Faceted Curves

[rfriedeman]

I'm having a problem, and I'm not sure if it's UCCNC or my CAM, VCarve Pro.

When I'm doing 2/2.5D cuts, non-circular curves (so non-G2/G3 curves) are coming out very faceted. They look very smooth in CAD, the toolpaths I generate look smooth in VCarve, and if I render them in a separate GCode viewer like OpenSCAM, they also look smooth. But when I cut using UCCNC, they're super choppy.

UCCNC can clearly produce smooth results on my machine (a DIY machine using a UC400ETH and Gecko G540). Circular arcs look really good, and 3d toolpaths also are very smooth. It's only 2.5D that's a problem.

I'm running version 1.2037, the UC400ETH has firmware 1.1300, and I'm using the 2017 screenset.

A render of the toolpath in OpenSCAM

What I actually see when I run the toolpath

Any ideas?
Thanks
Rich

[spumco]

Maybe check Linear Error/Addition/Unify settings under General tab? Similar questions seem to come up from time to time on the forum and I think the default units are in metric and don't work well for inch-setting machines.

I think - think - that if this setting is too large it will produce faceting in the code execution but wouldn't show up in a backplot. Someone more knowledgeable than me will hopefully chime in.

[rfriedeman]

That certainly would put me in the ballpark. I'm using an inch-setting machine and inch GCode, so that would make sense. I'll check it out. Thanks!

[cncdrive]

Possible settings issue causing this is is what Spumco described.
The default CV tolerance is in the 0.03 units which is a low tolerance if the units are millimeters, but not so low if the units are inches.
0.03 inches is 0.762mm which is a large enough distance that it can be seen on the toolpath like yours.
The tolerance defines how much the UCCNC can run off the toolpath in order to keep the feedrate, so if you set the tolerance to 0.03 inches then you allowing the software to run off the path with max. that distance.
If you want the toolpath to be smoother then lower the CV tolerances, linear and corner error parameters on the left side of the General settings page.

[rfriedeman]

That was it. I run my toolpaths in inches, and the tolerances were at the metric-minded defaults. All better now. Thanks!