Mp35n

This is my fist experience with this material. I have not started the job yet, I am trying to find out what kind of inserts I should use. I have ran A286, but I here this is harder than that at its lowest rockwell. Any info would be greatly appreciated.

You can run the same inserts, it's not much worse. Whatever you use for your exotics. Lots of positive clearance. I used to cut alot of A286 and MP35n. It's just gonna eat inserts. This is turning, can't comment on milling. Used to have to bottom tap 6-32's .150 deep in MP35n so a screw would bottom. Pure hell...

I know this thread is a month old. However.

In turning with carbide inserts I used 35 surface feet and .0015-.002 feed. Depth of cut .040".

Drilling went best with cobalt high speed steel 118 degree split tip drills. 10-15 surface feet, .001-.0015 feed.

A good rule of thumb is divide everything you would do in stainless by 10.

I believe Carpenter MP35N is the strongest commercially available malleable metal alloy. It consists of 35% nickel, 33% cobalt, 20% chromium, 10% molybdenum, etc. The material is usually purchased cold worked to a hardness of about 50 rockwell C, then machined, then age harden heat treated to achieve an ultimate tensile strength of 300kpsi +.

Still looking for some bar ends or a couple feet of 1-1/8" round.

here's an MP35N part. I just finished giving it a little heat to bring out some color.

hi,
i am reading this for the first time, and would like to know what you tapped with, doing the 6-32's?

Just use taps for stainless, I think hy-pro or exo taps or what ever they are called. Greenfields or Guhrings. They're all in the MSC catalog. Nothing is going to go right through it. You might only get one hole per tap. Drill as large as the handbook will allow.

When I have to bottom tap tough materials I make a series of taps where I grind one pitch off of the lead of a few taps. So I have a rougher with almost all of the incomplete threads, then another tap with a couple of incomplete threads, then a finisher with all of the lead ground off of the tap. But you can't just grind it flat. It needs to be relieved on the bottom to the cutting edge on each flute. I do all of this with a 100 grit wheel on the surface grinder. As you go you can grind the lead off of your "rougher" to make your finisher etc.. Just keep you taps sharp. If you've got a steady hand you can dress the edge of the wheel sharp and touch them up in gullet to get a sharp edge. This is not a job for the faint of heart.

I double nut the taps for the depth I need so I won't be hitting the bottom because there's times that you think you're at the bottom but you're still a full turn away from the bottom and you have to put enough torque on the tap to watch it twist but not break. Very high on the pucker factor!!

Breaking 6-32 taps off in a part that's worth about $17k and is the size of a pencil really sucks!!

Good luck and have fun.