Good morning all. I'm in the start of a project and have an issue with the new release of the Open Builds Controller Software. For some time now I've been getting prompted to update to the current version. Yesterday I was getting tired of that so I did it. The 1st file I tried to cut resulted in a Grbl error. I'm using Carve-Pro 11.5. I reverted back to early versions of Vcarve with the same results. I have no way to return to the older OB Controller software so I'm dead in the water. I've attached a screen shot of the error as well as the GCode file. Any Ideas/suggestions? Mark
CONTROL just acts as a middle man between the GCODE and the FIRMWARE. It sends the gcode along, if the firmware doesn't like it, the firmware raises an error. CONTROL is literally just the messenger. So no, this cannot be update related. Your gcode, was not liked by the Firmware, and it asked us to show you a message. that's all. Learn more at Grbl v1.1 Interface As for the error, exactly as it says onscreen, your gcode contains an uncomputable Arc. Are you sure you have the correct post processor?
Peter thanks for your quick reply. I have been using my machine on a regular basis making some boxes with an stl carved onto the top. No issues with them and they carved great. I never the less checked the post processor that was installed in Vcarce v11.5 and it was the "OpenBuilds GRBL Inches". The machine controller software was also set to inch-mode. The project which I'm working on now with the problem is a Vcarve/inlay cutting board. I was running some Start/Flat depth tests for good inlay fit using part of the design svg. This was done using the previous version of OpenBuilds CONTROL. I did not have any issues while doing the tests. Plugs and pockets were cutting out just fine. No GRBL errors were encountered. I decided to use a different angled V bit. In Vectric I created the project and generated the G-code files using the Vcarve option. Once I got back into my shop the software upgrade prompt was displayed again so I decided to go ahead with the update. Once done I went and ran the new test using the star outline Gcode files. The pocket clearing/profile operations ran just fine. When running the plug files the clearing operation went fine and the GRBL error was generated on the profile operation. Because I had not had issues previous I assumed there was an issue with the CONTROLLER upgrade and made my post on the forum. There was a slight upgrade to Vcarve available. I made that upgrade and also downloaded the post processor files. CONTROLLER software was set to inches mode and the post processor used was "OpenBuilds GRBL Inches". I ran the Gcode based on the star shape and generated the GRBL error on the profiling operation. I then ran that 3d stl file and had no issues completing the task. Now I'm really confused! I have a MacBook and it has the older version of the CONTROLLER software. I hooked it to my machine, ran the Star Shape Gcode files and generated the same error 33. Now because I hadn't had any issues prior to using that star shape as my test I created another Vectric project using a simple circle. Created the needed Gcode files and they run with out issue I'm sorry for the length of this post but I tried to be as descriptive as possible. There are no post processor issues it appears to have something connected to the shape of the object. I have attached both the failing star profile Gcode file as well as that of the circle. Any additional ideas would be appreciated as I don't ant to proceed any further with my cutting board. - Mark -
Exactly, whenever someone blames "the update" i do chuckle a bit. OpenBuilds-CONTROL/CHANGELOG.txt at master · OpenBuilds/OpenBuilds-CONTROL shows up on the update window. It tells you exactly what changed. And in this case the host application cannot even be involved, errors are raised by the firmware in response to actual problems (like an arc that is incomputable, or other gcode errors) As to why Vectric failed to generate valid gcode there, you would have to contact Vectric Support. But usually playing around with correct Post, up to date Vectric (updates fix things... Updates are good) and double checking toolpath parameters will help
so that is what REALLY changed, the size of the bit. A lot of automation goes on in generating Gcode, I don't know VCarve but Fusion360 has defaults for leadin and leadout radii that end up creating very small arcs. If you look at the I and J numbers in your error message you can see that the arc is very small, I and J are the offsets from the start point to the center point. The problem with small arcs is that it is very easy to have relatively large percentage difference between the radius from start to center and that from end to center, and that is what GRBL is complaining about. Here is your code Code: G1 X-1.7934 Y0.7948 G3 X-1.8332 Y0.7620 I-0.0128 J-0.0252 if we draw it it looks like this we see that the radii are 0.0003" different, which is a little more than 1% difference at this scale. if the post can use more decimal digits then try that. if the post can be forced to linearize all arcs, then try that. if Vcarve can be encouraged to not generate such small arcs, then try that (or linearize anything smaller than bit radius) if the programmer of the post can be convinced to recalculate the center of the arc and output the correct numbers, then try that.
