How to add tool break control cycle

[nubrandao]

hi, i found tool break control line in post processor, but hás no command,  how to make it Write the cycle tool break control?

Im using post processor Heideiain.

TCH PROBE 584 TOOL SETTING L,R ~
Q350=+2 ;MEASURING TYPE ~
Q351=+0 ;APPLICATION ~
Q352=+0 ;CUTTING EDGE CONTROL ~
Q355=-1 ;MEASURING POSITION ~
Q361=+2 ;NUMBER OF MEASURINGS ~
Q362=+0.002 ;SCATTER TOLERANCE ~
Q359=+0 ;ADD. LENGTH CORRECT. ~
Q360=+0 ;ADD. RADIUS CORRECT.

[a.laasW8M6T]

Hi

You can add that cycle to the COMMAND_BREAK_CONTROL area

BUT, you must also add some code to determine what to do if the tool is broken.

Do you have the information from the Blum(or DMG) manual for TCH Probe CYCLE 584 and how it works?

It must set a Q value to 1 if the tool is broken, or something similar?

do the machine axes need to be homed before calling the cycle?

including A and C rotary?

[a.laasW8M6T]

Do you have break control implemented in your Powermill posts?

If so you should be able to duplicate the format that the code is output from Powermill into Fusion

[nubrandao]

We never used on company, i found in Fusion NC manual command to check Control break check

I Saw in our machines to break cycle

Then i tried in Fusion, NC tool break, then i Saw that nothing happens

Then in post processor, i Saw empty in tool break command

Só i have no idea what to Write in post processor 

I just machine to stop M30 if tool cycle gets error

I Saw something like FN q199 = 0

Go to label 25

m30

[nubrandao]

In our case, its could BE very helpfull

In our DMG Evo 80

 We 4 tablet fixture, with robot to Change manual

Só the operator can input. 4 diferent fixtures

We had a lot of problems, some Times, a Rough carbide tool is used in the Four fixture,

We had a situation that broken in the first tool Path, all the tools were suposed to go there, broken, more then 10 tools at once.

The we started working in shift, so the operator could check  tools

But if we could use break tool Control, could BE a game changer and all the DMG operator could do normal shift again.

[a.laasW8M6T]

I can probably create something that will work but you will need to test and adjust yourself.

I can look at it over the weekend

[nubrandao]

Thanks you very much

[nubrandao]

I Will print a photo tomorrow of our tool break cycle

Our laser is the same place of tool changer...

Basically, at tool Change, we need to check it before put the tool in the magazine. Since they are in the same place. No worry about position Axis.

All i need is to input a cycle "tool break control"

If FN Q199 = 1

Go to Lbl 25

Lb25 M30

[nubrandao]

• I found this, could help 

TCH PROBE 584 TOOL SETTING L,R ~

Q350=+2 ;MEASURING TYPE ~

Q351=+0 ;APPLICATION ~

Q352=+0 ;CUTTING EDGE CONTROL ~

Q355=-1 ;MEASURING POSITION ~

Q361=+2 ;NUMBER OF MEASURINGS ~

Q362=+0.002 ;SCATTER TOLERANCE ~

Q359=+0 ;ADD. LENGTH CORRECT. ~

Q360=+0 ;ADD. RADIUS CORRECT.

FN 11: IF +Q199 GT 0 GOTO LBL 25

(At the end)

LBL 25

END PGM 1234 INCH

[a.laasW8M6T · Accepted solution]

Hi

See attached post

Video for explanation:

[nubrandao]

I Will try it. Thanks you very much for your effort

[nubrandao]

One question, in our post processor, we had m30 removed because its stops allways at the end of NC program,

for example, i usually create an NC for rough strategys, other NC for finish.

so the operator some, creates a NC program that will call NC-rough + NC-finish

with M30 by default, the machines never starts the second NC because it stopped with, so in this line, i removed M30

  //writeBlock(mFormat.format(30)); // stop program, spindle stop, coolant off

  writeBlock("LBL 0");

but i was thinking, will the machine read M30  in label 25 if the tool is ok? if so, it will stop the machine

should i change the label 25 (m30) for m5? it only pause the machine and spindle right?

ONE 

[nubrandao]

is this valid?

the result

i think this way that if tool is broken, it will jump at the end program right?

i noticed if i manual run tool break cycle, the tool that is broken, becomes locked in the table and i cant run until i unlock it.

maybe, the best way to use this post processor, is to put all toolpaths inside, so it always read M30 at the end, what do you think?

[a.laasW8M6T · Accepted solution]

Yes, if you change it like that it will jump to the end and then return to the calling Program

If you want it to stop the program and not continue, then M5 won't work, it will just stop spindle.

To stop the program you would use M0.

But i think just having it jump to LBL 25 just before the end of program should work fine

I just put all my program in the one file but the sort of work I do is very different than yours, I am the programmer/machinist/operator of just the one machine, so do everything myself.

[nubrandao]

Yes you right 

[marcelVNUJC]

Tank you very much for your explanation.