[callganesh]

Hello! I wanted to know the machinability of 430 F stainless steel. what kind of cutting speeds are recommended are recommended for this grade?

Information on the internet indicates that it is a machinable variety. so will it be similar to 1214 steel or at least 75% of it? I am worried about tool life! I had a bad experience with SS316 grade! and I generally work with free cutting steel grades.

Thnaks in advance for your replies

[Geof]

It will be much better than 316L but 75% of C10L14 is too optimistic.

Many stainless steels work harden when they are machined so you normally need to go slowish on the rpm, for 316L I would be as low as 100SFM even with carbide, and you need to keep a good chipload so the cutting edge is underneath the hard skin created by the preceding cut.

I have little experience with 400 series stainless so I don't know if they work harden the same, but if you start out slow with a good cut you may be able to work up from there.

[g-codeguy]

I have no milling experience with 430F, but do with lathe. I rough at 900 SFM with a Sandvik insert, finish at 1100 SFM with cermet, or a little slower with ground PVD insert, groove at 500 SFM with a PVD insert. Threaded a 15/16-26 UNF thread at S1800, but that was a bit slow because of the need to clear a narrow thread relief. Otherwise I could have gone with a higher RPM. That was with a CP500 insert. Very good tool life. This job ran for about 4 years so cycle time was important, but considering the people running the machine, I also had to be cognizant of tool life.

There were a lot of dimensions to check on the job plus this wasn't the only machine the operator was running.

Hope this has been of some help to you.

EDIT: Forgot to mention drilled at 165 SFM F.0052, 1.21 deep in one shot with carbide (no coolant thru). Higher performance drills with better coatings have come out since this was originally programmed so you should be able to increase feeds and speeds if using one of them.