[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

[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

[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