Turning and threading 17-4 PH SS
I have milled 17-4 PH SS in the annealed state several times without too much problem. I had to do some turning and single point threading this week and got a piece of 2.5" round in the annealed state. I had to turn extremely slow and single point threading was a bear. Should I send the rest of the bar to heat treated before making any more parts? To what state should I HT too?
I used to cut a lot of it in the H900 state I believe and it machined well, better than annealed for sure. I wanna say that it came back in the mid 30's on the C scale, but it's been a few years since I cut it and I'm too lazy to look it up at the moment, being friday after lunch and all Gettin close to the Rockies at the moment!
I am doing it right now .. it is slower than steel , but not slowww.
If you have carbide, positive geometry( sandvik 2025 grade ) , a lot of oil-coolant.
For threading Iscar(908 grade) single point threading insert ...
You should fly
I am surprised with tool life i am getting from my tools .. holds size perfect
Are you using annealed or HT? I was only running 160 sfm. And threading was at 50 rpm with a bazillion passes to keep from breaking the insert.
In past six months i run i run it in every conditions... I was scared , but realy did not have any problem
For roughing i believe i am running about 280SFM
I live just .01-.015" per side for finishing pas . I have 1600 RPM for .425 " diameter ( using 35 deg-V insert R.015 Sandvik 2025 grade ... i do not have calculator to calc. SFM
For threading Not sure 100% but something about 1000 RPM on .475" dia.. i am cutting 28 pitch about .008-.01"(total) per pass. I use to cut 56 pitch on H1150 maybe .006" per pass
I can give you exactly Monday.
Thread last about 1000 pcs
Finishing tool 1500 pcs , part is long 2" ( .4 threading length)
I've run heat-treated condition 17-4 at 375sfm with no problem. Using Valenite VP9605 grade in a CNMG432M5, .150 d.o.c. @ .016 ipr. Excellent tool life, perfect chip control. Almost like I was turning steel.
O.D. x .2618 x rpm
Originally Posted by IndGild
If you have a computer running WinDoze, you have a calculator. Now you have the formula. You were running 178 sfm.
Agreed. 160 sfm is far too slow for turning, and 50 rpm is only appropriate for a manual machine with a HSS threader. For coated turning inserts, start with 400-500 sfm & CSS. I usually single point thread @ 600 to 800 rpm. The stuff we have Rockwell's @ 34 on the C scale. 17-4 usually does give you a nice surface finish.
I believe H900 is 40-47 HRC, don't know of the top of my head the H# for the mid 30's but that is where 17-4 cuts nice at. Not that 40-47 is impossible, but not as nice to work with.
Originally Posted by Kris P
I'm thinking you want H1000 or H1050.
A bug misconception about SS is that it is hard.It's not hard,it's rather soft and gummy.Most of the time on SS if your tools is braeking your running too slow.I run it at 430 SFM for roughing & 575 for finishing & 550 sfm for threading.
Originally Posted by walesham
You can certainly make SS hard.