Machsupport Forum
Mach Discussion => Mach4 General Discussion => Topic started by: OHICAD on August 24, 2020, 01:10:12 PM
-
We recently got the panel router here at the shop running and it's working great for making things flat, but any time I've produced any g-code from Fusion360 it loses its Z reference.
Sheetcam generates g-code that does not cause such issues.
I'll admit that I'm a bit out of my depth on this side of things, would anyone have any ideas about why the machine would be losing its Z ref?
-
Are you talking about 3D cutting when the machine looses position, if so it could be that the motor tuning on the Z axis needs slowing down or the accel/decel needs upping to stop it loosing position.
-
Are you talking about 3D cutting when the machine looses position, if so it could be that the motor tuning on the Z axis needs slowing down or the accel/decel needs upping to stop it loosing position.
It's losing z ref when the machine finishes a cut, retracts, rapids to the new start point, and comes down with an entirely new z ref. I've had it lose small amounts coming to something like 0.1 inches and large amounts like 4 inches. My current thought is that it's partly how the machine is setup and partly the g-code being produced.
Additional wrinkles, we are using servos rather than steppers.
Bear in mind it only does this with g-code generated from Fusion 360 and both the Mach3 and Mach4 posts have the machine do this.
-
from yours post sound like its some thing wrong with the pp in Fusion 360
try send sample of small nc file that work good and one sample that make that error
try both will be with same tool and same cuting depth ,so we can try help here
-
from yours post sound like its some thing wrong with the pp in Fusion 360
try send sample of small nc file that work good and one sample that make that error
try both will be with same tool and same cuting depth ,so we can try help here
Here you go,
-
i don't know which file work which not but i see 2 different
1. nc files the z top its 0.3937 while in tap file its 0.2
2. tap file you have in each time go to z the command S5903 i don't know what is this mean?
3. nc file height correction line its"G43 H103" while in tap its "G43 Z0.6 H1" why this z in the line?
-
i don't know which file work which not but i see 2 different
1. nc files the z top its 0.3937 while in tap file its 0.2
2. tap file you have in each time go to z the command S5903 i don't know what is this mean?
3. nc file height correction line its"G43 H103" while in tap its "G43 Z0.6 H1" why this z in the line?
Here's what I can clarify and answer,
1. The .nc file is generated by Sheetcam, the .tap files were generated by Fusion360 using their published post processors.
2. The Z axis on the machine has about 12" total travel and the stock is usually between 2-4" in height, so having retracts at that height are not a problem.
3. The tool used in Fusion for this sample had a spindle speed of 5093 RPM, so I suspect that is the Fusion post being very redundant and setting the spindle speed again.
4. I have no idea why there would be any tool height correction (G43) in the g-code for either the .nc or .tap files. I suspect that tap file is essentially saying move the tool up 0.6 inches plus the height listed in H1.
I'll admit to a moderate degree of uncertainty here, don't forget I'm about as competent on most of this as a reasonably clever hamster.
-
I've also contacted Autodesk about this, if I end up with an answer from them I'll make sure to share the findings here.
Marc
-
you can at first step ,change this by notepad and test
but i also suggest you use same tool ,same program(more or less) to be sure the nc file its the problem
-
I switched from Fusion360 to Sheetcam due to this issue. Since sheetcam is not creating this problem I included the file to provide a possible means of diagnosis from something that does work on the same equipment vs something that doesn't.
-
The more I read, the more I suspect that G43 is the problem.
-
so ....change by notepad and test
-
Doing so, just trying to find the time to do it.
-
Nope didn't fix it, tried it with a different job, still losing Z with code generated by Fusion 360
-
The Autodesk rep said it looks like a post problem and gave the issue to someone else.......
Disappointing.
-
This from the autodesk support folks:
"delete this in the NC code in all spots where it shows up and carefully take a trial in the machine.
G20
G28 G91 Z0.
G90"
Did so and the problem appears to have ceased, which makes me wonder why those codes ended up producing this issue.
-
Read this and see if you can glean any info regarding your machine and G28. G28 can be a weird one!!
https://www.mmsonline.com/columns/g28-versus-g53
Tom