GCode doesnt match the toolpath

Hello Les.

I encountered a issue today that I think might be an issue with sheetcam. I am using 4.1.1 and have not tried to replicate it on other versions.

I have a DXF file (attached) of a gear. This particular gear (and I cut quite a few gears as building geared wooden clocks is my hobby) should have perfectly even teeth. But the gcode has uneven teeth, some with sloped sides and others that are not cut as deep. However, even after multiple passes the teeth cut exactly the same. I initially suspected my machine, as the toolpath displayed is also perfect, but ran the same DXF file it though a friends copy of VCarve Pro and the resulting Gcode gear cuts perfectly.

This only seems to happen with a couple of the smaller gears I have tried. The ones under two inches or so. I’ve cut dozens of larger gears and never had this happen.

One other thing I found out is that SheetCam is the best value out there. Things I could do in seconds took my friend minutes to do on his program that costs 8 times as much as SheetCam. I almost feel guilty complaining.

Hmm. Maybe it’s my lack of understanding. I notice that sheetcam’s gcode file is quite a bit smaller and it uses arc’s rather than a series of points. Is there a place where I set something like this for the output?

If the g-code displays correctly in Mach it has to be a settings issue in Mach or an problem with your machine. Try running a lower feed rate. Does that help? Try using exact stop in Mach (Config->general config->motion mode).

When SheetCam loads a drawing it will convert a series of lines that form an arc into a single arc. Arcs generally cut more smoothly thna a series of short lines. Howerver you can disable this. In SheetCam go to Options->application options->drawing import. Set the arc fitting tolerance to 0 and reload your drawing then run the post processor. The g-code will probably now consist of a lot of line segments.

Setting the Arc to zero seems to have helped quite a bit. It’s still not perfect and I see arc’s in the gcode although not as many. (I know that the arc’s are generally a good thing.

It’s not a Mach issue as the toolpath in Mach and also using NCPlot is off. It only looks good in SheetCam. Are there other settings I should try adjusting?

Sorry, I thought the paths looked right in Mach. I’ll take another look and see if I can figure out what is going on. The number of arcs should not make a noticeable difference to the final part.

OK, I’m confused. I just merged the two tap files together and loaded them into Mach. This way I could see both tool paths at the same time. I had to zoom in very close to see any difference between the tool paths at all.

I can’t understand how they would show differently in ncplot.

I didn’t try that, I just looked at them visually and it looked to me like it was off. Perhaps it’s a bug in Mach that’s specific to arcs? Let me chat with Art.

I still think it is more likely a tuning issue with your setup. Have you tried dropping the acceleration and maximum feed rate?

No I haven’t, but there are a couple things that lead me to think that its not my setup.

First it’s highly repeatable. The exact same teeth cut incorrectly even after a total reset of the machine. When I make multiple passes, they are cut incorrectly perfectly the same.

Second, the problem goes away when I remove the arc’s entirely, and when I use the sheetcam settings to minimize the arc’s it almost goes away.

I finally got a good picture that shows how much it’s off.

Hmm, Try this: Move the cutter to 0,0 and jog the Z down to make a mark on your sheet. Cut a gear then move to 0,0 and check it lines up exactly with the mark.

Missing steps can sometimes happen under very specific circumstances. Changing the arcs to line segments could make enough of a difference.

I talked with Art and he suggested that the acceleration value I set for my motors might be too low. I increased this from 1% of the speed to 20% of the speed and it seems to have made quite the difference.

I think I have stared at these teeth profiles too much as they still look off to me in the toolpath display sometimes, but when I really zoom in and look they are fine. I apologize for suggesting otherwise.