[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)

[twocik]

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 ?

[philbur]

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

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)

[twocik]

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 ?


.

[Don Clement]

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

[twocik]

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 ?


.

[Don Clement]

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

[twocik]

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

http://janproducts.com/SCREW_THREAD_INFORMATION.html

[Don Clement]

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?

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

[twocik]

"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 ?


.

[Don Clement]

"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.

[David Bord]

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

[300sniper]

i have one of the old style tormach tapping heads still in the box. i think it is the reversing style (i remember it being quite a bit more expensive than the ones listed now). i don't see it on their site anymore. i am wondering if this style is better than the new style, even if i do upgrade to the new spindle drive.

i have not had to tap many holes yet but i guess someday i will need to unpackage it and try it out.

[Don Clement]

Don,

Is it just the 1E that is workable or will any reversing tapping head work? What others would you recommend?

David

David:

The Procunier 1E very works well for me, especially with the Procunier Pro-Quick quick change collets for each tap size. BTW I have a two Tapmatic brand reversing tapping heads but never use them. You can take that as a recommendation. I really don't like to bother with those pesky Tapmatic rubber-flex collets not to mention Tapmatic and many other reversing tap head brands use a kind of dog clutch instead of the far superior Procunier "cushioned" double-cone clutch http://www.rockford-ettco.com/Default.aspx?tabid=1459 . The Tapmatic rubber-flex collets are a real PITA when changing taps fiddling with those thin wrenches. The Procunier Pro-Quik collets http://www.rockford-ettco.com/Portal...ro-QuikTap.pdf are very similar to the quick change tap arraignment found on the Tormach T/C tapping heads. My assortment of Pro-Quik quick change collets for each tap type allows me to enter each tap height in the Mach III tool table and then easily change the tap size by simply snapping a new tap into the Procunier tap head (no wrenches needed), then reference the tap size tool number. See: http://i72.photobucket.com/albums/i1...erQuickPro.jpg

Don

[twocik]

Don what cam program are you using to write your tapping gcode or are you hand writing them as well ?


I'm using Cambam and have to apply a custom script to a drill mop and my code still needs to be hand written every time. I haven't tested the gcode file yet, and wanted to know if you're doing the same or if anyone here has a TC Tormach head and how or what program you're using ?

[Don Clement]

[QUOTE=twocik;808408]Don what cam program are you using to write your tapping gcode or are you hand writing them as well ?
QUOTE]

twocik:

No need for a CAM program with the Procunier reversing tapping head. With the Procunier reversing tapping head: Spindle does not stop or reverse, feed is 100%, no dwell, the reversing rate is 2:1, and the clutch disengages within 1/3 revolution. So only two lines of code are needed. e.g. for a 4-40 thread in a 0.25" deep blind hole here is the code with the spindle running at 1200 rpm: G1 F30 Z-0.25 : G1 F60 Z0.1 and if I used a canned cycle this could be one line of code. I have tapped thousands of blind 4-40 holes using my TTS modified Procunier 1E tapping head on the Tormach PCNC using only those two lines of code.

I use SprutCAM 7 to generate the really complex G-code of many thousands of lines but not for something as simple as tapping a blind hole with a Procunier reversing tapping head. BTW SprutCAM 7 is a great bargain when bought with a Tormach mill. MasterCAM, an equivalent to SprutCAM was priced at ~$10K, ten times the price of SprutCAM when bought with a Tormach mill.

Don

[twocik]

Wow that's simple enough ! Well I'm going to give this TC head a shot and see how it comes out, good thing is I'm learning all of the code & technique now. At some point I'll probably look into one of those. Yes next on my list is Sprutcam.

[twocik]

Ok after testing the code that me and few other people thought would work, nope ! Shattered the tap like glass. I took out the locking pin to the tapping collet and tightened it as tight as I could get it until my spanner wrench gave out. Looking over the wrench looks like one of the inner walls were grinned a little to close, pin popped out. Finished tightening the collet with a camera lens spanner wrench I had laying around. Not to mention I've tried everything to get the rest of the broken tap out. (chair)

I used a Dremel + diamond bits to make a slot for a flat head screw driver - next tried tapping it with many tools to try and shatter the rest of it, last was to use an end mill to hopefully get rid of it, nothing worked. Broke my $13 tap, 1/8 carbide $20 end mill, and screwed a bunch of my tool tips up. I'm clueless to why the tap shattered like that....


For perfect alinement I spot drilled and pre drilled the hole with a .113 drill @ .25" depth. Next was the 6-32 spiral bottom tap @ .21" depth in 6061 aluminum (blind hole). I left .04" for clearance, which I thought was plenty of room, but could have been wrong. The tap broke at about .170" - .198" is when I glanced at the screen.






Here's my gcode if anyone would like to take a crack at it



( Drill3 6-32 Tap )
( T4 : 0.14 )
M09
G28
T4 M6
G43 H4
M3 S500
M08
G0 Z0.15
X-0.431 Y-0.431
G4 P4
G1 Z-0.225 F15.625
M4 S500
G4 P0.5
G1 Z0.15
X-0.259 Y0.259
Z0
M3 S500
G4 P4
G1 Z-0.225 F15.625
M4 S500
G4 P0.5
G1 Z0.15
X0.258994 Y0.258994
Z0
M3 S500
G4 P4
G1 Z-0.225 F15.625
M4 S500
G4 P0.5
G1 Z0.15
X0.431 Y-0.431
Z0
M3 S500
G4 P4
G1 Z-0.225 F15.625
M4 S500
G4 P0.5
G1 Z.15
G80

[philbur]

I know very little about CNC tapping or about the detailed functioning of your tapping head, so I guess that means I am fully qualified to comment.

In the Tormach example in post #1 the basis for the calculation was 500 rpm but the code shows S400, which is a 20% reduction from the calculated. So I guess the scheme is for tapping head to let out the slack. In your G-code you use the calculated Z feed of 15.625 inch/min at the calculated spindle speed of 500 rpm. What happens to the function of the tapping head if the spindle speed is actually 525 rpm?

Just a thought.

Phil

PS: Second rule of CNC work, always practice new processes on parts you don't care about.(very especially tapping, it's a b***h to get those broken taps out. Google "Broken Tap", everybody has their favourite).

[twocik]

Yes Phil it is !!! I tried everything, except the mig/tig welding idea (don't own one). I also agree that I should have tested it in plastic or something like wood before, but got a little too confident I guess. I was told that this tapping head runs best/most accurate at 500 rpms. so my math was 500/32=15.625 IPM


I'm going to try again, but this time with more tapping clearance. Hole depth at .25" tapping at .18". Andy over at Cambam mentioned I should take the taper of the drill into consideration which I thought I had covered, but maybe not. I'm thinking maybe the chips might have stopped the tap too. Well see...

I think if I tap clear lexan I'll have a better look at what's going on.




I was also thinking about using the drill + taps bits I have. Any advice on these ?