Touch off after manual tool change

More
08 Feb 2018 20:15 #105600 by Donno
OK Thank you

1. I when to touch plate and run MDI G30.1 that set the X,Y
2. Set g38.2 z-60 f100 in reference.ngc
3. MDI o<reference> call it go to G30.1 and lowers till hits the touch plate and stops there is purple line in Preview windows
4. go to job and set G54
5. Start the job and it asks for tool 1

when i hit continue it does not go to touch plate it just starts cutting must i insert the o<tool-probe> call in my g-code after the N30 T1 M6 ?

Here is spinet of code

(DRILL2)
N25 M9
N30 T1 M6
N35 T2
N40 S1000 M3

.......


(POCKET1)
N125 M9
N130 M1
N135 T2 M6
N140 T1
N145 S1000 M3
N150 M8
More
08 Feb 2018 20:48 - 08 Feb 2018 21:46 #105603 by Todd Zuercher
The process should work like this.
1) Set up your G30 position (you should only need to do this once as the values are saved)

2) Set up g-code file(s) for part: (With a manual tool change machine it is often better to break up a file using multiple tools into a separate file for each tool.)
T1M6
o<reference> call
s1000m3
(insert code that uses the 1st tool here)

T2M6
o<tool-probe> call
S1000M3
(insert code that uses the 2nd tool here)

T3M6
o<tool-probe> call
S1000M3
(insert code that uses the 3rd tool here)
...
M30

3) Set up first tool and the part in the machine, adjust machine coordinates for G54 for that tool and part,

4) Start the milling file, doing the reference probe. (if the tool should happen to break, you can stop the run, change the tool, run the o<tool-probe> call from MDI, then restart the file.)

5) When it is time to change the tool the machine should pause over your probe, change the tool, press enter, and it should continue.

If you want to make it so you don't need to insert the o calls you would have to remap the M6 code. I am not very familiar with remapping, But I think there are some examples where people have done it for this very purpose. But like I said, I don't know enough about it to guide someone through it.
Last edit: 08 Feb 2018 21:46 by Todd Zuercher.
More
09 Feb 2018 08:11 - 09 Feb 2018 08:12 #105622 by Donno
Following your instructions and all works good on first tool change and first cut

5) When it is time to change the tool the machine should pause over your probe. It stops over G54 Z0 which is fine

T2M6
o<tool-probe> call
S1000M3
(insert code that uses the 2nd tool here)

The second tool change pauses i change the tool when i click continue the cnc goes to G30 then stops it does not move down ???

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 z-60 f100 (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

Is there other settings i need to set up ? Using LinuxCNC 2.7.0 do i need to update ?
Last edit: 09 Feb 2018 08:12 by Donno.
More
09 Feb 2018 13:08 #105628 by Todd Zuercher
I have an M0 pause inserted after the M30, If you press "s" on the keyboard or the "pause" button on the screen to un-pause it and it should continue. (If it doesn't i'm not sure what the problem is.)

If you don't need or want that pause there (I put it in for changing the tool if need be) just remove it.
More
11 Feb 2018 20:29 #105765 by Donno
Thanks for helping me, got it right after a few tries



I have two things that I still want to do :

1. Move fast to touch plate after trigger move back and fine trigger plate
2. after tool touch off want it to go to Z0

Posted my code below do see any problems with it ?

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 z-60 f480 (measure change z to a number that works for your setup) <-- Fast touch
g91 g0 z5 (off the switch) <-- retract 5mm
g38.2 z-60 f20 (measure change z to a number that works for your setup) <-- Fine tune
g91 g0 z0 (off the switch) <-- Set offset
g43.1 z[#5063-#1000] (set new tool offset)
(print,new length is #5063)
g90 (done)
Z0 <--- Go to Z0
o<tool-probe> endsub

Thank you in advance !
Moderators: piasdom
Time to create page: 0.087 seconds
Powered by Kunena Forum