Introduction to MasterCAM X4,7

Transcription

1 Introduction to MasterCAM X4,7 Spring 2014 By Meung J. Kim, Ph.D., Professor Department of Mechanical Engineering Northern Illinois University 1

2 Preliminaries C-Plane: flat Construction plane that can be used for sketching T-Plane: flat machinable TOOL plane GW: Graphics Window WCS: World Coordinate System OM: Operations Manager 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 Alt + G to display grids for easy picking (make sure to check Active and Visible grids) 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 2

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. ESC key can be used to cancel any command. Alternatively, End Selection without any sketch done cancels sketching. 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 LINES 3

4 Example 1. Draw a horizontal line from [0,0,0] with size = 2. Select Line menu Enter starting x,y,z. Alternatively, Fast Point and enter 0,0,0 > CR Enter the size Select Horizontal option Move the mouse to the right of starting point and click the graphics window OK (done) User can select any sketched lines one by one or using the rubber-band window, for example, to delete them (hit Delete button) Example 2. Draw am perpendicular line to the previous line at left end. Select Line Perpendicular Pick the line (to which the line will be perpendicular) Select End Point option Pick the left end (the line appears on both sides) Click the side to keep 4

5 Enter the size 3 > CR OK Example 3. Draw a parallel line at the other end point to the vertical line. Parallel Line Pick the vertical line Select End Point option Pick the right end of horizontal line (see above middle) OK Example 4. Draw a bisecting line at the lower left corner. Bisecting Line Pick both lines at lower left corner Enter the size 2 > CR (see above right) OK Example 5. Extend the bisecting line to right and trim the vertical line above the intersecting point. Trim/Break/Extend Pick the line to extend Pick the line to extend to OK Select Trim/Break/Extend from the recent menus on the right toolbar Click the side of the line to keep Pick the line to trim to OK 5

6 Example 6. Create rounds of radius 0.5 at bottom right corner. Fillet Pick both lines at the corner Enter the radius OK CIRCLES/POLYGONS Example 7. Draw a circle of radius 2 and then inscribe a pentagon with the vertex at bottom. Fast Point > enter 0,0,0 > CR Enter the radius 2 > CR OK Create Polygon Pick the center point and drag to inscribe, and place it by clicking Enter the number of sides 5 OK XForm Rotate 6

7 Select all five sides of pentagon > End Selection Check Move > enter the rotation angle 180 User can play with different angles with Preview/Regen button checked OK Example 8. Draw an arc of radius 1/2 between 0 ~ 90 degrees. Alt + g > check both Active/Visible grids > OK Right click on GW > Isometric (WCS) Arc Polar > pick the origin > pick the starting point and ending point OK Example 9. Draw a circle by two points at [0,0] and [1,0] as well as by three points at [0,0], [1,0], and [1,1/2]. Circle Edge Points Select Two point Pick the first point and then the second Select Three point Pick three points OK 7

8 Example 10. Draw an arc by two points at [0,0] and [1,0] in positive y-direction. Arc End Points Select both points Pick a point in positive y-direction to anchor it Enter the radius 0.5 > CR OK Note: If the radius was entered first before anchor the arc, both arcs above and below appear and user can select the one to keep. Select both points first and then, enter the radius 1 (both arcs appear) > pick the side to keep > OK Example 11. Draw an arc by three points at [0,0], [1,0], and [1,1/2]. Arc Three Points Select three points OK Example 12. Draw an arc by starting point at [0,0], radius 1/2, starting angle 0, and ending angle 180. Arc Polar End Points Select the starting point Enter the radius, starting angle, and ending angle > CR OK 8

9 Example 13. Draw a vertical line at origin and copy it at some horizontal distance. Then, create a tangent arc to both lines between the lines above tangent points. Arc Tangents Select both lines. Four arcs (in two circles) appear. Pick the arc to keep OK Example 14. Use Rectangular Shapes with width = 2 and height = 1.5 and draw a rectangle starting at origin first. Then, change the shape to Obround and see the change. Change again to D Shape as well as Double D Shape. Rectangular Shapes See the dialog with various options Enter the width and height 9

10 Pick the starting point at [0,0] See the rectangle Change the shape to Obround and see the second figure Change the shape to D Shape and Double D Shape and see other two shapes Note that user can also rotate the shapes by entering angles to rotate OK Example 15. Draw an ellipse at the origin with semi-major axis of 1 and semi-minor axis of 1/2. Ellipse Select the center at origin Enter semi-major and minor axes in dialog OK Example 16. Create a text MEE633 at origin. Letters Enter text as below with parameters > OK 10

11 Pick the starting point (repeatedly if needed) ESC (to finish) SOLIDS Example 17. Create a right cylinder at center (0,0,0) with radius 2 and height 3. Cylinder Check Solids in the dialog Pick the origin or Fast Point > enter 0,0,0 > CR Enter the radius 2 and height 3 > CR OK 11

12 Example 18. Create a box of size 5 x 4 x 3 at center (0,0,0). Block Check Solids in the dialog Pick the origin or Fast Point > enter 0,0,0 > CR Drag to size the width and click > drag to size the height > click Change the size in the dialog > hit CR after the height 3 is entered Play with Flip Direction to change the depth to other direction or both directions (in this case, the center moves to bottom) OK 12

13 Example 19. Create a torus of radius 3 and the section radius 0.5. Torus Check Solids in the dialog Pick the origin or Fast Point > enter 0,0,0 > CR Move the cursor to size the radius and click the graphics window Move the cursor to size the section radius (i.e., minor radius) and click Change the values in the dialog OK Analyze 1. This menu can be used to analyze and modify properties of entities. Sketch a circle > OK 2. 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. 13

14 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 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) 14

15 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 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 15

16 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 15. Create/Surface > Swept a. Across contour > pick the circle > OK b. Along the curve > pick the spline > OK 16

17 II. Toolpaths III. Starting with 2D/3D Contours Contour 1. Machine Type > Mill / Default 2. Drop down Properties Generic Mill in OM 3. Now, user needs toolpaths. 4. Line > sketch lines starting at (1,1,0) with horizontal length of 4 and the rest of lines have length of 3. 17

18 5. 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. It can be entered or picked by the mouse (easy to pick with the grid on [alt+g]). 6. Toolpaths > Contour > enter a name > selection dialog appears as 7. Select the line and choose the direction 18

19 8. Toolpath dialog appears 9. Toolpath Type = Contour. Other toolpath can be chosen here Also, see Chain geometry if needed. 10. Tool > use Select library tool > select the 5/16 Ball Mill. 19

20 11. Alternatively, right click the tool list window > New Tool a. Select the ball mill > change the tool diameter = 0.3 and other parameters as below. In this case the tool holder is not used. b. Change the name under Parameters tab > OK 12. If needed, right click any tool and choose any menu like Edit tool > the name of tool can be changed under Parameters > the tool numbers may be same 13. Holder = no holder display 14. Stock setup > click All Solids > change the size as below 20

21 15. Cut Parameters a. Select the following parameters for the tool compensation b. Lead In/Out > check the followings > OK 16. Linking Parameters: Select as below 21

22 17. Planes (WCS): See WCS, Tool plane and Construction plane and make sure they are correct for current operation. 18. OK (close) 19. Right click Toolpath in OM (Operations Manager) > adjust the speed and play, see below > OK 22

23 20. Right click the graphics window > WCS:TOP > see the toolpath above right. 21. The toolpath display can be toggled on/off by 22. Observation a. Tool moves to retract plane above the approach point and plunges to feed plane, then plunge cut first and follows the toolpath. b. Approach/Exit movements are along a straight line and a tangent arc. c. Toolpath compensation is to left to the toolpath. Note that MasterCAM X produces CL data at compensated positions and does not use any tool compensation NC codes because the toolpath generated is the final NC code. 23. Click Parameters in OM > Cut Parameters > change the tool compensation direction to Right > (It can be turned off if not needed) > OK 24. Play the toolpath simulation and see it. Observe the Approach/Exit movements. 23

24 25. Back to Parameters in OM > Lead In/Out > see the approach/exit parameters. By default, the entry move has a straight line (100% of tool radius) and an arc with radius (100% of tool radius) and 90 o sweep. Note that the Length or Arc of entry/exit moves can be made zero in order not to execute the part of entry/exit moves. The following shows tangent entry/exit moves with Length = 1. The second shows the toolpath with Arc extr/exit moves. 24

25 The first toolpath can be also generated by using Adjust start of contour for both entry/exit moves as below. The result in this case is same as the above. 25

26 26. Any changes need to regenerate the operations by. 27. To generate the G-codes, click (Post selected operations) > OK (with only NC file checked) > enter a name for NC code > see the g-codes and compare every line with the toolpath simulation. 28. In this case, the toolpath is generated at offset positions off the actual sketched chain. 26

27 [Generating G-Code for Fadal-Compatible CNC with Tool Compensation] 1. The tool compensation codes like G41 and G42 can be used. 2. Cut Parameters a. Compensation type = Control > OK 3. Run simulation and generate the g-code and see it as below. Note that the toolpath refers to original geometry. 4. Back Plot and see the actual tool motion. Quick verify can be turned off if desired. It uses tool compensation in the first straight approach and cancels in the last straight exit. 5. The g-code appears as 27

28 (Closed) Contour When there is a contour that crosses out itself, selecting the contour is tricky. See some tricks below how to use Entry and Exit moves in both Computer and Control compensations. 1. Machine Type > Mill / Default 2. Create a workpiece as above 3. Toolpaths > Contour a. Partial > pick the first two lines 1,2 > Loop > pick the loop 3 > Partial > pick the last line 4 > OK b. Select # inch ball end mill for the tool (use Filter to choose) in the library > right click it > Edit tool > Parameters tab > change the name c. Cut Parameters > Compensation type = Computer, Compensation direction = Right > turn off the rest 28

29 d. Linking Parameters > Feed plane = -0.3 with Absolute checked [this will prevent any back off of the tool at start/end of each chain], Depth = -0.3 > OK e. See the toolpath below gouging due to last cornering to close the loop. f. Click Geometry of the toolpath in OM > Rechain all > Partial > pick two lines 1,2 > pick following two lines 3,4 as below g. Play and still see gouging at transition of two chains. h. Alternatively, select 1 and 2, then pick the 3 for branch line. This completes the first chain. Continue with second chain. 29

30 i. To avoid the abrupt change from one chain to another, Parameters in OM > Lead In/Out > turn off Entry and Exit > check Adjust end of contour and Extend for Exit and enter 50 % for Length (this is percentage of tool diameter) > OK j. Play and see smooth transition between two chains 1,2. Now, change the tool compensation to Control (i.e., programming). Tool compensation by Computer produces toolpath at offset distance from original positions while Control option generates toolpath with tool compensation g-codes. 4. Parameters in OM > Cut Parameters > Compensation type = Control, Compensation direction = Right > turn off the rest > OK 5. Play and see the toolpath that the tool compensation restarts at beginning and cancels at end of each chain (see left figure below) 6. There are various ways to fix this problem. 30

31 7. Method 1: Perpendicular Length at both Entry and Exit and Extend. a. Lead In/Out > check Entry and Exit > check Perpendicular for both > enter 50% for Length and Arc = 0% for both > uncheck the rest of them > OK b. Back Plot to see gouging above right c. At the corner, the tool motion causes gouging. See the actual toolpath. d. Gouging can be removed as before by Adjust end of contour and Extend for Exit and enter 50 % for Length. e. The g-code is still incorrect because of two chains and must be modified manually. 8. Method 2: Tangent Arcs for both Entry and Exit a. Lead In/Out > check Entry and Exit > check Tangent for both > enter 0.0 for Length and Arc = 50% for both > uncheck the rest of them > OK b. Back Plot and Verify and see the toolpath below 31

32 c. Generate the g-code and modify as 9. Method 3: Only the Loop Toolpath with Entry and Exit Moves a. Entry In/Out with tangent Arc and Line as b. Linking Parameters > Home/Ref Points > select as below and pick the starting/ending point 32

33 c. Run and see the good toolpath as [More Discussion] When there are several closed loops for toolpath, MasterCAM must split the loops into several chains. Problem is that each chain begins a new toolpath with entry/exit moves. To be able to handle this issue, user must understand implications of tool compensation and entry/exit parameters. The following summarizes them briefly for a chain. For all cases, the feed plane = incremental / 0.1 and the retract plane = incremental / 0.25 are used unless changed and the HOME position is at (0,0,0.25). No Tool Compensation and No Entry/Exit 33

34 Tool Compensation = Computer/Right and No Entry/Exit Tool Compensation = Computer/Right and Exit/Line=50% Tangent Tool Compensation = Control/Right and No Entry/Exit Tool Compensation = Control/Right and Exit=50% Perpendicular & Adjust end of contour=50% Extend 34

35 Tool Compensation = Control/Right and Entry=50% Perpendicular, Exit=50% Perpendicular & Adjust end of contour=50% Extend Now, with both proper Entry and Exit moves above, the second chain can be added to complete the toolpath. See that the toolpath has redundant transition between chains. Turn off Retract Plane and change the Feed Plane to same level as the machining depth. The following shows the toolpath. 35

36 Now, despite the toolpath looks good, user must know that the transition toolpath is done by G0 code rather than G1 code. This must be corrected in the NC program. Pocket 1. Using same as above for most, sketch a similar pocket shape as below. 2. It is useful to know how to use both Trim/Break/Extend and Break at intersections in order to break and trim. 3. Toolpaths > Pocket a. Choose Loop b. Pick the contour > switch the direction if necessary c. Linking Parameters > Depth = > OK 36

37 4. Sketch a rectangle along the workpiece top 5. Geometry in OM > right click the collector > Add chain > Loop > select the new chain > make the direction same as the direction of inner loop > OK 6. Parameters in OM a. Cut Parameters > Roughing > Entry Motion > Off > OK 7. Toolpath appears as below left 8. Change the direction of second loop so that it is opposite to that of inner loop. Toolpath appears as below right. 9. Verify shows some leftover materials at four corners. 10. Change the pocket type to Facing [Parameters > Cut Parameters > Pocket type] and run it again. See it above right. 11. Parameter in OM > change Roughing angle to 90 > play and see 37

38 12. Trim/Break/Extend > trim and extend the inner loop into two loops as below [First, extend the horizontal lines by Trim_1_entity and then trim between two lines by Divide/Delete ]. 13. Geometry > right click the existing chain and delete it, right click in the Chain Manager > Add chain > add one loop by clicking near the starting point of the loop > repeat it for another loop > play and see above 14. Turn off all toolpath displays by and extend the horizontal lines as below and then select all redundant vertical lines > Delete button > Delete all selected lines to see the geometry below. Now, use under to break at every intersections of vertical lines [select the first vertical line on left edge and then pick all horizontal lines that divide > click End selection to end. Repeat this for right edge line.] 15. Geometry in OM > delete all chains > use Add chain to add the first chain [click the line near starting point for each segment until loop is complete]. Repeat this for two other chains [see above right]. 16. Parameters > Cut Parameters > Pocket Type = Open 17. Play and see 18. Change the pocket type to Facing as before and see the better machined part. 38

39 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 3. Note that face milling uses two opposite boundaries to cover the area between them. Also, the tool moves out of the boundary. The color, red, shows the tool interference with stock. Contour (3D) 1. Sketch as below using WCS (TOP, FRONT, RIGHT), and Dynamic Transform or XForm Translate. 2. Stock Setup 3. Toolpaths > Contour a. Chain > pick the first line segment (to select the whole chain) > switch the direction if necessary b. Toolpath Type = Contour 39

40 c. Tool = ¼ Flat End Mill d. Linking Parameters > Depth = > OK e. Look at the g-code how the rightside circular motion on vertical plane is excuted. Point 1. Toolpath can be created by Point. 2. Create several points at (0,0,2), (1,1,0.5), (4,1,0.5). Use Z=2 for first point and Z=0.5 for the rest. 3. Toolpaths > Point a. Toolpaths > Point b. Pick the points in sequence > OK c. Toolpath Type = Point d. Linking Parameters > Feed plane = 0.5, Top of stock = 1, Depth = 0.5 e. Create a tool and a workpiece as before > OK 4. Create a circular arc at Z=0.5 similar to below [create a large arc and trim] 5. Toolpaths > Contour a. Select the arc > OK b. Toolpath Type = Contour c. Tool = same tool d. Cut Parameters > Compensation Type = Off > turn everything off > OK 6. Create points at two end points of the arc and at (1,3.5,0.5) as below 40

41 7. Toolpaths > Point > create another toolpath from the end of the arc to the first point as 8. Click Geometry of the first Point toolpath a. Add > pick the last point > pick the next (new) point at beginning end of arc 9. Select Toolpath Group-1 in OM a. Play the toolpath in Back Plot and Verify and see below b. MasterCAM assumes there are collisions of tool with workpiece and shows the red color that can be ignored. c. Also, the combination of three sequences leave some redundant moves at beginning of some toolpath. Paramters of contour toolpath > Linking 41

42 Parameters > turn off Retract plane and make the Feed Plane level same as the cut depth > OK d. Regenerate all dirty operations e. Play the group toolpath that looks ok now. 10. Note that no tool compensation can be used for Point toolpath. 11. Toolpaths > Point a. Pick the point at the center of arc b. Tooltype = Helix Bore c. Cut Paramters > Circle diameter = 1 > Rough/Finish > Rough pitch = 0.15 d. Linking Parameters > Top of stock = 1, Depth = 0.5 > OK e. Play and see the helical boring as f. Tooltype = Circle Mill > play and see below 42

43 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 43

44 3. Stock Setup > All Entities > OK 4. Plane (WCS) > change the origin of the Tool plane if not correct as well as the Tool plane view. 5. Play and see the drilling as 6. Gview (determines the construction plane view) > View by solid surface > pick the front face > select the correct orientation of axes by clicking the arrow > OK 7. Sketch a rectangle with corner rounds 8. Toolpaths > Pocket a. Chain > pick the front rectangle > OK b. Linking Parameters > Depth = -0.5 > OK c. Planes (WCS) > if needed, change the Tool plane and C-plane views as well as the origins > User can copy one from the other using double arrow key. d. Play and see above right 9. Gview > View by solid face > pick the right face > OK 10. Sketch another rectangle on rightside face 11. Toolpaths > Pocket a. Chain > pick the front rectangle > OK b. Linking Parameters > Depth = 4.5 > OK 44

45 c. Planes (WCS) > if needed, change the Tool plane and C-plane views as well as the origins. 12. Select Toolpath Group-1 in OM > Verify selected operation > play and see as 13. See also the toolpath with point-to-point (PTP) motion in light yellow color and the machining in light blue. 14. Parameters of first Pocket in OM > Entry Motion > Off > OK > Back plot 15. 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. d. Observation: A-90 changes the Tplane with a local coordinates. 45

46 16. When all toolpaths are generated, the first Gview is identified by G54 WCS, the second by G55, and so on in sequence. 17. Let s add a sketch of an ellipse in the rear surface and machine it by Contour. a. Gview > View by Solid Face > pick the rear surface > choose the correct coodinates b. Sketch an ellipse c. Toolpaths > Contour > Loop > pick the ellipse > change direction for CCW d. Tool > pick the tool e. Cut Parameters > Compensation type = Off f. Linking Parameters > Top of stock = 5 and Absolute > Retract = 0.25 and Incremental > Feed plane = 0.1 and Incremental > Depth = -0.5 and Incremental g. Planes > Tool plane = BACK and Comp/construction plane = BACK > OK 2D High Speed This has several toolpath type as shown below. First, sketch two curves by Spline similar to below. 1. Toolpaths > 2D High Speed 46

47 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 l. Delete the contour and sketch two others as below (use Line, Offset, and Fillet) m. Parameters in OM 47

48 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 48

49 I. 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 49

50 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. 50

51 1. Alt + G for Grid > check Active 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) 51

52 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 52

53 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 53

54 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 54

55 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 55

56 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 56

57 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 57

58 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 58

59 II. 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) 59

60 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 60

61 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) 61

62 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 62

63 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 63

64 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 64

65 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 65

66 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 66

67 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 67

68 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 68

69 69

70 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: 70

71 Problem. 3 (a) Sketch the contour in Example 2 in the textbook add a line to the beginning as shown below. (b) Create the 0.2 inch thick workpiece with some extra materials around. Simulate contour milling starting from the line added and moving CCW along the outline. Use SP(0,0,0.25) as Approach/Retract Points and turn off Lead In/Out. The Linking Parameters are as below. Soultion: 1. Toolpaths > Contour 2. Set up the workpiece with z=0 at top 3. Choose a tool 4. Set up the parameters 5. Geometry a. Single > pick the starting line > (End) b. Chain > pick the first line of the loop (and pick the last line of the loop) > Done 6. Simulation a. Verify > turn on only the shoulder in Tool Components > Play b. In Mode group, click Backplot > Play and see the table moves 71

72 7. Note that Loop does not include any hanging lines to it. Thus, the starting line was a separate chain by itself. Problem. 4 For the same example problem above, produce MCD (machine control data, i.e., NC code) for Fadal compatible CNC machines using the tool compensations like G41, G42, G40. Hint: Since MasterCAM does not use any such tool compensation codes, produce g-code without tool compensation and then add tool compensations at proper places in the program manually. Problem. 5 Sketch the shape similarly and machine as shown below. Describe the steps. 72