Resetting the default Work offset code.

[RdHawg]

On a Fanuc 160is-m control is there an easy way to change the default work offset?

Ie. right now when I hit the reset key the controller always goes to G54 - I would like to be able to change that to the fixture offset of whatever part I'm currently working on.

[Mitsui Seiki]

Why do you want to do that?The program changes it in to what ever you want it to be.

[dcoupar]

I believe parameter #1201 bit 7 (WZR) controls whether the Work Coordinate system is set to G54 upon reset. (0 = no, 1 = yes). Yours is probably set to 1?

[RdHawg]

Originally Posted by Mitsui Seiki Why do you want to do that?The program changes it in to what ever you want it to be.

Because sometimes I restart a program in the middle of it and the controller never reads the line with the offset in it. (Not good)

[RdHawg]

Originally Posted by dcoupar I believe parameter #1201 bit 7 (WZR) controls whether the Work Coordinate system is set to G54 upon reset. (0 = no, 1 = yes). Yours is probably set to 1?

My #1201 Has ZPR over bit 7? Same thing? Where could I double check that before I do something tragic?!

[psevin]

Par. 1201 bit 7 is WZR -
Upon reset, the workpiece coordinate system is:
0 : Not returned to that specified with G54
1 : Returned to that specified with G54

bit 0 is ZPR -
Automatic setting of a coordinate system when the manual reference
position return is performed
0 : Not set automatically
1 : Set automatically

Note that - ZPR is valid while a workpiece coordinate system function
is not provided. If a workpiece coordinate system function is provided, making a manual reference position return always causes the workpiece coordinate system to be
established on the basis of the workpiece origin offset (parameters No. 1220 to No. 1226), irrespective of this parameter setting.

Hope this helps.

[Mitsui Seiki]

Originally Posted by RdHawg Because sometimes I restart a program in the middle of it and the controller never reads the line with the offset in it. (Not good)

Ok.So if you have G55 in your program and reset it and start over, it uses G54?
I have made it a habit to always read the work zero in what ever program I'm running before I start over.

[codyst]

Mitsui, he's not starting over from the beginning, he's starting the program in the middle. Since his work coordinate is called at the beginning of the program it doesn't get reinstated when he starts from whatever line number he chooses to restart at.

[Mitsui Seiki]

I know.Read the work zero in the beginning and then turn to edit,step down to where ever you want to start,turn to prog. and run.