[SwampDonkey]

I have a rather critical part I need to thread and Im not quite confident enough in my new 30 yr old Jet 1024p to do the job (it needs a bit of work). Im new to PP and thread milling in general, and just wondering what to expect. I really dont want to scrap this part so any info or advice you gurus might have would be invaluable.

Thanks,
SD

[Tormachmaster]

I have a rather critical part I need to thread and Im not quite confident enough in my new 30 yr old Jet 1024p to do the job (it needs a bit of work). Im new to PP and thread milling in general, and just wondering what to expect. I really dont want to scrap this part so any info or advice you gurus might have would be invaluable.

Thanks,
SD

I always tell people who are new to simply take a piece of aluminum the same size you are going to run and run it first if it comes out good you are good to go if you cannot do this then run it above the part it looks good then go for it. Either way PP does thread milling pretty easy so i think you'll be fine. Are you using a single point thread mill or? what rpm and feed? carbide cutter I assume.

[SwampDonkey]

I always tell people who are new to simply take a piece of aluminum the same size you are going to run and run it first if it comes out good you are good to go if you cannot do this then run it above the part it looks good then go for it. Either way PP does thread milling pretty easy so i think you'll be fine. Are you using a single point thread mill or? what rpm and feed? carbide cutter I assume.

Yeah I was thinking of using this one:

3 8" 14 40 TPI Single Pitch Thread Mill Brand New TiAlN Coated | eBay

Ive just never done thread milling before so im pretty nervous about where to start.

[Tormachmaster]

Yeah I was thinking of using this one:

3 8" 14 40 TPI Single Pitch Thread Mill Brand New TiAlN Coated | eBay

Ive just never done thread milling before so im pretty nervous about where to start.

On a piece of scrap if you are that worried it does not matter if you mess up a piece of scrap aluminum. What is the thread you are cutting? What material? Inside or outside thread? How long? You can post your program on here to be checked. When in doubt take your time it's only one thread. What type part is it on?

[kstrauss]

Have you considered purchasing thread mills from Tormach rather than eBay? The prices appear similar.

[keen]

I have done 3 videos on this subject including.

Keen

https://www.youtube.com/watch?v=jY9vuLFT13g

[TurboStep]

Using a thread mill ground to a point, or close to a point, and setting the thread OD based on the thead mill diameter will give you an undersized thead. The thread OD is not as important as the pitch diameter. See the last drawing on this page:
Unified Screw Threads and Tolerances (Inch)
The default values generated by PathPilot simply set the thread OD, regardless of the thread mill form and without adjustment will often create threads which are too tight. This is not a PathPilot specific problem, most first attempts at thread milling suffer from this issue (there are lots of youtube videos demonstrating this effect )
Step

[kstrauss]

I'm glad that you've brought up the importance of truncating the pointed end of the cutter in order to get the right thread form. Perhaps I'm confused but it also seems that the "top" of the cutter must be rotated to the helix angle of the thread in order to get the correct shape of the flanks of the thread. Is that correct? Is this addressed with commercial thread mills by restricting the range of TPI for the mill? Or have I completely missed the point?

[keen]

I'm glad that you've brought up the importance of truncating the pointed end of the cutter in order to get the right thread form. Perhaps I'm confused but it also seems that the "top" of the cutter must be rotated to the helix angle of the thread in order to get the correct shape of the flanks of the thread. Is that correct? Is this addressed with commercial thread mills by restricting the range of TPI for the mill? Or have I completely missed the point?

No you have not missed the point - you are just thinking deeper than most. In theory the cutter should be set to the helix angle and in lathe thread milling this is possible. With milling the cutter rotates and this is not possible.

The thread milled form is seldom perfectly accurate as any specific cutter is not ground for each thread form and pitch etc. However in practice usually a close enough form is produced. It is only in some extreme circumstances where this issue is a problem, but it is really good to be aware it is there.

Even on internal thread milling, because the cutter sweeps away on a smaller radius it actually fouls up the thread form less than it would appear to. I have studied helix profiles, cutter trajectories, tests and measurements in the past and have found it is an issue only in extreme situations. Eg when the thread is internal, the thread form is deep, with a steep pitch, and the cutter, is relative to it, big in diameter.

All the same - be aware the thread milled form on internal threads is unlikely to be perfect.

Keen

[kstrauss]

Thanks. After some conversations with another machinist I was beginning to doubt my understanding of the limitations thread milling!

An upcoming project requires some relatively large diameter multi-start threads: ~1-inch diameter, 20TPI, 5-start. The resulting helix angle is about 4.5-degrees if I've calculated correctly. The funny specs are necessary because the threads are on rather thin walled tubing and therefore can't be very deep. Multi-start threads are a pain on the lathe so I'm thinking of thread milling. Should I mount the stock to be threaded on a tilted 4th axis or...?

[keen]

Thanks. After some conversations with another machinist I was beginning to doubt my understanding of the limitations thread milling!

An upcoming project requires some relatively large diameter multi-start threads: ~1-inch diameter, 20TPI, 5-start. The resulting helix angle is about 4.5-degrees if I've calculated correctly. The funny specs are necessary because the threads are on rather thin walled tubing and therefore can't be very deep. Multi-start threads are a pain on the lathe so I'm thinking of thread milling. Should I mount the stock to be threaded on a tilted 4th axis or...?

Hi - steep pitch is a challenge, but your big diameter bore and shallow thread helps. Is it a V thread? If you might just get away with it with a small diameter cutter, find some way to trial it eg cut a sample in clear plastic or cut a cross section out to inspect.

A tilted 4th axis may give you issues as the Z travel will be off parallel with the part axis... if done in a mill.

Keen

[kstrauss]

Actual thread form doesn't really matter since it will only need to mate with a nut that I will also be making. However, yes, I planned to use a normal V-form. That said, if I cut the internal and external threads with the same cutter I believe that the errors will be in opposite directions so rather than cancelling they will make the deviation twice as bad. Or maybe again I don't have my head cocked the right way!

As you mentioned, Z-travel will not be parallel with the part axis. In my case the threaded area is only about an inch long so with a 4.5-degree tilt the X-axis is only displaced by about 0.08 inches total or +/-0.04 inches over the length of the thread. My plan is to use a tooling ball to align the tilted 4th axis with the mill's spindle and a coordinated A/Z/X move to compensate for the tilt while cutting the threads.

Are you aware of any book or website that discusses issues such as thread milling high helix threads?

[keen]

Actual thread form doesn't really matter since it will only need to mate with a nut that I will also be making. However, yes, I planned to use a normal V-form. That said, if I cut the internal and external threads with the same cutter I believe that the errors will be in opposite directions so rather than cancelling they will make the deviation twice as bad. Or maybe again I don't have my head cocked the right way!

As you mentioned, Z-travel will not be parallel with the part axis. In my case the threaded area is only about an inch long so with a 4.5-degree tilt the X-axis is only displaced by about 0.08 inches total or +/-0.04 inches over the length of the thread. My plan is to use a tooling ball to align the tilted 4th axis with the mill's spindle and a coordinated A/Z/X move to compensate for the tilt while cutting the threads.

Are you aware of any book or website that discusses issues such as thread milling high helix threads?

You may not need to go to all that trouble - I would try a test piece (without the 4th axis) as mentioned above and section it to see if there is an error. No need for multistart, just cut the pitch and depth with a small dia thread mill and cut it in section to view..

If the error is too much - You could then adjust the cutter form to compensate... if it is a simple fly type cutter.

keen

[tbev]

I just wanted to stop by and vouch for Tormach's thread mills , I've threaded quite a few m7x0.5 holes in aluminum, hundreds, and a handful im titanium, with the same one. I broke it last week but that was bc I crashed it really hard, to be expected, my fault, but it is a fantastic thread mill. Good luck w your project,

Sent from my SM-G900V using Tapatalk