I'm having a problem with Intercon lathe tool offset

[fusion]

Hello,
I have a very simple lathe program that cuts off a small disc of material. My cutoff tool is #3 and I have entered that in Intercon, and it shows 0303 in the tool/offset window.
Here's the problem, when I post the program it outputs N0002 T0300 ;.125 wide cutoff. It's dropping the offset. I've tried this several times and it always drops the offset.
What do I have setup wrong? In my tool table, it shows offset 03 and tool 03 for that tool.
Thank you!
Mike

[Chaz]

I've also noticed this, its a pain and not sure why it does it.

But what you will notice is that during the run, it changes to the correct offset (check a bit later in the code, its shows T0303) and then when its done, the code takes it back to offset 00. I'm not sure why Centroid do this. Perhaps someone could let us know.

I know when I modify offsets when I fine tune, I try and understand why the change didnt work and its due to the offset being back at 00. A pain.

[suntravel]

Explanation in the JPG

Uwe

[Chaz]

Yep, suppose the question is why does Intercon insert the T0300 at the start and end? Its frustrating not to have the offset once the program finishes. Be nice to know if we can edit the 'post processing' which resets the offsets back 00 at the end.

[fusion]

And then at line 31 it call T0300. This turns off the offset correct?
I was making 4 each of this part. After it cut off the first part, I would move the tool to Z0 and set the stock to that length, then run the program again. This didn't work because it the machine was at offset for T0. So the work around was to MDI back to T0303, then move to Z0, set the stock and run the program. This is all very confusing. Intercon should not call T0300 at any time in this program unless I have set something up wrong.

[Chaz]

Its done by Line 31, the parting Op is the section above.

It will always do the correct offset within the Operation.

Its normal behaviour, nothing wrong but its a bit different. Z remains consistent, just set your part back to a known good location to start from.

[suntravel]

If you set parameter #3 to 8, Intecon will not cancel the offset at the end of the g-code

Why not doing 4 cut off cycles in intercon?

Anyway you can set part zero with any tool if they are setup ok, regardless if the tool offset is active or not.

You can also use MDI for T0303 to make the offset active again.

Uwe

[Chaz]

Thanks for the parameter tip.

[suntravel]

Yeah, the manual is always a good source of information...

[cncsnw]

Starting the tool with no offsets; then activating the offsets just before the first cut; then cancelling the offset when the cycle is finished, is long-standing tradition in CNC programming. Centroid was trying to be consistent with prevailing practice.

That has not really been necessary for decades, probably not even on Fanuc controls. Old habits and traditions die hard, though.