error 200 in rigid tap

[ianD01]

I'm trying to tap for the first time on a lathe using fanuc-OT controls with a G32 and I keep getting an error 200: S value is out of the range or is not specified. I tried entering speeds from 100 to 4000(not that I'd actually tap that fast) and keep getting the same alarm. Any ideas?

[underthetire]

Is it a live tool machine? Most lathes don't have ridged tap unless they have live tools, and especially on a 0T.

[angelw]

I'm trying to tap for the first time on a lathe using fanuc-OT controls with a G32 and I keep getting an error 200: S value is out of the range or is not specified. I tried entering speeds from 100 to 4000(not that I'd actually tap that fast) and keep getting the same alarm. Any ideas?

G32 is not used for rigid tapping. It does synchronize the feed with the spindle, but only when the spindle and feed is constant. When the slide decelerates at the end of the tapping feed the spindle and slides will not be in synch.

Rigid tapping is an optional function, and is called with G63 M29 S???? preceding the G84 tapping cycle with the "O" series control. Any motion commands such as G0 or G1 between M29 and the tapping cycle call will result in an error. G63 sets tapping mode and G64 sets cutting mode. If you still have the Fanuc specification sheet for the control, it will list Rigid Tapping if the control has it. Alternatively, try programming the above G and M code in a test program. If you get an error when the code is executed, then your control will not have the option.

Regards,

Bill

[sinha_nsit]

Use G97, constant rpm mode.

Bill,
Cann't we tap / rigid-tap without G63?

[angelw]

Use G97, constant rpm mode.

Bill,
Cann't we tap / rigid-tap without G63?

Hi Sinha,
I don't believe so. But its more the M29 that's important; that turns rigid tapping on and invokes the synchronization of the spindle and slide. In late controls one only needs to program M29, but with an early "O" series I had some involvement with recently, G63 had to be programmed before the M29, otherwise an error would result.

The G32 that the OP was trying to use is a threading G code and would be subject to the same lead error due to acceleration/deceleration, whether being used when thread cutting with a single point tool, or with a tap. I've often used G32 instead of G01 when deep hole drilling with an Ejector Drill system, where it was critical that the feed should not be varied with the feed override switch. But in tapping the spindle rotational direction needs to be reversed at the end of the tapped hole, and so you would have both deceleration and acceleration, in that order, at work at the end of the tapped hole. I think that would end in a mess.

Regards,

Bill