I have been carving some clipart and I am getting a GRBL error I can carve the roughing toolpath 1.54 hours and the finishing toolpath 1.26 hours both without any problem, but the profile stops after 1 minute
the error is ( caution GRBL detected an error if a G code error it is on or before line 81)
I have run this file several times without any problems, and I have had this same error on different files lately
I have just upgraded from V carve pro to Aspire, has that anything to do with the problem
What error?
As I mentioned above, that is all I got
( caution GRBL detected an error if a G code error it is on or before line 81)
Exactly like that? That doesn’t make sense. What sender?
Can you get a screenshot?
Can you share the gcode around line 81?
There are a lot of grbl errors. Grbl will report an error number.
Neil, thank you for trying help, I am using Picsender and this is the pop-up error, it says read message above but there is no message [image]
G code
1
G17
G20
G90
G0Z0.8000
G0X0.0000Y0.0000
S16000M3
G0X3.1624Y0.7874Z0.2000
G1Z-0.0555F10.0
G1X3.2177Y0.8939F40.0
G1X3.2357Y0.9295
G1X3.2530Y0.9656
G1X3.2699Y1.0025
G1X3.2863Y1.0403
G1X3.3022Y1.0789
G1X3.3177Y1.1182
G1X3.3325Y1.1582
G1X3.3469Y1.1988
G1X3.3606Y1.2399
G1X3.3737Y1.2815
G1X3.3862Y1.3235
G1X3.3980Y1.3658
G1X3.4092Y1.4085
G1X3.4196Y1.4513
G1X3.4294Y1.4943
G1X3.4385Y1.5379
G1X3.4604Y1.6472
G1X3.5072Y2.0201
G1Y4.2841
G1X3.4903Y4.2921
G1X3.4567Y4.3085
G1X3.4228Y4.3261
G1X3.3892Y4.3444
G1X3.3559Y4.3635
G1X3.3230Y4.3833
G1X3.2904Y4.4039
G1X3.2581Y4.4251
G1X3.2262Y4.4471
G1X3.1948Y4.4698
G1X3.1637Y4.4931
G1X3.1331Y4.5170
G1X3.1029Y4.5415
G1X3.0731Y4.5667
G1X3.0439Y4.5924
G1X3.0151Y4.6188
G1X2.9869Y4.6456
G1X2.9591Y4.6730
G1X2.9320Y4.7009
G1X2.9054Y4.7293
G1X2.8794Y4.7582
G1X2.8540Y4.7875
G1X2.8292Y4.8173
G1X2.8050Y4.8475
G1X2.7815Y4.8782
G1X2.7587Y4.9092
G1X2.7366Y4.9406
G1X2.7152Y4.9724
G1X2.6946Y5.0046
G1X2.6747Y5.0371
G1X2.6556Y5.0699
G1X2.6372Y5.1030
G1X2.6240Y5.1283
G1X2.6070Y5.1273
G1X2.5477Y5.1229
G1X2.4842Y5.1168
G1X2.4181Y5.1093
G1X2.3519Y5.1007
G1X2.2881Y5.0914
G1X2.2292Y5.0817
G1X2.1782Y5.0721
G1X2.1368Y5.0628
G1X2.1034Y5.0542
G1X2.0679Y5.0444
G1X1.9915Y5.0214
G1X1.9122Y4.9953
G1X1.8317Y4.9667
G1X1.7522Y4.9364
G1X1.6759Y4.9053
G1X1.6045Y4.8739
G1X1.5722Y4.8588
G1X1.5398Y4.8429
G1X1.5100Y4.8288
G1X1.4796Y4.8163
G1X1.4501Y4.8067
G1X1.4218Y4.8013
G1X1.3833Y4.8032
G1X1.3538Y4.8146
G2X1.2898Y4.8697I0.045J0.117
No issues there.
It’s unfortunate that picsender doesn’t report the error.
Can you try another sender?
Sometimes reported errors are due to USB communication issues. If you can upload the entire file, I can check it out.
Patrick,
First, your code snippet does not produce an error here.
Second, I purposely changed the last line to generate an error, and this is what displays. The error number is in the message above the error box in red text.
What does your error report?
What PicSender version are you using?
Since VCarve 10.5 is being widely reported as having the same problem with arcs in grbl due to a change in the post processor, I wonder if Aspire has the same problem?
Hey @JohnChamplain, I’m glad to see that pic sender does, in fact, show the error number.
It does.
1 Like
John
the version of Picsender I am using is 3.3.5 and the error code is 33, I did not see the error at first, my fault
I did run the code again using Vcarve Pro instead of Aspire and again both roughing and finishing toolpath’s went well but it failed on the profile toolpath, it went a little further to line 142
the version of Vcarve Pro is 10.5 the same as aspire, I am waiting for fo a reply from Vectric but it seems to be the upgrade on both software that is causing the problem, maybe the Postprocessor
Neil
do you still want the entire file
Patrick,
I have not investigated the post processor issue, but others have reported that switching back to using the post processor from VCarve ver 10.0 works for them.
Thank’s John, I will wait to hear from Vectric first in case there is a fix, but I will keep that in mind
Why aren’t there parentheses around G code and 1 at the top of the file? A line number usually has N in front of it. So I copied what you posted and ran it in mach 3. It came up with the line errors because of no parentheses. I put brackets around them and it runs. It kind of stops at line 77 and there is a message that said " Too fast for pulley using Max.". I’ve never seen that before.
Apparently that message has something to do with the spindle speed. I don’t have a machine hooked up to my desktop, so I don’t know if this is a problem or not.
I removed one zero from the spindle speed and that took care of that. I also stuck in an M30 to reset the program at the end.
It’ll run to the end of the shape ( backwards C sort of ) and then reverts back a bit to a segment around line 87 and doesn’t reset.
So I stuck an M30 after line 76 and it does stop there and reset. I think you have something wierd going on after that point.
For anyone having problems with VCarve 10.5 and error 33 (G2/G3 arc gcodes), I have posted the file locations for the post processors on my computer. I recommend copying the older post processors from v10.0 or v9.5 VCarve versions to the My_PostP folder in v10.5 for testing. This way the v10.5 original post processors will not be disturbed. When you go to generate a gcode file, the only post processors you will have to chose from will be those you saved to the My_PostP folder.
I hope this helps.
Vectric VCarve Post Processor Locations
C:\ProgramData\Vectric\VCarve Desktop\V9.5\PostP
C:\ProgramData\Vectric\VCarve Desktop\V10.0\PostP
C:\ProgramData\Vectric\VCarve Desktop\V10.5\PostP
C:\ProgramData\Vectric\VCarve Desktop\V10.5\My_PostP
XCarve/Grbl post processor files
Grbl_inch.pp
Grbl_mm.pp
X-Carve_inch.pp
X-Carve_mm.pp
Vectric readme.txt file in My_PostP folder
“If any post processors are placed here, they will become the only ones displayed
in the Post-Processor list.”
2 Likes
Thank’s Martin
this is the reply from Vectric
Many thanks for your inquiry.
I think that it might be the case that your particular configuration has problems running arc moves.
Could I please ask you to download install and select the attached post processor
to see if this resolves your problem.
Please find the attached post processor (link below).
Please copy the file to the “PostP” folder of VCarve Pro.
Thank’s John
I did get a reply from Vectric before I read your post, telling me the same thing, the sent me a link to a post-processor, I am not sure which version it is from but I put it in my post-processor, and it is the only one in there now, it is working fine at the moment, it is X-carve inch (*gcode), do I need to put X-Carve_mm.pp in there as well in case I do any work in millimetres
1 Like
Patrick,
I have not looked at the mm pp, so not sure. I’ll dry run some tests when I can make time. Maybe Neil will know.