Experienced a glitch at line 39021 of 162652. Would one of you experts explain to me how I can re-probe home and restart the job at line 39021?
@Griff, I don’t know the exact answer, but when I’ve had problems like this in the past and researched, the answer seems to be always that you have to edit the G-code file. You can do this in an advanced text editor like Notepad++ which will help with the line numbers. The problem is, you have to go from a line where you are telling the machine an absolute coordinate, not a relative one. In other words, the machine needs to start from Coordinate 20, 20, 20 for example, where as sometimes the G-code lines are just giving commands like “Go +3 X, -2 Y, and +1 Z from the last position.”
There are certain Gcode commands to look for, but I have to look them up real quick. Its a shame you can’t post your file somehow, that might be helpful for those in the know.
Edit: Maybe this will help explain more than me:
https://www.cnccookbook.com/g91-g90-g-code-cnc-absolute-incremental-programming/
1 Like
And the Gcode Wiki page is always helpful for trying to read the code:
1 Like
Oh…boy!
Crap, nothings ever simple. I was hoping it would be possible to truncate the code at the line I noted and plug in the “start here” code.
That might very well be possible, but I have not been successful yet. I think you have to be careful what you cut out. Like I said, I think you need someone to take a look at the code who is more knowledgeable on Gcode than me.
I think you can do that with UGCS…
1 Like
I started looking at the surface quality (not the best) of the pocket I aborted the cut on and decided to change up the path. So I re-probed and started over. Alls good now.
I think I’ll do a bit more research on the issue, for next time…there will be a next time.
2 Likes
You probably don’t want to try it then, though.
This can be done by hand editing the gcode. Essentially, you need to keep the necessary headers (G21, G54, G90, etc), delete the code you’ve done, save, re-home (if you need to) and go. I always backtrack a bit and also find a line where there was a retraction followed by a travel to start with that retraction.
2 Likes
I’m not sure about UGS, but I’m told that you can go to a specific line and start a program in Mach 3, however Mach 3 requires a parallel port on a desktop machine and some other painful requirements. So not really an option either. It would be nice if UGS or bCNC offered this feature, but I haven’t found it yet.
Thanks neilferrei, understanding a bit more about is on my list. Need to repriortize.
Griff,
I have had to do this before, due to static electricity disconnects. I have been (mostly) using inkscape and makercam, so the beinning gcode commands will look different, but I believe it should work the same.
I use just plain old Windows notepad to make the edits, since it provides line numbers as well.
For me though, I have any number of hundreds of holes to choose from to index my machine again.
I pick a hole I know (such as identifying the first hole drilled) and look at the gcode to determine what hole it is ont he board, as well as the X and y location in the gcode.
I find the first drilled hole, and let’s say the gcode to move to that hole location is: G1 X0.3041 Y4.1336
Since I am using CM for my controller, I navigate to my hole, get the bit centered in the hole and then “zero” the machine telling it I am now at X = 0.3041 and Y = 4.1336, but since CM uses metric for zero, I just multiply those values by 25.4. Z zero is however you zero your Z axis (+0.25 or whatever depth allows you to air cut for a quick test run).
Now, you save your gcode file with a distinctive name that you will not accidentally use again if you forget to delete it after you finish your job. For me, I use FU001.nc, FU002.nc, FU003.nc. . . Each time cutting away more of the gcode each time I had a disconnect.
I leave in the initial gcode info and delete everything between the first rapid move and the last rapid move before the disconnect.
For example:
(Generated by PartKam Version 0.05)
G20 G90 G40
(Nums 5-25 0236)
G0 Z0.1
T0 M6
G17
M3
G0 X0.2392 Y4.2526
G1 Z-0.04 F20
G2 X0.2381 Y4.244 I-0.0353 J0 F30
G2 X0.2355 Y4.2379 I-0.0203 J0.0051
G2 X0.2315 Y4.2327 I-0.0289 J0.0181
G2 X0.2269 Y4.2287 I-0.021 J0.0197
G1 X0.2165 Y4.2239
I delete everything below:
(Generated by PartKam Version 0.05)
G20 G90 G40
(Nums 5-25 0236)
G0 Z0.1
T0 M6
G17
M3
G0 X0.2392 Y4.2526
Then I actually zero my machine if everything looks good.
Before I got a handle on my static electricity issue, I could have 2-3 disconnects per cribbage board.
If you are running your machine in absolute mode (G90), which makercam does, it should work fine. I am unfortunately intimately familiar with doing it.
Also, if your notepad is not showing the line and col numbers in the bottom right corner of the window, just go to [View] - [Statusbar] and it will appear.
Let me know if you have any questions.
2 Likes
This topic was automatically closed 30 days after the last reply. New replies are no longer allowed.