What's new
What's new

South West Industries Prototrak VMC2 RMX Control Strange Tool Motion


Dec 15, 2015
We are having tool path issues with our Prototrak VMC2 we received in July of 2023. The problem manifests itself in longer G code programs (saved as .GCD) with G02 and G03 moves not making the correct radius moves. The amount seems to be variable and only shows up in longer programs. If, for example, I edit a program to removing every but the problem area the new program will run without issues but as soon as I try to run the full program the errors come back. The machine will also run a program with all the arcs broken into line segments without issue but this either bogs the machine down or leaves a rough surface depending on the tolerance set in the CAM software. The machine seems to run fine using it's built in conversational programing. I can't seem to upload a video but if you watch the "Show Path" on the control it will actually show the tool deviating from the programed path. I may have to sign up for Imgur or something so I can link it.

We have been in contact with the factory and our factory tech has been fantastic. He has done everything he can as far as troubleshooting and replacing electronics and mechanicals. I feel like we are at the point that this is definitely a software issue but I can't seem to get anywhere with South West's software people. In fact the only time I seem to hear from them is when our tech prods them. We just got the most recent version of software installed on out machine and it hasn't fixed our issue.

I am just trying to figure out if we are the only ones with this problem or if there are others who have run into this. If there is anyone with another VMC2 that is willing, I will send a copy of my programs to see there are the same issues on other machines.


Here is one example, the part on the left was programmed using the Prototrak conversational software and the part on the right was a G code program done on Mastercam. Notice the oblong counter bores on the legs and the diamond shaped center hole.

Here is our most recent issue:

I cut the 4 counterbores by "helixing" straight line moves with an 1/8 endmill. I unfortunately didn't have the finish pass set to be straight line moves. The machine cut the helix correctly but turned counterbores into hotdogs on the finish pass. The 2 bottom counterbores were cut with a program with only the counterbore tool path. The top 2 were cut with the same tool path in the full program.

I have attached the full program and the helix counterbore only program.


  • OP 1 Cage End Cap Helix Only.txt
    18.1 KB · Views: 2
  • OP 1 Cage End Cap.txt
    177.4 KB · Views: 4
Last edited:
I'm not seeing any issues with the code, but if the machine is choking on long programs I would not break up the circular moves into linear interpolation.
Try reposting the code to use just G3/2 moves instead of the linear breakup.
If that works then the issue would be with the controls software or hardware.
I'm not seeing any issues with the code, but if the machine is choking on long programs I would not break up the circular moves into linear interpolation.
Try reposting the code to use just G3/2 moves instead of the linear breakup.
If that works then the issue would be with the controls software or hardware.
That is how the clear acrylic pieces were programed. My pet theory that I have no way to easily test or prove is that the machines are running everything as metric in the background and the weird inconsistent circular interpolation moves are the machine trying to reconcile the stack up errors. I know every other machine tool builder does this, but when I set backlash constants on our older prototrak machines with SMX controls it changes the input value to a metric conversion, ex: .0010 becomes .000984. Our other machines also have to be run with straight line moves on more complicated program or else they will error out at some point in the program. I don't remember the exact error message but it is something to the effect of the end point and center point are irreconcilable. I was told this machine with the newer RMX control wouldn't have these issues

I could be way off base with my theory. That is why I am hoping to hear from others with this machine or possibly any machine with the RMX control if they have this problem and/or could help me test it.

Or maybe our machine is a special little unicorn.
I've got a unicorn FANUC 31i that will randomly mill through the side of one part into the next if nano smoothing is turned on in one particular program.
Sent the program to FANUC and they couldn't figure it out either.....

I only have FANUC and Yasnac controls here so there isn't much more I can do.

The only other thing I can think of is to be more explicit in the G2/3 moves, like this:
X.7996 Y-.742 Z-.1138
X.7935 Y-.7408 Z-.1144
X.7874 Y-.7404 Z-.115
G03 X.7874Y-.8344 I0. J-.047
X.7874Y-.7404 I0. J.047
X.7874Y-.7874 I0. J-.0235
X.7874Y-.7394 I0. J.024
X.7874Y-.8354 I0. J-.048
X.7874Y-.7394 I0. J.048
G00 Z.1

The post is omitting the X position that shouldn't be needed but it doesn't hurt to add it.
I finally had a chance to test the program with the X values added and unfortunately it didn't have any effect.

Thanks for the suggestion though.

I think I finally got the software people at SouthWestern Industries to understand and acknowledge the problem last Friday but I still haven't heard back from them. If anyone has any suggestions or any experience with this I would be interested to hear it.
I think we finally figured out the issue. It turns out the K value from the drill cycle is modal and was being applied to the G03 moves as a Z center. Why that affects a circular interpolation move in XY doesn't make sense to me but when I added a K0. to the first G03 move after the drill cycle the tool path cut correctly.

Our CAM provider updated our post to output a K0. on the first circular interpolation move after a drill cycle. I think this is solved but I will update this if any new issues arise.
I think the reason is SouthWestern can do whatever want with how their machines interpret G code and that is how they chose to interpret it.

I do agree that it shouldn't be interpreted that way or should at least be canceled at the G80 when the G83 drill cycle is canceled.
I may be missing this and it may have already been adressed but does the vmc have the trak control or the siemens control?
edit : NVM it is in the title my bad. :nutter: