Broken tool detection

[zufan4]

We are wanting to use the breakage detection function. Sub-program name"OO30" on our horizontal Okuma MX-40HA mill with OSP-U100M control.

The machine has the touch probe that is mounted to the Z axis saddle.



We have a big job that has some expensive special tooling. We are wanting to run it lights out after second shift leaves.
All that we need to check is the tool length in the Z axis. To verify if the tool is broken or not and stop the machine if it is.
There is a page full of variables in the manual, and I'm not sure what I need or don't need.



Can someone send me a sample program on how to use it in auto mode?

Thank you!

Similar Threads:

• Need Help!- Broken Tool Detection
• Broken Tool detection
• Need Help!- Tool Breakage Detection
• Tool Breakage Detection Down to 0.125mm!
• Tool length detection

[deadlykitten]

There is a page full of variables

hello zufan, i googled after the variables for u100m, but i did not find something at 1st try

please share that page, maybe there is something / kindly

[Superman]

This is a blast from the past ...... LINK to a past thread for a MX-40HA

There is a library file with a macro for OBREK which gauges a previously gauged tool and compares the results

(*******************)
OBREK (TOOL BREAKAGE DETECTION)
VFST=128
N1000 G15 H20  (TO SET TOOL OFFSET CENTERLINE)
CALL OO30 PLE1=0.25(TOOL WEAR TOL.)
VFST=129
G15H0
RTS
()

PLE1=value is the allowable difference between the gauging result and the stored length
- if gauged length is not outside the tolerance range, program continues
- if gauged length is outside range, program stops ( or program can be configured to use tool management ie a replacement tool ) ( which is another big learning curve )

[deadlykitten]

hy Superman it is possible to execute oo30 in this way, at least on ops300; i have done this before, but after a while i quit, because this method provides relative results : for example, if the tool slides with 0.1 after each cycle, and the tolerance is 0.2, after 4 cycles, the tool would change it's position with 0.4, but no error would occur

however, if this possibility exists on u100m, than it should be possible to detect the system variable that stores the answer ( = svsa ), and use something like this simple code ( simple because it does not cook, and also it does not fly into space ) :

    value_before_oo30 = svsa
    call oo30
    if not ( | value_before_oo30 - svsa | ≤ tolerance ) than error_case

kindly

[Superman]

hy Superman it is possible to execute oo30 in this way, at least on ops300; i have done this before, but after a while i quit, because this method provides relative results : for example, if the tool slides with 0.1 after each cycle, and the tolerance is 0.2, after 4 cycles, the tool would change it's position with 0.4, but no error would occur

however, if this possibility exists on u100m, than it should be possible to detect the system variable that stores the answer ( = svsa ), and use something like this simple code ( simple because it does not cook, and also it does not fly into space ) :

    value_before_oo30 = svsa
    call oo30
    if not ( | value_before_oo30 - svsa | ≤ tolerance ) than error_case

kindly

It is not how it works, you want to set up a type of check (( of a check ) of a check ) scenario.... that's just dumb
IT IS ALREADY A CHECK CYCLE.... don't F*** with it

It doesn't update with a new tool length.... it is a compare operation...... the PLE1 tolerance is how much the OBREK check cycle can be from the original tool gauge value
- if tool slides 0.1 after each use, and the tolerance is 0.25...... the OO30 operation would give a result that the tool is outside the tolerance ( and STOP if tool management is NOT enabled ) on the 3rdcheck cycle
- If tool management is used, it would say that tool is expired and a sister tool used in it's place ( don't ask .... never had a need to go down this path )

[deadlykitten]

you are right Superman, when i tested it, i was no aware of VFST, which was described a few pages before

but i found my way arround it : it took me less time to write alternative code, rather than rtfm

thank you for your reply using VFST also comes with CTR, so thank you again

why using G15 H* ? whatever the H* value, oo30 will always go to same phisical location; perhaps G56 ? but even so, i dont think that you need it, because there is PX & PY, and if those arguments are omited, than spindle will be coaxial with the senzor

[zufan4]

Ok thanks for the replies!

Now I was looking and this control has only "TIME" as an option on the tool life management page. Is there a way to change that to pcs? So that we can count the number of pcs instead of time.

[deadlykitten]

hello zufan, i would suggest something like this :

  IF [ V123 LE 23*1 ] N1
  IF [ V123 LE 23*2 ] N2
  IF [ V123 LE 23*3 ] N3

    NLOOP M0 ( all tools have been used )
          GOTO NLOOP

    N1 T020202
       GOTO NOUT

    N2 T111111
       GOTO NOUT

    N3 T030303

    NOUT