Accidentally stopped a job

Probably, *if* you know roughly which line it stopped at *and* haven't turned off the machine *and* haven't rehomed *and* haven't changed tools. In theory you can rehome but you're at the mercy of the repeatability of your limit switches if you do.

Like the thread says, you need to be sure of all your modals, and then you'll need to create a copy of the g-code file and open it up in the notepad app of your choice (N++ or similar is good). Usually you can keep the header block- it should say something like G20 G90 G17 G54 F800 blah blah blah. Delete everything after that, up to near the line where it stopped- maybe keep one or two lines before it, if they're physically long enough to target or at least you can use the numbers later. Any circle or horizontal/vertical (ie. x-only or y-only) line is easier to target. If there are any G0 rapids, that's way easier than cuts, because you can just bring the machine [*very*] close to where it needs to be and hit run- the rapids will do the rest. Try not to restart on finishing cuts, only roughing cuts, if possible. Remember now you have zero linking moves between "wherever the machine happens to be" and "the cut I want to do", so you have to rebuild that without accidentally going through something you really didn't want to.

First you'll need a G53 safe Z line, to get the spindle up above everything. Then you've gotta calculate the arc to start outside of your cut line, move safely through a short amount of space, and end up perfectly co-linear and/or tangential with your cut line, so there's no obvious gouge where the machine set itself down again. Look up the LinuxCNC G-code page on arcs- they have precisely defined parameters. And if you're slotting, you'll need to change your G17 mode, because you can't X-Y arc, you'll have to do an arc down into the slot. Though if the slot's a little rough, you can probably get away without arcing into it.

Once you've used the LinuxCNC page section 5.2 to calculate your arc starting point, the ending point based on the block right before the one you're trying to merge into, and its radius origin offset from the starting point (which is just however big you want to make the curve, really), you can do your setup. After your G53 safe z move, you can G0 rapid to the X-Y position above the start of your arc, a Z rapid to a safe starting position a couple of millimetres above the surface, and then M3 start your spindle and you can go into your G1 Z feed down and your G3 counterclockwise (climb cutting!) arc into your existing file's cut location. Then it'll automatically continue the rest of the file as-is.

In other words, this is an excellent learning opportunity! Remember,