FreeCAD Path with Shapeoko

Post Reply
Posts: 1
Joined: Sun Feb 24, 2019 4:19 am

FreeCAD Path with Shapeoko

Post by Uriah » Thu Feb 28, 2019 3:20 am

I've been using FreeCAD Path with the Shapeoko XXL for about a couple of weeks and wanted to share a few things I've learned in hopes of helping out someone else. Overall, FreeCAD Path has worked well and so far has enabled me to cut all of the models I've need to.

The Post Processor
By default, new Jobs will be set to use the "centroid" post processor. This needs to be changed to either grbl if you are not doing any drill operations or grbl_G81 if you are.

Drill Operations
If the grbl post processor is selected, drill operations will be implemented with the G81 code. The Shapeoko does not support G81 and will not drill your G81 holes. If you select the grbl_G81 post processor, the drill operations will be implemented with G1. However, the drill movements are very very slow. It appears that grbl_G81 is not applying the same scaling to the vertical feeds as whats taking place for the horizontal. A horizontal feed speed of 65 mm/s results in GCode with speeds around F3900 while a vertical feed speed of 22 mm/s results in F22 GCode speeds. This appears to be a bug where the vertical feed should be written in mm/minute but is instead written as mm/second. Instead of drill operations, the Profile Edge operation with Cut Side set to Inside can be used to drill holes.

Pocket Operations
The default pocket pattern (ZigZag) and most other patterns will not clear all of the material from a round pocket. The Offset pattern will generate a tool path that clears all the material but for some reason doesn't cut right on the Shapeoko. Measurements of a 16 mm diameter pocket resulting from the simulation in FreeCAD measure as 16 mm. Loading the GCode in CAMotics results in a pocket of 16 mm. Cutting the pocket on the Shapeoko results in a pocket of 15.5 mm. A Profile Edge operation of the same face results in a cut accurate within 0.05 mm. For this reason, I have been following up all Pocket operations with a Profile Edge operation of the same face.

Speeds and Feeds
These settings have worked for me so far cutting 1/4" plastics. The stock Carbide3D #102 endmill would crash while drilling holes quickly, so I switched to the bit below, and that fixed the problem.
Material - 1/4" ABS and HDPE
Endmill - 1/8" mm Spiral 1-flute bit - ... UTF8&psc=1
65.00 mm Horizontal Feed
22.00 mm Vertical Feed
1.585 mm Step Down Expression (depth per pass)

The feeds are inputted into the Tool Controller for the Job but the step down is inputted at the bottom of the SetupSheet spreadsheet that is automatically added to the Job. The step down defaults to the tool diameter which I found to be a bit too much.

I used the following version of FreeCAD for my testing - FreeCAD Version: 0.18 15860 (Git)
If you would like to learn the basics of FreeCAD Path, Sliptonic has a series of tutorials on most of the operations


Post Reply