Emco 325-II (Fanuc 21TB) live tool alarms

Need some help with my 325-II (Fanuc 21TB) if anyone's run in to this problem or has an idea.

Trying to use the live tools and I'm getting two alarms when I activate the M-codes.

Commands:

M52 (C-axis on)
G97 Sxxxx M13

As soon as the M13 (or M14) is called the live tool engages (I can hear the solenoid) and rotates 1/4 turn then it throws an alarm and the C-axis and live tool disengages.

Alarms:
8132 AXIS ACCESSED BY MULTIPLE CHANNELS
8203 FATAL AC ERROR (0-PTR IPO)

Both alarms are in the programming manual, but are cryptic:

Cause: Internal error
Remedy: Restart software or reinstall when necessary, report to EMCO, if repeatable

I've re-started WinNC, no luck. Happens in MDI and during normal program execution.

Live tools worked last year, but I haven't tried using them in about 10 months. No crashes or major problems/maintenance since they last worked.

Maybe the G-code syntax is wrong? The Emco manual is pretty terrible...

Anyone have suggestions?

Thanks,
Ralph

M5 before M52. I ran cross your post somewhere about tapping with live tools. I've only been successful with G33.

Quote:

---

Originally Posted by Diesel_Pilot

M5 before M52. I ran cross your post somewhere about tapping with live tools. I've only been successful with G33.

---

You're thinking this, right?

M5
M52
G97 S5000 M13

Doesn't make sense to me as it alarmed when I was using MDI one line at a time. The spindle wasn't running (in spindle mode), and I could do an M52 and then jog the C-axis just fine. It only threw up when I tried to engage the M13.

But Emco is insane and anything's possible.


After some serious searching, I found a single example in the Emco 21TB programming manual (ver C2003-7) on page D49
...
G90 G40 G95
T0909
M52
G28 G0 C0
M13
G97 S5000
...

I wonder if the order is the difference? i.e. M13 on a separate line before the S-word.

Thanks for the advice regardless of outcome. I'll have a go with both versions a bit later tonight.

-Ralph

Changing the g-code order and adding a pause did the trick.


M52 (C-axis on, also homes C-axis so no need for)
M13 (live tool CW)
G4 X1 (needed pause before the speed command. No pause = alarm)
G97 Sxxxx (spindle speed)

Subsequent speed changes or start/stop/reverse don't require a G4 pause as long as the M52 is active.

Now I've just got to try editing my post so it outputs correctly.

Thanks for the help Diesel_Pilot!