Milling PCB workflow

(experimental)

Using Eagle, Tracespace.io, InkScape and Fusion 360

Circuit and PCB layout

• Make circuit and PCB layout in Autodesk Eagle (version 9.4.0)
• File > Generate CAM data
• Click OK. This will generate a zip archive with Gerber files (2D vector files used for PCB manufacturing).
• Unzip the .zip file and open the GerberFiles folder.
• Open https://tracespace.io/ to convert the desired Gerber files to SVG vector files.
• Open the desired .SVG files in Inkscape.
• use view > display mode > normal / outline to analyse the vector image.

Seeing the image in the outline display mode (right), it becomes apparent that the traces have a width of zero mm.

• edit > select all (ctrl + a)
• object > ungroup (shift + ctrl + g)
• the circles and squares are clones from hidden shapes. select one clone-object.
• edit > select same > Object type (shift + alt + a)
• file > clone > unlink clone (shift + alt + d). The clone objects have now been changed to circle and rectangle objects
• edit > select all
• path > objects to path
• path > stroke to path
• path > break apart
• path > union
• file > save as Choose SVG.

Now you have a proper outline

• insert the SVG file in fusion 360
• set scale to 0,003779527597 (The dimensions set in Eagle are correct in InkScape, but with scale set to 1, 1,27mm in eagle becomes 336,02083mm in Fusion 360)
• select contours, extrude and configure setup and trace operation for milling

• circles are actually 4 arcs. This won't be selectable for a bore or drill operation.
  • Draw 2 construction lines between the points
  • draw a circle to measure the diameter of the intended circle. Note the dimension and cancel the circle.
  • Delete the arc segments
  • Draw a the new circle with the measured diameter

If traces come close together, the tool will lift, cutting a thinner trace. This allows to set a relatively deep trace over-all to accommodate flex in the PCB substrate.

• Select the area in between traces and push it down a small amount. The depth doesn't matter. This creates a pocket we can use to select the engrave toolpath.
  
  
• Add an engrave toolpath strategy and select the traces. You don't need to select the holes yet, but make sure to select a contour line around all the traces. That way Fusion knows at which side of the lines the tool need to be placed. I tested 0.3mm depth, but 0,2mm or shallower should work better.
  
  
  Here you can see the cut is made on the outside of the traces.