Has anyone ever machined this stuff?
What could it be comparable to for the sake of quoting a job?
Similar to your other PH grades. Don't just guess on the material price, whereas 17-4 is around or under $5 a pound, 13-8 will cost you $11-13 a pound, 15-18 in rectangular bars. I'm not sure where 15-5 fits in, probably on the high side since it doesn't seem to be used much. Machinability, a little tougher than 17-4, but not as bad as 13-8.
I have machined a TON of 17-4 and 15-5. Boeing specs say that 15-5 may be used in place of 17-4 but 17-4 may NOT be used in place of 15-5. They are VERY similar to machine.
Turning, I've heat treated up to 180-200 ksi and machined with no issues. Most of the mill work I've done that needed to be heat treated, I've machined to finish and heat treated with the exception of some bores that were close on clevices but you'd want to bolt in spacers and such for that anyway...Hope that helps
15-5 is vacuum melted 17-4 which insures removal of all impurities.
It looks like you all agree it is much like 17-4 but,unfortunately,I have never machined that type of SS either.
My experience has been pretty much with 300/400 series SS.
My concern about the 15-5ph is the machinability factor.Is it going to give me a heck of a time?Will high speed or HSS CO end mills touch the stuff or am I looking at using carbide only?That's a big thing considering the tooling needed will mostly involve roughing & finishing end mills 1 - 1.25" diameter with at least 4" of flute.
Here's a way I would probably relate to it,,how much tougher or not is 15-5ph to machine compared to say 304?
Hey Jim (PBMW)
Just curious what size parts (thickness) you have made out of 17-7 and how the heat treat affects the tolerance?
I have heard 17-7 is pretty good for holding tolerance after heat treat, but I am wondering how much it moves?
I would have to go look but if I recall correctly the 15 is chromium and the 5 is nickel
same with all the rest of those like 13-8, 18-8 etc and the PH is precipitation hardened.
I think the 15-5 and 17-4 machine a little easier than 304. I haven't used HSS on stainless in a long time but machinerys sez: HSS wants about 55 sfm for milling and carbide between 210 and 585 sfm both of them feed between 4 and 7 thou per.
That would match my experience. I have had very good luck using Iscar helical inserts in a single fluted endmill for roughing. You can really crank up the feed if you calculate the radial chip thinning.
I've cut some shafts from 17-4 that were turned to a half inch with a three inch flange in the middle that was about .080 thick and they were fine as I heat treated the bar before turning them. (I thnk they went about 180ksi) But got a bunch of them rejected from mag for delta ferite indications. remade them from 15-5 and that problem went away
I think this stuff moves less in HT that say 4340 or 4130. I did some pins that were 5" dia and about 21" that would grow .0007 per inch made from 4340. Get into thin wall stuff and I think it's easier to machine after HT. I almost always turn after HT. It's not that hard.
You should be OK with Co endmills, I've had good luck with Co roughers at about 75sfm with 17-4. The long Co finishers on the otherhand didn't last too long, though the machine was a big piece of spaghetti noodle. If you are running a decent machine(not from the 70's) you should be OK.
You didn't say what heat treat your parts will go to, I do know that 17-4 at an H1150 is actually harder than when you get it, but it cuts so much easier. I'm not too keen on H1000 or lower.
As for another question about heat treating, the PH grades are used because they don't move much when heat treated. They only come up to a fairly low temp so distortion/expansion/shrinkage is basically a non-factor. I may be off or just plain wrong on the temp reasoning, or the usage, but they pretty much don't move.
PH alloys come in the alpha condition. This is achieved by heating and soaking at over 1900F if memory serves. The H number used to designate the heat treatment indicates the temperature in degrees F. This stuff is very nice to cut after heat treat. Even at H950 which gives hardness in the low 40's Rc, it's clean cutting if the tool geometry is positive and sharp. If you have to tap, use a tap with a helical action. Gun taps for through holes and helical flute taps for blind holes. Circle grind away the teeth leaving only 3 or 4 complete threads behind the cutting part of the tap. This will reduce torque load caused by the stock "closing" in on the tap. I like Crisco for tapping.
I've machined stuff as large as rotor blade adaptors used to balance Chinook and Blackhawk blades in our whirltowers. These things started out too heavy to lift and weighed only 20 pounds or so finished. Because the PH alloys are so stable you can take a workpiece to net size before heat treat a lot of times.
One caution: the stuff is useless for any purpose unless it is heat treated. In the alpha condition it is very prone to stress cracking.
Im in the same situation as Metal Slave. Will be looking at machining about 150 parts a month of 15-5 14"x14"x3" and am looking for handy advice for heavy duty roughing of this stuff. At the moment the only little success i have had with roughing is using a SECO 50mm 12mm round insert (MS2500 grade) face mill. Using the round inserts as a scallop 200mm x 40mm needs to taken out (a hell of a lot of material). I am running it at 95 cutting speed with 1.5mm DOC and o.2mm chip/tooth. I tried same cutter but 63 at the similar figures but insert life low. Set up and machine is quite ridged. Would you be able to offer some advice with roughing this stuff.
15-5 you want to heat treat first then machine to finish spec.
15-5 annealed is gummy like 304 but when heat treated it will chip nicely and give sweet finishes. I use carbide all the way with this material and drilling I have used CO with low SF.
I see your in CA. give Xceliron a call. He is here in Chatsworth and his tooling is made for these tough stainless materials.
15-5 and 17-4 cut like butter as long as its under 35RC. I have several videos showing what can be done with 17-4. We havent done a bunch of 15-5, but use the same parameters. Keyword search on youtube for my channel is "jamesu229".
The butter part I'm not sure about, maybe butter that has just come out of the Fridge but I agree that the stuff is good material to work with and I would prefer it to both 304 and 316 especially if it is H900 or above. I can't understand why you would even consider using steel tools, this is a tough material and it needs high performance tools. We regularly do high speed milling on our turn mills in this material and typically run the mills at 600 SFM and 10% step over. We get great predictable tool life
Originally Posted by jamesu229