Autodesk Fusion 2D Contour Machining

Autodesk Fusion 360 Process for Contour Machining

This page is a step-by-step walkthrough for setting up a contour milling operation in Autodesk Fusion for the WorkBee CNC specifically, but it should be easy to adapt this to any similar machine.

You will start with a New Fusion 360 Document and end up with a G-Code file ready to upload to the machine.

For further information and the explanation for each step, consult the Fusion 360 Documentation

Prepare

To get started, you will need to create the 2D geometry you’d like to mill out.

• For testing, a simple square with about 50 mm side length is a good starting point.
• Extrude it by the material thickness you plan to machine.

example test part

In the top left corner of Fusion 360, switch from the “Design” workspace to the “Manufacture” workspace. This is where you’ll define your toolpaths and machine settings.

Import Workbee CNC machine definition

Before you get started, make sure you have properly imported the latest version of the machine definition and post-processor into Fusion 360.

You can find the newest version of these required files here. Feel free to submit improvements.

• at the top of the Fusion 360 Interface, select "Manage > Machine Library".
• under "My Machines > Local" you can import (NOT CREATE) the machine definition. (Filename: WorkBee.mch from the GitHub link above).
• the "Rebuilt WorkBee Comakingspace CNC" will appear, with a red exclamation mark indicating "file not found". This is the post processor, which you will now also need to import:
• click on the folder icon next to "file not found" and the "Post Library" window will open.
• click on the "Import" icon and select the CPS file (Filename: coms-workbee.cps) from the GitHub link above.
• click "select", which brings you mach to the Machine Library import window. There should now be a green tick mark next to "Post: coms-workbee.cps"

• 
  Step 1: Open Machine Library (german Screenshot)
• 
  Step 2: Import machine to local machines

Create your Milling Tool inside Fusion's Tool Library

At the top of the Fusion 360 Interface, select "Manage > Tool Library" to open the tool library. Navigate to "Local > Library". This is where you'll save all of your endmill data.

Click on "[+]" to add a new tool. Select the appropriate geometry, most likely "Flat End Mill".

The tool creation menu

• Tab 1: General Here you can name your endmill. Describe them well, you'll mix them up otherwise. Also enter sourcing information (such as aliexpress links) here, you'll thank yourself later.
• Tab 2: Cutter Take Measurements of your tool for dimensions using calipers (Messschieber) and populate the values accordingly. Adjust number of flutes and the geometry to match your endmill. I recommend setting "length below holder", "shoulder length" and "flute length" to the same value, that being the length of fully formed cutting flutes of your endmill.
• Tab 3: Shaft leave as is
• Tab 4: Holder leave as is
• Tab 5: Cutting Data The following cutting data is a recommended starting point for a 1/8” (3.175mm) 2-flute flat nose endmill cutting plywood. Many of the values (marked with fx) are calculated automatically and don't need adjusting.

  

  Tweak these values as you gain experience:
  • Spindle Speed (Drehzahl): 16,000 RPM
  • Cutting Feedrate (Schnittvorschub): 1000 mm/min
  • Ramp Feedrate (Helixvorschub): 500 mm/min
  • Plunge Feedrate (Eintauchvorschub): 500 mm/min
  • Coolant: DISABLE (To prevent errors, the WorkBee doesn’t have a coolant system)
• Tab 6: Post Processor leave as is.

Sanity check all data once over and click "accept" to confirm.

Configure Setup

Back in the Manufacture workspace window, go to "Setup > New Setup"

• Tab 1: Setup
  • Machine:
    • Select the latest machine definition
  • Workpiece Coordinate System (WCS)
    • Orientation: Model Orientation
    • Origin: Model Box Point
    • Model Point: Select Front-Left-Top corner
• Tab 2: Stock
  • Mode: Relative size box
    • Stock side offset: 10 mm
    • Stock top offset: 0 mm
    • Stock bottom offset: 0 mm
• Tab 3: Part Position leave as is
• Tab 4: Post Process Optional: adjust program name. leave as is.

Setting the Workpiece Coordinate System (WCS) origin

Set up 2D contour operation

At the top of the Fusion 360 Interface, select "2D > 2D Contour" to create a new 2D contour milling operation.

• Tab 1: Tool
  • Tool: Select the appropriate milling tool
  • Feed & Speed: Ensure the cut parameters are sane and have been properly inherited from the tool
• Tab 2: Multi-Axis leave as is
• Tab 3: Geometry
  • Contour Selection: Select the 2D contour you want to machine (the bottom edge of your design)
  • Tabs: Enable
    • Tab Shape: Triangle
    • Tab dimensions: Width: 6 mm, Height: 3 mm. Distance: 40 mm
• Tab 4: Heights leave as is
• Tab 5: Passes
  • Passes: Sideways Compensation: Right (Rechtsfräsen)
  • OPTIONAL: Preserve order Check this box if you have nested features (cutouts within cutouts) to maintain the cutting order
  • Disable all the other options
• Tab 6: Linking
  • Lead-In: Deactivate
  • Lead-Out: Deactivate
  • Ramp: Enable
    • Maximum Ramp Stepdown: Start with 3-6 mm and adjust based on endmill strength, desired cut quality, and material thickness

Confirm the Operation with OK. Fusion 360 will now display a preview of the operation.

How your preview should look

Simulate to check & Export

post processor menu

• At the top of the Fusion 360 Interface, use the “Actions > Simulate” tool to check you haven’t missed anything
• At the top of the Fusion 360 Interface, use "Actions > Post Process"
• Use Machine Configuration (“Maschinenkonfiguration verwenden”):
  • Select Machine: “Rebuilt WorkBee Comakingspace CNC”
  • Double-check Post-Processor: “WorkBee CoMakingSpace RRF”
• Export

Your G-Code file is ready for upload to the CNC!