[itstom]

What sketchy documentation I do have says G10 is date setting.

If I write the value to G54 I loose the original number and won't be able to just have the operator enter his part stick out into #101. If I write to work shift I think it would accumulate if you reset and started the program from the top.

Again, the hope was that the operator could enter his part length or stick out in a parameter at the top of the program. New part, new #101 value and hit go.

Tom

[dcoupar]

What sketchy documentation I do have says G10 is date setting.

If I write the value to G54 I loose the original number and won't be able to just have the operator enter his part stick out into #101. If I write to work shift I think it would accumulate if you reset and started the program from the top.

Again, the hope was that the operator could enter his part length or stick out in a parameter at the top of the program. New part, new #101 value and hit go.

Tom

Tom,

Work Shift doesn't accumulate. He could just enter the value there rather than editing the program or setting a macro variable. It could also go into the EXT Z offset on the Work Coordinate offset page.

G10 can be either Offset Modification or Programmable Parameter Entry.

You don't say what model 18T you have, but for the A series, parameter #5013 controls the maximum amount of tool wear compensation. This could be causing your alarm if it's set to < the value you enter in #101.

[itstom]

I'm not sure what model 18T I have.

Actually, I think the best solution would be to send this variable to the sub via the macro that will send the other part to part variables. I'm working with a family of 14 parts. (Probably should have mentioned that awhile ago.)

I'm just not sure what parameter I should write to.

#210X ? (where X is the tool number)
#5082 ?
#5222 Gave the same ILLEGAL...G10 message.

Thanks for the replies,
Tom

[FANUCCNC]

#5082 is a read only variable of the current offset amount in the second axis (Z).
#5222 is a read/write variable for the G54 workpiece zero point offset for the second axis (Z).
#2101 is a read/write variable for the Z axis, tool wear offset 1

The program used would generate the ILLEGAL OFFSET VALUE IN G10 error if the #101 value is greater than parameter 5013.

Check the 5013 parameter value and make #101 smaller than that value to test.

It doesnt make sense that the #5222 is generating the same message. Does it need to be a negative value in the workpiece offsets?

See attachments for addition information.