1. ## Learning How To Use A TC Tapping Head

My TC tapping head just came in yesterday and I've been doing a little reading trying to figure out how to use it. I see there's a math to the timing and was curious if anyone here made a list with speeds, feeds, etc. (if not lets make one ?

My first hole I need to tap is a blind hole in 6061 aluminum at .25" depth. I've bought a bottom spiral tap as recommended and if anyone here can take a look at the math to make sure it's correct.

Using a #36 drill (diameter of .01065) and a 6-32 bottom spiral tap.

6-32 - at 200 rpms @ 64 IPM

Math

32 tpi (.32) x 200 rpms = 64 IPM ?

Now I understand the PCNC 1100 Z axis maxes out at 65 IPM, so I'm limited to smaller tapping sizes.

Tormachs Example -

1/4 - 20 tap - 500 rpms @ 25 IPM

(Tapping with TC head for 1/4 - 20)

G0Z1 - (Rapid motion to plane z=1)
X0Y0 - (Rapid motion to hole center location)
Z.150 - (Rapid motion to plane z=.150)
M3s400M8 - (Spindle on CW, 400 rpm, Coolant On
g4 p4 - (Dwell for 4 seconds)
g1z-.9 f25 - (Feed tap to z= -.9 and 25 ipm)
m4s400 - (Spindle on CCW, 400 rpm)
g4 p0.5 - (Dwell for 0.5 seconds
g1 z.150 - (Retract tap to z=.150)

2. I bought from ENCO and know they sell ok stuff, but this round is just for testing. If I go into production, what taps would you recommend ?

3. Don't you divide rpm by number of threads per inch to get inches/minute!

If so then 200/32 = 6.25 inches/minute

Phil

Originally Posted by twocik
My TC tapping head just came in yesterday and I've been doing a little reading trying to figure out how to use it. I see there's a math to the timing and was curious if anyone here made a list with speeds, feeds, etc. (if not lets make one ?

My first hole I need to tap is a blind hole in 6061 aluminum at .25" depth. I've bought a bottom spiral tap as recommended and if anyone here can take a look at the math to make sure it's correct.

Using a #36 drill (diameter of .01065) and a 6-32 bottom spiral tap.

6-32 - at 200 rpms @ 64 IPM

Math

32 tpi (.32) x 200 rpms = 64 IPM ?

Now I understand the PCNC 1100 Z axis maxes out at 65 IPM, so I'm limited to smaller tapping sizes.

Tormachs Example -

1/4 - 20 tap - 500 rpms @ 25 IPM

(Tapping with TC head for 1/4 - 20)

G0Z1 - (Rapid motion to plane z=1)
X0Y0 - (Rapid motion to hole center location)
Z.150 - (Rapid motion to plane z=.150)
M3s400M8 - (Spindle on CW, 400 rpm, Coolant On
g4 p4 - (Dwell for 4 seconds)
g1z-.9 f25 - (Feed tap to z= -.9 and 25 ipm)
m4s400 - (Spindle on CCW, 400 rpm)
g4 p0.5 - (Dwell for 0.5 seconds
g1 z.150 - (Retract tap to z=.150)

4. You know Phil I might have read it wrong, that looks much better than what I had, can anyone confirm this math ?

6-32 - 200 rpms / 32 tpi = 6.25 IPM Plunge rate

Does anyone know how do you determine the correct RPMs or is this whatever you feel comfortable with ?

.

5. The slow feeds and spindle rpm are one of the reasons why I never use my T/C tapping heads. For example I have tapped tens of thousands of 4-40 blind holes. I prefer to use my Procunier 1E tapping head as it is run at 1200 rpm, 30 ipm downfeed, 60 ipm up feed. No dwell. I only use two lines of code:
G1 F30 Z-0.25 followed by G1 F60 Z0.1 The T/C head requires really slow speeds and feeds in blind holes because the spindle just can't stop fast enough. BTW in aluminum a Balax form tap works really well for blind holes as there are no chips.

Don

6. Yea I can see that, wow your setup does move along pretty quick.. Well luckily I'm not making cheese plates and only need a few taps here and there.

How much was your tapping setup ?

What would a Balax tap like that cost ?

Last, does our math look right on the 6-32 hole for the TC tapping head ?

.

7. Twocik:

If I want to tap just one or two holes I use a Fisher micro tap guide http://www.cartertools.com/fmpdtg.html and T handle tap holder and just do the tapping by hand as shown here: http://i72.photobucket.com/albums/i1...tap-holder.jpg Note yet another 5C collet chuck use this time on my Tormach 8" rotary table.

Cost is that of a Procunier 1E tapping head and TTS ½” holder. Basically I used a standard Procunier 1E tapping head that I have had for ten years and added a ½” TTS set screw holder to it. Cost of Balax 4-40 BH5 EDP#10725-000 form taps is ~\$12 each. The bracket that holds the anti-rotation rod was made with the Tormach from aluminum plate. See: http://i72.photobucket.com/albums/i1...rmUnderVie.jpg
Here is a video of tapping two 6-32 blind holes using a Balax 6-32 form tap.
http://s72.photobucket.com/albums/i1...t=100_3184.flv

I added the Pro-Quick quick change spindle on the 1E tapping head a few years ago that allows me to have a quick change holder for each of my taps. That way I enter each tap height in the Mach III tool table. see; http://i72.photobucket.com/albums/i1...erQuickPro.jpg

BTW I don't use my T/C tapping head set so couldn't say if the math is right. Anyone interested in a barely used Tormach T/C tapping head kit P/N 31163?

Don

8. Wow that's a pretty thick piece of bar stock. Looks like you've spent some time putting that together. I'd probably hand tap myself, but I'm absolutely horrible at it. I've looked at tapmatic and the tapping arm machines.

I thought they would have been more than that, at \$12 that's not bad at all. I was looking at a few on MC masters close to \$35 a piece. I bought a few cheaper taps normally at \$13 each for \$7 or so for testing, because I know I'm going to break a few learning this.

As for the math, phil was right. Found this site, really helpful

http://janproducts.com/Tap_Feed_Calculator.html

9. Originally Posted by twocik
Wow that's a pretty thick piece of bar stock. Looks like you've spent some time putting that together.
Not really. The split-clamp bar stock is 1" thick by 4” wide. The 3.375" diameter hole was trepanned quickly using a 1/2" end mill on the Tormach then finished to size with a boring head. http://i72.photobucket.com/albums/i1...blankFlynn.jpg The slot was hand cut on a bandsaw but could have been easily made using a slitting saw like this one http://i72.photobucket.com/albums/i1...TSblankSaw.jpg

The bracket I was really referring to was the bracket bolted to the Procunier as shown here: http://i72.photobucket.com/albums/i1...ierBracket.jpg This bracket was designed in Solidworks then the Gcode generated using SprutCAM. Isn't that what having a CNC mill is all about?

Originally Posted by twocik
I'd probably hand tap myself, but I'm absolutely horrible at it.
The Fisher micro tap guide makes it almost foolproof to hand tap and very much reduces the chance of breaking a tap.

Be aware that form taps such as the Balax threadflor use a different drill size than cutting taps do see: http://www.balax.com/forming.html For example for a 6-32 cutting tap the recommended drill size is a #36 (0.1065") for 65% thread. For the Balax 6-32 form tap the recommended drill size is a 1/8" (0.125") for 65% thread.

Don

10. "Not really. The split-clamp bar stock is 1" thick by 4” wide. The 3.375" diameter hole was trepanned quickly using a 1/2" end mill on the Tormach then finished to size with a boring head. http://i72.photobucket.com/albums/i1...blankFlynn.jpg The slot was hand cut on a bandsaw but could have been easily made using a slitting saw like this one http://i72.photobucket.com/albums/i1...TSblankSaw.jpg

The bracket I was really referring to was the bracket bolted to the Procunier as shown here: http://i72.photobucket.com/albums/i1...ierBracket.jpg This bracket was designed in Solidworks then the Gcode generated using SprutCAM. Isn't that what having a CNC mill is all about?
"

I was looking at the spindle clamp bracket. Really nice splitting saw BTW. Yes that's what having a CNC is all about, but at the moment if I continue with the personal projects I'm never going to get what I bought the machine for done. Don't get me wrong I would love to have a solid, fast tapping head like the one you've made and will probably make one at some point, just need to finish a few products before I do so. Awesome work Don !

Would this be the one ?

http://cgi.ebay.com/Procunier-Tappin...#ht_2351wt_913

Here's my favorite one

http://cgi.ebay.com/Procunier-4-Tapp...#ht_500wt_1154

I'm curious on what makes this style tapping head faster than the one I currently own ?

.

11. "I'm curious on what makes this style tapping head faster than the one I currently own ?"

With the T/C tapping head the spindle must be able to stop and reverse. The Tormach uses a VFD 3-phase motor controlled spindle and cannot quickly stop and reverse. So spindle speeds and feeds must be very slow when tapping in order not to have over travel especially when tapping blind holes. The Procunier tapping head has a double-cone clutch and 2:1 reversing mechanism so that the spindle does not reverse or stop. In addition the cone clutch allows for disengagement within 1/3 revolution. This means that tapping can be done at high speed with the spindle running continuously even in blind holes. If the Tormach had a servo controlled spindle that could stop and reverse quickly then a tapping head such as the Procunier would not be needed for fast tapping particularly when tapping blind holes. For me , the Procunier works very well with the Tormach VFD 3-phase motor controlled spindle allowing me to tap blind holes at high speed. I have successfully tapped tens of thousands of 4-40 blind holes using the Procunier 1E tapping head on the Tormach at high speed.

12. Don,

A few of that brand tapping heads on ebay. Is it just the 1E that is workable or will any reversing tapping head work? What others would you recommend?

David

Page 1 of 5 1234 ... Last

1. ###### Tormach Personal CNC Mill &gt; Reversing Tapping head vs Tension/Compression tapping Head
06-11-2013, 09:06 PM