[RussMachine]

Hey guys,
I have a job coming up for some parts milled out of 17-4Ph Stainless.
Basically side milling, opening holes via helical milling, Chamfering, maybe some drilling.
Anyone with experience running 17-4 in the 770?
I'm hoping to use 3/8" end mills for this job.
Coated Carbide i'd assume.
SFM? Feeds & Speeds?
Any good, recommended End Mill brands?
Fishing for knowledge here.

[jwatte]

I've only cut a very small amount of stainless, on an 1100, so I'm mostly repeating what my elders told me :-) (And it worked.)
Are you getting it in heat treated or annealed condition? Annealed apparently needs quite low speed because it's soft and gummy.
If you get it heat treated, you don't need to worry about shape shifting after the part is done, and it won't work harden. Then cut it as hard alloy steel.
Although online, people say that super aggressive feed can make up for the gumminess and slow speed. Try at your own risk!

[GLCarlson]

There's a NYCCNC video about cutting 4140, and I think one where he cut some other tool steels (S2, maybe) and another where he did some stainless. Take a look at those for speeds & feeds.

EM brands. Lakeshore Carbide, Tormach, Maritool have all sent me excellent quality tools. Tormach tends to be lowest cost. Lakeshore will provide advice if you call.

I don't do much stainless, and never 17-4, but a comment on mill size. I kept trying to use bigger diameter mills on steel for a long time. Eventually, NYCCNC videos convinced me to use quarter inch and push 'em harder. That seems to work. For sidemilling S&F, aim for a minimum 1 thou cut per tooth, stepover of 0.2 of tool diameter or a bit less, DOC up to 2xD, and start out with the published SFM (for steels, 60-200 sfm, 80 is the book for 17-4). That'll get you in the range, adjust from there.

There's a useful thread over at Practical machinist that has a comment about the more aggressive conditions.
17-4 ph stainless steel machining ?
900 SFM(!), .01D cpt, .06D WOC. 5Krpm, 200 ipm. Wow.
They included a video

https://www.youtube.com/watch?v=luxYaX2n9p4

[Peter Neill]

I did a test run a few years with pre-hard stainless on th 1100. Used feeds and speeds from HSMAdvisor (which was a little scary to start with...), but ended up with quite an amazing performance!
Small write up with pics, wish I'd had a camera to film it at the time.
https://www.cnczone.com/forums/torma...4-tormach.html

[jwatte]

900 SFM(!), .01D cpt, .06D WOC. 5Krpm, 200 ipm. Wow.

The thing with "high speed machining" is that it's not just pushing a regular cut a bit faster.
It's pushing way past the barrier of regular cut physics, to the point where most of the heat escapes in the chip, rather than into the tool.
So, you can't get there by bumping up a little bit at a time; you'll run into the overheat hump on the load curve.
You have to jump all the way across that curve to the point where it comes down again.
The problem then becomes one of RPM limitations (770 goes to 10k RPM, so better than 5k for the 1100!) and horsepower.
Quoting the video comments: "This placed the 30 hp haas in a 200% load."

[IMT]

I've done quite a bit of 17-4PH on my 1100. LSC variable 4 flute 1/4" EM works good. Use high efficiency tool paths, low WOC (~.030) high DOC (up to .375) and calculate the correct chip thickness due to chip thinning with the low WOC. Also pay attention to the effective WOC on inside corners, if you try to do a .180 rad corner with a .125 rad (.250 dia) tool the effective WOC becomes much larger (and thus the chip thickness) and the material is not forgiving.
17-4 machines nicely in condition A or 1150 (~35HRC) and isn't particularly gummy.