Need Help!- Fanuc series oi-TC Offset clearing

[TysonTJ]

Hi,
I have a question regarding a Fanuc series oi-TC control on a Toshiba VBM
The machine is on a 3 shift rotation. Some operators set tool offsets by using wear offsets & others using the fine offsets. While this in theory is ok, it has lead to confusion between operators, especially when switching between different part programs.
What I would like to do is, at the end of each part program, set all the tool offsets to zero.
Can I do this with a single code? Or will it require a command for each offset number cancellation?
If so I could use a parameter command? i.e. #2001=0, #2701=0 etc. This would require quite a number of lines. I suppose it could be put in a subprogram though.
Can anyone suggest an easy solution?
Regards,
Tom Tyson

[dcoupar]

I would think you could use a macro that started at offset #1 and then used G10 to set the particular offset to 0. Then the counter would increment by 1 and loop. When the counter exceeded the number of offsets, it would exit.

O9101 (CLEAR ALL OFFSETS)
#1=1(INITIALIZE COUNTER)
N1 G10 P#1 X0 Z0 R0 Q0 (CLEAR WEAR OFFSETS)
G10 P[10000+#1] X0 Z0 R0 Q0 (CLEAR GEOM OFFSETS)
#1=#1+1 (INCREMENT COUNTER)
IF[#1 GT 64] GOTO 2
GOTO 1
N2 M30

[tobyaxis]

Originally Posted by TysonTJ Hi, I have a question regarding a Fanuc series oi-TC control on a Toshiba VBM The machine is on a 3 shift rotation. Some operators set tool offsets by using wear offsets & others using the fine offsets. While this in theory is ok, it has lead to confusion between operators, especially when switching between different part programs. What I would like to do is, at the end of each part program, set all the tool offsets to zero. Can I do this with a single code? Or will it require a command for each offset number cancellation? If so I could use a parameter command? i.e. #2001=0, #2701=0 etc. This would require quite a number of lines. I suppose it could be put in a subprogram though. Can anyone suggest an easy solution? Regards, Tom Tyson

Tom,

To be honest you really need to organize a Shop Standard for setting Offsets. It isn't a big deal which method you decide to use but it avoids this type of confusion among the operators.

Here are two examples:

One Shop programs their machines to include Cutter Comp in the initial program then uses the Wear Offsets to make adjustments. In other words Tool Center Line Programming. This method makes it so an inexperienced operator that forgets to enter the Actual Tool Radius (when programming direct print geometry) won't make scrap.

Another Shop will use the Direct Geometry on the print to write a program. They will then enter the Tool Radius on the Offset Page under Geometry.

Either will work depending on how experienced the operators are but a Standard has to be issued as Shop Practice to avoid making scrap or worse "cause crashes".

Just my 2 cents