How do you resume a carving after a stop

Discussion about the CNC Shark Pro Plus HD

Moderators: al wolford, sbk, Bob, Kayvon

Post Reply
Mr. Toad
Posts: 4
Joined: Sat May 09, 2020 12:49 pm

How do you resume a carving after a stop

Post by Mr. Toad »

I was 24 hours into a carving when I accidentally hit the stop. How do I start the file again from where I hit the stop?

Rando
Posts: 757
Joined: Tue Jan 06, 2015 3:24 pm
Location: Boise, ID
Contact:

Re: How do you resume a carving after a stop

Post by Rando »

Well, do you want the short answer, or the easy answer?

The short answer is that restarting at some arbitrary point in a GCode file is not a built-in feature of the system....at all.

The easy answer is there IS NO easy answer.

The hard answer is that it's possible, but you have to first develop a freeze-reflex.

The freeze-reflex is necessary because when you stop (end, not pause) a running GCode program on these machines, you have to immediately get some information, and stop movement of the machine and the part before some registration gets moved. And, you need to be at least a little knowledgeable about reading GCode. You don't need to be an expert, but you need to not just glaze over and see "nothing." After all, a 24-hour run is not a small file, and it's all human-readable text (at least in our style of GCode; some machines do have much less-readable code). But, there's like over a hundred-thousand lines, if not a million. Not all text editors can handle files that large, so beware.

So. When you are going to hit stop, get in the habit of taking note the approximate range of line number it's running on. For a 24 hour run, it's going to be a big number, but write it down. You WILL need it. If it's an unplanned stop, then make sure that's the first thing you do when you hit that stop: know what line number it was on. Doesn't have to be exact, but it's helpful.

Now, once you've stopped the machine in panic, mistake, or because the bit's gone dull, DON'T MOVE ANYTHING!

Take your favorite text editor (I use notepad++, a free really cool text editor for geeks like me) and open that gcode file.
Save a copy to another name, right....you already did that....

Try and figure out what part of the run it's doing. What it's machining in that area; what area of the part is it cutting in? That's important because you need to know the Z-safe height that the bit gets moved to when it goes between areas. We're going to try and find the spot in the GCode where it went to that safe height the last time before it stopped.

Now, scroll down to the GCode line number where it got stopped.

slowly scroll upward toward the start of the file, and try to find a G01 Z<safeHeight>, so a linear move upwards on the Z-axis to that safe height. Of course, replace <safeHeight> with the value. Don't do a text search, just slowly scroll upwards. It will likely be within 20-50 lines, depending on what it was doing at the time.

Put a bunch of empty lines there, and cut out everything (Leave the G01 Z<safeHeight> in place) all the way to the top of the file....up to the first G01 move that has an X and Y block.
Leave that first "G01 Xx.xxx Yy.yyy" in place. If you save and run that new file, that should start very close to where it left off. It's not always easy to figure out what it's doing, but looking for that G01 Z<safeHeight> is always a sure bet.

IMPORTANT: If this long GCode file included more than one toolpath, you'll need to cut out from where it stopped (the G01) to the first G01 move IN THAT SPECIFIC TOOLPATH, and then remove all the toolpath information to the top of the file, above the one(s) we want to keep.

Hopefully the above will give you want you need. It's not a fun thing, but it happens sometimes. There are potential mitigations, but sometimes they require either preparation or effort, or both.

Regards

Rando
=====================================================
ThomR.com Creative tools and photographic art
A proud member of the Pacific Northwest CNC Club (now on Facebook)

Post Reply