Touch off after manual tool change
07 Feb 2018 11:12 #105523
by Donno
Touch off after manual tool change was created by Donno
I have been using LinuxCNC for about an year on my mill and router for simple jobs, i want to add touch plate to offset tool length ising probe-in pin so basically
1. Want to have blank tool to zero job/touch off using G53
2. then run program on tool change 1 want to manually insert tool
3. then go to X,Y where touch plate is.
4. then tool touches plate using Z and start spindle and complete cut
5. on tool change 2 insert tool and repeat from number 3.
A lot of tutorials have little info and most links are broken or the tutorial is so complex(Windows user)
Any one that can help please ?
1. Want to have blank tool to zero job/touch off using G53
2. then run program on tool change 1 want to manually insert tool
3. then go to X,Y where touch plate is.
4. then tool touches plate using Z and start spindle and complete cut
5. on tool change 2 insert tool and repeat from number 3.
A lot of tutorials have little info and most links are broken or the tutorial is so complex(Windows user)
Any one that can help please ?
Please Log in or Create an account to join the conversation.
- Todd Zuercher
-
- Away
- Platinum Member
-
Less
More
- Posts: 5000
- Thank you received: 1409
07 Feb 2018 14:33 #105530
by Todd Zuercher
Replied by Todd Zuercher on topic Touch off after manual tool change
What do you need help with, connecting your probe switch, or writing the g-code for your probing routine?
Please Log in or Create an account to join the conversation.
07 Feb 2018 14:44 #105531
by Donno
Replied by Donno on topic Touch off after manual tool change
g-code for your probing routine please
Please Log in or Create an account to join the conversation.
- Todd Zuercher
-
- Away
- Platinum Member
-
Less
More
- Posts: 5000
- Thank you received: 1409
07 Feb 2018 18:57 #105536
by Todd Zuercher
Replied by Todd Zuercher on topic Touch off after manual tool change
The probe routine I am using will be different from what you want. I probe on the part rather than a fixed probing station on the machine.
How you set up your file is going to depend on how your machine is set up, and how you plan to use it.
Does your machine have repeatable tool lengths? (Are tools mounted in tool holders that you swap out or are you taking tools in and out of collets with a wrench)
How do you intend to reference your touch plate?
There are a lot of little details like these that you have to work out before you can build your file.
How you set up your file is going to depend on how your machine is set up, and how you plan to use it.
Does your machine have repeatable tool lengths? (Are tools mounted in tool holders that you swap out or are you taking tools in and out of collets with a wrench)
How do you intend to reference your touch plate?
There are a lot of little details like these that you have to work out before you can build your file.
Please Log in or Create an account to join the conversation.
08 Feb 2018 01:56 #105553
by Donno
Replied by Donno on topic Touch off after manual tool change
I have a fixed probing station on (X,Y)
My first post describes the use
1. Want to have blank tool to zero job/touch off using G53
2. then run program on tool change 1 want to manually insert tool
3. then go to X,Y where touch plate is.
4. then tool touches plate using Z and start spindle and complete cut
5. on tool change 2 insert tool and repeat from number 3.
Does your machine have repeatable tool lengths ? Answer is NO
How do you intend to reference your touch plate? with the blank tool which will be replaced by touch probe in future but now will be a blank piece of mild steel with sharp point which will have repeatable tool length.
My first post describes the use
1. Want to have blank tool to zero job/touch off using G53
2. then run program on tool change 1 want to manually insert tool
3. then go to X,Y where touch plate is.
4. then tool touches plate using Z and start spindle and complete cut
5. on tool change 2 insert tool and repeat from number 3.
Does your machine have repeatable tool lengths ? Answer is NO
How do you intend to reference your touch plate? with the blank tool which will be replaced by touch probe in future but now will be a blank piece of mild steel with sharp point which will have repeatable tool length.
Please Log in or Create an account to join the conversation.
- Todd Zuercher
-
- Away
- Platinum Member
-
Less
More
- Posts: 5000
- Thank you received: 1409
08 Feb 2018 04:27 #105557
by Todd Zuercher
Replied by Todd Zuercher on topic Touch off after manual tool change
G53 is the raw machine coordinates (no offsets). You don't do any machining in G53. You can only make single line movements with it.
I think this is how I would try to set this up. I'd set up two probe files. The first one would be the reference tool probe. You would set up your first tool, run the reference tool probe routine and then run that part of the file for the first tool, then when it is time to change tools. Then you would change tools run the tool length probe routine and continue your milling.
There is an example g-code program called tool-length-probe.ngc that is included with Linuxcnc that appears to be almost exactly what you need. i would suggest breaking it up into two sub programs like so.
reference.ngcThe code for measuring the next tool (or subsequent ones)
tool-probe.ngc
I think this is how I would try to set this up. I'd set up two probe files. The first one would be the reference tool probe. You would set up your first tool, run the reference tool probe routine and then run that part of the file for the first tool, then when it is time to change tools. Then you would change tools run the tool length probe routine and continue your milling.
There is an example g-code program called tool-length-probe.ngc that is included with Linuxcnc that appears to be almost exactly what you need. i would suggest breaking it up into two sub programs like so.
reference.ngc
o<reference> sub
g90 g49
g30 (above switch)
g38.2 z0 f15 (measure change z to a number that works for your setup)
g91 g0z.2 (off the switch)
#1000=#5063 (save reference tool length)
(print,reference length is #1000)
g90 (done)
o<reference> endsub
tool-probe.ngc
o<tool-probe> sub
(measure next tool)
g30 (above switch)
m0 (pause to change tool)
g49 (measure without the last tool's offset)
g38.2 z0 f15 (measure change z to a number that works for your setup)
g91 g0 z.2 (off the switch)
g43.1 z[#5063-#1000] (set new tool offset)
(print,new length is #5063)
g90 (done)
o<tool-probe> endsub
Please Log in or Create an account to join the conversation.
08 Feb 2018 15:34 #105578
by Donno
Replied by Donno on topic Touch off after manual tool change
You right its not G53 it is G54 where my gig is i created the two files how do i execute the subroutine ?
Do i run a MDI command ? or do integrate it somehow in the integrated in the tool change ?
Do i run a MDI command ? or do integrate it somehow in the integrated in the tool change ?
Please Log in or Create an account to join the conversation.
- Todd Zuercher
-
- Away
- Platinum Member
-
Less
More
- Posts: 5000
- Thank you received: 1409
08 Feb 2018 16:13 - 08 Feb 2018 16:17 #105583
by Todd Zuercher
Replied by Todd Zuercher on topic Touch off after manual tool change
Save the files in your nc_files directory or the directory specified by SUBROUTINE_PATH = in your ini file.
Do not forget to set the postion for G30. The simplest way is to move to that point then issue the MDI command G30.1
Call them by using these lines in your file where you want to reference or measure a tool in a g-code program, or with an MDI command.and
Do not forget to set the postion for G30. The simplest way is to move to that point then issue the MDI command G30.1
Call them by using these lines in your file where you want to reference or measure a tool in a g-code program, or with an MDI command.
o<reference> call
o<tool-probe> call
Last edit: 08 Feb 2018 16:17 by Todd Zuercher.
Please Log in or Create an account to join the conversation.
08 Feb 2018 16:45 #105589
by Donno
Replied by Donno on topic Touch off after manual tool change
G30 is that where the touch plate, X and Y coordinates are ?
Please Log in or Create an account to join the conversation.
- Todd Zuercher
-
- Away
- Platinum Member
-
Less
More
- Posts: 5000
- Thank you received: 1409
08 Feb 2018 16:48 #105590
by Todd Zuercher
Replied by Todd Zuercher on topic Touch off after manual tool change
Yes
Please Log in or Create an account to join the conversation.
Moderators: piasdom
Time to create page: 0.083 seconds