Fusion 360 CAM for Hobby CNC: Complete Guide

Getting Started Fusion 360 is free for hobby use and includes a full professional CAM engine. Switch to the Manufacture workspace from the dropdown at top left. Step 1: Create a Setup Manufacture, Setup, New Setup. Configure: Operation Type: Milling Stock tab: enter your raw material dimensions (width x depth x thickness) Setup tab, WCS origin: click the front-left-top corner of your model. This is X0 Y0 Z0 on the machine. X should point right, Y toward you, Z up. Use axis flip buttons to correct if needed. Step 2: Tool Library Manage, Tool Library, New Mill Tool. Enter for each bit: Type: Flat End Mill, Ball End Mill, Chamfer, V-Groove Diameter: 6.35mm for 1/4 inch, 3.175mm for 1/8 inch Flutes: 2 for standard spiral bits Cutting Data tab: feeds and speeds per material Save to My Tools, Local for reuse across jobs. Step 3: 2D Toolpaths 2D Pocket: removes all material inside a closed shape. Select top edge of pocket area. Set stepdown (1.5-2mm hardwood, 2-3mm softwood), stepover (40-50% of tool diameter for roughing). Enable Multiple Depths. 2D Contour: cuts along a profile path. Select top edge of the shape. Enable Tabs (3mm wide x 3mm high) to hold parts during cutthrough. Enable Multiple Depths with per-pass stepdown. 2D Adaptive Clearing: high-efficiency roughing that maintains consistent chip load. Much faster than standard 2D Pocket for large material removal. Engrave and V-Carve: select paths or closed shapes. Fusion calculates V-carve depth automatically based on stroke width. Step 4: 3D Toolpaths For relief carving and organic surfaces: 3D Adaptive Clearing: roughing with flat or ball end mill 3D Parallel: finishing with ball nose at 3-8% stepover for smooth surface Step 5: Simulate Right-click any setup or operation, then Simulate. Watch the tool animate through the material. Check for collisions between tool holder and workpiece, missed areas, and incorrect depths. Fix all issues before posting G-code. Step 6: Post Process Right-click the setup, Post Process. Select your post processor: LongMill, gSender, any GRBL machine: use the grbl post from cam.autodesk.com Shapeoko, Carbide Motion: grbl post or Carbide-specific post Mach3: mach3mill post Set units to Millimeters. Click Post to generate the .nc G-code file. Verify in ncviewer.com or gSender before running on the machine. Common Beginner Mistakes Z-zero wrong: Setup WCS Z=0 must be at the top surface of your stock, not the bottom Units mismatch: set both Fusion and post processor to metric to avoid 25.4x scale errors Compensation type: always set to In Computer for hobby CNC No tabs: parts break free during cutthrough. Minimum 3mm wide x 3mm high Red in simulation means holder collision. Reduce stepdown or use shorter tooling.

Related Guides

Loading_