Resume Job After Computer/CNC Reboot

[roy_okc]

Hi, newbie here with only a couple weeks under my belt on my DIY CNC router. I've figured out quite a bit about EMC2, and have it running my rig pretty well, but still have a lot of learning/refinement to go yet.

I'm trying to determine if it is possible to resume a job after interrupting it and powering down/rebooting everything. For instance, to support a long photo carving session may need to span multiple evenings and I don't want to leave everything powered on while I'm not around it.

I don't yet have home/limit switches, so I manually home X&Y to a convenient spot and Z to the bed. Then I touch off the X,Y,Z axes to the material. Is this the best way to prep for a job?

I know there is a setting to save the home settings between sessions, does it also save the touch-off settings? If so, my thoughts are to pause or stop the job, note the line #, power off the router/not moving it, close EMC2, power down, leaving material in place, power up, start EMC2, load the .ngc file, scroll to the noted line, power up the router, and restart at or a line or so before that line. I also would like to do this for multi-file jobs, starting the next file on another day.

Thanks,
Roy

[judleroy]

There is no way I know of to save a touch off point and accurately get back to it without a home switch to reference to. For a machine with encoders you can save where your at in some cases but with steppers you must have a home. You can buy microswitches at radio shack the will work for limit/home. There only about five dollars each. Good luck.
Judleroy

[cncbasher]

your doing the resume , about the only way you can , it's not possible to resume to a line and continue , as gcode is a modal system , i.e it reads one line at a time and reacts , and some commands are in force until told to change which could be even at the begining of the program for example .

short of leaving it all switched on , it's difficult to resume especialy with stepper systems as their is no positional feedback to emc , so you power down , someone unknown to you has a play by moving an axis or just knocks the handwheel a few clicks , emc and you would never know , for example .

always make sure you have a repeatable x,y,z point to return to , or perhaps split the job up into smaller gcode programs , and cut one at a time , so at least you only need to wait for a shorter time

[Michael In Cali]

I am barely starting out in CNC myself and carved my first practice image mostly last night and finished during my lunch break today.

For that job, I paused EMC and then powered off the stepper controller but not the computer nor did I shut down EMC. I was able to re-power up the cnc controller and continue without difficulty. However, if someone were to bump the machine or anything it would not have been sucessful. If your controller jumps a step or two when it powers up, that could also be a problem.

In my mind, I have the following scenario for resuming a job, but have not experimented with it.

Once homed, jog over to where you wish to touch off. Record by hand the X,Y,Z coordinates prior to touch off. Then touch off.

Start your job and run until you wish. When you stop for the session, write down the line number you are executing.

In my carving CNC file, I notice that after the first initial lines, everything is very much identical so there are no settings througout the rest of the file except x y and z until the very end.

One should be able to capture the first few lines of the G-code and store them as a separate initialization file.

Upon reboot/resumption, one could re-home, then issue a command line of G-code to traverse over to the previous touch off location and then re-touch off.

Then execute your initialization file which will set up feeds, speeds, and whatnot.

Then, reload your original g-code. Scroll down to the last line previously executed and right click, and "start from here" (or whateverthe menu pick is).

Of course, this presumes you have limit switchs and that the limit switches are pretty accurate and don't vary much, if any.

A bit of risk, but it should work in thoery.

Please feel free to comment and clobber me if I'm wrong. I'm new at this after all.

[roy_okc]

@ judleroy and cncbasher,

Thanks for those insights. I do have limit switches, simple mechanical ones, just not installed yet as I need to get some material to mount the switches to and then mount to my rails. I haven't figured out how to do a Z home switch due to bit length changing; I guess this is why many people use a metal plate and probe down to the plate???

My CNC is in my home workshop, and I'm the only one in there, so don't have to worry about getting bumped.

@ Michael In Cali,

Interesting thoughts, sounds like you've thought this out a bit further than I have. Could even edit the file and figure out what is safe to delete and maybe edit in a couple XYZ moves to just above where you want to resume; vim would be great for this as you could go to the line you want to start deleting (knowing in advance how many lines you want to delete) and type, for instance, '100000 dd' to delete 100K lines starting with the current line.

Sounds like I absolutely have to get homing switches added before I can even think of doing anything, though.

Thanks for your thoughts and suggestions,
Roy

[Michael In Cali]

Roy,

I home Z to top of travel, not the bottom. Top of Z isn't hard to do. I would presume in my scenario one would not want to change the bit either preserving the Z touch off.

[roy_okc]

Roy,

I home Z to top of travel, not the bottom. Top of Z isn't hard to do. I would presume in my scenario one would not want to change the bit either preserving the Z touch off.

Okay, that makes sense. That was what I thought I would do prior to actually getting it running, but the settings didn't seem to jive for me. Just have to figure out how to set so a bad Z plunge doesn't run through my bed and into my frame with an extra long bit.

Sigh, so much yet to learn.

Thanks,
Roy

[judleroy]

Home has nothing to do with tool setup or part setup. It is a absolute zero reference for each axis of your machine. Usually it is defined in g-code as G53 or absolute machine coordinates. You set you parts up with g54-g59. These are your machine offsets to define your part zero. These settings are saved and can be reused for the same part over and over as long as you make no changes to them. The z value must be reset any time you change a tool. If your part is setup in g54 for example and you do not change the tool between stopping and restarting your job no changes need to be made. The flow is like this. Home machine. Set coordinate system to g54. Jog to where you want to setup your part.(edge of part or center of part...everyone does it a little differently). Set your z.(top of part or bottom of part depending on how you write your code). After that g54 will always go back to this spot after you home and then pick the g54 offset. If you run a long job and want to stop in the middle you would run the part in g54 then stop the program when your ready to stop for the day. Record where you left of in your code. Open your code in a text editor and erase everything up to a few lines before you
stopped. You will need to write a few lines of code to make restarting work properly. First add g54 to the top of your code. Then add lines to rapid over to where you left of in x
and y at a safe z height above your part. Add lines to feed down to where you left off at your plunge rate. That should lead right into your code where you left off at. There is a bit of a learning curve to breaking up code like this successfully but you'll catch on. I hope this is clear enough and understandable. You can also break the code up in manageable pieces in your cam program from the get go if you know what your looking for. Remember if you change your tool z must be reset if not you can go right back where you left off. Good luck.
Judleroy

[judleroy]

I didn't say so above but to be clear when in g54 when you jog over to your x and y reference point you need to zero x and y at that point and then jog down z to your reference and zero it also.
Judleroy

[Michael In Cali]

Home does have something to do with his issue. Between sessions after the machine is shutdown and the carriage may have moved, if you don't have a way to home, you cannot set where you want G54 to start from again. You need to have a good home reference and then some way to get back to the exact same coordinates to set G54. Or am I full of crap?

[roy_okc]

@Judleroy,

Thanks, this is what I was hoping to hear, and kind of along the lines of what I was thinking. I need to look at the .var file and see what is in it, sounds like it records the G54-G59 settings (touch off points). I obviously need to get homing working well to make this possible.

I haven't seen a way to split up jobs for photo carving (PhotoVCarve), which is what led me to this question to begin with. If I wanted to do, say an 8x10 cut, it looks like it could easily take 12 or more hours on my router.

Thanks,
Roy

[CaptainVee]

Just a quick thought but has anyone tried putting emc on pause and then hibernating the machine?