Grbl supports G2. Vectric products support G2. PicSender supports G2. UGCS supports G2. Easel does not support G2 even if you are just using Easel as a G-code sender.
Strange, because this is the fifth sign that Iāve made with the same program.
I just re-calculated the tool path and named it as something else.
Its running right now but it will be ~1 1/2 hours before I know if it works.
I still would like to know why something like this happens and how to find the problem.
You must have changed something when recompiling. It has happened to me before, too, with VCarve gcode. It is an arc problem that Grbl has detected.
āError:33 The motion command has an invalid target. G2, G3, and G38.2 generates this error, if the arc is impossible to generate or if the probe target is the current position.ā
Not sure āfinding itā any closer than this will help to fix the problem.
I avoid G2/G3 commands when running Grbl. What VCarve post processor are you using? The one for XCarve by Edward Ford (X-Carve_inch.pp) has G2/G3 commands edited out to avoid similar errors.
"+================================================
+
- Grbl - Vectric machine output configuration file
+================================================
+
- History
- Who When What
- ======== ========== ===========================
- EdwardP 11/02/2015 Written from Grbl_mm.pp but
-
set G20 - EdwardP 11/02/2015 Commented out arcs as these
-
slow GRBL performance appear -
interpolated anyway - Mark 24/11/2015 Updated for interim 0.9 spec.
-
Renaming to be machine specific. -
Removing M30 from Footer.
+================================================"
John
EDIT: Jan, my face is very red. My research shows that the pp you are using came from me. Since posting it to you (in Feb 2017?) I found that some of my VCarve files would throw errors, and I no longer use it. Please accept my apology. Switch to the X-Carve pp if you have it. It does not use the G2/G3 commands. It uses very short straight line segments to simulate arcs.
John,
Thank you for the reply.
The only thing that I changed is the cutter speed from 70imp to 90ipm.
And the step over from .010 to .015
I made these changes to reduce the machine time.
I donāt understand because Iāve done this before on other programs with no problems.
I will switch to the X-Carve pp and try it again.
But for now, its getting late for me and it will be next week before I get a chance to get back into my shop.
Thanks for your help.
Jan,
I found that the errors are very inconsistent in occurrence, sometimes happening only after many other G2/G3 commands completed successfully in a file, and only in some gcode files, as you also found. Drove me near bonkers trying to find the cause. It is apparently some type of an incompatibility between VCarve and Grbl, probably in the math computations for arcs each uses, but as to which is āwrongā it is impossible (for me) to determine. Maybe some programmers smarter than myself can explain it, but I now just avoid all G2/G3 commands with Grbl, and problem solved for me.
You can avoid this problem by eliminating arcs from your G-code.
You might want to open a trouble report with the Vectric people as that is where the arc commands get generated.
They have been very responsive when I have contacted them.
You can also check your G-code in advance by using the $C button in PicSender.
Ok,
Both you gentlemen are talking waaaay over my head now.
I googled G2 and G3.
It appears to be used for either clockwise or counterclockwise movement.
In my simple mind, you would still need that option for cutting efficiently and clean side cuts.
I wouldnāt even begin to know how to eliminate the code.
It depends on the post processor you use. Some post processors allow arc commands and some do not. To eliminate arc commands you would use a post processor that does not allow arc commands.
You can think of a circle as an arc. You can draw that with one arc command (G2/G3) or you can break the circle up into very small straight lines that approximate the circle.
If your post processor uses arc commands it will send one command to grbl and grbl will break the circle up into very small straight lines to approximate the circle.
If your post processor does not allow arc commands, then Vcarve will break the circle up into very small straight lines to approximate the circle and will send 10s to 100s of commands to grbl.
Easel does not use arc commands, and it will not pass arc commands as a G-code sender.
Other than that, I suppose it is just personal preference.
Ok, now youāre starting to talk about Easel.
Please keep in mind that I do not use Easel at all.
I use Vectric desk top exclusively.
Noted. Just answering Angusās question.
Gentlemen,
Changed the post processor as suggested.
Ran all day yesterday and currently running today without a hitch.
Thank you once again for your help.
1 Like