Help on understanding G Code data

I have generated a G Code file using Aspire for CNC Carving.
When I open the file in Luben it shows the actual paths in black.

There are some paths shown in light blue.

Can someone explain to me what those light blue paths are?

These light blue paths are also being routed resulting in the job being ruined!

I have attached the corresponding G Code along with what I see in LubanV-Carve 3-2.cnc (61.4 KB)

With Luban 3.11.0 I see:

and with the latest update today Luban 3.13.1 the image has changed to:

Does anyone have any ideas as to why this is happening?

M3 S12000 is not “great” gcode for the snapmaker, but will work for full speed

Other than that I can’t comment on why Luban does anything, but the gcode looks fine in ncviewer

I think Luban’s convention is Z=0 is the bottom of the workpiece, and your gcode is using Z=0 as the top, so I’m guessing Luban is rendering the XY plane as opaque, so you’re only seeing the G0 moves and none of the G1 moves which are all at a negative Z height.

From the side in ncviewer, the gray line is Z=0:

EDIT: refined S12000 opinion

It works with SM. Set spindle speed to 12000 rpm.



ErrCode ToolHeadCNC::SetOutput(uint8_t power) {
  if (power > 100)
    power_ = 100;
    power_ = power;

  return TurnOn();

It works because it truncates it to 100%. If you want 6000rpm you would use S50, not S6000

I never go less than full speed ahead. :wink:


Sorry complete nube to all of this so not sure what all of these numbers mean.
I was more concerned with the fact that the post process is provided by snapmaker, and when it was imported into Luben it shows some strange lines. I don’t know what the difference is between the light blue circles, and the black lines. I only expected to see the black lines, they would be the carving of the letters 20. When I ran this G Code it carved out the 20, but also carved out two circles relating to the blue lines.

Also I am a bit confused as to why 2 different versions of Luban should produce two completely different results for the same G Code file as shown in the images.
I have not tried to carve the second result.

From what I can see (from observations while routing) the CNC follows all paths as shown in Luban, which would probably mean the latest software would produce a complete mess!!

I don’t know why Luban does anything it does, but since Luban isn’t moving the machine, the controller makes things moves, it doesn’t really matter what Luban thinks the path will be. The gcode looks good when viewed in a viewer online.

The blue lines are the G2 moves in your cnc files. (G2 is making an arc around a certain center)
If you remove all those, you’re only left with the number 20 being carved. (I assume that is what you want?)

So Luban shows exactly what the gcode will do. It’s the same as what camotics shows. (That’s the previewer I usually use).

If you didn’t order those circles, then it must be an issue with V-carve or the post processor you’re using.

Thanks for all of you input, and explanations of some intricacies of G Code.
I guess this is a question I need to ask the Snapmaker / Luban people as to why their post processor is causing this to happen.

Which postprocessor are you using? Did you try the latest version from the github page? The last commit on that one is “fix arc movements” But not exactly clear what the changes do.

However, what does happen in the cnc file you posted every arc movement is a G2 clockwise arc, while some of them should be a G3 counterclockwise movement. So in stead of making a very short arc in the counterclockwise direction it’s making a very large one in the clockwise direction. Hence, the circles you see.

I haven’t looked at the documentation of vcarve and/or their postprocessor files but don’t see anything obviously wrong with the file on Github. GitHub - Snapmaker/snapmaker_cnc_post_process
So make sure that’s the version you’re running.

If you still have that problem: report an issue on the github page detailing this problem: Issues · Snapmaker/snapmaker_cnc_post_process · GitHub

In essence, what seems to be happening is that all arc moves seem to be converted to clockwise moves (G2) while some should be counter clockwise (G3).
Make sure you provide them with the necessary files to be able to reproduce that issue.

This file has it fixedV-Carve 3-2_fixed.cnc (61.4 KB) But you would also need to have the file before the postprocessing for them to easily understand where it goes wrong.

But first; try the last version of the postprocessor on github to make sure it’s still a problem

Thanks @brvdboss the version you pointed to certainly seems to have fixed the problem.

Next problem is trying to understand why the visualisation of the output from VCarve is different beween v3.11.0 of Luban and 3.13.1.
I guess that’s another topic for another location :slight_smile:

Did you ever solve this issue? I’m having the exact sam problem…

With the latest version of the post processor available on Git, all worked fine, as can be seem from the attached picture.