Answered
Breaking up a large job into smaller parts.
I have some really long 24-48 hr 3d relief carves I want to do but was looking for a way to break that up into several parts. Is there a way to take one project g-code and split it up into multiple parts for the same carve?
Comments
Splitting up the gcode is something that can be done outside of Carveco, manually or using a 3rd party app.
I've always chosen to break the machining up in rectangular tiles, with an overlap at least as large as your largest bit. For instance, if the model is 48x96 and you wanted 24x24" tiles, and you used a 1/8" ball, I'd make the machining boundary vector 24.125" and the adjacent tile the same so you get a little overlap on both to feather in the transitions. Just make rectangles that overlap and select the vector you want to machine and cycle through the set. Then save out each tile with a name and number you understand.
This gives you the ability to see the what and where without relying on your minds eye like hand coding or gcode cooking via some app.
Thanks that seems like a really simple way to do it. I appreciate the tip.
Is there an example of that anywhere. I know nothing whatsoever about gcode. I would not know where to start but because of social issues need to learn how.
Not sure if this will help: https://youtu.be/RN_5aKk4u9M?t=19
Thank thank you. That’s exactly what I need. Have not yet tried it but I feel confident it’s going to deal with my issue.
thanks for the help.
I got another answer back on this so I thought I would post it.
When you have to stop in the middle of a long running program, and try to resume, as stated by others, you need to note which block number was active when the program was stopped.
Now you can make a copy of this file and open the file on your computer with an editor such as notepad. However, if your post processor does not output line numbering (“N” numbers), you may need a different editor such as Notepad++ which will number the lines for you.
Now that you have your file open, search down for the line when the program stopped. I recommend restarting a few lines before this. Check to see if this line has positions for X,Y,and Z. If any of these are missing, you need to search upwards to find the most recent position for each axis. Take note of these positions. You also need to take note of which G code is active (G0,G1,G2, or G3), and the active feedrate (F???). If your post processor outputs the active feed mode (G0,G1,G2, or G3) on every line, then you don’t have to worry about this, but if you don’t see one of these codes, be sure to look at previous lines to see which one is active.
At this point you can delete all lines before this except for your setup codes which look something like this.
%
T1 (MSG, Insert Tool 1)
G0 G17 G20 G90 G40 G49 G64
G0 Z3.000
G0 X0.000 Y10.000 M03 S15000
M0(MSG, Click ‘Continue’ when the spindle is up to speed)
The Z3.000 above is a clearance point above your carve, if this is not high enough, change it to an appropriate number.
The X0.000 and Y10.000 should be changed to the X and Y positions that you noted where the program will resume.
After the M0 add a feedrate move to the proper Z level and feedrate (G1 Z-??? F???) that you noted.
If the next line(the line where you are resuming to) is missing the active feed mode (G1,G2 or G3) that you noted, add it to the beginning of the line.
Now you should be able to run this copy of the program to resume at this point.
Thanks for that update. A bit beyond my current abilities, but I’m learning. :)
Please sign in to leave a comment.