What's new
What's new

Machining Hardened 17-4 Rings

Orange Vise

Stainless
Joined
Feb 10, 2012
Location
California
1)Saw the raw stock into 10" chunks
2)Send to HT
3)Part them off in your cnc lathe
4)Make big monies.

+1 on this.

One step I might add, after sawcutting, is predrilling the ID with a 1.5" indexable. Hit it from both sides so you only need a 6" drill.

17-4 is easier to drill in Condition A, IME. Also, your max material thickness gets reduced significantly, making heat treating faster and easier.
 

plastikdreams

Diamond
Joined
May 31, 2011
Location
upstate nj
Any reason I can't drill it with High speed steel and then finish with a boring bar?

There's no reason you can't. I've drilled many holes in 17-4 with hss drills, uncoated. You can probably get a little more life getting coated drills, but really it's not worth it.

17-4 isn't really bad to machine, after doing it every day for a few years it became my favorite material to work with. Once you figure out how to do it and how it reacts you'll find out it's good stuff to work with.

For some reason there's an aura with this stuff that it's really hard to work with, it's not. Good carbide cutting tools, air blast cooling, and steady feed rates are all you need.
 

Ianagos

Stainless
Joined
Sep 23, 2014
Location
Atlanta
Sounds like gravy work to me. If you don’t feel comfortable feel free to sub it out to me. I absolutely love turning 17-4. Makes me look good when the customer just receives mirror shining parts.

Here is a simple part done in h1050 which is very close to your h1025.

Picture doesnt show it too well but part looks beautiful
4003d45710d65b5abe84fcb6fad1468e.jpg
 

plastikdreams

Diamond
Joined
May 31, 2011
Location
upstate nj
I remember my first real machining job. I had broken a carbide tool, so I grabbed a has endmill...and quickly turned a 4 flute square endmill into a ball endmill lol. Quite a amazing how 17-4 will chew the wrong tooling up.

One thing I learned is high helix (45°)) endmills will clog much faster than 35° regular or ,my favorite, variable helix endmills. Much better chip evacuation. Recutting 17-4 will net you a broken endmill quickly.

As far as drilling, fast steady pecks, no dwelling, and make sure you keep chips out. Look at the color of the chips coming out, you want golden color, if they start turning rainbow you are pushing it too hard.
 

Ianagos

Stainless
Joined
Sep 23, 2014
Location
Atlanta
Did you just buy it heat treated and machine or heat treat then machine?

I do both. If it needs certs I get it done professionally. If no certs required I heat treat in house and hardness test. Have nist traceable standards etc for hardness tester.

17-4 is very easy to heat treat.
 

Ianagos

Stainless
Joined
Sep 23, 2014
Location
Atlanta
Thanks for all the insights. I am gonna order some hardened 17-4 from McMaster and do some test pieces this week.

Funny enough for finishing I’ve had great luck with some inserts for stainless from shars. That chinesa $5 insert beat out the more expensive Kyocera stainless specific stuff and another name brand I can’t remember.

If you need the grade let me know I can try to see if I can find it. It was a black purple insert vnmg
 

Ianagos

Stainless
Joined
Sep 23, 2014
Location
Atlanta
How come you guys use v's ? I hate those things. Are you plunging in on contours or something?

I tend to use a lot of vnmg for finishing and I can plunge for thread reliefs. Mostly an old habit and I had inserts and holders.

I do a lot of prototype and small batch runs so I don’t fight for the best tool life just the most versatile tools. Have my 40 tool changer full and the lower turret full.

I used to use a ton of dnmg for roughing but we are starting to move to cnmg these days.

Also why do you hate vnmg inserts? I just have a tiny machine nowadays so no huge cuts for me anyhow. .1doc .012” per rev is the most ill typically do

0b0570a402737b575a383104a9d1a780.jpg

I also like these types of holders because I can face with them then index the tool 180 degrees and turn with it.

Can also do b axis count oring but I’m too dumb to know how to do that
 
Joined
Apr 14, 2018
Location
Airstrip One, Oceania
I used to use a ton of dnmg for roughing but we are starting to move to cnmg these days.
Yay cnmg 543 :)

Also why do you hate vnmg inserts?
Because they are so fragile :( My pref was cnmg for roughing or even finishing, push it hard, then if there was contouring to do, sandvik knux. Dnmg if I absolutely had to.

But we're probaly talking different part sizes ... I'm more in the 3" to 12" size range.

I just have a tiny machine nowadays so no huge cuts for me anyhow. .1doc .012” per rev is the most ill typically do
Had a South Bend Cyclone as well, usually would try to use positive rake in that guy. Still avoid vnmg, they are fragile even taking baby cuts. Maybe I'm just too aggressive with doc ...
 

Brett W

Aluminum
Joined
Jan 10, 2014
Location
Huntsville AL
Last Xmas time, I picked up some CNMG inserts from HAAS that were for stainless and some I labeled "Titanium", but I suspect they are for harder to machine materials. I will probably use those for the test and see how how they do. Will need to switch my boring bar over to one of those for this job, (maybe I burn all of them up and look for something else, LOL)

Does 17-4 machine like 304 or is it much harder?
 

plastikdreams

Diamond
Joined
May 31, 2011
Location
upstate nj
Last Xmas time, I picked up some CNMG inserts from HAAS that were for stainless and some I labeled "Titanium", but I suspect they are for harder to machine materials. I will probably use those for the test and see how how they do. Will need to switch my boring bar over to one of those for this job, (maybe I burn all of them up and look for something else, LOL)

Does 17-4 machine like 304 or is it much harder?

17-4, even annealed, is easier to cut than 304. 17-4 machines like tool steel. It's very consistent cutting as well.

Get a piece and experiment.
 

MaxPrairie

Hot Rolled
Joined
Jul 9, 2015
Vnmg is less nose contact than C or D. Can help if you have problems with chatter on a long stickout and no tailstock. Also, thread relief.
 

Brett W

Aluminum
Joined
Jan 10, 2014
Location
Huntsville AL
Got my 1in hardened bar in and did some turning, facing and threading last night. This stuff cuts really nicely, although the chip is more of a tightly curled string, it threads nice, seems to drill OK. I think I am going to bid the job and plan for the process. Should work out nicely.

Thanks for all the info on this material.
 








 
Top