Haas fanuc-emulator G98/G99 subprog problem?

[MauserBob]

I have a head-scratcher here guys, and I hope someone can help me understand what's going on. First, background....

We're running a multiple-up part program with a hole pattern, and transforming it out in subprogram form...something we do all the time. We've got a variety of machines that we do this on...two Hardinge VMCs, two older Leadwells, and a Haas VF-3 which I have written about here before. The first four are true Fanuc while the Haas is the Fanuc emulator, IIUC. NOt sure if that makes a difference here because the g-code is the same between all the machines for all intents and purposes. We do create most of our programs as sub-prog based so that we can transform them out across the whole table for multiple-up cycles while reducing program size to save room in memory...been doing it this way for years and it's never been a problem. The only caveat here is that we do not often transform a hole-pattern as part of a program in the Haas all that often so we don't have many examples to go back and look at, as we do for the other machines. Most of the time hole-pattern xform progs wind up getting run any of the other machines...no rhyme or reason to that, it's just the way things go. So my other guy pulls up an old prog in Mcam this morning to update it, posts it to the machine and begins running, when, in the first subprogram, the drill sunk itself up to the collet-nut, which wasn't expected. We've been looking at this for 1/2 hr now and even ran it again in single-block to see if we could figure out why it's doing that but we just don't see anything out of the ordinary. I've posted the relevant bits of the prog here in hopes that someone with more Haas-based insight can see if the format we're running just isn't Haas fanuc-emulator friendly. First, the main body of the drill routine followed by the sub-prog itself.



T5M6
G0G90G54X6.4Y2.145S4200M3
M83
G43H5Z1.T2
M8
G98G81Z-.1R.25 F15.
Y4.725
X10.64
X14.86
X19.1
Y2.145
X14.86
X10.64
G80
X20.9
M97P7904
G90X6.4Y6.515
M97P7904
G90X20.9
M97P7904
G90X6.4Y10.885
M97P7904
G90X20.9
M97P7904
G90X6.4Y15.255
M97P7904
G90X20.9
M97P7904
M84



N7904
G91
G98G81Z-1.1R-.75 F15.
Y2.58
X4.24
X4.22
X4.24
Y-2.58
X-4.24
X-4.22
G80
M99


We saw no cumulative error or initial-plane height differences throughout the dry-run; everythign looked perfectly normal except that the drill in the sub just ran way too deep. We've really been wracking our brains trying to find the stack-up error but looking at the dist-to-go display and single-blocking it through, it just doesn't seem to be there so...anyone know what we're missing here? When I first saw the prog he created somethign struck me as "off", but I couldn't put my finger on it...and after dry-running I'm still stumped. Any help would be appreciated.

In other words,...is this a case of Haas controls not being particularly happy with transforming a canned-cycle like a hole pattern in a sub-program?

Thanks guys.

Rob.

[Machineit]

Put the G91 in the subprogram after the drill canned cycle. You are using it for incremental location I guess, but messes up the canned cycle. The first move in the cycle will be to move Z-.75 then drill Z-1.1 further, so the total depth will be 1.85.

The Haas does not need the G98 either.

Mike

[Machineit]

When using a sub cycle or program I always put a G90 to a safe plane at the end of the sub too. Just a safety thing.

Mike

[MauserBob]

Okay, I'll try moving the G91 to after the canned cycle call.


Meanwhile, when you say the Haas doesn't need the G98, do you mean just the G98 or both the G98 and the G99? I would not think that to be the case because how would it know the difference between the two concepts if you didn't specify one or the other? Does a Haas always operate drill cycles in a G98 method regardless of the programming?


Thank you again.


Rob.

[MauserBob]

When using a sub cycle or program I always put a G90 to a safe plane at the end of the sub too. Just a safety thing.

Mike

I hear ya, and I do too; this is my assistant's program...I just posted it as he wrote it.


Rob.

[Machineit]

Okay, I'll try moving the G91 to after the canned cycle call.


Meanwhile, when you say the Haas doesn't need the G98, do you mean just the G98 or both the G98 and the G99? I would not think that to be the case because how would it know the difference between the two concepts if you didn't specify one or the other? Does a Haas always operate drill cycles in a G98 method regardless of the programming?


Thank you again.


Rob.

The G98 returns the Z to the previous Z plane after the cycle, but you have none in this but the G43 Z1. etc, where it will go anyway.

Just leave it in in case you put any clamps in there to avoid them!!!!

Mike

[haastec]

Put the G91 in the subprogram after the drill canned cycle. You are using it for incremental location I guess, but messes up the canned cycle. The first move in the cycle will be to move Z-.75 then drill Z-1.1 further, so the total depth will be 1.875.

The Haas does not need the G98 either.

Mike

+1 on the G91 for the sub.