/
CNC | Fusion | 2.5D Milling

CNC | Fusion | 2.5D Milling

Preparation | Rhino

  1. Create your stock material within Rhino

  2. Place your model within the stock material at the location you want to mill it from

  3. Draw a polyline perimeter around the top of your model

  4. Export the stock as an .stl

  5. Export the model as an .stl

  6. Export the perimeter as a .dxf

  7. Ensure you’re naming these exported files something logical

Design | Stock

  1. Start in the Design workspace

  2. Verify units for your scale

  3. In Fusion, select insert mesh

  4. Select your stock model .stl file

  5. Click OK

  6. Change the opacity of your stock material by right-clicking the item on the navigation tree -> opacity control -> 50%

Design | Model

  1. Still in the Design workspace

  2. On the top navigation bar, select Insert → Insert Mesh

  3. Select your mesh model .stl file

  4. Click OK to insert your file

Design | Perimeter

  1. Still in the Design workspace

  2. On the top navigation bar, select Insert → Insert DXF

  3. Select the X,Y plane

    1. image-20251103-193917.png

  4. Click the folder icon

    1. image-20251103-194023.png

  5. Click “Select from my computer…

    1. image-20251103-194225.png

    2. Select your file, click Open

      image-20251103-194322.png

  6. Fusion will need to think about your .dxf for a moment, then the Insert menu will change a bit

  7. Confirm that the units are correct

  8. Click OK to insert your file

  9. To view all of your imports, expand the Bodies and Sketches sections of the navigation tree

    1. image-20251103-195251.png

Manufacture | Setups

  1. Select the Manufacture workspace

  2. image-20251103-195357.png

     

  3. Expand the Models → your file name → Bodies and Sketches sections of the navigation tree

    1. image-20251103-195842.png

  4. On the top navigation bar, select new setup

    image-20251103-195438.png

  5. Setup tab

    1. Configure Work Coordinate System (WCS)

      1. Select the Model orientation

      2. WCS should be Model origin

    2. Model

      1. Use the navigation tree to select your mesh model (best method)

  6. Stock tab

    1. Stock

      1. Mode is From solid

      2. Use the navigation tree to select your stock (best method)

    2. image-20251103-195756.png

  7. Click OK

 

Manufacture | Create From Template

  1. Must be in the Manufacture workspace

  2. Right click the setup you just created and select 'Create from Template'

  3. If you haven’t used the template before, you need to click on “Select Template” and select the 2.5D Template

    1. If you have used the template before, it will be selectable next to “Create From Template”

  4. Select the template titled 2.5D Contours

  5. You should see new operations load in from the template

  6. Select the edit icon (highlighted in red) to open template configuration

  7. Starting from left to right, we need to configure settings for this operation

  8. Tool tab

    1. Select the tool required for your job as referenced on Templates for Fusion360 wiki page
      Tool = the bit used for this operation

    2. Select a material preset
      Preset = feeds & speed variables are baked into preset profiles

  9. Geometry

    1. Select Geometry

      1. Geometry = Line work for tool path

      2. Use the navigation tree to select your line work (best method)

      3. Geometry settings cog will display a window to select cutting on the inside or outside of a specified line

    2. Select Stock Contours

      1. Stock Contours = Creates a boundary box, keeping the tool within a certain perimeter

      2. Select the boundary stock contour

  10. Heights

    1. This tab can be very helpful when you only need to etch the contour rather than cut it all the way out, or if the stock is deeper than the bit

    2. The one we recommend changing for either reason listed above is 'Bottom Height”

      1. Stock bottom is selected by default, but there’s 0.00” Offset

        1. You’ll change the Offset to the thickness of the stock material you want to leave OR

        2. The difference between the stock depth and the tool length

          1. Example, you have 3” foam and a 2” bullnose bit on CNC2, you’d want a 1” offset

    3. image-20260413-210018.png

       

  11. Passes

    1. The number of passes depends on your material, and you almost never leave this as a single pass at full depth

    2. For foam, a 1/4” (0.25”) or 1/2” (0.5”) maximum pass depth should work well

    3. For solid or laminated wood, you’ll want to use 1/16” (0.0625”) maximum pass depth

    4. For a single sheet of plywood, a 1/16” (0.0625”) or 1/8” (0.125”) maximum pass depth.

  12. Linking

    1. Is configured for the School of Architectures ShopBot CNC machines and should not be changed.

 

Manufacture | Simulate

  1. Must be in the Manufacture workspace

  2. Right click your setup template and select Simulate

  3. Watch the tool path simulation

    1. Take notes on the order of operations, making sure inner cuts are done before outer cuts

    2. Remember the simulation to help you out when you bring it to the ShopBot CNC as all the tool path and cuts will be exactly the same as in the operation

  4. Once the simulation looks good, proceed with post-processing

 

Manufacture | Post-Processing

  1. Must be in the Manufacture workspace

  2. Right click your setup template and select Post-Process

  3. Fill in the fields for

    1. Post = What type of machine?

      1. Use ShopBot OpenSBP found on Templates for Fusion360

    2. Name/number = Operation name within the ShopBot software

      1. May be left default

    3. File name = File name

      1. Recommended naming syntax 'EID - Operation type - Project'

    4. Comment = Displays during job

      1. Recommended to time and date the comment as multiple iterations may be needed to have a successful cut

    5. Output folder = location to save the file

      1. Will save as *file_name.sbp*