Arcs explode in UCCNC (Solidworks generated gcode)

[Santtu]

Hi,

I'm trying to draw a wakeboard and the front and back where there are tighter curves does not seem to output properly. The workflow is Solidworks -> Solidworks CAM with MACH_III_G54 post processor -> UCCNC -> Stepcraft. The file seems to be ok in Solidworks CAM NC Editor but when I load the same gcode file to UCCNC (or https://ncviewer.com/), I see that the curves become huge circles, like the center point would be in a wrong location. I thought this could be a visualisation problem but the cnc machine also starts to do this huge circle. I have isolated the problem to be the contour mill and have excluded everything else to make debugging easier.

This is how UCCNC and ncviewer.com draws the file

This is how Solidworks CAM NC Editor looks like

The gcode file attached as .txt. I can't figure out if there is a setting in Solidworks which makes this happen, this is the first time I'm seeing this but is sure annoying... It's just the contour mill which fails, all other operations are fine.

Any help would be highly appreciated

[cncdrive]

Make sure the Arcs coordinates are set as "incremental" and not "absolute" in your CAM software, otherwise the toolpath will look like as on your picture.

[ger21]

Does the post you are using use absolute IJ mode? UCCNC uses incremental IJ.

[Santtu]

Thank you so much for your replies, it helped me to look at the right direction! I can confirm that the incremental/absolute IJ was the problem, when I drew the gcode manually with https://www.geogebra.org/m/VWN3g9rE I observed exactly this behavior (see the picture with correct IJ coordinates).

The solution, however, was not that clear. There is no option in Solidworks CAM for absolute/incremental IJ (or for anything else) so I changed the post processor to something else than MACH_III_G54 and then back. This seemed to fix the problem... Not quite happy with this 'solution' but it seems to work now. Maybe there was just a glitch in SW CAM...

[ger21]

Mach3 can use either absolute or incremental IJ, so the post is probably good with Mach3. But UCCNC requires Incremental IJ.

[cncdrive]

The RS274NGC standard says that it has to be incremental, so that is the standard.
Mach3 implemented some codes G90.1 and G91.1 to switch between incremental and absolute, but these g-codes are not standard.
Anyways, so far what I saw CAM softwares basically all had the option to switch between incremental and absolute output, so it should be not a problem that UCCNC supports only the incremental mode.