Threadmilling problem

[Matthew Hajicek - Conventus 4,142]

Did you use the sharp pointed Harvey threadmill, or the "tipped off" one for "hard materials"?  The sharp pointed ones break down much faster.

[taperlength 105]

For a UNJC  thread make it the max minor hole diameter,  .094 inch.    Another trick is to run progressively bigger passes,  starting .001 higher each time so its cutting on one side like a lathe threading tool.

[Sumac Andy 7]

 A bit late to the party, but.....

I'm with the tapping guys here - we use WNT and tap 316etc... with this tap - Blind hole – Machine taps, right hand | CERATIZIT | WNT | KOMET - and it works with a decent oil.
Unsure if you can get these tools in th US though?

[clayallen 1]

Your threadmill tips are worn. Likely way too high sfm. We had this same problem a few weeks ago with a single form tool. For the really small shank threadmills use 1/4 the recommended SFM. 

I would also add a spring pass. The tiny shank tools deflect. 

0.50 deep for a 4-40 is ridiculous. If you can find a Tri-form 4-40 that is long enough go with that, or grind the shank to get the clearance you need. Single-form threadmills are not great for the small & deep holes. Way too much cycle time. 

[bd41612 86]

I have not used these in anything as soft as 321, but with the PN coating I'd give it a shot.  No drilled hole - just threadmill into solid material, deflection not much of an issue because the tool is cutting 100% at the nose.  I have used these on hardened stainless and cobalt chrome, they work great.

http://www.mmc-hitachitool.co.jp/en-US/products/thread-mill/et-edt/

A few months ago, I submitted an enhancement request along with formulas to CNC Software that may be in a future release to threadmill by volume.  If you have ever used G76 single point threading on a lathe, you know what I'm talking about.  The idea would be to enter in your toolpath parameters the desired amount of passes you would like to take and Mastercam would calculate each pass of the threadmill to take an equal volume of stock on each pass.  When I do this now, I take an average depth of roughing passes and a final pass radial depth of cut.  It's OK for 2 or 3 passes but if more are needed, then I build multiple operations and have each one take an equal volume.