FreeCAD Gcode not working in Linuxcnc

Thank you for your engagement. That is exactly what I drew in Freecad, lcnc draws huge circles.
I just wonder why the postprocessor from freecad for Lcnc don't match.

​​

Yes, It does seem that LinuxCNC is interpreting it incorrectly.

If you zoom in a long way where the circles intersect on the left side then you can see the rest of the plot.

It may be best to raise a new issue on Github.
github.com/LinuxCNC/linuxcnc/issues

I opened an issue on Github, thank you for the link.
@ phillc54: just curious; how did you edit that file to change the lines with the big numbers,
did you do all by hand or did you write a macro in vim or did you use Excel or libreoffice?

By hand, it is easy to find the required line by selecting it in the preview.

Looks like Linuxcnc is doing what the g-code says.
The huge I and J numbers are just wrong.
It has to be a Freecad issue.

No, the huge numbers are perfectly valid to define an almost-straight arc.

The problem is that LinuxCNC is seeing a start and end point of the arc with such a small angle between them that it assumes that the start and end are identical, and that a full-circle is required.

The underlying cause is assuming that a very small angle is enough of a check, whereas there should also be a check that the distance between the start and end is very, very tiny too. (it's really a check that they are identical, with some allowance for digits of precision)

Fixing the actual tool motion was fairly easy, but it took me longer to fix the graphical preview, which uses different logic.