Okuma Mill tool length check

[zufan4]

We have a couple special combination tools that have a small diameter drill protruding from the end. I want to check the tool length from the registry that it is within a certain limit. So that if the tool length is changed it has to be between these set lengths.
For example.
If tool is under 11" then N...
If tool is over 11.5" then N...

Also I've done multiple tool offsets many times on a lathe. What does that look like for a mill? We have an older horizontal with 150 magazine.

Thanks

Similar Threads:

• CNC programming, just getting started cnc mill, tool length offset question
• Tool table, tool length management, 'master' tool
• Need Help!- set up tool length offset and ref tool on mill
• new (to me) mill...z0 is 2" high after tool length measure
• Need Help!- programing tool length offset in a 3axis mill

[deadlykitten]

hello zufan i can help for osp300

... what control do you have ?
... why do you need this check ?
... what do you mean by " Also I've done multiple tool offsets many times on a lathe " ?

kindly !

[Superman]

Simplest would be to place something in your NC program that interrogates the length that the tool offset has been set to, after your header
- you may also place the same code after your tool call, so if a restart situation occurs, any out-of-range tool length would make the program stop

ie

IF [ VTOFH[11] GE 11.5000 ] M00 ( TOOL SET-OUT TOO FAR )
IF [ VTOFH[11] LE 11.0000 ] M00 ( TOOL SET-IN TOO SHORT)
T11 M6 ( Call in Special Tool )
T12 ( Prepare Next Tool )

[kurmay]

System variables list for OSP-P200M

[deadlykitten]

if condition_evaluated_to_true then execute_true_branch

execute_true_branch allowed syntaxes are : " GOTO N* " and " N* "

    IF [ VTOFH [ 13 ] GE 11.5 ] NGOOD
         M0 ( hey )
    NGOOD

    IF [ VTOFH [ LV01 ] GE LV02 ] NGOOD
         M0 ( hey )
    NGOOD

( LV01 may contian the value of VTLCN, or may be replaced with VTLVN, etc )
( LV03 may contian the value of a real number, or may be replaced with a real number, etc )
( local variables can be created when a tool change macro is called : CALL LV01=13 LV02=next_tool LV03=11.5 )

a tool change macro may be called to also execute the following :
... offset > minimal_target ( m : greater than minimal )
... offset < maximal_target ( M : lower than maximal )
... minimal_target < offset < maximal_target ( mM : bounding )
... if you consider :
...... ( minimal_target + maximal_target ) / 2 = medium_offset
...... maximal_targer - minimal_target = 2 * tolerance, than above condition becames | offset - medium_offset | < tolerance ( mM : symetrical bounding )
... offset = target, thus no corrections are allowed
... etc

i have developed this for lathes, and i will write codes for mill only when a series will kick in now we are machining uniques ...

i can raise the safety level, at least for osp300 kindly !