Problems with metric rigid tapping on 15M

I run a Mitsui Seiki HU63A, a 4-axis HMC with a Fanuc 15M control. Rigid tapping works great with standard thread pitches using G84.2, but it consistently screws up metric threads done the same way.

I don't even understand how the machine could possibly care whether the thread pitch is standard or metric, but it does. Small taps break unless they're in a floating holder, big taps make really bad, ugly threads. Once, using an M16x2 tap pretty far from the center of the pallet, the machine threw a B axis overload alarm (it does that if I'm using a big drill too far off center and forget the M10 to lock the B axis). So it does get fairly close to the right feed, and it certainly acts like it's rigid tapping, it just gets it wrong by a bit.

Sample code for M16x2 tap:
G84.2 R.1 Z-1.25 S127 F10.0

Working code for 3/4-10 tap:
G84.2 R.1 Z-1.25 S130 F13.0

This makes no sense to me. Any ideas?

Is it possible that the machine is assuming I meant to do a standard thread and doing some misguided rounding? I really hope somebody knows what's going on here so I can stop tapping 16mm holes by hand...

Values are ok.
Is the metric tap, by any chance, a fine-pitch tap? (measure to confirm that the pitch is 2 mm)

Yes, it's the right tap, and I've seen this issue with several other taps with different pitches in different materials. Inch pitches work very well, metric pitches consistently go awry, everything from M6x1 to M20x2.5.

Quote:

---

Originally Posted by mysticofjesus

Sample code for M16x2 tap:
G84.2 R.1 Z-1.25 S127 F10.0

Working code for 3/4-10 tap:
G84.2 R.1 Z-1.25 S130 F13.0

Any ideas?

---

What material ?
What type of taps ? spiral or gun
Thru or blind holes ?
Depth of thread ?
Coolant or cutting oil ?

Me.....I work with G95 ( Feed per rev )....set S to the recommended cutting speed, set F to the thread pitch
- then set back to G94 after tapping ( G94 is always stated after each tool by default )

found this link
- it is saying G84.2 is a one shot code to enable rigid tapping, where G84.1 is the actual code in the NC file

Looks like it is a parameter issue when you try to rigid tap a metric thread in inch mode. Whenever I have time, I would study this cycle in more detail. Meanwhile, please check if you get the correct metric threads in mm mode, G21.

Quote:

---

Originally Posted by Superman

What material ?
What type of taps ? spiral or gun
Thru or blind holes ?
Depth of thread ?
Coolant or cutting oil ?

---

1: HRS, CRS, 4140, Aluminum.
2: All of the above, mostly Widia gun taps, though it does the same thing with an Emuge spiral flute.
3: All of the above.
4: Which thread? With the taps that don't fit in my floating holders (ie. 16mm and up) the threads start getting mucked up if I try to get more than about .2" of full threads. What I've been doing is tapping deep enough to give me two full threads or so, just enough to guide a hand-held tap, then I tap most of the way by hand once it's off the machine. (I make mostly workholding fixtures for the machinery and firearms industries, so this is about the farthest thing from production work.)
5: Moly-dee.

I think I've pretty much ruled out anything mechanical or tooling-related, since inch taps under the same conditions work every time. It has to be a control/parameter issue, which means it's a bit out of my area of expertise.

Quote:

---

Originally Posted by sinha_nsit

Looks like it is a parameter issue when you try to rigid tap a metric thread in inch mode. Whenever I have time, I would study this cycle in more detail. Meanwhile, please check if you get the correct metric threads in mm mode, G21.

---

That is a good idea, trying metric mode. I don't think I've ever used a G21 on this machine before, since all our prints and the cam software are in inches. I'll try that out when I get the chance.

I am more or less convinced that the problem is because of floating point error in unit conversion. While such a small error would be insignificant in most cases, this may not be true in the case of rigid tapping where even a small axial mismatch may result in a lot of axial stress. The solution, therefore, is to make matric threads in matric mode.
It is just my guess. Please do revert back with your results. There is something to learn.

i think that sinha_nsit may be on to the correct idea that there is a rounding issue maybe with the spindle. my guess would be with the spindle at 127 rpm and it is rounding up/down where the 130 rpm is not being rounded. try an even rpm like 110 rpm and 8.6614 feed rate

As it turns out, metric rigid tapping does work very well in metric mode (G21). It's a bit of a pain to rework the programs and offsets, but I guess I can live with that for the few jobs I get with multiple large, metric, tapped holes.

In inch mode, I've tried using round numbers for RPM before, and it didn't seem to make a difference.

Thanks for the help guys, you've selflessly saved me an awful lot of time turning tap wrenches.

We all learnt something new!