Trouble rigid tapping with FANUC 21-TB 2-axis lathe

I am trying to use rigid tapping on my EMCO Turn 325. It has a FANUC 21-TB control.

The manual for the machine says it does have rigid tapping (G84) and I can either set up parameter 5200, "bit 0" as a "0" and use a M29Sxxxx command prior to the G84 command or set "bit 0" to "1", do not use a M29, and have G84 as a default rigid tapping cycle.

When I try either, I get the same result; the spindle turns at the commanded tapping speed, then attempts to stop at position, but slowly rotates back and forth for a few seconds and the control throws a time out error.

Here is a simple program with "bit 0" set to 1 allowing G84 to function as a rigid tapping cycle:


(TAP 1-72)
N14 T0808
N15 G54
N16 M8
N17 G98
N18 M5
N19 M20
N20 G97 S1000 M3
N21 G0 X0. Z0.15
N23 G84 X0. Z-0.125 R0.15 P0 F13.88889
N24 G80
N25 Z0.15

I have not had any problems with the machine otherwise and it does external threads fine, so I would imagine the spindle / encoder are fine.

Any help is appreciated.

jj80909 said:

I am trying to use rigid tapping on my EMCO Turn 325. It has a FANUC 21-TB control.

The manual for the machine says it does have rigid tapping (G84) and I can either set up parameter 5200, "bit 0" as a "0" and use a M29Sxxxx command prior to the G84 command or set "bit 0" to "1", do not use a M29, and have G84 as a default rigid tapping cycle.

When I try either, I get the same result; the spindle turns at the commanded tapping speed, then attempts to stop at position, but slowly rotates back and forth for a few seconds and the control throws a time out error.

Here is a simple program with "bit 0" set to 1 allowing G84 to function as a rigid tapping cycle:


(TAP 1-72)
N14 T0808
N15 G54
N16 M8
N17 G98
N18 M5
N19 M20
N20 G97 S1000 M3
N21 G0 X0. Z0.15
N23 G84 X0. Z-0.125 R0.15 P0 F13.88889
N24 G80
N25 Z0.15

I have not had any problems with the machine otherwise and it does external threads fine, so I would imagine the spindle / encoder are fine.

Any help is appreciated.

Click to expand...

Hello jj80909,
Many will not agree, as they have not in the past, but my Japanese Fanuc Colleagues are adamant that the correct method for turning the Spindle on is via the actual rigid tapping cycle and that the immediate previous use of the spindle, for drilling the tapping hole for example, should be stopped with M05 prior to the Rigid Tapping exercise. Having said this, it is to some degree MTB dependent, but normally, having the Rigid Tap Cycle start the spindle will work irrespective.

Just for the purpose of testing, try the following:

1. Set parameter bit 5200.0 and parameter 5210 to Zero
2. Run the following program

N14 T0808
N15 G54
N16 M8
N17 G99
N18 M5
N19 M20
N20 G0 X0. Z0.15
N21 M29 S1000
N23 G84 Z-0.125 R0.15 F0.01389
N24 G80
N25 Z0.15

It will not be the cause your issue, but with all the lathes with rigid tapping via the Main Spindle (not live tooling), I've encountered, the max spindle speed is 1000rpm. This is due to the considerable inertia at play with even a relatively small Main Spindle Chuck.

A rule of thumb, if the Lathe truly has Rigid Tapping on the Main Spindle, M19 will work to orientate the spindle irrespective of whether the machine has a "C" axis and live tools or not. This is also MTB dependent, but is normally the case.

Regards,

Bill

Just because the manual describes how to do rigid tapping it does not mean your machine has the option.
And the program sample you posted you said it was with bit "0" set to 1 which means M29 should not be used.

Anyway, if you can't do rigid tapping and have to use a floating tap holder then this is what you should try

G54
T808
M8
G99 (stop using G98 on a lathe)
G97 S150 M3 (yes, 150rpm)
G0 X0 Z.15
G33 Z-.125 F0.01389
M05
Z.15 M4
G0 Z.5
G28 U0 W0
M01

Many fanuc dosent use g80s cycles aswell. I ridget tap by reversing the spindel with m04. Never had problems with it and I've made small and big threads in all materials.

Sendt fra min EML-L29 med Tapatalk

angelw

I tried your program:

N14 T0808
N15 G54
N16 M8
N17 G99
N18 M5
N19 M20
N20 G0 X0. Z0.15
N21 M29 S1000
N23 G84 Z-0.125 R0.15 F0.01389
N24 G80
N25 Z0.15

The program stops at line N21 and times out without starting the spindle.

As for the other suggestions, I don't have a floating tap holder that will fit in this tiny lathe and I'd like to take advantage of rigid tapping if I can.

jj80909 said:

angelw

I tried your program:

N14 T0808
N15 G54
N16 M8
N17 G99
N18 M5
N19 M20
N20 G0 X0. Z0.15
N21 M29 S1000
N23 G84 Z-0.125 R0.15 F0.01389
N24 G80
N25 Z0.15

The program stops at line N21 and times out without starting the spindle.

As for the other suggestions, I don't have a floating tap holder that will fit in this tiny lathe and I'd like to take advantage of rigid tapping if I can.

Click to expand...

Hello jj80909,
Again with Parameter Bit 5200.0 set to Zero, run the following program (M29 Block Omitted):

N14 T0808
N15 G54
N16 M8
N17 G99
N18 M5
N19 M20
N20 G97 S1000 M03
N21 G0 X0. Z0.15
N22 G84 Z-0.125 R0.15 F0.01389
N23 G80
N24 Z0.15

If the above program runs, your machine doesn't have Rigid Tapping. Its common for a 2 axis lathe, without live tooling, not to have the G84 Canned Cycle. If a ps10 alarm is raised when attempting to run the above program, your control is not equipped with G84.

Regards,

Bill

Hey Bill, I got it working. You only missed it by this much (M3).

I had to add a M3 to the end of the G84 command. I doesn't make that much sense to me as it's a right-hand tapping cycle

N14 T0808
N15 G54
N16 M8
N17 G99
N18 M5
N19 M20
N20 G97 S1000 M03
N21 G0 X0. Z0.15
N22 G84 Z-0.125 R0.15 F0.01389 M3
N23 G80
N24 Z0.15

Thanks for the help!

Was the manual you were using a Fanuc manual or an Emco manual? Needing the M3 on the G84 line has to do with how the machine builder's ladder logic is written, not a requirement of the Fanuc control. If you were using an Emco manual, I'm a bit surprised that the M3 was not shown to be required on the G84 line.

jj80909 said:

Hey Bill, I got it working. You only missed it by this much (M3).

I had to add a M3 to the end of the G84 command. I doesn't make that much sense to me as it's a right-hand tapping cycle

N14 T0808
N15 G54
N16 M8
N17 G99
N18 M5
N19 M20
N20 G97 S1000 M03
N21 G0 X0. Z0.15
N22 G84 Z-0.125 R0.15 F0.01389 M3
N23 G80
N24 Z0.15

Thanks for the help!

Click to expand...

Other than the M3, what in your code is determining that it is RH?



----------------------------

Think Snow Eh!
Ox

jj80909 said:

Hey Bill, I got it working. You only missed it by this much (M3).

I had to add a M3 to the end of the G84 command. I doesn't make that much sense to me as it's a right-hand tapping cycle

N14 T0808
N15 G54
N16 M8
N17 G99
N18 M5
N19 M20
N20 G97 S1000 M03
N21 G0 X0. Z0.15
N22 G84 Z-0.125 R0.15 F0.01389 M3
N23 G80
N24 Z0.15

Thanks for the help!

Click to expand...

Hello jj80909,
Are you saying that the above gave you proper Rigid Tapping, with the assumption being that Parameter Bit 5200.0 is set to "1".

Did the Spindle start with:

N20 G97 S1000 M03

then stop, synchronize and start again with:

N22 G84 Z-0.125 R0.15 F0.01389 M3


Regards,

Bill