Tutorial 8: CNC-Milled Aluminum Part with a CAM Overview

Goal#

Design a 80 mm x 50 mm x 20 mm aluminum 6061-T6 mounting block with a 40 x 20 mm pocket, four M5 tapped holes, a counterbored through-hole pair, and a 0.5 mm edge break. Then set up CAM in Fusion's Manufacture workspace: define stock, a work coordinate system, facing, adaptive roughing, finishing, drilling and tapping, run the simulation and post-process G-code. You will not need a machine to do this; the goal is a verified toolpath set.

This tutorial is the longest conceptual leap in the section because it adds a new discipline: you now design for a cutter. The rules are different from 3D printing: tool radius defines minimum inside corner, tool length defines maximum pocket depth, and fixturing defines what you can machine in one setup.

What you'll learn#

• Applying design-for-machining rules: inside corner radii, pocket depth to width ratios, wall thickness.
• Modeling threaded holes properly so CAM can drill and tap them.
• Entering the Manufacture workspace, creating a Setup, choosing stock and the WCS orientation.
• Choosing tools from the library, speeds and feeds basics.
• Creating Face, 2D Adaptive Roughing, 2D Offset Roughing (formerly 2D Pocket), 2D Contour, Drill and 2D Chamfer operations.
• Simulating stock removal and checking for gouges.
• Post-processing and generating a setup sheet.

Prerequisites#

• Tutorial 1 (parameters) and basic solid modeling.
• Understanding of terms: stepover, stepdown, feed, spindle speed, climb milling. Brief definitions appear below.
• Capability: CAM is part of standard Fusion; some strategies belong to the paid Manufacturing Extension and Personal-use has restrictions (see Manufacturing Extensions and Licenses and Plans for current limits). The 2D strategies used here are the ones Autodesk documents as core milling operations.

Design for machining rules used here#

Steps: Design#

Part A: Stock block and pocket#

1. New design named CNC Block. Add parameters: L = 80 mm, W = 50 mm, H = 20 mm, pkt_l = 40 mm, pkt_w = 20 mm, pkt_d = 10 mm, corner_r = 4 mm.
2. Sketch. Center Rectangle on XY, dimensioned L x W. Extrude downward H (set direction so the top face is at Z = 0, or leave upward). Fillet the four vertical edges of the block 3 mm (equal to the radius of the 6 mm cutter used to profile it).
3. Pocket sketch. Select the top face, sketch a center rectangle pkt_l x pkt_w. Fillet its four corners with corner_r.
4. Cut. Extrude Cut by pkt_d. The default Operation is Cut when the sketch is on a face and the direction goes inward.
5. Floor fillet. Add 0.5 mm to the pocket floor edges to reduce stress concentration (a 0.5 mm radius corner is produced by a bull-nose or a small ball finishing pass; if you do not want that op, skip it).

Part B: Holes#

6. Tapped holes. Press H. Choose the top face. Placement: use From Sketch after creating a sketch with 4 points at X = +/-32 mm and Y = +/-17 mm (these are 8 mm from the short ends and 8 mm from the long edges, and 4.5 mm clear of the 20 mm wide pocket's side walls). In the Hole dialog set Hole Type Simple, Hole Tap Type to Tapped, Thread Type to ISO Metric profile, Size 5, Designation M5x0.8, Class 6H, Depth 12 mm. Leave Modeled off (the thread stays cosmetic, which is what CAM hole recognition reads).
7. Counterbored through holes. Add two Ø6.6 mm counterbored holes through the thickness at X = 0, Y = +/-18 mm (the 11 mm counterbore then clears the pocket by 2.5 mm and the block edge by 1.5 mm) for M6 socket head screws: Hole Type Counterbore, Diameter 6.6 mm, Counterbore diameter 11 mm, counterbore depth 6.5 mm, Depth All or 20 mm.
8. Edge break. Press chamfer and select the top outer edges and the pocket opening edge: distance 0.5 mm. Chamfers like this are produced by a chamfer mill or a 90 degree spot drill and add a Chamfer operation.
9. Material. Right-click the body > Physical Material, choose Aluminum 6061. The calculated volume is about 69 cm3, so the mass should read about 187 g.

Part C: Quick design checks#

10. Section analysis through the pocket to verify the floor is 10 mm thick.
11. Measure that internal radii equal 4 mm.
12. Dimension drawing. Optionally create a drawing with tolerances (see Drawings section): general tolerance +/-0.1 mm, hole positions +/-0.05 mm.

Steps: CAM overview#

Part D: Enter the Manufacture workspace and create a Setup#

13. Switch workspace. Choose Manufacture from the workspace dropdown. The process tabs are Milling, Turning, Additive, Fabrication and Inspection; the Milling tab holds the Setup panel, the 2D, 3D and Drilling strategies, and Actions.
14. New Setup. Click Milling > Setup > New Setup. In the Setup tab choose a milling Machine (optional at first; the machine defines the operation type, otherwise leave Operation Type as Milling) and under Work Coordinate System (WCS) set Orientation Select Z axis/plane & X axis. Select the top face of the block for the Z axis and a long edge for the X axis. Origin: Stock box point and choose the top-front-left corner so Z0 is the top of the stock.
15. Stock tab. Stock Mode Relative size box. Set Stock offset mode to Add stock to sides and top-bottom, with 1 mm at the sides, 2 mm at the top and 0 at the bottom. The extra 2 mm lets the Face operation clean the top. Alternatively choose Fixed size box 82 x 52 x 22 mm (80 + 2, 50 + 2, 20 + 2).
16. Fixturing. The part is gripped in a vise; Fusion's setup does not automatically model the vise, but you can import one as a fixture body or use the "Model" selection. For toolpath safety, ensure all cutting stays above the vise jaw tops (verify with simulation).

Part E: Tools#

17. Tool library. In the Tool Library (opened by selecting a tool in an operation > Select), use a Local or Cloud library (or a sample library if your installation has one). Create a few tools if needed:

• T1: Face mill, 50 mm, 5 inserts (or a 12 mm end mill if you do not have a face mill)
• T2: Flat end mill, 6 mm, 3 flutes, carbide, 18 mm flute length
• T3: Flat end mill, 3 mm, 2 flutes
• T4: Spot drill 90 degree, 10 mm
• T5: Drill 4.2 mm (M5 tap drill)
• T6: Drill 6.6 mm
• T7: Tap M5 x 0.8
• T8: Chamfer mill 90 degree, 8 mm

18. Feeds and speeds. For the 6 mm 3-flute carbide in 6061: surface speed about 250 m/min gives about 13,000 rpm; many hobby machines cannot reach that, so use 10,000 rpm and a feed of 2000 mm/min; chip load 0.07 mm per tooth. Set these values in the tool's Feed & Speed tab; Fusion computes the cutting feed from the chip load. Always scale to your machine (verify with the manufacturer).

Part F: Operations#

19. Face. 2D > Face. Tool T1 or the 6 mm end mill. Under Geometry select the stock; Passes: set Stock to Leave 0. Heights: Bottom Height from the model top (Z = 0). This removes the extra 2 mm in one or two stepdowns.
20. 2D Adaptive Roughing. Milling > 2D > 2D Adaptive Roughing (formerly 2D Adaptive Clearing), tool T2 (6 mm). Geometry: select the pocket floor contour (the pocket edge loop). Passes: Optimal Load 1.2 mm (20 percent of diameter). On Heights, Bottom Height set to Selected contour(s) with -10 mm. Under Passes set Maximum Roughing Stepdown to 10 mm (the full pocket depth in one pass) or 6 mm if your spindle is weak. Leave Stock to Leave radial 0.2 mm and axial 0.1 mm for the finish pass.
21. 2D Contour (outside). 2D Contour with T2. Geometry: select the outside edges of the part, bottom height at the part bottom plus tab or use the vise. Since the block is cut from stock that is already near finished size, the contour trims only the 1 mm offset. Add Lead-in/Lead-out arcs and finish pass.
22. Pocket finishing. 2D Contour with T2 along the pocket walls with 0 stock to leave, one pass. Finish the floor (left 0.1 mm axial in the previous step) with 2D Offset Roughing (formerly 2D Pocket) at zero axial stock to leave and a finishing pass.
23. Drilling. Drill operation with T4 spot drill depth 1 mm, then T5 drill 4.2 mm with Cycle Chip Breaking or Deep Drilling (Peck) depth 13 mm, then a Drill operation with the T7 tap to depth 12 mm using the tapping cycle (select it on the Cycle tab; see Drilling, Tapping and Hole Operations); hole recognition (Milling > Drilling > Hole Recognition, or the Geometry tab's hole selection tools) can select the holes from the model. Counterbores: select the counterbore holes; use a Bore or Circular Pocket operation, or helical Bore operations with T3.
24. Chamfer. 2D Chamfer with T8, geometry the top edges, chamfer width 0.5 mm. Distance tolerances: the cutter tip offset must not touch the floor.

Part G: Simulate and check#

25. Simulate. Select the Setup in the browser, click Actions > Simulate. Turn on Show tool (and Show holder for holder collision checks) and step through; look for gouge or collision warnings (red) and for rapid moves through the part.
26. Compare. In the Simulate dialog open the Compare tab to see leftover material and gouges against the model. Material left in an inside corner is the one you must check.
27. Cycle time. Read the machining time in the Simulate statistics; it depends on your feeds.

Part H: Post and setup sheet#

28. Post Process. Select the Setup, click Milling > Actions > Post Process (or right-click the Setup > Post Process). Choose a post for your controller (for example, Grbl, Haas, Mach3, Fanuc; the post library lists these). Select the output folder, the program name and number and click Post. Fusion writes an .nc or .tap file.
29. Setup sheet. Actions > Setup Sheets produces an HTML document listing tools, speeds and operation times; operators use it at the machine.
30. Review the code. Open the G-code in a text editor and check the header: units (G21), work offset (G54), tool changes (M6). Do a dry run above the part before cutting.

Checkpoints#

• All tool numbers unique and consistent with the machine's carousel.
• Simulation shows full stock removal with no red collision marks.
• No tool is asked to cut deeper than its flute length plus shank clearance.
• The WCS X axis, Y axis and Z axis arrows agree with the way the part sits in the vise.
• G-code header shows the expected units.

Variations#

1. Second setup. Flip the part for the underside operations and use Stock from Previous Setup.
2. Fixture design. Model soft jaws and use them as fixture bodies.
3. Add 3D finishing. Add a Scallop or Parallel finishing on a curved pocket floor.
4. Different material. Change to 304 stainless or ABS and adjust the feeds.
5. Tolerance study. Add tolerances in the drawing and check them on the actual part.

Troubleshooting#

Related#

• Hole and Thread (modelled threads vs cosmetic).
• Design for Manufacture (sheet metal and plastic section) lists general rules.
• Dimensions and Tolerances (Drawings) for the inspection drawing.