Tapping

[wbleeker]

I have a job that requires a series of 4/40 tapped holes as well as a series of 6/32 tapped holes, they are through holes as well the material is 6061 al 6mm thick, I will use two ER16 tension compression tapping heads, as the job is metric dimensioned I will change the tap to metric pitch for the conversational program, I'm just wondering if anyone has any guidelines as to feed speed and dwell time? That they know will work!
Will

Similar Threads:

• Solved Tapping with Torus Pro and Reversable Tapping Head
• tapping on a mini mill without rigid tapping???
• Tapping with the Tormach Tapping Head
• Rigid tapping or tapping head
• tapping head vs hand/cordless tapping machine....

[frankee]

Hi,
The most important consideration with the tension/compression tapping head is the length of time that it takes the spindle to stop and reverse. If you are drilling through holes you have some chance of it working, otherwise in my experience, having run a series one machine for (must be) 10 years, you may find that it's faster and cheaper to tap the holes with a good electric drill: good luck though.

Sent from my XT1064 using Tapatalk

[oneineight]

For the 6-32 0r 4-40,
4- 40, 40 revolutions for 1 inch of feed so a speed of 40 rpm and 1 inch per minute feed would be right for the tap.
But your machine does not run at 40 rpm, so multiply both 40 rpm and 1 inch per minute by the same number to give you a speed and feed you can use. 40X20= 800 speed 1x20= 20 feed.
I have not used dwell in tapping, and do not think it is recommended.

[GLCarlson]

I have a job that requires a series of 4/40 tapped holes as well as a series of 6/32 tapped holes I will use two ER16 tension compression tapping heads, as the job is metric dimensioned I will change the tip to metric pitch for the conversational program, I'm just wondering if anyone has any guidelines as to feed speed and dwell time? That they know will work!
Will

Feed and rpm are proportional when tapping with the t/c head. Pick an rpm (low range, say 200 but choose something that is a multiple of your tpi). So for a 20 tpi thread, 200 rpm with an advance of 0.05/rotation = 10 (200x0.05) ipm feed. The t/c head has a built in "dwell managemen"- that is, when you hit the depth programmed, your code should stop and reverse the head. What you'll see, in practice, is that the head will compress and then release. That spring action takes care of the time needed to reverse, so no dwell needs to be programmed. If you're running PathPilot, the conversational routine works just fine for taps (threadmilling is another matter).

I typically try to stay in the 250-500 rpm range, and adjust feed to match. So far, that's worked just fine. I think I'm too conservative; in aluminum at least, I'm confident I could run at least twice that with anything bigger than 6-32.

If you poke around the forum, you'll find several discussions about tapping. You're well within normal parameters.

One key point. The speed DRO reads out commanded speed. It's a really good idea to know actual speeds, as Tormach can vary 10% (at least) up or down. Either do the adjustment (there's a service bulletin) or just use an optical tach to build a calibration curve (in PP, there's also a way to add the calibration curve to your system, see the thread on that). The t/c head will compensate some, but too far out will break taps as feed gets further out of sync with tpi.

Also consider what taps you are using. Tormach sells several styles, and they differ for thru hole tapping vs blind hole. What you don't want to do is use cheap "hardware store" grade, hand taps. You didn't state a material, but that will also influence speeds/feeds. Don't forget tapping fluid. A-9 for aluminum if you can find it, and for steel I still use chlorosulfonated threading oil.

[IMT]

I have done quite a bit of tapping on my series 3 machine. I use the ER20 T/C tapping head. For 4-40 and 6-32, 8-32, 10-32 I feed it at 10ipm and set the rpm accordingly, 400 for the 4-40 and 320 for the x-32. I set the dwell time to 0.3. The spindle stops very quickly from 300-400 rpm and still has enough torque for smaller taps, I haven't tried anything over 5/16-24 in aluminum. I use the electra coated spiral flute taps from OSG and CoolTool II tapping fluid. I've tapped 416SST, 303SST, 6061, 2024, 7075, 12L4 and O2 with the same settings.
I also adjusted my spindle drive to be accurate at 400 rpm, measured with a optical tachometer.

[wbleeker]

Thanks for the replies, I've edited my original post to include material details etc. I am waiting for some new taps to turn up as this size isn't common here in Australia but will order a supply off Tormach as well.
Will

[C*H*U*D]

I tap a lot of M3 holes, and since I hate changing the belt I to do it at 525 rpm with no problems. I also use the T/C head and do it on my 770. The small diameter is not affected by the low torque. Use spiral point for through hole and spiral flute for blind and make sure it's a quality tap.

[Steve Seebold]

I do a lot of tapping on my PCNC 1100 and I have yet to break a tap.

I run my taps at 500 RPM and I use flood coolant.

I go in at 10% slower than the calculated feed rate, and come out 10% faster.

I'm using an ER16 tension/compression tapping head.

Here's the way I do it:

6-32 thread

S500M3

G0G90 and all that stuff, X? Y? Z1.

Z.25

G1Z- (depth) F14.0625

M4

G4 P.25

G1Z.25F17.1875

(Copy This)

Move to next hole

Paste

And so on.

For 4-40 thread

Same start up as 6-32 but feed rate 11.25 in and 13.75 out.

My machine is now 5 1/2 years one and I have been tapping this way for over 4 years.

Any questions, you can call me at 714-420-2453 any time after 9:00 AM and before 8:00 PM.

[IMT]

Steve,
What is the logic behind increasing the feedrate when retracting, even though the spindle speed is not changed? I have heard of doing this on the clutch type tapping heads but not T/C.
BTW, Tormach's examples in the T/C head instruction sheet has the feed in and out the same.

[wbleeker]

Thanks for all the replies, I have it working fine now, I calibrated the spindle speed and got rid of the dwell.
Will