Machining hardened stainless - 17-4 H1075 (approximate)

So I have very little exp with stainless, not to mention hardened stainless. Anyone with experience care to share feeds/speeds? Will be milling and drilling and tapping. I think the setup will be rigid, machine is a new Mazak.

I'm looking at HSMadvisor for a face milling op and it seems very slow to me.

Not sure how to make that bigger, but the numbers are .120 doc (question about that to follow) 311 rpm, 5.71 ipm, ,0045 ipt with a 50mm insert face mill. This has the speed and feed slider at a tad over 100% and tool life at 78%. If I crank the sliders to 150% I get 434 rpm, 11.07 ipm, .0063 ipt and tool life down to 32%. Do these numbers sound right? At these numbers that is only 224sfm which seems low to me, but like I said no exp with this stuff.

Also, Sandvik recommends light depth of cut and fast feed for face mills, here about half way down the page https://www.sandvik.coromant.com/en...erials/milling_hard_steels/pages/default.aspx
I know on trochoidal(?) milling that is right, but does that sound right for a face mill? I will be doing an approximate 80% stepover. Can I take .12" doc like that, or should I split that?

How about solid carbide end mills? Still in the 200-300 sfm range, or..?

thanks for any help

H1075 is not hard, about 30 Rockwell. Machines fine.

.120 DOC should be okay depending on your setup, 300 rpm is pretty slow. I'd probably start around 500- about 250sfm. Same with end mills.

The 17-4 I cut is H900. And yes, face milling is the slowest part. How big is the part? Sketch or drawing?
Small carbide end mills, run fast, using HSM paths is the best solution for my part, even some area that could have been cleared using larger tools. You should be able to go a lot faster than I can, since it's in an easier to machine condition. I also used HSM Advisor to get started, but was able to increase tool life/decrease cycle time with more rpm and faster feed. YMMV. The small carbide end mills last a lot longer with a radius/chamfer on the corner, and the right coating. Got mine at Mari-Tool.
I used to use OSG when I had really nasty hard stuff to tap.
I know other guys will be along with ideas...
good luck!

I've done 17-4 heat treated to 40 Rockwell. I used Emco carbide endmills at their recommended feeds and speeds and they worked great, good tool life and low spindle load. Face milling is slow. Start with what you got, and nudge it up slowly until it sounds good.

I've done a bunch of H1025 H1050 17-4 over the years and been able to successfully run 250-300sfm. Usual mix of inserted and solid carbide tools.

Did a batch of muzzle brakes with H1100 (which simply means tempered@1100°).
They came out looking beautiful. The pile of broken carbide: not so much.
Only trouble was with small tools; .187 endmills drilling and milling plus small (3/8") boring bars and solid carbide threading.
303SS for sanity's sake.

We mill that everyday. I like HSM toolpaths 5% radial step, full depth, 250-400 sfm, 50-120 ipm depending on the size cutter and conditions. I would not want to tap that. We use thread mills exclusively. I agree that face milling this is slow. I think .05 - .09 would be a better depth for a big face. My favorite tool for that is a 3/8 7 flute emco with a .06cr.

Thanks guys, I appreciate the info. I will start with 250sfm and see how that holds up. I wouldn't normally think 40Rc is 'hard', but was unsure being stainless. Milled lots of A2 in the mid 50 range so I know with the right tools/speeds you can get good results, just wanted to ask the PM crowd. I am getting taps from Emuge and Guhring that are supposed to work... we'll see.

17-4 in that range is quite pleasant to machine really. Turning and milling it cuts much more like an alloy steel than a stainless, nice finishes pretty much come free, and it's not particularly hard on tools.

However, it is not so cool to drill and tap. Form tap or threadmill, I have broken quite a lot of cut taps in 17-4PH and I avoid using them now.

X2 on the roll tapping.

To make it easier to search, it's Imco, not Emco: IMCO

And I'll take working on that hardness 17-4 over most stainlesses.

Booze Daily said:

X2 on the roll tapping.

Click to expand...

Get your diameters and lubrication right, and this works. Make sure the customer is OK with formed threads.

I cut 17-4 H900 all the time. I found I get better material removal rates and much better tool life dynamic milling with solids rather than using inserts. I use Helical cutters for anything over 1/4", and the Helical Milling Advisor in addition to HSM Advisor. Sometimes the two show a fairly wide difference in parameters.