Working on a 16" x 36" Teak Wood Project… Roughing runs at 10hrs, and my power dipped at 9 hours run time. System shutdown with just 1 more hour to go and 90% roughing. I know, can it get better than this?
I don’t want to run the job again for another 10 hrs, cutting air for 9 of those hours. I read in the forum that I can mod the g-code to pick up (somewhere) where I might have dropped off.
Is this correct?
What part of the leading code must stay?
I’m not too keen on editing this gobbledygook.
My Post Processor has these initial 10 lines of code:
%
T1 (MSG, Insert Tool 1)
G0 G17 G21 G90 G40 G49
G0 Z20.320
G0 X0.000 Y0.000 M03 S27000
M0(MSG, Click ‘Continue’ when the spindle is up to speed)
G0 X186.686 Y17.360 Z5.080
G1 Z-2.500 F800.0
G1 X20.788 F1600.0
G1 X20.444 Y17.619
Hey Jenn, you can splice the g-code but you have to be very careful when doing this. I would start here to understand editing code.
Next you should keep this startup code…
The next line “G0 X186.686 Y17.360 Z5.080” is a rapid move to X,Y, and Z locations. I would search your code to find another “Z5.080” or something above Z0 so it is not going to crash into your work piece.
Well, I did not note which block number was active when the system shut down. I suffered a power shutdown. There was an electrical outtage.
I am guessing that I will have to “GUESS” at where more or less I should pick up. Well, it’s probably best to catch it before the crash, so that even if I have to wait an additional 20 minutes or so while the machine is cutting into air, it will eventually pick up where it disconnected and let it eventually engage, so to speak. Because if I come in after the fact, it might leave materials that should have been removed by previous g-code.
Correct me if I’m wrong, as I wrap my head around this. This is a first for me.
My next head scratcher will be doing the actual (guessing where on the lines of code that One Hour to go might be; since the g-code does not include a time-stamp like video.
So if I am understanding this correctly, I should keep the first six lines of start code, and then start line seven with g-code from way down the list, somewhere right? I have like over 63,000 lines of code.
You need to keep the first few lines because they are part of the setup but also you might have to modify the first line that you keep with some other parameters.
Have you listened to @charleyntexas explain how to split g-code:
I have not (yet) tried myself but it does not look very complex… apart from figuring out where to cut. Indeed you should err on the safe side, it’s best to cut 20 minutes of air rather than crash into the piece.
Jenn you are correct. You will have to take your best guess as to where the program stopped. Lets say you start looking around #40,000 (or wherever you want to restart from) then start looking for a Z value that is above 0 (not in a cut/ above your work). If you want to post some of the code where you want to start from I can try to help you splice it in.
Yes, I just downloaded the video, let me get some headphones. Sorry, Running around here. Hurricane Elsa is making its way into my Home State of Florida. Oh no, more power outages!
Here’s a thought: I know that the rough run was 10hrs, and I lost power 1 hour before it finished. If I spliced at a given point and upload the g-code file and it says the run time is 1 hr. 15 min, then that will work just fine. If I did not cut off enough g-code and it says that I have 3 hrs. to go, then it’s safe to go ahead and look for a better spot up ahead to splice. Makes sense?
That looks pretty good Jenn. I would however find your last Y position right before that G0 Z5.080 move and insert it in your G0 line
(find last Y value- example Y42.000)
G0 Z5.080
G0 X305.400
G1 Z-22.500 F800.0
G1 X305.469 Y46.500 F1600.0
Start of Program:
%
T1 (MSG, Insert Tool 1)
G0 G17 G21 G90 G40 G49
G0 Z20.320
G0 X0.000 Y0.000 M03 S27000
M0(MSG, Click ‘Continue’ when the spindle is up to speed)
G0 X305.400 Y42.000 (Goes to X and Y locations first)
G0 Z5.080 (Then brings Router down to part)
G1 Z-22.500 F800.0
G1 X305.469 Y46.500 F1600.0
(…and so on)
You have got the idea
charleyntexas
(Charley Thomas (Onefinity/Triquetra Touch Probe))
16
One way to find out where you should be restarting without wasting a ton of time is to first re-zero your machine to the work piece. Then Jog you machine close to the last successful cut. Then jog all the way to the right or left until you are against the last part that was cut on the X axis. Look at your DRO and it will give you a Y axis location. Open your gcode file in Windows Notepad and start searching for a Y axis value that either matches the DRO or is just slightly Less. When you find it start going backwards in the code to find the X axis with the lowest value. This should be the line (along with everything after it) you want to follow the edited version of you code. Taken from the sample that was posted by Jennifer Kentt above.
T1 (MSG, Insert Tool 1)
G0 G17 G21 G90 G40 G49
G0 Z20.320
G0 X0.000 Y0.000 M03 S27000
M0(MSG, Click ‘Continue’ when the spindle is up to speed)
G0 Z5.080
New starting point begins here
Yes I’ve heard Charlie
The recording I posted was Charlie
I recorded a phone call from him where he gave step by step instructions on how to do this if you need the recording let me know I’ll repost it
