Setting Wear Offset via NC Program

Control is 18T.

I want to assign Z wear offsets for my tools via parameters in my program. I want to accommodate varying part lengths from the chuck face. I could set tool geometry like this (not that I want to):

#101 = .625
#2803 = #101
#2804 = #101

But when I try to set wear offsets like this:

#101 = .625
#2103 = #101
#2104 = #101

I get an alarm "ILLEGAL OFFSET VALUE IN G10". Unfortunately, I don't have any manuals for this control.

Thanks in advance,
Tom

Quote:

---

Originally Posted by itstom

Control is 18T.

I want to assign Z wear offsets for my tools via parameters in my program. I want to accommodate varying part lengths from the chuck face. I could set tool geometry like this (not that I want to):

#101 = .625
#2803 = #101
#2804 = #101

But when I try to set wear offsets like this:

#101 = .625
#2103 = #101
#2104 = #101

I get an alarm "ILLEGAL OFFSET VALUE IN G10". Unfortunately, I don't have any manuals for this control.

Thanks in advance,
Tom

---

I don't see a G10 in the blocks above. Are you using G10 or trying to write directly to the parameter?

If you're trying to shift all the tools back 0.625, why not put the value in G54 or the Work Shift?

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

Quote:

---

Originally Posted by 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

---

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.

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

Did you check parameter #5013?

#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.