A question for Fanuc gurus

[gcode]

We just purchased a couple of HNK horizontal boring mills
The control is Fanuc 31i
The operators are complaining about something.

On our Ikegias ( Fanuc 16i) you could stop in the middle of a program,
change the tool length offset and keep going.
The machine would pick up the edited TLO on the next Z move.
On these new machines, you have to go back to the start of the toolpath and
read the G43 H** line

I'm guessing this behavior is controlled by a parameter.
Any idea which one it may be??

[JParis]

I'll leave the more complete answer to the "gurus" but I've always just set a G43 H** whenever I want to pick up a change...

[gcode]

I'll leave the more complete answer to the "gurus" but I've always just set a G43 H** whenever I want to pick up a change...

The operator has already tried this.
The control will not allow the edit as the program is live in memory

The part is a Ti aircraft bulkhead
The toolpath is a surfacing operation with a 3+ hour cycle time
I guess the guys could stop the toolpath, go to the start and read in the new TLO
then search for the correct N block to restart.
That is not an optimal solution for a $250k part.
We try to keep this part reserved for our most skilled and senior operators
but sometimes a younger guy has to step in.

On our old HBM, we had to DNC the file because it's too big for the control
We lost a part last year when the wireless DNC hickuped and drove a Ø1.25" button cutter through the part.
That was an expensive accident and a very awkward conversation with our vendor.
I'm an old school guy and in my book, wireless DNC in a building full of machines and electromagnetic
radiation is madness. We never determined a definitive cause for the crash but we did bag the wireless
DNC after that.

[JakeL]

I guess the guys could stop the toolpath, go to the start and read in the new TLO
then search for the correct N block to restart.

This is how we always get the H value if we need to start in the middle of a toolpath. If there is a parameter that controls this behavior then I'd love to hear about it because we'd use it.

I honestly didn't know there were controls that automatically pick up the H value on every Z move. I thought you needed the G43 to pick up an H value. Learned something new today.

Not sure if this would work, but for a workaround could you feed hold the machine, jump to MDI and execute a G43 H** then go back to the program and continue running from there? We do this sometimes for things like big spindle speed changes.

[JakeL]

Jake - be very careful if you're going to try this while running lookahead (G5000/G05/G08 etc) - although the control may show you at X, the reality is it's way down the road with already processed data....

Thanks for the heads up, we have run into this issue (G5.1 for us). We'll make a jump in the program and the machine will just revert back to the original line we were jumping from as soon as we hit cycle start. Almost like the machine has a mind of its own.

[mkd]

Been able to jump into mdi and back in a program on fanuc, since forever. Heidenhain too.
 There are some advanced tool calls that CNCappsguy has listed here and there. Good breadcrumbs to look deeper.

[MIL-TFP-41]

I think Fanuc has a "Program Restart" option that might be the ticket for what you are describing. I've always just restarted from the last toolchange - but I don't typically have a 3 hour cycle time on a tool.

[CNCAppsJames]

I'm in Hawaii... I know rough life.

I get back tomorrow night. I'll dig up the parameter. You are correct, that behavior is dictated by parameter.

[CNCAppsJames]

Ok there's a couple things in play; as some have alluded, Look-Ahead (also know as buffering) will play a part in when the next compensation move takes place.
That said the parameter to look at is 
#5001.4 (EVR) 

Bit 4 ... if 0 then it enables the change next block where H/D call. 
Bit 4... if 1 then it enables the change where buffering is next performed

This is for Tool Offset C.