Strange milling error that I do not understand.

I’m fairly new to sheetcam and CAM in general so I may not use the proper terms while describing this problem. Its a problem I can work around, but I’d like to understand where its creeping in…

The setting : 14x24 CNC mill. .125" single flute end mill. Driving with Mach3. Sheetcam to generate gcode. Original drawing in CorelDraw.

Lets assume I want to cut a 2x2 hole in plastic sheet. Sheetcam shows the plunge, a move X, a move Y, a move X, and a move Y back to the origin plunge. Mach3 shows the same. When I mill the part that is in fact what it does… however, I would expect the inside rounded corners to match. Instead the radius of the plunge is as expected. The other 3 radii are noticeablylarger. The side to side / end to end dimensions of the hole are correct.

If I radius the corners of the hole with a radius slightly larger then my tool size, the corners all match. And of course I do not have the issue if I cut on the outside.

I just don’t understand where the error is coming from and some pointers would be extremely helpful.



Could you attach a copy of the job file. I’ll take a look and check the settings for you.

I havent had time to just do up a quick sample of the problem, but here is the full job I’ve been running. All the holes it cuts are square/rectangular inside routes and they all have differing inside corners.

I’m a little late, but sounds like you have either backlash problems on the mill… or possibly an issue with reaching exact position before it starts to take off in the next direction.

This usually only happens at pretty fast feed rates… you are only moving 8 ipm, I see this typically when I get up to 40-60ipm, the X axis starts slowing down in anticipation of the Y axis taking over, and the Y takes a bit to get up to speed, on inside corners this will cause the effective radii to be bigger than the actual cutter.

You can call up a G code, G61 on my machine, that means exact stop, it won’t start moving y until it reaches the end of the X travel and so on. Without that being on, it will always anticipate and start moving one axis before the other is completely in position.

Interesting. I’d never have thought that one axis might start moving before another. I was able to work around my issue by changing that initial plunge to a radius and I haven’t revisited things. I think I need to get some sacrificial foam and just do some experimenting.

Thanks for the pointer, I’d never have thought to look in that direction…

Could be an accell/decell setting in Mach 3 too… I’m honestly not that familiar with it.

Where we used to see the problem is when doing an outside contour, if you had a 90º corner and it needed to be “sharp”, you would have to keep the feed rate within reason or you’d see the next axis starting to go before the last axis got to final position and it would give you kind of a tapered round off on the corner.

Been a while since I needed to use the CNC. Finally got around to playing with this error some more. Using G61 seems to solve the problem. I really need to spend some more time with this whole setup but at least I’m making it useful for some things at this stage.

Thanks for the reply!

Glad it worked out. I still suspect you might have some settings a bit out of whack if it’s having issues at feed rates under 50-60ipm, but hey, as long as it gets the job done, you can always work on things when you have time.