Help with radius vs IJK

[Anonymous]

I'm running LinuxCNC Version 2.7.0 that came installed in Debian build 3.4.55-4linuxcnc i686.

I've been able to model, toolpath and machine from Fusion 360, but the models were simple(surfacing, drilling, machining out holes and such).  The next step was to try a 3d surface (model attached). It's a half-cylinder on its side.

I used the LinuxCNC post and posted it to the file test001.ngc(attached).  When I sneakernet the posted g-code out to the Linux machine in the shop and load it into LinuxCNC I get this error:
Near line 2405 of /home/ken/test001.ngc: Radius to end of arc differs from radius to start: start=(X-5.1010, Y0.2006) center=(X-5.0888, Y0.2224) end=(X-0.0208, Y0.3723) r1=0.0250 r2=5.0702 abs_err=5.045 rel_err=99.5073%

The next step was to consult the silicon oracle, where the answer was that I was in radius mode and needed to be in IJK mode.  The only thing that I could find in Fusion 360 remotely like that was in the post processor, where I selected "useRadius" "yes" (which would seem to indicate that I was already in IJK and was moving to radius) and posted to test002.ngc(attached).

Out to the mill and the response was:
Near line 2439 of /home/ken/test002.ngc: Arc radius too small to reach endpoint.

All the paths are just flat endmills.

.ngc files have been renamed to .txt for posting to the forum.

Any help would be greatly appreciated.

Ken

[randyT9V9C · Accepted solution]

Based on the line number of your error it appears to have an issue with the operation Pocket2. Your usage of pocket in this instance is wrong. Yes, fusion generated a path, but it is ugly.

It appears you attempted to make it work by changing the Tolerance to 0.0002" and Smoothing Tolerance to 2e-05 in (0.00002") on the Passes tab. Sometimes you can fix these kinds of issues by lowering the tolerance, so you were on the right track, but normally 0.0001" is adequate if the default causes issues.  I suspect the issue is a default in linuxcnc.

Your should read this thread about linuxcnc arc tolerance. It appears the default is set abnormally low out of the box. The thread is a few years old so YMMV.

https://forum.linuxcnc.org/20-g-code/28689-arc-tolerance

I believe you need to adjust TOLERANCE_INCH and TOLERANCE_MM in your linuxcnc ini file.

Post one path at a time and confirm the others backplot fine. Interestingly, I backplotted both your files without issue using NCPlot, and it normally complains when arcs don't line up within 0.001" by default.

Update: I fiddled with my backplotter arc fitting tolerance and your files. With the tolerance set at 0.0001" it complained but 0.0002" plotted fine. I set the tolerance and smoothing tolerance both to 1e-05 and let the computer crunch for a while. The path then backplotted with the arc fitting set at 0.0001 which really is more than needed imho.

[Anonymous]

Thanks! That sounds like good advice which I will try when the temperature goes down.

I think I originally had 3d Adaptive Clearing but was going through every strategy on the list just to get something to load at all. It makes sense that it would be in the controller, since that's the common denominator.

Fingers crossed...

Ken

[Anonymous]

Thanks! That sounds like good advice which I will try when the temperature goes down.

I think I originally had 3d Adaptive Clearing but was going through every strategy on the list just to get something to load at all. It makes sense that it would be in the controller, since that's the common denominator.

Fingers crossed...

Ken

[Anonymous]

Randy,

A combination of your advice and the LinuxCNC article was the medicine.  The addition of

#TOLERANCE_INCH = .002 and

#TOLERANCE_MM = "whatever"

was the answer.  Re-did the toolpath aid it was on.

Thanks very much.

Ken 

[Anonymous]

Randy,

I promise I'm not trying to be a help vampire.

After adaptive clearing worked, I tried to do some smoothing with parallel and got the same error from the controller machine.  They're very coarse passes, but I'm just trying to baby step to a something that works.

Is there another place besides the .ini file where a tolerance can be set?  Are "tolerance" and "minimum circular radius" in the post processor dialog applicable?

Line 1412 is the offending line.

Ken

[randyT9V9C]

Your g-code back plotted fine for me. Line 1412 precedes an arc in the ZX plane (G18). This is the only arc called out in this plane in the entire file.

1412: N7045 G1 Z-0.4968 F60.
1413: N7050 G18 G3 X2.1118 Z-0.4977 I-0.003 K0.
1414: N7055 G1 X2.1084 Z-0.4878 F20.

Like you, I think it appears to be  a minimum radius issue, most likely lead in/out. Try changing your lead in/out radii to something that is at least equal to the cutter radius. Some controls require the straight lead to be at least equal to the radius. The radius on the offending arc is 0.003". 😉

[Anonymous]

Sounds like a plan.  Thanks!

[Anonymous]

Thanks, changing the horiz. lead in rad to radius of cutter solved all the problems I have been having!!!

[Anonymous]

Hi

I have recently installed Linuxcnc 2.7. I have been having this problem with the start arc and end arc differ as many people are having with Linuxcnc. I have read up on many blogs about changing the tolerances in the ini files. I hav a mill and lathe setup and not any of the two ini files have tolerance_inch or tolerance_mm in them for me to change. I have also seen some patch at some blog but do not know if this will activate the function on tolerance in the ini files.

Could a more informed person maybe help me out on how to get to set these parameters if they are not in my ini files?

Thank you

[Anonymous]

Dont know if this helps, in your gcode with S1000 just before the first arc
start, there is probably a better way but that was easy solution for me.

[randyT9V9C]

Post up a sample of your code and/or your model and I'll take a quick look. Verify you have smoothing on and check your lead in/out radius is reasonable. I believe you may have to add the lines to the ini file to override the defaults. Depending on your build they may or may not be there by default.

[Anonymous]

Hi
Thank you for your reply. Just need to go get the code to load it. Do you perhaps have an example how to load it in the file if it is not there?