We were carving a 3D project and the machine was on the finishing part of the carve. We paused the machine for the night and my wife heard it reset over night. I think I know the answer here but is there a way to continue from “previous carve” or location? We did not seem to have a power outage or glitch overnight and the computer doesn’t look like it restarted - windows update’s). Any thoughts?
UPDATE:
Went to task manager and checked for “uptime” to find out if the computer restarted and indeed it did. I guess win blows updates must have happened even though updates are not supposed to happen unless we select them to happen. NUTS!
I’ve had laptop stupidity too. I do all my updates and then disconnect the internet.
Hopefully your project is still clamped down to your machine. If so, all you need to do is:
- Reestablish your XYZ zero position to where it was when you started. This is why you need a 3 axis touch plate for zeroing. (www.triquetra-cnc.com)
- When you have your zero rest, jog your bit so that it is located just short from where you paused it for the night.
- Next, Look at your DRO’s and write down the current location for both X and Y axis. In Easel, you can view this in the Machine Inspector.
- Now load your gcode file in windows notepad. I recommend downloading Notepad++ for this. It shows line numbers and makes it easier to keep track of what you are doing. Do a search or find for your X and Y coordinates. Be sure to use spaces in your search criteria if they are used in your gcode file. If nothing is found then you will need to start reading through the code and find something close to where it was paused and jog your machine to that location. When you get reasonably close to you paused location but not passed it , go to step 5.
- Now it’s time to decide wat to delete. Start reading the gcode lines moving backwards until you find a line that includes a Z axis move. Make a note of the line number so you can easily find it again.
- Start reading from the beginning of the3 gcode file. You are looking for a line that contains G0 XO.OOO Y0.000 Zx.xxx. You will keep that line and everything prior to it which should contain spindle start commands (SxxxxxM03) and other parameters for the cut. If the spindle start comes after the G0 X0Y0 then move then move it to the line before G0X0Y0. Every that follows this should be the actual carving commands.
- Time to make the change! With your mouse, left click the beginning of the line AFTER G0 XO.OOO Y0.000 Zx.xxx. then scroll to the new beginning of your carve identified in step 5 and hold down your shift key and left click at the end of the line preceding the new start point. this should select everything between the gcode startup stuff and your new start point. Hit the delete key then save the gcode. I recommend using “save as” and adding recovery to the file name to preserve your original file. The gcode is now ready to go but please read on first.
- If you are supremely confident in you changes then go for it. However, considering the time invested already, lets add a couple of minutes to be sure first. Do this by running the attached file “Increase z height.txt” which will increase the height of your z axis zero location by 1/2 inch so when you run your file it won’t actually cut but you will be able to watch the movements and decide if it looks correct or not. When you are satisfied and ready to go for it, run the second attached file “Decrease z height.txt” to rest the previous z height increase.
Decrease Z height.txt (55 Bytes)
increase Z height.txt (55 Bytes)
If you have any questions you can PM me on this forum or at:
charleyntexas@gmail.com
903-436-0675 call or text
1 Like
Hi and thanks for the info. The fortunate part was the machine brought the bit to the starting position so I just had to get the “Z” axis adjusted and restart the finishing pass. All was good fortunately. Although we have had the machine for a couple years I would still call us green at using the system. Reading the gcode and understanding what to look for will be a bit of a challenge for now, Will have to go though your notes and try and figure this stuff out. The carve is done so I can’t replicate the exact issue we had but learning more on the gcode I think will be a good thing. Thanks again
