What's new
What's new

Thread Milling Nitronic 60

Pete Deal

Stainless
Joined
Apr 10, 2007
Location
Morgantown, WV
I have a few parts (6) to make from Nitronic 60. Each has a 10-24 threaded hole .375" deep thread. I need to do some mill work on them anyway so i figured I would thread mill them. I wonder if any of you that are very adept at thread milling would check my numbers before I snap it off.

Cutter: single thread form, .135" od, 3 flute.
Hole: #25 (.1495")

I see 150 sfm recommended so I will be running about 4200 rpm.
.0003" per tooth is also recommended. On the straight this would be about 3.8 ipm.
Planning on .004" per pass. This seems like a lot to me but looking at various online references they seem to recommend less passes than I have.

Since my first cut will be .004 in a .1495 hole I used .158" as the outer diameter and calculated the feed as follows:

Programmed Feed = 3.8ipm x (.158-.135)/.158 = .55ipm.
 
Single point. I got it from onlinecarbide.com. I used one of their threadmills before and it worked great but it was for an M10x1.25 hole- a little more meat to it.
 
Update- Those parameters are not good. Snap! I think .004 per pass was too much. They seem to tap ok so since I have so few I think I will do that instead. Thanks for the input anyway.
 
I made a spreadsheet to quickly convert linear feed for ID interpolation. Just punch in your sfm, threadmill dia, thread major, and desired fpt and it'll spit out a number for you.

PM me if anyone would like it. Simple formula but helps when you are punching it in to your calculator a lot.
 
If you did try again, i'd try slowing the SFM down a bit. Would help reduce the vibration a bit which may have lead to the failure. Id run my threadmills around 50-75 sfm for hastelloys with great success.
 
If you did try again, i'd try slowing the SFM down a bit. Would help reduce the vibration a bit which may have lead to the failure. Id run my threadmills around 50-75 sfm for hastelloys with great success.

Thanks! What about your cut amount per pass for itty bitty cutters? My gut told me .004" was too much. Of course with a single thread cutter I would have been there 6 weeks per part. But it still would be nice to know how to make it work. Thread mills make expensive fuses.

I should have just hand tapped the stupid things in the first place. It's only a few parts and it hand taps pretty well. I drilled them with HSS and got 2 parts and had to sharpen the bit.
 
I'd have honestly tried probably 3 passes at .006-.007 stepovers with 1 spring pass. Lowering the spindle seems to be the only thing to work for me with smaller tools in tough materials. The vibration will shatter the tool in no time or best case scenario leave a terrible finish in the threads.
 
.004 should have been fine. I think your problem is using a no-namo pos threadmill from carbide land or where ever. Try a real one, like from SCT or Emuge next time. We threadmill 4-40's in Inconel all the time, and have NEVER broken one.
 
.004 should have been fine. I think your problem is using a no-namo pos threadmill from carbide land or where ever. Try a real one, like from SCT or Emuge next time. We threadmill 4-40's in Inconel all the time, and have NEVER broken one.

Buying a $110 thread mill for a job that I quoted $450 for was not going to work. I think my mistake was not hand tapping them as i said. And, they worked well for me before. Live and learn.
 








 
Back
Top