Hi, I have been using SheetCam with a CandCNC system, really like the capabilities of sheetcam, so much so, that I want to use it with my new machine using Openbuilds Black Box and Control software, cant seem to get a Post Processor that works without fail. I’m using Solid Edge 2D for cad, only have X and Y, no Z at all, I adjust it manually. Please send me a post processor that will match my criteria
Running two axis will be hard work. You have to be careful to set the correct depth each time. If you make a mistake you will probably ruin the job you are cutting. I have attached a post that should work for this application.
To install this post, save the attachment to any convenient folder on your computer then run SheetCam and go to Options->machine->post processor. Click on the ‘Import post’ button. Using the box that appears, navigate to your post and open it. Go back to Options->machine->post processor and make sure your post is selected.
GRBL mill-router 2 axis.scpost (2.55 KB)
Forgot to mention, this is a plasma
Do you have a post processor available for plasma and Open Builds Black Box, if you do, found a lot of interest for it on the Openbuilds forum, router posts are there, nothing for plasma
Here is a 2 axis plasma post.
GRBL plasma no Z.scpost (3.04 KB)
M67 E0 Q10 (DTHC OFF) This is causing me a warning, if erased from the G-Code rest runs perfect, how to eliminate?
“You have the rule set ‘EOCAnti-Dive’ set to be always applied. Go to Tools->Cutting rules. Set ‘Always apply tool set’ to ‘None’” found this in another post and it solved my problem
I want to give my torch some time to fire before the motors start moving the machine, I’m not familiar with changing my post processor, checked out the Openbuilds forum, they recommend something like G1F1\nM3S1000\nG4 P400 code added before each fire, please implement it in my post processor, thank you
It seems to be implemented in the post processor.
Is the Pierce delay in the tool settings set to anything else than 0 seconds?
I set it to 0 sec, then set it to 4 seconds, made no difference, its only moving while the torch is firing on tabs, the start up works fine
The post do not change the pierce time from seconds to milliseconds. Maybe that’s the problem making 4 seconds being just 4 milliseconds delay. Here’s a version which outputs milliseconds.
GRBL plasma no Z.scpost (3.05 KB)
I forgot to make the same change to “endDelay” and “preheat”. Use this one instead.
Black Box plasma no Z.scpost (3.04 KB)
That’s odd. I checked the GRBL docs and they state G04 uses seconds. Oh well, give the post a try and see if it helps.
Yes, You are probably right Les.
pdevloo, If my hack doesn’t help, maybe you can attach the g-code output or the entire job file.
Ive figured out I had to set sheet cam to ms instead of seconds and it delayed the torch, problem is, it also delayed the table. Its now doing the same thing where is starts cutting and motors travelling at same time but now has delay before it does it. Is there a way I could get the torch to fire before the table starts to move?
Disregard the last post, figured it out, problem was with Openbuilds GRBL settings, the Laser Mode was enabled which is in place to fire a laser immediately with table motion as far as I understand, that relates to the safety of it, anyway, disabled it and table works perfectly as it should, thanks for your help! Great service! Sheetcam works great!