[carlboe]

I Hope this is not dumb a question but there goes dose thread milling with a single point use the same g code as with a multi point insert. I have about 105 holes to do. And I think a threadmill would be better way to go.

Thanks
Carl Boe

[Steve Seebold]

Single point will work, but a single element threading tool will be a whole bunch faster.

What thread are you cutting? Internal or external?

MSC shows a thread mill that won't break the bank on page 395.

[carlboe]

Steve

It will be 1/2-20 in 4041 Preharden. Internal 5/8 deep

Thanks
Carl Boe

[txcncman]

Modern multi-point inserted thread mill tools should handle this just fine. No need for single point. Are you sure your machine is up to the task?

[Steve Seebold]

What machine are you doing it on?

[wbleeker]

Single point will work, but a single element threading tool will be a whole bunch faster.

What thread are you cutting? Internal or external?

MSC shows a thread mill that won't break the bank on page 395.

It seems that MSC thinks there are only two other countries in the world Canada and Mexico? I tried to register and that is what wouldn't let me, who blew the rest of the world up?
Will

[carlboe]

I have a Tormach and a Haas TM 1. But I would like to use the Tormach 1100.

Thanks

Carl Boe

[neilw20]

I milled this Left Hand M22 thread on my SX3. Tap was too expensive to contemplate purchasing.
2800 RPM, single point, three passes. 20mm deep to a blind shoulder.
Test piece was able to be re-machined to get the cut size exact after testing on male thread.
Final piece is a smooth snug fit, maybe 0.002" clearance.





Thread Milling Photos by neilw20_2008 | Photobucket

[DareBee]

105 holes to thread will take a very long time with a single point.
Any 3 axis machine can do it though.

I have a Vardex 2mm pitch threadmill that has done well over 100 holes (1" dp) in A2 and still going strong.

[carlboe]

Do you guys think I would be better off with a tap. The holes are though holes.

Thanks
Carl Boe

[neilw20]

If it hard material, mill it, if normal then tap it.

[nitewatchman]

Being a cheap skate and having the need to sometimes do odd things.

I have good luck using a modified tap for a thread mill cutter. Granted the tooth geometry is not exactly correct and the 60 degree thread angle will have a slight error, the results are very good and repeatable for both internal and external threads.

I would start with a 1/4"-20UNC straight tap and grind away all but one of the flutes and then grind off the end of the tap to remove the incomplete threads. The remaining flute would be backed off for primary relief by grinding the heel of the flute away treating the leading edge like an end mill. This is then used as the cutter.

I use the Thread Milling Wizard in Tormach Mach 3 and make the cut in one pass but by spiraling down or up (climb mill verses conventional mill) the full length. For 5/8" deep at 20TPI this would be 12.5 turns. I have used this approach for example to produce 5/8"-32UN internal and external threads cut to within .030" of a shoulder to produce a housing and matching cap.

I would thread mill for sure.

nitewatchman

[sirbean]

Great tip nite. From one cheap skate to another, thanks.

Sent from my DROID RAZR using Tapatalk 2

[MetalZilla]

Vardex used to make some really good thread mills.

[carlboe]

Neilw20

Did you make that threading tool? Nice one if you did put if you bought where did you get it?

Thanks

Carl

[neilw20]

Neilw20

Did you make that threading tool? Nice one if you did put if you bought where did you get it?

Thanks

Carl

Carl,

I designed and made it from a 16mm high tensile bolt.
The deck the insert seats on is 1.925mm below center.
The upper deck is 1.5mm above center.
The hole is offset 0.354mm to the right of center.
The apex of the triangle is 6.73 from the hole.
The end is 3.77mm from the hole.
The diameter at the tip is 12mm
It free cuts at 15.0 diameter so the smallest you could do is M16 x 1.0, just.

I carefully modeled the insert to get it at the correct place.
The position of the screw hole is just slightly closer to the apex so that when tightened it pulls the insert in tightly.
You need a high tensile 3mm CSK screw (pinched from a lathe tool holder)

Slowest part was the finishing passes with the 3 mm end mill.
It was hogged out with a 10mm 3fl carbide mill.
The rounded bit was a 1/2" ball end mill.
ODs surface ground to look nice.
It would be nice if it was solid carbide as the extra stiffness would mean heavier cuts can be taken.

It would take me just tooooo long to even contemplate machining that stuff.:drowning:

I only have fragments of code and they were tuned on the job so are really not much use so you need to grow your own.

The front of the insert has a tiny front clearance ground on it. Maybe 0.005"
It takes 55º or 60º inserts. for whitworth or iso/unc/unf.
The angular error in the thread form is trivial for most applications.

Neil

[David Bord]

I milled this Left Hand M22 thread on my SX3. Tap was too expensive to contemplate purchasing.
2800 RPM, single point, three passes. 20mm deep to a blind shoulder.
Test piece was able to be re-machined to get the cut size exact after testing on male thread.
Final piece is a smooth snug fit, maybe 0.002" clearance.





Thread Milling Photos by neilw20_2008 | Photobucket

Neil, Very nice tool! Man that a great idea, and if you don't need to do much thread milling that's a great option!


David

[DareBee]

definite kudos Neil.
I didn't look at it close enough to notice it was homespun (til now).
The usual suppliers make these indexable single point tools as well for those that don't want to machine their own.

Back at the OP.
105 holes @ 1/2-20 in 4140HT, I strongly suggest you get a thread mill and just be done with it. You will be very pleased with the result and will likely save the cost of the thread mill in labour alone (not to mention the number of taps you will burn out).

[mrquacker]

It seems that MSC thinks there are only two other countries in the world Canada and Mexico? I tried to register and that is what wouldn't let me, who blew the rest of the world up?
Will

Nigerians, with their mail order internet scams.

[kevinro]

Nigerians, with their mail order internet scams.

This just reminded me of a story on This American Life. If you have a few minutes, listen to the start of this. The full story is about 29 minutes, but it is really very interesting.

Enforcers | This American Life