-
Configuring LinuxCNC
-
Advanced Configuration
-
Manual tool change + tool lengh touch off
Manual tool change + tool lengh touch off
Less
More
-
Posts: 24203
-
Thank you received: 4795
-
-
06 Jul 2016 12:54 #77075
by andypugh
This is the sequence that I think you will need to do to keep things in synch.
Put in the tool and manually run the M600 sequence to measure the tool.
(At this point the tool number in the spindle is correct and the tool length has been measured)
Touch-off to the workpiece and offset the G54 coordinate system to set Z = 0.
To test, run M600 again, check that the Z = 0 still matches the work.
Now things should work OK (assuming the M600 sub is correct).
I think that your problem lies with touching-off the top of the work with unknown tool-length. Or possibly touching-off the top of the work into the tool table and not the work-axis offset.
Please Log in or Create an account to join the conversation.
Less
More
-
Posts: 14
-
Thank you received: 1
-
-
06 Jul 2016 13:50 #77081
by hancock
This is the sequence that I think you will need to do to keep things in synch.
Put in the tool and manually run the M600 sequence to measure the tool.
(At this point the tool number in the spindle is correct and the tool length has been measured)
Touch-off to the workpiece and offset the G54 coordinate system to set Z = 0.
To test, run M600 again, check that the Z = 0 still matches the work.
Now things should work OK (assuming the M600 sub is correct).
I think that your problem lies with touching-off the top of the work with unknown tool-length. Or possibly touching-off the top of the work into the tool table and not the work-axis offset.
Hello andypugh,
thanks for your help but if I do it that way, the G54 is put into the TLO offset and (of course) it says that the Joint is hit, so the machine stops.
But thanks for the input - it was worth a try!
Please Log in or Create an account to join the conversation.
Less
More
-
Posts: 14
-
Thank you received: 1
-
-
06 Jul 2016 13:55 - 06 Jul 2016 13:56 #77082
by hancock
I'd check the installation, to ensure there isn't some problem with the way the M600 command has been configured (maybe the filename is incorrect, or the file is missing...) It's almost certainly the case that the g-code that should be associated with M600 is not being run.
Hey orangecat,
thanks again for your help! I've double checked now and the file is there, the link to the file name is correct and the only error I could find was that I put the "TOOL_CHANGE_AT_G30 = 0" under "EMCMOT" instead of "EMCIO". But that also did not solve the problem.
It seems that the offset is reversed: I tested by putting in the second tool a little bit deeper into the spindle and it mills in the air, just like it would have reversed the offset - like -2mm would be needed to get to Z0 and it uses 2mm.
Really strange because everything else within my tests with MDI commands works like a charm...
Last edit: 06 Jul 2016 13:56 by
hancock.
Please Log in or Create an account to join the conversation.
Less
More
-
Posts: 24203
-
Thank you received: 4795
-
-
Less
More
-
Posts: 14
-
Thank you received: 1
-
-
06 Jul 2016 14:52 - 06 Jul 2016 15:05 #77085
by hancock
It looks like the TLO is calculated correctly but it seems that my job-file resets this offset immediately when it starts milling again.
I looked into my gcode and i found that after every tool change
The exact command is inserted in the gcode after every tool change. Is it correct that is always uses Z15 and also H1 for every tool?
Somehow I know it can't be the problem but why is it there?
Thanks a lot in advance guys!
Last edit: 06 Jul 2016 15:05 by
hancock.
Please Log in or Create an account to join the conversation.
Less
More
-
Posts: 14
-
Thank you received: 1
-
-
06 Jul 2016 14:59 #77086
by hancock
Sorry - it means that the offset that's currently stored in G54 after touching off the workpiece is now somehow the same value shown in the TLO.
Please Log in or Create an account to join the conversation.
Less
More
-
Posts: 24203
-
Thank you received: 4795
-
-
06 Jul 2016 15:14 #77087
by andypugh
Sorry - it means that the offset that's currently stored in G54 after touching off the workpiece is now somehow the same value shown in the TLO.
That might not be wrong.
Please Log in or Create an account to join the conversation.
Less
More
-
Posts: 24203
-
Thank you received: 4795
-
-
Less
More
-
Posts: 14
-
Thank you received: 1
-
-
06 Jul 2016 16:38 - 06 Jul 2016 16:40 #77089
by hancock
Hey Guys,
I recorded the screen of whats actually going - maybe it's easier
The video starts after I touched off the material and I issued the M600 before the file starts. The TLO is 0.
I placed the second tool deeper in the spindle and the calculated TLO is -2.263mm which would be correct as the Z-axis moves negative to the table.
Then the milling starts, TLO is shows 0 again and the tool is above the workpiece. Pretty much the height of the first tool that was a bit longer outside the spindle.
I hope this shows my problem
Last edit: 06 Jul 2016 16:40 by
hancock.
Please Log in or Create an account to join the conversation.
Less
More
-
Posts: 17
-
Thank you received: 21
-
-
06 Jul 2016 17:08 #77094
by orangecat
I looked into my gcode and i found that after every tool change
That's the problem. G43 H1 will reset the tool offset that the touch-off set, to be the tool offset stored in the tool table for tool 1.
By removing G43 H1, all should work well. I don't know if you want to move to Z15 at this point. Maybe not, in which case the entire line can be removed.
Please Log in or Create an account to join the conversation.
-
Configuring LinuxCNC
-
Advanced Configuration
-
Manual tool change + tool lengh touch off
Time to create page: 0.096 seconds
