Greetings, I am new here, so ill start with a small introduction. I work for a company which produces motor drives and battery management solutions for multiple applications. I work in the mechanical department and my work also consists of creating parts in Solid Works, generating the g-code and cutting the parts on our CNC machine with mach3 software. We recently switched to a different post processor, and I was tasked to learn it and create test parts. What happened was that with the old post processor the parts came out correct, and with the new post processor they came out smaller (pocket sizes) around 0.5 mm difference than modeled. I used Solid Works cam 2022 and created my own tool library with all the tools we use on the CNC machine. I am certain that the tools were set correctly and all the diameters were correct. So now with the same tool in the CNC machine and two differently generated g-codes, the result comes out different. And I can't figure it out why this is happening. I would be very grateful if anyone has any info to share of a similar problem or if they know a solution to this. I tried a lot of things so far and nothing helped. I will try to respond regularly to extra questions. Thank you for the help in advance.
Hi Marko, Most of the time its machine related but it sounds like you have done your checks there. If you have the option to do a finish pass or water line type clean up try running it without these option(s) and see if that helps.
Thank you for the comment, I will try programming a fine contour pass to finish the job. But by comparing the g-codes, all the coordinates match up. Even if I made the pocket with a rough contour pass.
are both posts cutting in the same direction? this can affect outline sizes. maybe the new post is obeying a 'radial stock to leave' setting that the old one ignored? if you draw a 1 inch square and contour around it (and inside it as another test) in one pass, how do the gcode files compare?
Hi, same problem here. After checking calibration and a multitude of other things, I'm stuck undersized cuts. It's particularly the x axis. In a test cut of 30mm square, it is short for 2,5mm. After g code analysis, is seems to be the postprocesor problem. Anyone found a solution?
I'm running openbuilds lead 1010, Blackbox32, fusion 360 and latest post processor from github. I also tried two releases before, same problem.
So the options for off-size-but-correct-location are kinda limited, and you can check them in order: The designed feature isn't the size it's supposed to be (old file version?) The CAM is picking up the wrong contour line/faces (sketch vs model?) CAM has radial stock to leave settings (finish pass settings changed?) Machine is mis-calibrated (would scale the entire part accordingly) Machine has backlash (multiple features would be off-size) Machine is flexing (common on undersize pockets; reduce stepover, feed rate and/or add multiple finish passes) Tool is over/undersize (or the wrong tool was put in the holder/pocket) Beyond that, there's not a huge amount that can affect it. I doubt it's the post processor. Sometimes it's a combination of multiple issues. Sometimes you just have to look at the machine calibration file 75 times over three days before you see the glaringly obvious problem (which in retrospect, you definitely remember typing)
It seems that it was a assembly issue. One of screws on motor-screw attachment went loose. Not with postprocesor for sure. Although I cannot confirm for sure cuz machine stopped working yesterday. Control program just stopped running nc programs. I will report back after resolving this new problem.
We have a similar problem. Our Omio cnc machine runs on Mach 3 from Fusion 360 and has consistently cut extremely scaled down versions of our designs since firing it up from stagnation over the summer. There appears to be no issue with the machine itself and the designs are scaled correctly. Any suggestions?
How much smaller? Is it possible an inch design is being cut in mm ? Precise details help us diagnose the issue. Alex.
It is MUCH smaller, proportionally to all sides. At least 90% smaller than the various models we used
The measurement confusion was brought up, since one of our guys likes metric despite all of our stuff being imperial, but the machine was recently loaded up with an older file that should have been cut perfectly (it had been last time we consistently used the cnc) but it was scaled down to roughly the same dimensions as the ones we tried to do earlier
Check mechanicals first (grubscrews on shaft couplers, pulleys, stop collars, etc amongst others) Then run CONTROL > Wizards and Tools > Calibration
then it is critical that no gcode program should ever be missing a header G20 or G21 code. NEVER. (always set the modals to what is needed in the Gcode file = no surprises) I would issue some MDI commands setzero somewhere convenient G21 G0 X100 did X move 100mm right? if not, you have a calibration issue if yes you have a G20/G21 issue, probably.
I think @David the swarfer has hit the nail on the head. You are using Mach software and (I'm guessing) using a *.tap post processor? I've noticed those post processors don't put all the codes needed in the header when sorting problems in the past. Alex.
