Results 1 to 8 of 8
03-26-2009, 11:33 AM #1
Nitronic 50 or 60 if you have a choice
I have a part to quote that the customer only asks for "nitronic"
Never having cut this stuff before (and after some searching on here) I get to chose, but I am not usre which one.
Also, I read that this stuff will move.
This part will come from 4"Ø x 3" long bar.
Will this part move out of tolerance after, or during cutting?
03-26-2009, 11:58 AM #2
I have some experience with it, not as bad as everyone says.
I don't recall it moving much if you use a CNGP insert ground edge or such with hi-pos geometry.
Assuming this is turning..
I think we turned it in the 140 SFM range, .090 DOC, .012 feed.
Machined pretty well if I remember right, just can't get too froggy with it.
I used to have a pic of the part, it was an exhaust nozzle for some kind of NASA chemical rocket motor test. I think they mentioned Hydrazine
03-26-2009, 12:16 PM #3
What do you have milling wise that will cut this stuff?
03-26-2009, 03:01 PM #4
Nitronic 60 I used to machine all the time for boat prop shafts and rudder shafts. We machined taper, undercut, external threads a thru hole and two keyways per shaft. Sizes ranged from 7/8" diameter x 18" long to 3-1/2" diameter x 20 foot.
I set up to machine basically the same as I would for 17-4ph or 316SS. Sharp tooling, flood coolant whenever possible. Slow speed High feeds and No Dwells. Real sharp chips so avoid stringy chips.
I machined with Carbide and HSS tooling without issue as long as tooling was sharp.
HSS tooling ran about 20-35 SFM and Carbide around 100-150 SFM, feeds and speeds really varied from op to operation and setups.
03-26-2009, 04:54 PM #5
I've never really noticed much difference between machining nitronic 50 or 60. Stuff is stable during and after machining, never had a problem with it moving around. We use inserted cutters plus carbide end mills and drills for milling. For threaded holes we 've had better luck thread milling than trying to tap this stuff. Good rigid setups, sharp tools, moderate speeds and fairly aggressive feedrates to avoid work hardening. If you've got to buy the material Trident is one of the best places in Houston to get it. Good luck.
03-26-2009, 06:26 PM #6
I agree with what has been said already. Seemed very stable. Grooving internally was a chore, rigid and don't dwell. The only milling we did was to mill a hex, so I can't comment much on that. 95% was turning, boring, threading, grooving, facing. We used carbide exclusively.RJT www.progtool.net
03-28-2009, 02:17 PM #7
As has been said, not much dif between 50 and 60. I've machined a lot of ot too. The only thing I could add is if you are deep drilling, it can sieze teh drill. Lots and lots of coolant. Through the tool is best. More pressure (coolant) is more better too.
03-29-2009, 08:13 PM #8
I've cut tons of both, you can run 200/300 FPM with carbide tooling and if you have the choice get whatever is cheapest, but both WILL move under some conditions, we make thin wall .25/.375 thick sleeves out of it a lot and then have to cut a slot in the end for a drive key, if you finish the bore and then cut the slot the bore IS going to go out of round .001/.003, so we rough in the part, cut the key slot, then finish the bore and O.D..