Skip to main content

Fusion 360 CAM

Step-by-step: Facing → Profile → Spot Drill (Fusion 360)

Preparations (before creating operations)

  1. Open your design in Fusion 360 and switch to Manufacture.

  2. Confirm units (mm or in) in the lower right — set to what your CNC expects.

  3. Save the file (version your CAM changes if needed).

  4. Quick checklist: material selected, correct model orientation, correct stock size, tooling on hand.

1. Create a Setup

  1. Manufacture → Setup → New Setup.

  2. Operation Type: Milling.

  3. Model: Confirm the body/component you will machine is selected.

  4. Work Coordinate System (WCS / Origin):

    • Choose a logical origin — commonly top-center, top-front-left corner, or a machinist-placed datum hole.

    • Set Zero position to Top (for Z) and Center or Model Box Min/Max for X/Y as fits your fixturing.

  5. Stock:

    • Mode: From solid or Relative size box (e.g., add 2–3 mm / 0.08–0.12 in of stock as allowance).

    • Confirm orientation matches how the part will sit on the machine.

  6. Click OK.

2. Facing Operation (2D Adaptive / 2D Face)

Goal: remove top material to create a clean, flat face and establish final Z height.

A. Choose Operation

  1. 2D → 2D Face (or use 2D Adaptive for larger stock removal).

  2. Select the top face(s) of the stock that you want to face.

B. Tool Selection

  1. Click Tool → Select. Pick a face cutter or flat endmill (example: 6 mm / 1/4" flat endmill).

  2. Example starting values (adjust to your machine/tool/material):

    • Spindle speed: 8,000–16,000 RPM for aluminum with carbide; lower for steel.

    • Feedrate: 800–1500 mm/min for aluminum (or ~30–60 ipm for 1/4" endmill).

    • Cutting speed/feed should follow tooling manufacturer charts for your material.

C. Heights & Passes

  1. Heights tab: Set Top Height to stock top (usually Stock top). Set Bottom Height to final face Z (usually 0 or model top).

  2. Passes: Step-over ~40–60% of tool diameter for finishing; step-down small if face is shallow (0.5–2 mm typical). If heavy stock, use multiple passes or Adaptive clearing first.

D. Linking

  1. Set lead-in/out as needed (short linear).

  2. Set Feed override if you want to reduce feed for finish.

E. Generate & Simulate

  1. Click Generate.

  2. Actions → Simulate. Watch for gouging or collisions. Use Stock visualization to confirm material removal.

  3. If safe, proceed. If not, adjust heights/clearance or origin.

3. Profile Cut (2D Contour)

Goal: cut the outside profile (or an interior profile) to final shape or rough to near-net.

A. Choose Operation

  1. 2D → 2D Contour.

B. Select Geometry

  1. Select the face or sketch edge(s) that define the contour to cut.

  2. Pay attention whether you want Outside, Inside, or On path; choose Multiple passes for deep cuts.

C. Tool Selection

  1. Select an appropriate tool: for finishing profile choose the same flat endmill or a smaller endmill (e.g., 4 mm / 1/8") for tighter radii.

  2. Example params (finish profile in aluminum): spindle 10,000–14,000 RPM; feed ~500–1200 mm/min depending on tool size.

D. Heights & Passes

  1. Heights:

    • Top Height: Stock Top (or model top if already faced).

    • Bottom Height: Set to final cut depth (eg: part bottom or through).

  2. Passes:

    • Multiple depth passes: set Maximum roughing stepdown appropriate to tool (e.g., 1–2 × tool diameter for carbide roughing, or smaller for finishing).

    • For finishing, use single pass at final depth or small stepdown (0.1–0.5 mm) for surface quality.

E. Compensation & Lead

  1. Tool orientation: Climb vs Conventional milling — choose per machine / fixture preference (climb is common for better finish on many mills).

  2. Stock to Leave: If you plan a separate finishing pass, set small radial/axial stock to leave (e.g., 0.1–0.2 mm).

F. Quick Retracts & Clearance

  1. Ensure Retract Height clears clamps and features.

  2. Use Ramp In or Helical Lead-in if cutting into a closed profile.

G. Generate & Simulate

  1. Generate toolpath and simulate.

  2. Use Toolpath Color and Stock display to check full travel and final geometry. Confirm no collisions.

4. Spot Drill (Drilling Operation or CAM Drill Cycle)

Goal: create a small conical center or guide hole before using a twist drill.

A. Choose Operation

  1. Drilling → Spot Drill (or use Drill with the spot drill tool). If Fusion lacks explicit spot tool, use a small 82° or 60° countersink/spotter as the tool.

B. Select Geometry

  1. Select the points where you want to spot (hole centers). Use sketch points, hole features, or pick model faces.

  2. Verify XY coordinates match intended locations.

C. Tool Selection

  1. Pick a spot-drill (or countersink) with the desired included angle (82° is common).

  2. Typical parameters: slow plunge feed, shallow depth (0.5–1.0 mm), spindle speed lower than profile milling if tool is small.

D. Heights & Pecking

  1. Heights:

    • Top Height: Stock top (or model top).

    • Bottom Height: Small negative value to create a conical dimple (e.g., −0.5 mm).

  2. Pecking: Not needed for spot drill — single plunge sufficient.

E. Feed & SFM

  1. Adjust feed to match tool size and material (small tools = lower feed).

  2. Use conservative plunge feed to avoid tool breakage.

F. Generate & Simulate

  1. Generate. Simulate full sequence including facing and profiling to ensure the spot-drill toolpath aligns after previous operations.

  2. Verify that the spot drill does not collide with clamps and that Z retracts clear.

5. Run Order & Stock Updates

  1. Confirm operation order in the Setup tree: Facing should be first, then Profile, then Spot Drill (or Spot Drill before profile if you need holes established before cutting the outer profile). Drag operations to reorder if needed.

  2. If facing changed stock heights, right-click Setup → Update Stock or regenerate subsequent toolpaths.

6. Final Simulation & Verification

  1. Run a Full Simulation of all operations together.

  2. Use Play and Material Removal views to confirm final shape and check for collisions.

  3. Verify tool changes and tool holder clearances.

7. Post Process & Export G-Code

  1. Actions → Post Process in the Setup or individual operation.

  2. Select the correct post-processor for your controller (Haas, Tormach, Mach3, GRBL, etc.).

  3. Set file name, safe retracts, and post options.

  4. Click Post and transfer G-code to the machine per shop procedures.

8. Shopfloor Checklist (Before Spindle On)

  1. Confirm correct tool in spindle and correct tool offsets set in controller.

  2. Verify workpiece is securely fixtured and zeroes match Fusion origin.

  3. Dry-run through the program at reduced feed (handwheel or MD mode) to confirm motion.

  4. Emergency stop location checked; PPE on.

Tips & Troubleshooting

  • If facing leaves scallops: increase step-over or use a larger face cutter, or add a finishing pass with lighter cut.

  • If profile chatter occurs: reduce feed, increase spindle speed, or use a shorter tool stick-out.

  • If spot drill misses XY: double-check WCS origin and whether you used model or stock top as reference.

  • Use Stock to Leave on the profile if you want a final finish pass to get accurate dims.

Quick Example Parameters (Aluminum, 1/4" flat endmill)

  • Facing: 6 mm endmill, 12,000 RPM, 900 mm/min feed, step-over 50%, step-down 1 mm.

  • Profile finish: 4 mm endmill, 12,000 RPM, 600 mm/min feed, step-down 0.5 mm.

  • Spot drill: 82° 6 mm spotter, 6,000 RPM, 200 mm/min plunge, depth 0.5 mm.

(These are example starting points — consult tooling tables & your machine limits.)

Back to top