Greetings all,
I have been searching the internet for about 3 hours. I did not want to clutter this forum with my question but I am unable to find a viable solution to my issue. I’ve ran sheetcam and Mach 3 in the past on a DIY CNC we had back in college. It was the perfect set up for me and I’m comfortable with the basic operations.
I’ve recently purchased and received a Sienci Longmill (3 axis cnc router). My plan was to get a smooth stepper and G540 to run the machine as I have in the past, but I’m trying to spread out my expenses.
In short, I cannot find any information on a post processor for GRBL protocol. This machine is managed by an arduino and has the code sent via UGS, since Mach 3/4 does not work with this protocol.
Is there a post processor built into sheetcam that I can use with GRBL?
I’ve seen some discussion on here about GRBL. Did you try the search function at the top of the main forum page?
Hello. Thank you.
Yes I did. There were about 84 queries. most of which showed up in google earlier this morning. There is one post with a download I am going to try tonight. I do not know if it will work because it appears to be specific to a plasma application. I will try it regardless and see what happens.
So to report back. It looks like I can use this file I found on the forums “GRBL Plasma (Edited)”. I tried the file “GRBL with THC (Edited)” but the issue I had is there appears to be a code for homing the Z axis right before the job starts. I get an error running that post processor.
“[Error] An error was detected while sending ‘G38.2z-50.0F500.0’: (ALARM:5) Probe fail. Probe did not contact the workpiece within the programmed travel for G38.2 and G38.4. Streaming has been paused.”
I don’t know what “THC” is referencing in this file name. I’ve no experience with plasma tables.
The machine reacts predictably until this happens. I’m thinking if I can be rid of the probing feature, it may continue through the remainder of my code.
Since I don’t know how to do this I tried “GRBL Plasma (Edited)”. It seems to work fine on a very simple part I have.
Now, I think I am good to buy the license, but I want to get some confirmation from you guys. Is there anything that I cant see I should be aware of? I will most likely have a CNC controlled spindle on/off and maybe speed. Does this post processor have this ability even though it’s “Plasma” post processor? I have limited knowledge on how the post processor affects the G-code. I’m still confused on that…
I will wait until I can get some explanation. Maybe, Mr. Les will weigh in. Through my extensive research today, it seems he is the godfather!
Thanks!
-Jake
GRBL plasma.scpost (2.82 KB)
GRBL THC with scriber.scpost (7.73 KB)
Thc is torch height control. It is a device that uses a voltage feedback from the plasma arc to detect the torch to work distance and adjust the z axis to maintain the desired distance while cutting. This is critical to getting good quality cuts. Irrelevant with routing.
Les is the creator of SheetCam. He usually is pretty quick to chime in. He is very willing to modify post processors if there isn’t something available that will work for you.
You can always email him Les at SheetCam dot com.
Thank you. I will email Les for confirmation. Appreciate the help.
Both of those post processors are for plasma cutting. Try this post for routing. 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.scpost (2.35 KB)
Thanks Les.
I will try it this evening and report back.
Hi Les,
No go on the Post processor. The machine only lifts up the Z and just before rapid to the start point it faults. Error message displayed here.
G10 P0 L20 X0 Y0 Z0
ok
G21
Skipping comment-only line: (Mill/router, 0.8 mm diameter)
T1M06
G0Z10.0
S1000M03
ok
G0X34.6Y52.5
G0Z2.0
G1X34.6Y52.5Z-3.5F100.0
G3X37.5Y49.6I2.9J0.0F1000.0
G1X42.4Y49.6
[Error] An error was detected while sending ‘T1M06’: (error:20) Unsupported or invalid g-code command found in block. Streaming has been paused.
**** The communicator has been paused ****
**** Pausing file transfer. ****
The G code below:
G21
;Mill/router, 0.8 mm diameter
T1M06
G0Z10.0
S1000M03
G0X34.6Y52.5
G0Z2.0
G1X34.6Y52.5Z-3.5F100.0
G3X37.5Y49.6I2.9J0.0F1000.0
G1X42.4Y49.6
G3X45.3Y52.5I0.0J2.9
G1X45.3Y59.75
G3X44.9Y60.15I-0.4J0.0
G1X40.9Y60.15
G2X40.9Y60.85I0.0J0.35
G1X44.9Y60.85
G3X45.3Y61.25I0.0J0.4
G1X45.3Y68.5
G3X42.4Y71.4I-2.9J0.0
G1X37.5Y71.4
G3X34.6Y68.5I0.0J-2.9
G1X34.6Y52.5
G0X34.6Y52.5Z0.0
G0X0.0Y100.0
G0Z10.0
M5 M30
Thank you for the help sir.
I removed the line in question from the G code and the file ran fine visually.
My limited knowledge says T1M06 is a tool change command? Am I correct?
How would I proceed normally with no tool change function at this time? I do want to try this in the future.
Sorry for the delay. I somehow managed to post my reply on the wrong thread.
Give this one a try.
Note this post completely ignores tool changes. Maybe it should do an M1 pause. Does GRBL support M1?
GRBL mill-router no toolchange.scpost (2.17 KB)
Hi Les,
Sorry for the late reply. I will try the new post you have added here.
I was able to modify the last post through some trial and error.
I will test it out and report back. I do not know about M1 off the top of my head.
Hey Les,
Looks like that Post works good. I did not see any major issues with my cuts over the weekend.
I am having a problem with a drilling operation tho, is this a limitation of the demo version of the software? This is all I get trying to drill out a hole pattern.
G21
;Rotary tool
T3M06
G0Z15.0
S1000M03
M05
M5 M30
Works great now. Thanks Les.
