Probing and automatic tool length measurements
22 Nov 2015 17:06 #65662
by cahlfors
Replied by cahlfors on topic Probing and automatic tool length measurements
Oh, sorry for publishing this before being satisfactorily complete. I have spent many months just to get it to work and I am hoping that others can get going a lot faster by having a reasonably working example to look at. ![:) :)](/media/kunena/emoticons/smile.png)
IMHO, at least TLO probing should be part of the basic setup. And 3D probing sure is nice! And together - wow!![:) :)](/media/kunena/emoticons/smile.png)
Thanks,
/Chris
![:) :)](/media/kunena/emoticons/smile.png)
IMHO, at least TLO probing should be part of the basic setup. And 3D probing sure is nice! And together - wow!
![:) :)](/media/kunena/emoticons/smile.png)
Thanks,
/Chris
Please Log in or Create an account to join the conversation.
14 Dec 2015 20:03 #66980
by cahlfors
Replied by cahlfors on topic Probing and automatic tool length measurements
A couple of changes have been made to improve z precision from 0.15 mm to 0.03 mm with my TLO measurement mushroom.
First, the manual_change.ngc had these last three rows added to make a second probe move at slower speed:
Then the *.ini was modified with new PROBEFEED:
Thanks,
/Chris
First, the manual_change.ngc had these last three rows added to make a second probe move at slower speed:
F #<_ini[toolsensor]rapid_feed>
G91 (relative mode)
G49 (cancel tool offset)
G38.3 Z #<_ini[toolsensor]maxprobe>
G0 Z2
F #<_ini[toolsensor]probefeed>
G38.3 Z-4
Then the *.ini was modified with new PROBEFEED:
# start of tool length touchoff probe
[TOOLSENSOR]
# Control probe rappid feed
RAPID_FEED = 1500
X = 0
Y = 102
Z = 275
MAXPROBE=-274 # abort change if no toolsensor contact after this probe distance
PROBEFEED=50
RAPID_SPEED = 1500
Thanks,
/Chris
Please Log in or Create an account to join the conversation.
29 Mar 2016 12:08 #72315
by tommy
Replied by tommy on topic Probing and automatic tool length measurements
I'm planning to implement this automatic tool length measurement on my machine and as far as I tested in simulation I don't understand function of Reference Tool button?
Also there I have question about procedure to touch-off Z from workpiece with first tool which I usually already have in spindle before running any code, should I manually enter T1 M6 to let machine know that first tool is already present and it will be used as "reference tool"?
Also there I have question about procedure to touch-off Z from workpiece with first tool which I usually already have in spindle before running any code, should I manually enter T1 M6 to let machine know that first tool is already present and it will be used as "reference tool"?
Please Log in or Create an account to join the conversation.
29 Mar 2016 20:03 #72348
by cahlfors
Replied by cahlfors on topic Probing and automatic tool length measurements
Hi Tommy!
Yes, I suggest manually entering T6 M1 before running the program. This will cause the machine to go to the tool change position. There, you should go to the tool change tab and make sure the reference tool button is active and the hit the probe button. This initiates the probing which should result in the reference tool length being updated. You can then proceed to touch off against your workpiece. I use my 3D probe for this, but that is not a requirement. Any tool, dowel or custom designed tip suitable for touching off can be used. When done, you can start executing your code, which will take you to the tool change dialog again. This time, be sure to uncheck the reference tool button and proceed. I am not sure what will happen if your code specifies tool #1 again. Maybe it skips the touchoff and just starts executing. Should work either way, I suppose, but I have not actually tried that.
The purpose of using a reference tool, is that any other tool will get a tool length offset (TLO in the readout) with a non-zero value in relation to this.
Hence, I have found (the hard way, of course...), you want to start every operation with M2 and G49 before T6 M1 to make sure any pending settings and active tool length offsets are canceled. That is what I was planning to use the reset button for.
Good luck and please report back with your findings!![:) :)](/media/kunena/emoticons/smile.png)
/Chris
Yes, I suggest manually entering T6 M1 before running the program. This will cause the machine to go to the tool change position. There, you should go to the tool change tab and make sure the reference tool button is active and the hit the probe button. This initiates the probing which should result in the reference tool length being updated. You can then proceed to touch off against your workpiece. I use my 3D probe for this, but that is not a requirement. Any tool, dowel or custom designed tip suitable for touching off can be used. When done, you can start executing your code, which will take you to the tool change dialog again. This time, be sure to uncheck the reference tool button and proceed. I am not sure what will happen if your code specifies tool #1 again. Maybe it skips the touchoff and just starts executing. Should work either way, I suppose, but I have not actually tried that.
The purpose of using a reference tool, is that any other tool will get a tool length offset (TLO in the readout) with a non-zero value in relation to this.
Hence, I have found (the hard way, of course...), you want to start every operation with M2 and G49 before T6 M1 to make sure any pending settings and active tool length offsets are canceled. That is what I was planning to use the reset button for.
Good luck and please report back with your findings!
![:) :)](/media/kunena/emoticons/smile.png)
/Chris
Please Log in or Create an account to join the conversation.
01 Apr 2016 13:01 #72524
by tommy
Replied by tommy on topic Probing and automatic tool length measurements
My findings after implementation to config of my machine, so procedure I was trying is:
- Fresh start of LCNC (reference and current Z lengths are both zero)
- execute T1M6
- insert tool #1
- activate Reference tool button
- click Change complete
- after tool was measured Current Z length is still zero, Reference Z length is negative number (I guess probed distance from absolute Z0) then I touch off for all three axis on workpiece
(no g-code was executed)
- execute G49
- execute T2M6
- insert tool #2
- deactivate Reference tool button
- click Change complete
- after tool was measured, value in Current Z length is way way to big to be used for tool length!
Did I missed something?
- Fresh start of LCNC (reference and current Z lengths are both zero)
- execute T1M6
- insert tool #1
- activate Reference tool button
- click Change complete
- after tool was measured Current Z length is still zero, Reference Z length is negative number (I guess probed distance from absolute Z0) then I touch off for all three axis on workpiece
(no g-code was executed)
- execute G49
- execute T2M6
- insert tool #2
- deactivate Reference tool button
- click Change complete
- after tool was measured, value in Current Z length is way way to big to be used for tool length!
Did I missed something?
Please Log in or Create an account to join the conversation.
11 Apr 2016 17:49 #73123
by cahlfors
Replied by cahlfors on topic Probing and automatic tool length measurements
Yes, executing G49 in the middle will clear the tool offset you just measured and set, so skip that and you should be ok.
/Chris
/Chris
Please Log in or Create an account to join the conversation.
19 Apr 2016 09:26 #73585
by metsuko
Replied by metsuko on topic Probing and automatic tool length measurements
Hi, can someone help me how to install this extesion auto tool measurement. I am novice at linuxcnc.
Thx Martin
Thx Martin
Please Log in or Create an account to join the conversation.
20 Apr 2016 12:02 - 20 Apr 2016 12:03 #73639
by andypugh
Tool length probing is, in principle, fairly easy.
1) Move to a safe height
2) Move to the tool height measurement station
3) Ask for the new tool and wait for confirmation
4) Make a probe move and set the tool length.
The moves happen in absolute machine space, so need a G53. hal_manualtoolchange can do the tool change, G38.2 and friends do the probe and G10 sets the tool length.
If you put the following in a file called toolprobe.ngc you will then be able to call it from the MDI window with "O<toolprobe>CALL [3] for tool 3, etc.
linuxcnc.org/docs/2.7/html/gcode/g-code.html#gcode:g38
linuxcnc.org/docs/2.7/html/gcode/g-code.html#gcode:g10-l1
linuxcnc.org/docs/2.7/html/gcode/overview.html#gcode:parameters
Bear in mind that is is an example routine, and might not work. For example I am not 100% sure what coordinate system the numbers in the #5061 to #5070 prove results paramters are reported in, I have assumed machine-absolute.
Once you have that working you can then configure the machine to automatically call the routine when it finds an M6 in the G-code. That is described here:
linuxcnc.org/docs/2.7/html/remap/remap.html
specifically this section
linuxcnc.org/docs/2.7/html/remap/remap.h...lated_codes_t_m6_m61
That is very detailed documentation, and you can skim-read most of it. You really just need the new INI file line in section 5.6
Replied by andypugh on topic Probing and automatic tool length measurements
Hi, can someone help me how to install this extesion auto tool measurement. I am novice at linuxcnc.
Tool length probing is, in principle, fairly easy.
1) Move to a safe height
2) Move to the tool height measurement station
3) Ask for the new tool and wait for confirmation
4) Make a probe move and set the tool length.
The moves happen in absolute machine space, so need a G53. hal_manualtoolchange can do the tool change, G38.2 and friends do the probe and G10 sets the tool length.
If you put the following in a file called toolprobe.ngc you will then be able to call it from the MDI window with "O<toolprobe>CALL [3] for tool 3, etc.
O<toolprobe>SUB
G53 G0 Z0
G53 X100 Y100 ; need to be the actual tool sensor position
M6 T#1; do the change
G53 G38.2 F100 Z -200 ; the speed is critical here, it must be slow enough for the machine to stop inside the probe travel
G53 G38.3 F20 Z 0 ; slow probe back off the switch
G10 L1 P#1 Z[213 - #5063] ; 213 would be the distance from the spindle nose to the sensor at top of travel
G53 G0 Z0
O <toolprobe> endsub
M2
linuxcnc.org/docs/2.7/html/gcode/g-code.html#gcode:g38
linuxcnc.org/docs/2.7/html/gcode/g-code.html#gcode:g10-l1
linuxcnc.org/docs/2.7/html/gcode/overview.html#gcode:parameters
Bear in mind that is is an example routine, and might not work. For example I am not 100% sure what coordinate system the numbers in the #5061 to #5070 prove results paramters are reported in, I have assumed machine-absolute.
Once you have that working you can then configure the machine to automatically call the routine when it finds an M6 in the G-code. That is described here:
linuxcnc.org/docs/2.7/html/remap/remap.html
specifically this section
linuxcnc.org/docs/2.7/html/remap/remap.h...lated_codes_t_m6_m61
That is very detailed documentation, and you can skim-read most of it. You really just need the new INI file line in section 5.6
Last edit: 20 Apr 2016 12:03 by andypugh.
Please Log in or Create an account to join the conversation.
21 Apr 2016 05:02 #73675
by metsuko
Replied by metsuko on topic Probing and automatic tool length measurements
Hi,
Thank you for your fast answer. But can you tell me how to install it.. Whitch file copy/put to.... I am distracted. I sucessfuly install probe screen to my Linux cnc but i dont know how to install this screen ,, auto tool measurement,,. Sorry if my questions are stupid.![:) :)](/media/kunena/emoticons/smile.png)
Thanks Martin
Thank you for your fast answer. But can you tell me how to install it.. Whitch file copy/put to.... I am distracted. I sucessfuly install probe screen to my Linux cnc but i dont know how to install this screen ,, auto tool measurement,,. Sorry if my questions are stupid.
![:) :)](/media/kunena/emoticons/smile.png)
Thanks Martin
Please Log in or Create an account to join the conversation.
- racedirector
- Offline
- Elite Member
-
Less
More
- Posts: 267
- Thank you received: 42
21 Apr 2016 08:27 #73678
by racedirector
Replied by racedirector on topic Probing and automatic tool length measurements
Have a look here, I use this touchoff and tool measurement on my machine:
forum.linuxcnc.org/forum/10-advanced-con...h-touch-off?start=30
Cheers
forum.linuxcnc.org/forum/10-advanced-con...h-touch-off?start=30
Cheers
Please Log in or Create an account to join the conversation.
Time to create page: 0.116 seconds