Update: In my case the anomally was caused by the backlash setting, removing it, the anomally disapeared!
I am getting an anomally using Pathpilot 1.9.12 on a Tormach machine.Sprutcam 7, I see this on different diameters always at the same spot in a radius, It appears to be where the XY transition takes place, this happens in the X plane transition, also in Y but it isnt as pronounced, it looks like the tool stops and rubs before continuing, it is mainly cosmetic but I sure would like to know what causes it..
I increased the preload on the spindle, (has always been too low).
I removed the backlash settings for the X and Y axes.(seems to make no difference)
I tried different diameters.
I set the error setting in sprutcam to .0001
I have the radius with arcs selected in Sprutcam, with this setting I get a nice smooth contour except where it makes the transition.
I havent been able to figure it out???
Maybe I am just too picky............ or nuts ha!!
Similar Threads:
mike sr
Update: In my case the anomally was caused by the backlash setting, removing it, the anomally disapeared!
mike sr
I tend to setup my profile operations with a lead in and lead out tool paths.
I recently noticed I get some sort of pause or bump when the tool gets to the end of the curved lead in.
Code and picture of a line lead in for a normal profile operation. . This code executes with no delay, pause, bump.
N2030 X-0.114 Y-0.8547
N2040 Z0.15
N2050 Z0.1075
N2060 G1 Z-0.215 F20.
N2070 X0.0025 Y-0.42
N2080 Y0.37
N2090 X-0.0622 Y0.6115
N2100 G0 Z0.15
Same operation with a curved lead in for the profile operation. This causes a delay, bump, whatever, right when the cutter finishes the curved lead in and starts the cut.
N4140 X1.7582 Y0.7318
N4150 Z0.15
N4160 G1 Z-0.5125
N4170 G3 X1.6 Y0.35 Z-0.5125 I0.3819 J-0.3818
N4180 G1 Y-0.35
N4190 G3 X1.6957 Y-0.581 Z-0.5125 I0.3267 J0.
N4200 G0 Z0.15
Any Ideas on what I have set wrong in Sprutcam, pathpilot. or other?
I just replaced my controller with a new tormach controller and I didn't notice this problem before.
Any help would be great!
Look at what your G64 is set to. That can do things to toolpaths.
Last edited by shred; 06-18-2018 at 11:12 PM.
I have noticed this when cutting my woood parts at a high feedrate but only on the start of the cut as you describe, I do have it set to cut with arcs instead of short line segments, this smooths out the arcs but I get the "hesitate-bump" on the start of the cut when the arc in ends and the straight section begines.
I am very interested in what you find out .....................
mike sr
I didn't have this problem before. All I did was replaced my old Mach computer with a new Tormach controller with PP 2.x and now I have some silly issue. This pause happens only on lead in and no problem on lead out. Direction makes no difference and the only way to avoid the problem now is to change to angled lines "no curves". I only find the problem with Sprutcam 2d contour operation. I don't see the same problem in any other operation. The reason I posted code snips for experts around here to look at.
Was hoping I could get someone else to try this. Very easy to duplicate in the air and see on lcd.
(2D contouringEnds)
N1710 T9 G43 H9 M6
(0.500 End Mill HSS)
N1720 S3450 M3 M8
N1730 G0 X1.6009 Y0.7267
N1740 Z0.15
N1750 Z0.1075
N1760 G1 Z-0.215 F20.
N1770 G3 X1.5 Y0.35 Z-0.215 I0.6525 J-0.3767
N1780 G1 Y-0.35
N1790 G3 X1.5647 Y-0.5915 Z-0.215 I0.483 J0.
N1800 G0 Z0.15
Have you tried different settings for G64? That's one of the changes between Mach and PP that affects cut toolpaths without any change to the source G-code.
It seems like it shouldn't really be a factor here, but it's a very quick MDI or code-edit to try.
https://www.cnczone.com/forums/torma...6-tormach.html
G Codes
The old computer was running pp1.9.x and I had no problem. I switched to new computer and newer pp version is all.
Anyway I guess were in the right area! the quote from Linux cnc site "velocity will be reduced if needed to maintain the path" is what I see is going on.
Any Idea on what has changed and why others don't have this issue?
Is Sprutcam the only program that generates this problem with code?
Does Fusion generate code with this issue?
Not doing anything fancy here and wondering why all the other master machinists out there have not run onto this problem years ago!
The old computer was running pp1.9.x and I had no problem. I switched to new computer and newer pp version is all.
Anyway I guess were in the right area! the quote from Linux cnc site "velocity will be reduced if needed to maintain the path" is what I see is going on.
Any Idea on what has changed and why others don't have this issue?
Is Sprutcam the only program that generates this problem with code?
Does Fusion generate code with this issue?
Not doing anything fancy here and wondering why all the other master machinists out there have not run onto this problem years ago!
No idea why it changed. FWIW, the default Tormach Fusion360 post outputs just "G64", which is the velocity-at-all-costs setting so unless people change that, they're likely to not see the bump much (assuming this is what's causing it). If your post never outputs a G64, the controller probably sticks with whatever the default is or maybe even whatever it was last set to which might change between PP versions.
I tweaked my F360 post to make the G64 value a parameter which is what Tormach/Autodesk/Sprut should probably be doing. I'll make a topic for that separately.
Last edited by shred; 06-19-2018 at 11:14 PM.
I've also noticed what appear to be very brief pauses when the Y-axis direction changes. Now that you mention it I believe that this started when I added "G64 P0.005" to the post for Vectric Cut2d. I'll try to remember to test things tomorrow with and without the G64.
This seems to be a reproducible bug and a tracker (in LinuxCNC) has been created:
https://github.com/LinuxCNC/linuxcnc/issues/447