Rigid tapping help

[Genguy]

I can't get rigid tapping to work properly on an Oi mate-c.
The problem is that after the tapping is complete, the machine hangs/stops and won't process any more blocks of code.
It will complete all 4 of the hole locations perfectly then just hangs up.
When it does this, I can hear the spindle motor making a slightly different sound than usual. I assume this is because of the M29.
It's like it won't cancel the M29.
I modified the code output by gibbs to get rigid tapping working in the first place.
I need to get a working sample so we can get our post processor file modified.

Any idea what I did wrong?

G54 S458M3 G90G0X28.575Y15.875 G43Z25.H9 M8 Z5. G94 M29S458 G84G99X28.575Y15.875Z-30.R5.F727.08 Y-15.875 X-28.575 Y15.875 G80G95 G0Z5. M9 G91G28Z0. M5 M30 %

[HuFlungDung]

Do you need the M3 and M5? Most machines start, stop, reverse and stop the spindle within the G84 logic.

I'm not sure about the G94 and G95 either. If needed, you might try putting the G95 on a line by itself after the G80. I've never used those codes except on a lathe for changing from synchronous feed to asynchronous.

Is M29 for gear shift override?

[cnc-king]

M29 orients the spindle, are you sure you don't need a M80 instead of a M29
you are not unlocking the spindle afterwards, i know the older fanucs require a M80 to initiate rigid tapping, I will post a tapping cycle from the older machines when i go to work in the am

[Genguy]

Thanks for the replies, I really appreciate your help.

Originally Posted by HuFlungDung Do you need the M3 and M5? Most machines start, stop, reverse and stop the spindle within the G84 logic.

Possibly not, I have not tried it without.

Is M29 for gear shift override?

The manual says M29 syncronizes the feed with the spindle rotation.
I guess I should have mentioned it's on a 3 axis vertical mill.

Originally Posted by cnc-king M29 orients the spindle, are you sure you don't need a M80 instead of a M29 you are not unlocking the spindle afterwards, i know the older fanucs require a M80 to initiate rigid tapping, I will post a tapping cycle from the older machines when i go to work in the am

The Fanuc manual also says the M29 is cancelled by any feed command such as G01 G00.

Tommorow I'll try to move the codes around and also try an M80 instead of M29 like you guys have suggested.

I'll scan that page of the manual and post it up as well. I have probably overlooked something.

[Ozemale6t9]

Put in a speed/direction after the G80 line. Eg. S500 M3

The manual should tell you this. BTW, M29 is correct for rigid tapping. If you use G84 without commanding M29 first, you need to use a floating tap holder, as the spindle and feed are not synchronised.

regards, Oz

[psychomill]

I'd like to know what you're cutting at a feed of F727.08 @ 458rpm??

[Genguy]

Originally Posted by psychomill I'd like to know what you're cutting at a feed of F727.08 @ 458rpm??

That is what Gibbs came up with based on the thread pitch and rpm I entered. I let Gibbs recalculate the feed and rpm.The threads turned out fine, so I didn't mess with the settings. It was a 3/8" tap in 6061.

Originally Posted by Ozemale6t9 If you use G84 without commanding M29 first, you need to use a floating tap holder

Gibbs does exactly that (with the post I am using). Rigid shredding was the result.

I'm going to try all of the suggestions tonight.

[Ozemale6t9]

Must have overlooked the feedrate...usually rigid tapping is programmed as thread lead(pitch).

regards, Oz

[psychomill]

You need to fix a few settings with your Gibbs. If you're tapping in G95 (IPR), then for a 3/8 tap (assuming its say a 3/8-16), your feed should only be F.0625 . Even as a programmed feed in IPM, at 458 rpm, your feed would still only be F28.625 .

Something else I see is you're calling G95 at the end of the tap cycle with G80. You should get rid of the G95. Machine might be hanging up because you're placing it into IPR mode....

Just a thought...

[Ozemale6t9]

Originally Posted by psychomill You need to fix a few settings with your Gibbs. If you're tapping in G95 (IPR), then for a 3/8 tap (assuming its say a 3/8-16), your feed should only be F.0625 . Even as a programmed feed in IPM, at 458 rpm, your feed would still only be F28.625 . Something else I see is you're calling G95 at the end of the tap cycle with G80. You should get rid of the G95. Machine might be hanging up because you're placing it into IPR mode.... Just a thought...

Feed per minute rate is spot on if the program is metric, which I assume it is because the tap would be going 55 inches if it is imperial (big machine). All the fanucs I deal with rigid tap in feed/rev mode, but the machine puts itself in that mode and goes back to feed/min mode upon G80.

regards, Oz

[psychomill]

I thought of metric after my post and saw that he's in Canada....

but the machine puts itself in that mode and goes back to feed/min mode upon G80.

I've never come across a FANUC parameter that controls that. Do you know? and for what version? I've seen FANUC based machines with a machine builder add-on on top of it that had parameters for it, just never on a FANUC stand-alone....

[Genguy]

I finally got a chance to play with this again today.
I re-read the rigid tapping page in the programming manual and at the very bottom it says "Specify G84 for rigid tapping (parameter G84 No. 5200 #0 set to 1)".
Since I have never messed with the parameters on this machine before I took a look at the parameter manual. The explanation for that bit is opposite of what the operators manual says.
So I figured I would try that first and set bit 0 of parameter 5200 to 1 and give it another try.

% ( OUTPUT IN ABSOLUTE MILLIMETERS ) ( PARTS PROGRAMMED: 1 ) ( FIRST TOOL NOT IN SPINDLE ) N5G17G40G80 N10T2 N15M6 ( OPERATION 2: HOLES ) ( WORKGROUP ) ( TOOL 2: 6. RIGID TAP ) N20G54 N25S1200M3 N30G90G0X12.7Y0. N35G43Z25.H2 N40M8 N45Z5. N50G84G99X12.7Y0.Z-15.R5.F1200. N55X-12.7 N60G80G0Z5. N65M9 N70G91G28Z0. N75M5 N80M30 %

That was an M6x1 in a fir 2x4, or maybe hemlock, not sure.

Low and behold G84 works fine now without the M29. Woo Hoo progress!
It still stalls at the R position after the last hole though.
So next I tried moving the G28 up.
N60G80G28G91X0Y0Z0
This was shown as an example in the manual under canned cycle cancel.
No change, same stall.

This time I left the program running in auto and tried some diagnostics.
On the screen that shows the active G&M codes the only one I noticed that changes when I reset the program is G26. The manual says G26 is "Spindle speed fluctuation detection on".
That is as far as I got for today.