One issue, the odd Arc there, shows its not a Grbl compatible Post (other clues like "%" tape start/end chars, Line numbers etc confirms - not typical of Grbl, more reminescent of Mach/LinuxCNC or older) But the preview is correct. Your job is only north west of the origin, and that's what the preview shows. There is no gcode in the lower half of your stock, so nothing to render there. Origins lines up, relative position of part lines up... Merged the two previews in GIMP with a little transparency to clarify. CONTROL's rendering your gcode's origin point at what would be about in the center of your "stock" the Part is where it should be. its all fine. Just use a proper Grbl compatible Post to fix the decimals rounding issue on the Arcs. See docs:software:cam [OpenBuilds Documentation]
Thank you, Peter. Can I run my nc generated by my Master Cam through Open Builds Cam somehow and it will correct it?
your Gcode is not good for GRBL controllers.... Code: % O00001(ARM) ; unsupported (but may come later on the X32) ( T1 | 1/8 FLAT ENDMILL | H1 ) N100 G20 N102 G0 G17 G40 G49 G80 G90 N104 T1 M6 ; filtered by CONTROL N106 G0 G90 G54 X-4.7953 Y4.9531 S4278 M3 N108 G43 H1 Z.5 ; unsupported tool offset N110 Z.1 N112 G99 G83 Z-.125 R.1 Q.045 F15. ; drill cycle? only supported on X32, not displayed correctly by CONTROL, so better to avoid it for now N114 X-1.0805 Y4.8146 N116 G80 N118 Z.5 N120 X-1.1816 Y4.9231 Z1. N122 Z.1 N124 G1 Z-.02 N126 G3 X-1.2508 R.0346 F30. ; R format is deprecated, prefer IJ arc formats ...
Well, I am just batting a thousand here aren't I. Master Cam is like a comfortable old shoe to me, but if I have to design parts in Open Builds Cam to rectify any further complications or delays, I'll give it a whirl. Thanks again gentlemen, I will keep you "posted"
Just make sure to Post with compatible GCODE format See above (Quoted below) OpenBuildsCAM is beginner friendly, basic. If you like Mastercam you won't like it (different spectrum of users entirely)
Sorry, $500. 4 high torque steppers, Black Box X32, Power Supply Bundle. Finally, all dialed in, and now my post processor doesn't output the G-code necessary to produce any parts. I have HUNDREDS of nc programs and can't run a one unless I go through the code line by line (if I could figure out what to do anyway) or use what you tell me is a basic Cam program that I won't like anyway (guess I don't fit into that spectrum of users) So until I fork out more Denero for a more GRBL friendly CAD program, I have $500 worth of electronic paper weights. Not your problem, again I appreciate all of you who have at least gotten me this far. I can be surly and sarcastic, but I am not angry at any of you, just myself for not researching the compatibility of new school and old school.
Well thats theoretically a $0 fix - find a Grbl compatible post for your choice of CAM - reach out to mastercam they'll probably have on right on hand for you! I respect your MasterCAM skills which is why I don't advise the beginner friendly OpenBuildsCAM to you (If you are used to the Ferrari, would you even want to drive the VW?) Nothing is stopping you, but if I was you, and you do love MasterCAM as much as you say - isn't finding a Grbl compatible post worth it. Grbl is more widely in use than Mach3 likely - surely your CAM vendor can step up to the plate like almost every other CAM vendor has (Or surely already did)
A guick search for "MasterCAM grbl post" turned up this post. I have not read through it, but since M6 was mentioned as an issue it can be noted that grblHAL can be configured to ignore M6 commands by setting $341=4. Some senders may also handle M6 commands, either by stripping them out or somehow implement tool changes sender side.
People on various Mastercam forums suggest that Fanuc post processor for Mastercam will probably work with grbl, although some of the posts I found went back to grbl 0.9! Alex.
I am not sure it will, the O word is currently only supported in macros, either called by G65 or by tool change macros. Used here for just naming the program? A tool table can be enabled in grblHAL allowing the use of G43, G43.1 and G43.2. It cannot be enabled from the Web Builder yet though. This is odd, turning off motion mode with G80 and then command a move... I have no idea about what this is supposed to do, and it is not a "legal" sequence according to the NIST spec - grbl/grblHAL will return error 31 - Axis words found in block when no command or current modal state uses them for line N118. I wonder which controller the gcode is for... I am curious about what the Fanuc post outputs for the same file.
I give up. What CAD/CAM software is similar to Mastercam that I can purchase that will produce the G code necessary to operate my new electronics? Thanks.
Our list of recommended CAMs can be found at docs:software:overview [OpenBuilds Documentation] Have you emailed your MasterCAM vendor (or MasterCAM themselves) yet though? Mastercam Support Grbl's such a widely used firmware I would be surprised if their support team doesn't have a post they can provide you with / advise on. Did you try the Fanuc suggestions?
I'm a bit confused as to why you are giving up on this last issue? Need to select a machine type to tailor the code for the machine, this will need to be done for any software you choose. Quick search on YouTube took a screenshot below, not sure if this is the same version you are using, but looks like Easel is supported try that one. If that is not there tell us what is so we can help.
I appreciate that, thanks. My version is not even supported anymore (Master Cam 4 2010) To get back up to speed is cost prohibitive. My version has a limited library of post processors as it is, and I tried them all. I was dialed in to Mach 3. I can't access any of the post processors on the website because they begin with version 9. I really do not know how to manipulate code, I always counted on the software. I will check out the overview and make a selection, probably for the best. Maybe I could post a G code generated by my post processor and you could red line/correct it? Perhaps I will get the jist of it from seeing it? I tried this (see attached) and tried to follow the pattern and failed. d.
Yeah then thats a problem. Looks like you are learning Fusion 360 - nice to be up to date for a change
