So not a Guru

Threadmilling problem

Recommended Posts

We have some 321 stainless parts that require 4 each 4-40 holes tapped 0.560" deep, they are thru holes. We purchased a couple of Harvey 2 flute single-point threadmills they have a 5/8" reach, .080" cutter dia 0.04" neck. The recommended speeds & feeds are 3 equal passes at 9550RPM 0.60IPM. We drilled them with 2.3mm holes.

We had to rerun the toolpath 13X, increasing the radial offset 0.0012" every time, before the thread gage would fit. That came to a total comp of 0.013"! It took over 4 hours to get the hole threaded.

When we ran the next hole, with the 0.013" of comp active, no surprise, it broke the tool. Harvey's tech representative doesn't appear to understand that the 0.0012" passes were necessary due to their recommendations perhaps being incorrect. He says we need to run with their recommendations...that we just told him we attempted.

Okay, I'm done ranting on.

Does anyone have any recommendations for us to be able to make this work?

Share this post


Link to post
Share on other sites

emuge

 

they give you the program

we had a 6-32 single point that the operator was supposed to put in the rad of cutter for cutter comp, he forgot

it cut a 1/4-32 in one shot from a .136 hole in inconel

  • Like 1

Share this post


Link to post
Share on other sites

The neck on that tool will be tiny...I am actually surprised with that much deflection that it's not breaking

I would find a multi-tooth threadmill instead...also make sure your major thread dia is programmed properly, 4-40 thread date says 0.1189 / 0.1120 I would make sure I programmed at .122

4 to 5 passes including spring "should be" sufficient 

 

 

  • Thanks 1

Share this post


Link to post
Share on other sites
1 minute ago, JParis said:

I would find a multi-tooth threadmill instead

I haven't been able to locate one for this DOC

Share this post


Link to post
Share on other sites

That might just be too deep for a tool that small....

Share this post


Link to post
Share on other sites
16 minutes ago, htm01 said:

emuge

They said they can only go to 0.396" deep.

Share this post


Link to post
Share on other sites
38 minutes ago, So not a Guru said:

321 stainless

Not much fun....not quite as bad as 324 and 348.

Very tough.

Share this post


Link to post
Share on other sites
Just now, nickbe10 said:

Not much fun....not quite as bad as 324 and 348.

Very tough.

Yeah, it's a pain, but I've always managed to be able to get thru it up till now! This deep thread at such a small size is kicking our fannies.

Share this post


Link to post
Share on other sites
Just now, So not a Guru said:

Yeah, it's a pain, but I've always managed to be able to get thru it up till now! This deep thread at such a small size is kicking our fannies.

it's crazy to be that deep, you don't get anymore holding power

  • Like 1

Share this post


Link to post
Share on other sites

You tried tapping it? I would try to roll form it and see if that works. If you chose to roll form it then make sure you ream to within .0005" of the size they call out and go .0005 bigger verses smaller. Use a good cutting oil not coolant if you attempt to roll form or tap it. Moly-Lube might work, but still a huge fan of tapping oil in SS.

  • Like 4

Share this post


Link to post
Share on other sites
1 minute ago, crazy^millman said:

You tried tapping it? I would try to roll form it and see if that works. If you chose to roll form it then make sure you ream to within .0005" of the size they call out and go .0005 bigger verses smaller. Use a good cutting oil not coolant if you attempt to roll form or tap it. Moly-Lube might work, but still a huge fan of tapping oil in SS.

The spec doesn't allow for form tapping.😡

  • Sad 1

Share this post


Link to post
Share on other sites
33 minutes ago, So not a Guru said:

The spec doesn't allow for form tapping.😡

That would have been a no bid for me then.

Share this post


Link to post
Share on other sites

It is a class 3 or class 2 thread. A class 2 thread allows for a bigger Min diameter. Try making the min diameter within .0002" of the max and try a standard tap. If your machine can peck tap then peck tap it using .01 to .02 pecks. I would start at 1000 rpms and go from there. Don't use a floating holder in peck tapping. All the best, but I would get away from Threadmill that deep. Maybe threadmill 1X and then chase by hand with a tap I have done that before with good success. Just have to have a good feel and steady hand on such a small tap. I have hand tapped 2-56 in Ti using this method and would only break a tap about every 40-50 holes, but that was 20 years ago. I don't have that feel anymore like I use to.

Share this post


Link to post
Share on other sites
40 minutes ago, crazy^millman said:

Moly-Lube

I have had good results with a mixture of Moly Dee and Copper Ease even with cut taps...

The tools tend to go off pretty quick so you would have to be pretty conservative changing tools.

I think I would agree with Ron on this one.

Share this post


Link to post
Share on other sites
6 minutes ago, crazy^millman said:

It is a class 3 or class 2 thread. A class 2 thread allows for a bigger Min diameter. Try making the min diameter within .0002" of the max and try a standard tap. If your machine can peck tap then peck tap it using .01 to .02 pecks. I would start at 1000 rpms and go from there. Don't use a floating holder in peck tapping. All the best, but I would get away from Threadmill that deep. Maybe threadmill 1X and then chase by hand with a tap I have done that before with good success. Just have to have a good feel and steady hand on such a small tap. I have hand tapped 2-56 in Ti using this method and would only break a tap about every 40-50 holes, but that was 20 years ago. I don't have that feel anymore like I use to.

It's actually a UNJC thread, so that requires a larger size hole. I had already decided to run the threadmill, then chase the holes with a tap. I can't see this working any other way at this point.

Dude, nobody asked me, or I would have no bid this as soon as I saw the depth & material. I'm just the guy who's supposed to make it work. 😉

  • Like 1
  • Haha 1

Share this post


Link to post
Share on other sites
3 hours ago, So not a Guru said:

Dude, nobody asked me, or I would have no bid this as soon as I saw the depth & material. I'm just the guy who's supposed to make it work. 😉

First step of journey level machining....establish the scapegoat...

  • Haha 3

Share this post


Link to post
Share on other sites
5 hours ago, So not a Guru said:

We have some 321 stainless parts that require 4 each 4-40 holes tapped 0.560" deep, they are thru holes. We purchased a couple of Harvey 2 flute single-point threadmills they have a 5/8" reach, .080" cutter dia 0.04" neck. The recommended speeds & feeds are 3 equal passes at 9550RPM 0.60IPM. We drilled them with 2.3mm holes.

We had to rerun the toolpath 13X, increasing the radial offset 0.0012" every time, before the thread gage would fit. That came to a total comp of 0.013"! It took over 4 hours to get the hole threaded.

When we ran the next hole, with the 0.013" of comp active, no surprise, it broke the tool. Harvey's tech representative doesn't appear to understand that the 0.0012" passes were necessary due to their recommendations perhaps being incorrect. He says we need to run with their recommendations...that we just told him we attempted.

Okay, I'm done ranting on.

Does anyone have any recommendations for us to be able to make this work?

We’ve had great luck with these in Ti. Buy 2, jig grind the neck on one, run the standard as deep as it will go...finish with the modified one.  Hope that’s of some use, good luck. 

Scientific Cutting Tools40 to 64 TPI, Internal/External Single Profile Thread Mill

#4" Noml Diam, 0.08" Cut Diam, 3/16" Shank Diam, 3 Flute, 0.045" Neck Diam, 0.3" Neck Length, 2" OAL, Bright Finish

 

  • Thanks 1

Share this post


Link to post
Share on other sites
4 hours ago, So not a Guru said:

The spec doesn't allow for form tapping.😡

Don't you just love when they do that 😅

Share this post


Link to post
Share on other sites
1 hour ago, Jespertech said:

Don't you just love when they do that 😅

Not particularly.😎

Share this post


Link to post
Share on other sites

Carmex mini style. they have 3 threads on them all day every day. I never use taps anymore. They make a series specifically for hard materials. I still program it as a single style so that I get the complete helix.... They even have 3 in 1 threadmills no hole required although I would not recommend it for your application. The key is multipass on holes like this.. Hard maerial like that I would give it 3 passes with the last one being almost a spring pass.  Also Harvey makes good tools but their techs are useless IMHO....

  • Like 1

Share this post


Link to post
Share on other sites

I would try reducing spindle speed & feed until you get the harmonics out of the cut. I used to thread mill a lot of 6-32's in 316ss and the mfg speeds were unusable. I'd always bring the SFM way down until it was a nice sounding cut. Probably will require 3-4 stepovers.

Share this post


Link to post
Share on other sites
1 hour ago, zachlancy said:

I would try reducing spindle speed & feed until you get the harmonics out of the cut. I used to thread mill a lot of 6-32's in 316ss and the mfg speeds were unusable. I'd always bring the SFM way down until it was a nice sounding cut. Probably will require 3-4 stepovers.

Yes, I cut the feed in half and got a lot closer to a usable thread. Still having to chase it with a tap afterward, but it's working.

Share this post


Link to post
Share on other sites
58 minutes ago, So not a Guru said:

Yes, I cut the feed in half and got a lot closer to a usable thread. Still having to chase it with a tap afterward, but it's working.

If you cut the feed more, maybe you wouldn't have to chase it at all?

It sounds like a classic case of tool deflection.

Share this post


Link to post
Share on other sites
5 hours ago, byte me said:

If you cut the feed more, maybe you wouldn't have to chase it at all?

It sounds like a classic case of tool deflection.

Yes, we are off Fridays thru Sundays, but I intend to do just that on the 1st part Monday.

  • Like 1

Share this post


Link to post
Share on other sites

Create an account or sign in to comment

You need to be a member in order to leave a comment

Create an account

Sign up for a new account in our community. It's easy!

Register a new account

Sign in

Already have an account? Sign in here.

Sign In Now

  • Recently Browsing   0 members

    No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us