Threadmilling 4140 hardened steel

[bdog123]

here's the scoop, I'm threadmilling a 5/16-18 bind hole .4375" deep. My cutting parameters are rpm 1600, feed 2.0, and stepover of .001 per pass. I am taking a total of 45 rough passes, with 2 finish and spring passes.
The problem is that it will cut one thread fine but 4-5 parts later the thread is not fitting properly. This is the first time i have cut a hardened material. It's hard to believe that I'm getting that much wear after running that small amount of parts. Below is the link to the tool that I'm using.

McMaster-Carr

McMaster-Carr is the complete source for your plant with over 595,000 products. 98% of products ordered ship from stock and deliver same or next day.

www.mcmaster.com

Any tips would be greatly appreciated.

 

[DouglasJRizzo]

I guess your feed/speed parameters are ok for the tool?
Flood coolant?
Pre drill hole correct size?

 

[Bill in PA]

How hard is the 4140? Nitrided or through-hardened?

Bill

 

[Booze Daily]

You're getting a lot of wear because of the .001 DOC. I'd try 2 roughing and 1 finish pass.
If you have a lot of parts, maybe add a finishing thread mill.

 

[bdog123]

The material is through hardened.

 

[Mtndew]

The material is through hardened.

What Rockwell?

Take it in 1 pass. 2 passes only if there is tool flex.

 

[eKretz]

I agree with the others. Push the cutter harder, you're almost rubbing it rather than cutting. One or two passes should be all you need. What you're doing now means that you're almost putting at least 20+ holes worth of wear on the cutter while cutting one part. Not surprising that it's only doing a few parts before getting tool wear.

"Through hardened" doesn't tell us much. Is it 58Rc? Q&T at 28-32Rc? Something else?

 

[Camputer]

I'm going to be honest, I don't have a ton of experience with thread milling but this is the first time I feel obligated to shout out a tool. I had to buy some threadmills for a part that had 1/4-28 x 1/4 deep blind holes with no room for a drill tip underneath without breaking through the material (which wasn't allowed). Material is hardened 17-4ph 38-42ish rwc.

I found these OSG bottom cutting thread mills (A brand AT-2 line) that advertised not needing a pre drilled hole, just helix down and let the bottom cutting action work. I'm not going to lie, I thought they wouldn't last me two parts but they seemed perfect for the job so I had to try them out. I bought two (and some traditional style threadmills as backup). We loaded up the first one and let her go and that bitch ran out the order, and the next order, and the next order, and the next order. I think we actually just retired her and loaded up the second one. In total I think it did about 1000 holes over the span of a few months. I still have the traditional backups in my drawer.

 

[Mtndew]

I'm going to be honest, I don't have a ton of experience with thread milling but this is the first time I feel obligated to shout out a tool. I had to buy some threadmills for a part that had 1/4-28 x 1/4 deep blind holes with no room for a drill tip underneath without breaking through the material (which wasn't allowed). Material is hardened 17-4ph 38-42ish rwc.

I found these OSG bottom cutting thread mills (A brand AT-2 line) that advertised not needing a pre drilled hole, just helix down and let the bottom cutting action work. I'm not going to lie, I thought they wouldn't last me two parts but they seemed perfect for the job so I had to try them out. I bought two (and some traditional style threadmills as backup). We loaded up the first one and let her go and that bitch ran out the order, and the next order, and the next order, and the next order. I think we actually just retired her and loaded up the second one. In total I think it did about 1000 holes over the span of a few months. I still have the traditional backups in my drawer.

That's impressive, I've always wanted to try one of those.

 

[Camputer]

That's impressive, I've always wanted to try one of those.

Full context, they're millturn parts on our old clapped out doosan MX, 1.5" barstock. Each part had two holes at a 45 degree angle on a turned (convex) surface, hanging out of the main spindle with no sub support so the head could reach. I wasn't even confident that the machine could interpolate accurately with the head tilted like that (it is really beat up). It was about the most un-ideal setup you could have to test out a brand new process.

So hats off, I don't think ever ever had that much luck with a tool before.

 

[Rick Finsta]

I caught this thread a little late, but I run a Harvey threadmill in 4140 at 44HRc (that is about as high as you can through harden up to 1.0" or so thick from what I've been told and these parts start from 1" thick material that has already been hardened) to make a 3/8"x24 thread in some repeat parts. I've made about 70-80 of these parts and I'm getting a little taper in the threadmill but still fits the 3B thread gauge just fine.

120SFM (1600RPM), 0.0005" per tooth (3.2IPM), three 0.015" stepovers and a spring pass. Takes about six minutes per part but the tool lasts and the threads turn out great. I haven't had much time to fiddle with speeds and feeds since I don't mind the unattended cutting time in this application.