I made my first test cut on my new Nomad over the weekend using Winston’s old tool tray gcode. It encompassed a number of firsts–the first time I’ve used blue tape & superglue for fixturing (brilliant!), the first cut on my new Nomad (brilliant!) and the first time I’ve ever run gcode I didn’t generate myself (not so brilliant…)
All the circular holes for the toolbits were very juddery. I looked at the gcode in Notepad (it’s a Windows machine) and discovered there are no G2/G3 arc commands. Circles and arcs are rendered as tens of little linear moves, thus the judderyness.
I then imported the DXF of the tool tray into my favorite 2D CAD program and drew some modified geometry (larger square pockets for toolbit boxes and larger holes for bare 1/4" toolbits), loaded the new DXF into Carbide Create (the non-pro free version) and generated gcode for the cuts using the Nomad3 postprocessor (inches, thank you…)
This code also only uses G1 cutting moves, no G2/G3.
I know that CC Pro has the ability to use custom-made postprocessors. Is there a way to enable arcs in the garden-variety version? It is a shame for them to be commented out, because especially small arcs would be much more smoothly cut with G2/G3 than with a bunch of little G1’s.
There are no circle events getting sent to the post. Posts have onLinear & onRapid event handlers, but no onCircle or onArc handlers.
It’s apparent CC is only creating linear motion in the toolpaths. (Not unreasonable for a free/cheap CAD/CAM program.)
One thing that might help is a linearization tolerance that we could specify to get more or less points along a curve.
One thing that might help is a linearization tolerance that we could specify to get more or less points along a curve.
Thanks, Tod. But linear moves along a curve will still be juddery depending on their length and whether it will trigger deceleration/acceleration at each move…
I’m sure it would be much easier just to uncomment the G2 and G3 lines in the postprocessor.
I’m assuming that they are there in the CC postprocessors, because the postprocessors in MeshCAM 8 have the G2/G3 lines–they are just commented out, same as in 2015 when I uncommented them the first time in MeshCAM…
It’s not an end-of-the-world thing, because I’ll only be using CC for casual stuff–all the serious work I’ll run through the MeshCAM 8 that came with my new Nomad and where I can uncomment the arc commands…
The internal toolpath in CC doesn’t have arc moves. I linearizes all the curves based on an internal tolerance that we can’t change. Plenty good enough for hobby/gift/sign work.
So when you run the post, CC is not sending any arc moves to the post to be processed. Only Rapid & Linear moves.
If you’re doing work that requires a better surface finish or tighter tolerances, you’ll need to use another CAM system.
For me the issue is just smoothly feeding a tool in simple operations like boring small diameter holes with small tooling. Say 3mm diameter hole with a 1mm tool. The controller tends to pause quite a bit when loading in new commands and be a bit jittery when executing them.
Keeping a smooth chip load on smaller diameter tools just seems to make them happier and a G2/G3 is orders of magnitude smoother.
I assume the controller can do maths/interpolate arc points much quicker than it can ingest a similar required number of linear move commands
Once you dip down past a certain scale, even basic hobby/gift/sign/fixture work becomes less reasonable. Kind of a shame because CC is so simple that I reach for it over fusion whenever possible but the lack of arc moves can be just brutal.
A fun fact for folks using Fusion 360: Setting your tolerance too loose can prevent G2/G3 paths in post.
Turns out if your tolerance is too loose, it can cause the post processor to not recognize circular features as…circles. So it generates linear commands instead of G2/G3. If that happens to you, try tightening up your tolerances/smoothing.
I went back to 3D contour of a circle. The path is nasty.
I changed the default .0004 tolerance to .0001 and it makes the circular paths as expected.
Thank you !
The standalond command line program GCodeClean on GitHub will post process G-code, recognize arcs built up from line segments, and convert them into G2/G3 arcs. It has other G-code optimizations that can be turned on and off with command line flags and many have adjustable tolerances. I’ve used it with older versions of Carbide Create and other CAM software. The author frequents the Maslow CNC forum and has been quick to fix the few minor issues I found with older versions
