4-digit feedrate on A Axis?

[ghyman]

We have recently purchased a YCM - TV158 Vertical machining center with a Fanuc MXP-200i (18-i) control.
The parts we are machining are actually larger than the machining envelope of the machine (Ø43"), so we have mounted a rotary table to the machine, and use the A-axis to generate several diameters on the parts, by positioning the tool to a fixed position, then rotating the part.
This works fine on four machines that we have here.

- however -

We are experimenting with some new tooling, and have reached a threshold of sorts...
The A axis is programmed in degrees per minute, which in and of itself is not a problem.
The problem is, as we find better and faster tooling, we are not able to program the table to rotate fast enough to give us a decent chip load.
The fastest we can program is F999.9999, which the table is capable of doing.
We can crank the override on the machine up to 200%, and the table will go right up to F1999.9998.
We know that the table is capable of considerably faster than this, but the problem we have is that the control will not allow a feedrate faster than the 3.4-digit format.
I have tried math lines, variables, and any other trick I can think of, but the control will not accept anything faster than 999.9999
(For those of you wondering, we would like to get up around 4100 degrees per minute.)
The supplier has not been able to help us on this; I have not found the right person to explain this to... it is not a question of the table's capability, it is an issue with the control accepting a 4-digit feedrate.

Is there anyone out there who knows a good way to do this? (Or for that matter, even a bad way that works right?!?!)

Thx

[beege]

Look in your manual to see if you have inverse time (G94?) feedrate.
Calculate the length of time needed to complete the cut.

Divide it into one. (1/t)
A feed of F.5 means it should take 2 seconds to complete (1/2)
A feed of F.02 means it should take 50 seconds to complete (1/50)

So let's see...

A cut at 3" from center, moving 360° all together, at 15 IPM....
6 X Pi = about 18.5" circumference
18.5 IN /15 IPM = 1.256 minutes, or 75.36 seconds
Invert that, 1/75.36 = .0651
So you'd program G94 F.0651

The feedrate you're currently using is in degrees per minute, and usually, there's a parameter that clamps cutting feedrate on the rotary axis. But your problem seems to be the command format of 3.4.I don't know how to overcome that. Someone more familiar with the Fanuc system might be able to help there.

Inverse time bypasses that clamped speed entirely, and hopefully doesn't exceed the rapid for the table ( never had an instance of that myself... )

[ghyman]

This would work if it was the tool that was moving around the table rather that the table rotating while the tool stays stationary.
But, as it is, all A axis feed commands are interpreted as Degrees of Rotation per minute regardless of the tool's (X/Y/Z) feedrate mode.

[HuFlungDung]

What is the rotary table's rapid rate? Can you run it at full rapid, or a percentage thereof?

I'm not sure about the inverse time thing. I don't believe it is tied to a linear movement occurring simultaneously. But you do have to turn it on/off with a gcode to get the new interpretation of the A feedrate.

[ghyman]

Sorry... should've been more specific... Our A-Axis rotation is not affected by G94/G95, only the actual tool feedrate in X/Y/Z. (We tried!)
Rotary table rapid travel is somewhere around 30 RPM, and we have considered capping that and just using a G0 A command, but we have a number of different tools that we are using on this part... Rough mill, Finish mill, form mill, slotting cutter... and each one has its own chipload requirements.

[beege]

G93 did work for me once, especially using the rotary axis with no movement in X,Y or Z (only had to use it once). Did you actually try it? I'm not trying to start an argument here, just trying to understand the difference between your experience and mine...

Sorry, G93 is supposed to be inverse time...been a while.

Soooo...... try G93?

Oh, and feedrates in G93 are not modal, so you have to program every move's feedrate.

[jamesweed]

on out oi-mc we had a parameter change to increase DPM feed beyond F999.9999. actually our problem was if we set feedrate with varaible... F#100, then 999.9999 was it. After parameter change #100=7920 is top for us. Check your parameters.