[cgroves]

Hello

I'm about to purchase a Tormach and I'm little stumped when it comes to the best approach for threading. I'm new to CNC (and largely metal machining) and currently use hand taps when I need a thread. I typically use taps in the M3 - M10 range.

From a mill pre-purchase stand point it seems to me that having a tapping head on the mill is likely to do a better job than I can achieve by hand and has the benefit of being quicker at doing multiple threaded holes.
Tormach has two types of heads available the "Reversing Tapping Head" and the "Tension/Compression (T/C) Tapping Head". They have some documentation on the technical aspects of the differences but I'm none the wiser on the practical benefits. I.e. is the difference in g-code for threading of relevance if using alibre/sprutcam?

The T/C tapping head is appealing because of the wider range of supported taps for a single head, the quick change aspect and the lower cost.

However applying the "you get what you pay for principle" what's the advantage of the Reversing Tapping heads?

In terms of my applications for the Tormach there's no one dominant one. Its going to be used from brass components for furniture to aluminium tooling for polyurethane components.

If anybody has any advice on threading it would be much appreciated.

Thanks, Christian

[saabaero]

I have a pair of the reversing heads from Tormach that are brand new that I would consider selling for 75% of new cost. (30612 & 30613) One advantage I see to the reversing head is that it can be used on machines other than a CNC such as mill/drill or drill press making them more versitle. They are also faster on the retract.

[bobeson]

I own both a reversing tormach tapping head and their new compression tapping head. Although I've cut hundreds of threaded holes with my mill in the year I've owned it, I've never used either of the tapping heads because I first discovered all the wonderful advantages offered by thread milling. Once you get the hang of hand-coding the cutting path, they are really easy to use - trivial almost.

I keep thinking that I need to sell my tapping heads, but then I get to thinking that I should at least learn to use them before getting rid of them. Whenever a hole comes along that needs threading, however, I find myself wanting to just mill the threads for expediency.

I modified a Vardex full-profile insert thread mill toolholder with a .750 shank to add a TTS shoulder, which I use often to cut ID and OD threads of various pitches for larger bore sizes, and also have a collection of solid carbide thread mills for smaller bores. BTW, thread mills are all insanely overpriced! What's up with that? They appear to be on par with nice taps in terms of materials and manufacturing complexity, they they cost 10x as much as a good tap! Lakeshore Carbide has by far the best deals I've found so far for solid thread mills - about $80/each vs. $160+ that's typical for most distributors. Thread milling can certainly set your pocketbook back pretty quickly if you are in the habit of breaking tools. Or so I've heard. Ahem

[wvines]

Hi Christian,

I haven't used the reversing tapping head but used the tension-compression head for several dozen holes in aluminum this week. I really like the t/c head and it worked very well once I did a few experiments to find the proper taps and fine-tune the g code.

Programming for through-holes is simple. The code from Tormach's Tapping Guidelines worked fine for those. For blind holes, it took some tweaking to get consistent threads near the bottom of the hole. That's a generic problem for non-rigid tapping and not specific to the Tormach tools.

I haven't had much luck getting Sprutcam to generate code for tapping that is directly useable. The Tormach postprocessor generates G84, which doesn't seem to be fully implemented by Mach. I replace the G84s with a subroutine call after the code is generated. If I had the "all-posts" version of Sprutcam I would update the postprocessor.

One tip: Don't use a tap that is described as "not suitable for aluminum" on aluminum. And if you do, Drano works well to unclog it.

Walter

[wvines]

...Lakeshore Carbide has by far the best deals I've found so far...

I have the Lakeshore Carbide threadmills and, I agree, they work great. And they're still expensive even though they're cheaper than most. I'm almost afraid to use them unless I have too. The only drawback I've seen is that I can't cut very long threads with them because they're fairly short.

I'll look into the Vardex threadmill toolholder. Thanks for the tip.

[cgroves]

Thanks for the replies. I think i'll go with the T/C tapping head. It seems the advantage of the reversing head is if you need to do lots of holes plus someone trying to sell nearly new ones is a little suspicious :-).

I asked the same question to one of the techs at Tormach and he said that both the reversing and TC heads need modification to the g-code produced by sprutcam.

The thread mill option sounds like something for the future if I need threads larger than M12.

Regards, Christian

[BobWarfield]

BTW, you may find something like the MariTool T/C tapper is cheaper:

www.maritool.com

I'd use a T/C before the reversing.

Best,

BW

[Don Clement]

I use three techniques for tapping under power on my Tormach: A Procunier tapping head adapted to Tormach TTS, Vardex insert threadmiller adapted to TTS, and Tormach Tension/Compression Tapping Head Kit (31163). Most of my small hole tapping less than ¼” is blind so the Procunier tap head works extremely well for me. I modified a Procunier 1E tap head that I have been using for many years for use on my Tormach. See: http://i72.photobucket.com/albums/i1...Tormachweb.jpg
http://i72.photobucket.com/albums/i1...ackviewweb.jpg
I have successfully used the Procunier tap head to tap tens of thousands of blind small holes in aluminum with Balax form tap. The Procunier has a cushioned double-cone clutch that has worked very well for me for many years. Recently I added the ProQuick quick change system to the Procunier tap head that allows for each tap to be easily changed and also each tap has its own entry in the tool table for height repeatability that is necessary when tapping blind holes without measuring tool height each time a tap is changed. See:
http://i72.photobucket.com/albums/i1...erQuickPro.jpg
Here are some videos of the Procunier tap head in action on the Tormach. Note that the Procunier feed is 100% , no dwell, reverse speed in 2:1.
http://s72.photobucket.com/albums/i1...t=100_3184.flv
http://s72.photobucket.com/albums/i1...6Procunier.flv
Because most all of my tapping is blind holes I rarely use the T/C.
For larger threading on the Tormach I use threadmilling such as this 102mm- 1mm internal thread shown here:
http://s72.photobucket.com/albums/i1...t=100_1311.flv
Don Clement
Running Springs, California

[bobeson]

Don, thanks for your detailed reply - it's nice to hear how Real Machinists (vs. amatuers like me do their work. I'm curious though - what prompts you to use a tapping head instead of thread milling for smaller blind holes? Replacement tool cost? Max thread length? Are there any inherent advantages to tapping vs. thread milling other than these? I'd really love to know if I'm going overboard with thread milling by ignoring my tapping heads - is there someplace they excell, other than cost/hole? Blind holes are one of the great strengths of thread milling in my experience so far; hence I'm really curious why you prefer the tapping head for those jobs.

Thanks again for your advice.

[Don Clement]

Bob,

Have you threadmilled 2-56 or 4-40 holes?

[bobeson]

No, I haven't.

[MichaelHenry]

4-40 and 2-56 have pretty darned small holes - are there thread mills small enough that can fit into the drilled holes?

Mike

[307startup]

I imagine a highly motivated individual with a decent surface grinder and a good setup could turn a standard tap into a thread mill.

But then again why? We both know there are advantages to be had, but if you aren't doing more than a few is it worth the extra work involved?

4-40 and 2-56 have pretty darned small holes - are there thread mills small enough that can fit into the drilled holes?

Mike

[Don Clement]

Most of my small holes are 4-40. I have tapped tens of thousands of blind 4-40 holes in aluminum 6061T6 using a Balax form tap and Procunier 1E tapping head with excellent results. (with Relton A9 tapping fluid) I haven’t tried threadmilling 4-40 size holes yet. IMO the main advantage of tapping vs. threadmilling small holes is that form taps forge the threads into aluminum and they are stronger than cut threads. Also for me the Procunier tapping head has worked very well with the Tormach.

Here is my TTS modification of a 3/4" diameter shaft Vardex insert threadmilling tool for larger holes: http://i72.photobucket.com/albums/i1...cationrear.jpg
http://i72.photobucket.com/albums/i1...dification.jpg
I machined a slot on the ¾” diameter shaft in my 12x36 lathe with a 5C collet using an insert grooving tool. A standard c-clip holds machined TTS ring from moving forward. The ring was also Loctited on the shaft using Red anaerobic Loctite. After assembly on the shaft, the inside of the machined ring was faced off while held in a 5C collet on the lathe.

BTW I will be receiving the Beta Tormach Power Draw Bar today that will make changing TTS tools a one button dream.

Don Clement
Running Springs, California

[Scott_M]

4-40 and 2-56 have pretty darned small holes - are there thread mills small enough that can fit into the drilled holes?

Mike

I guess they do...Lakeshore Carbide

The 2-56 will give you full thread .125 deep


.065" cut diameter , 1/8" shank.

That is a tiny threadmill !!

If the depth is enough for you Mike , I'd bet it would sure speed up your threading operations.


Scott

[justgary]

I imagine a highly motivated individual with a decent surface grinder and a good setup could turn a standard tap into a thread mill.

...Except that a threadmill does not have helical threads like a tap (the teeth are not offset as you go around the mill). You would end up grinding off all but one column of teeth, and then you would still have the problem of clearance into the hole. It would be easier to start with a blank rod to make a thread mill.

By the way, a thread mill does not need a "stack" of teeth. Just one ring of teeth will do. In fact, a single-ring mill will cut a wide variety of thread pitches, whereas a mill with stacked teeth will cut exactly one pitch.

Regards,

- Just Gary

[Don Clement]

Here is another method of tapping manually using the Fischer micro tap guide. I use this if I have a small number of holes to tap and do not want to set up the tapping head or program a threadmiller. Also works great manually tapping in a drill press or with the tailstock of a lathe. See:
http://i72.photobucket.com/albums/i1...tap-holder.jpg
http://www.cartertools.com/fmpdtg.html

Don

[MichaelHenry]

I use a similar alignment tool for hand tapping on my Tormach or my manual lathe and mill. For $10 or so it's a no-brainer. I have a bunch of 4-40 through holes to tap soon and expect I'll be using a Procunier 1E to do the job.

A form tap would be really nice for blind threaded holes - how well do those work in aluminum, PVC or Delrin?

Mike

[compunerdy]

I used my Tension/Compression head for the first time today and it worked pretty good. When I spin the one I used for my 8-32 tap the head and tap seem to wobble quite a bit so I will need to see if the tap or the holder is wonky. It still formed threads ok but they where a bit loose.

The tormach directions contradict themselves.. On this page http://www.tormach.com/document_libr...Guidelines.pdf

It says that..

For Inch Taps: Feed Rate (IPM) = Spindle Speed (RPM)/Threads per Inch (TPI)
For Example, 1/4×20 tap programmed for 500 RPM will need to be feed at
25 IPM

Then later on they show the sample code saying..

(accurate tapping with large reverse head for 1/4 20)
G0Z1 (Rapid motion to plane z=1)
X0Y0 (Rapid motion to hole location)
Z.150 (Rapid motion to plane z=.150)
M3s400M8 (Spindle on CW, 400 rpm, Coolant On)
g4 p5 (Dwell for 5 seconds)
g1z-.9 f25 (Feed tap to z=-.9 and 25 ipm)
g4p2 (Dwell for 2 seconds)
g1 z.150f44 (Retract tap to z=.150 at 1.75x the feed rate)

Shouldnt this code be set at 500 rpm or 20 IPM instead of 25?

I used the formula and ignored the code and it seemed to work ok.

[Don Clement]

A form tap would be really nice for blind threaded holes - how well do those work in aluminum, PVC or Delrin?

Mike

Mike,

4-40 Balax form taps work great on tapping 6061-T6 aluminum but not well at all on Delrin. A standard cutting tap works way better on black Delrin. The Delrin material seems to spring back when using a form tap.

Don