: 1 inch Bull End Mill with Cor. Rad > OK d. Holder > Open Library > C40.holder > OK > C2C e. Cut Parameters (accept defaults) f. Linking Parameters (accept defaults) g. OK (dialog) 23. Click Back plot selected operations in the menu or OM > Play 24. Verify selected operations or right click Toolpath in OM > play and see above. a. User can select Tool Holder to display. b. Turbo for fast simulation. c. Also, control the simulation speed bar as needed. 25. Toolpaths > Surface Finish > Contour a. All > OK > Done Selection b. Containment in Toolpath/surface selection > try to pick a point on looped edge of revolved surface. If no edge can be selected, then, try Unhide some > All > OK > Done Selection > Loop or Chain option > retry to pick the loop (there must be only one arrow that overlaps the ending arrow) as below > OK c. Select library > 1/2 Ball End Mill #256 d. Surface parameters > see e. Finish contour parameters > see > OK 26. Click Only display selected toolpath in OM > see the toolpath (above right) 27. Select Toolpath Group-1 in OM > Verify selected operations a. Select Simulate tool and holder > Play b. See the interference of handle with workpiece

25 28. Toolpaths > Surface Finish > Leftover a. All > OK > Done Selection b. Select library > Filter > select only Ball End > OK > 1/4 Ball End Mill #252 c. Surface parameters > see d. Finish leftover parameters > see > OK e. Verify selected operations > (if no material is left over, an error message appears) > play and see (no good) f. Select Toolpath Group-1 in OM > Verify selected operations > play and see more handle interference with stock (will be fixed later) (above right) 29. Click the insert arrow in OM > move it up 30. Select each operation in OM > click Toggle display on selected operation to turn off > repeat for all to turn off 31. Create > Surface > Offset > pick all revolved surfaces > Done Selection > enter offset 0.25 > choose the offset side to outside > OK 32. Clear Colors 33. Top (WCS) 34. Create Rectangular Shapes > Obround > select obround for shape > pick the center point in graphics window > click center for Anchor > sketch the obround > OK (see below left) 35. Toolpaths > Pocket a. Window > capture the obround and text by Window menu (see below middle) > pick a point on obround edge for approximate starting point > OK b. Tool > 1/8 Ball Mill #249 > accept default for all others c. Choose a handle like C4C d. Linking Parameters > Depth = > OK e. Verify selected toolpath > play and see below right

26 36. Toolpaths > Surface Finish > Project a. Pick both offset surfaces at bottom > Done Selection > OK b. Tool > 1/8 Ball Mill > accept default for all others c. Finish project parameter > Projection type = NCI > check Pocket operation > OK d. Backplot selected operation > OK e. Select Toolpath Group-1 in OM > Verify selected operations > play f. There is interference of tool handle with workpiece that must be fixed. 37. Right click and hold down Pocket operation in OM, drag down a little, and release > Copy after 38. Click Parameters of copied operation a. Tool > select tool #242 from the library b. Cut parameters > Pocket type = Remachining c. OK 39. Regerate all dirty operations in OM 40. Ctrl + pick Pocket (Standard) operation and Surface Finish Project in OM (only last one is highlighted) to select multiple operations > Verify selected toolpaths > see the toolpath simulation 41. Toolpaths > Surface Finish > Pencil a. Pick both offset surfaces > OK b. Tool > 1/8 Ball Mill > accept default for all others > OK 42. [Fixing handle interference] Select Surface Finish Leftover in OM

27 a. Alt + C b. Select CheckHolder.dll > enter the Holder clearance of 0.05 and defaults for all others c. Perform test > if there is interference in the test result, click Modify source operation d. Toolpath Group-1 in OM > Verify selected operations > select Stop after each operation or Stop after collision > play to find out problem operations e. Repeat checking and modifying the tool holder length for all operations where tool interferes with workpiece. f. Run the verification of the toolpath group and see it (above right) 43. Turn off Quick verify in Back plot selected toolpath and see the cutter location (CL) points. Case Create Block > enter width=5, depth=4, and height=1 and then starting position X=0, Y=0, Z=0 > OK 2. Create Cone > enter the base radius=1, the top radius=1.5, and the height=1 > Fast Point > enter the position at bottom center of the block as 2.5,2,0 > OK 3. Stock Setup in OM > enter as below 4. Toolpaths > Surface Rough > Parallel a. Cavity > OK > enter NC name > OK > pick the cone > End Selection > OK (toolpath/surface selection) > OK (Surface rough parameters) b. Click the tool in OM > enter sizes as

28 c. Geometry > pick the cone > OK d. Parameters > just use the defaults e. Right click Toolpath > play and see the result 5. Toolpaths > Surface Rough > Radial a. Cavity > OK > enter NC name > OK > pick the cone > End Selection > OK (toolpath/surface selection) > OK (Surface rough parameters) b. Pick the bottom center of cone as the radial point c. Right click Toolpath > play and see the result 6. Toolpaths > Surface Rough > Pocket

29 a. Pick the cone > End Selection > OK (toolpath/surface selection) > OK (Surface rough parameters) b. Pick the bottom center of cone as the radial point c. Right click Toolpath > play and see the result 7. Toolpaths > Surface Rough > Flowline a. Pick the cone > End Selection > OK (toolpath/surface selection) > OK (Surface rough parameters) > OK (Flowline data) [the cone surface becomes flowline]. b. Right click Toolpath > play and see the result

30 18. Starting with External Model Case 1. Pro/E Part File 1. Create a model in Pro/E or any CAD software. Alternatively, the model can be created within MasterCAM. 2. Open the file that was created in other CAD program. The following shows the imported model created in Pro/E [the file extension must be *.prt]. 3. Alt + G and check both Active and Visible grid 4. Isometric (WCS) > rotate it a little and see 5. The milling operation requires the z-axis aligned to the tool axis. In this model, the z-axis was not aligned with z-axis. a. XForm > Dynamic XForm c. All > OK > End Selection d. Anchor the gnomon axes at lower left corner e. Choose Move option. f. Move the mouse over the gnomon axes (below or above axis name) to display the translation or rotation marks as above g. Right (WCS) h. Anchor it at top left corner i. Click the Y or Z axis name for rotation > rotate place the model by 90 degrees CCW j. Isometric (WCS)

31 k. Click to select translation in X-axis > move the point to X = 1 position l. Click select translation in Y-axis > move the point to Y = 1 position m. Top (WCS) > see it n. OK 8. Isometric (WCS) > Fit and zoom in/out with MMB 9. Alt + G > turn off the grid 10. Expand Default Generic Mill in OM > Stock setup a. All Entities > OK

32 11. Clear Colors 12. Toolpaths > FBM Mill (feature-based milling) a. Click OK to accept the values in the dialog as it is (see below)

33 b. Enter a new NC name > OK c. The automatically generated processes appear in OM along with the toolpaths generated as d. Move the mouse over Toolpath for 2D High Speed (2D Core Mill) in OM and right click to bring Verify selected toolpath dialog as

34 e. Adjust the speed control and click Play (don t see moving?, then probably too slow) and see the simulation. The above right figure shows the completed part. f. Right click the other process and play the simulation to see the following. g. Out of two processes that were generated automatically, the user may keep either one or both and can modify them further. 13. Add FBM Drill as before from Toolpaths menu > OK (accept all defaults) a. Now, the Operation Manager (OM)/Toolpaths appear as

35 b. Play both sequences of Drill/Counterbore and Peck Drill as before. c. Select FBM Drill in OM > click Verify selected operations menu d. Play the FBM Drill operation and see. e. Click the drill tool in OM to bring up the tool as f. See also the Type tab as

36 g. Select Machine Group-1 in OM just created > click Verify selected operations > Play and see 14. Select 2D High Speed (2D Core Mill) in OM 15. Only display selected toolpath 16. Click Parameters in OM a. Cut Parameters Depth Cuts > check Depth cuts > Max rough step = 0.5 Transitions > Entry method > check Profile ramp > Plunge angle = 45 Linking Parameters > Home / Reference. Points > check both Approach and Retract and enter (0,0,2) for both OK a. Backplot selected operation > turn off Quick verify > see the toolpath cutter location (CL) points. Observe the helical or profile ramp motion has numerous points that slow down the tool motion (see below). b. Verify selected operation > play and see > OK

37 Case 2. IGES File 1. Save a part file in CAD software as *.iges (or *.igs) file 2. Open the file in MaxterCam 3. Dynamic Xform > rotate and translate so that the lower left corner is at (1,1,-2) 4. Expand Generic Mill in OM > Stock setup a. All Entities b. Enter as 5. Using View > Viewport > several views can be manipulated as

38 6. Toolpaths > Facing a. Select library tool > Filter > select only End Mill > OK > choose 1 inch with no corner radius (#243) b. Cut Parameters > Across overlap = 50 (%) c. Linking parameters > Depth = -0.4 > OK d. Back plot in OM e. Verify in OM 7. Toolpaths > Surface High Speed a. All > OK > Done Selection b. Tool > Select 1/2 Flat End Mill c. Cut Parameters > Step down = 0.25 d. Transition > check Profile ramp and Plunge angle = 45

39 e. OK 8. Toolpath Group-1 in OM > Verify > the shallow pocket was not captured 9. Parameters of Surface High Speed > select 1/4 Flat End Mill > OK > Verify and see the above right. Also, the step depth must be less than the pocket depth to capture it in machining. With smaller step depth, use Steep/Shallow > check Use Z Depths and Detect limits. Observation: Using a single Surface High Speed operation may be too costly with small step depth. Use several Surface High Speed operations. 10. For drilling, create points at centers of hole. Analyze > Dynamic a. Click an arc > move the mouse to place the position arrow at one end as below and get y-position b. Move the arrow to top of arc and get x-position c. Repeat this for center position of the other arc 11. Z = -0.3 (z-plane level at just above model) 12. Create > Point > Fast Point > enter the first center > CR > enter the second center > CR 13. Toolpaths > Drill a. Select both centers of hole > OK b. Tool > select 1/2 drill c. Linking Parameters > Incremental and Depth = -1.9 d. OK 14. Select Toolpath Group-1 in OM > Verify

40

41 Problems Problem. 1 Import the dxf file for key-ring in the textbook and contour mill with the one-inch thick workpiece. Use 0.1 diameter tool with left tool compensation. Solution: Problem. 2 Sketch the contour in Example 2 in the textbook and add a point for SP (0,0,0). Create the one inch thick workpiece with some extra materials around. Simulate contour milling with SP as Home/Retract Points. Soultion:

42 Problem. 3 steps. Sketch the shape similarly and machine as shown below. Describe the