What's new
What's new

Trouble turning and parting off 431 stainless

TommyGunzz

Plastic
Joined
Apr 30, 2010
Location
New Jersey, USA
Hello everyone my name is Tom and ive been on this forum for a little while now and absolutely love it. There is so much great information on here. So i got this job im running right now and I really need some help turning and parting 431stainless steel. I don't have any experience with 431. Burning up and chipping inserts. I'm running this job on our mazak quick turn 250. It's 1.500 diameter 431 staiess sticking out 2 inches from collet chuck. Tools are stuck back in turret as far as possible for rigidity. The company I work for uses Kennemetal. The first insert I tried for roughing the face and OD was a cnmg432mn kcp25 grade. We keep them stocked. Tried between 250sfm and 400 sfm and feed between .01 and .015. DOC range between. 05 to .100. Only made it through a few parts. Next i tried a cnmg432 KCM35B meant for roughing. Tried 300 to 400 sfm .012 feed and .08 DOC and was worse than previous insert. The one in there right now sounds way better. Only got to run 3 parts with it cause it was late in the day. It's a cnmg432mn kc5010 and ran it at 300sfm .01 ipr and .06 doc and sounds really good so far but I'm wondering if I should be using a different grade or running higher sfm? Like I said this insert sounds great now but just wanna use best insert possible. Have to make 300 parts. For the part off tool it's a blade style with a kennemetal A2 style insert. Don't remember the exact part number but it's. 125 wide and the two grades we have are kcu25 which I thought would be good but the geometry unfortunately isn't meant for stainless. It's a CM geometry style and kennemetal book said CF geometry with same grade would be better. The other one is also .125 wide and I believe it's the kcp25 grade. Tried those at 200sfm .0035 ipr with no luck. Right now I have max rpm set to 2000. I'm thinking of bumping it up to 2500. Using Blaser coolant at like 6 of 7 percent. Any help would be greatly appreciated!
Thank you,
Tom
 

FredC

Titanium
Joined
Oct 29, 2010
Location
Dewees Texas
Just looked up 431 and for insert tools speeds for a .15 depth of cut were 350FPM and .015 feed.
For a .025 depth of cut 400FPM and .007 feed. This is from an old Carpenter book, seems like modern inserts should work at higher speeds. Is the material from a domestic source? Positive it is really 431?
They had cut off recommendations on the next page:
1/8 C-6 carbide150-225 FPM feed.004 per rev.
 

TommyGunzz

Plastic
Joined
Apr 30, 2010
Location
New Jersey, USA
Just looked up 431 and for insert tools speeds for a .15 depth of cut were 350FPM and .015 feed.
For a .025 depth of cut 400FPM and .007 feed. This is from an old Carpenter book, seems like modern inserts should work at higher speeds. Is the material from a domestic source? Positive it is really 431?
They had cut off recommendations on the next page:
1/8 C-6 carbide150-225 FPM feed.004 per rev.
Thank you for getting back to me. Was off for a few days for the holidays so just got back to work yesterday. The customer has the material certs for the parts we are doing for them. I'm going to get a copy today. But the material is definitely really hard nasty stuff. It almost looks like a cast on the outside surface but finishes very nicely. Found some kennemetal part off inserts at work and the grade is ment for what we are running. It said 500sfm and .0035 per rev and surprisingly it sounds great. Now not sure what kind of life I will see yet but way better chips At that speed and feed combo. It definitely didn't like the lower speed. Chips were light tan/brown and very stringy. Now they are a nicer gold color an the chip is tightly curled. Still trying to get my cnmg dialed in. Running at 300sfm , .01 feed per rev and .06 d.o.c. don't know how long insert will hold up. I was thinking of switching to a .0156 nose radius instead of .0312. Maybe less contact area would be better. I personally feel with the right insert I should be able to do 500 to 600sfm. Gonna try and get a hold of tooling rep today. Again thanks for your help!
 

TommyGunzz

Plastic
Joined
Apr 30, 2010
Location
New Jersey, USA
I've never ran 431 SS, you might want to send Kennametal an email and see what they recommend.
Yeah I just got back to work yesterday after being off for a few days for holiday. Part off tool running at 500sfm at .0035 per rev and sounds way better. Still working on roughing insert. My boss will be back in today gonna have him get kennemetal on the phone and see what they say. It's some nasty stuff.
 

Blaser Swisslube

Aluminum
Joined
Jul 30, 2009
Location
Goshen, NY
We suggest to try increasing your concentration to 8-10%. That will help performance and, ultimately, the finish. You can always reach out to your Blaser rep, or feel free to private message us and we can connect you with your local rep.
 

Ox

Diamond
Joined
Aug 27, 2002
Location
West Unity, Ohio
Not sure why I didn't think of this earlier: :o

You don't mention if you have a through hole or not.
Cutting to X0 in Stainless in general is hard on cut-off blades.
The tool will last a LOT longer if you cut to .1 to .07 and then twist it off - somehow.
If you are picking off with a sub - this is a none issue - just shut down the sub for a second before pulling away.
Otherwise you may need to program a break-off move, or manually twist it off by hand.


-----------------------

Think Snow Eh!
Ox
 

TommyGunzz

Plastic
Joined
Apr 30, 2010
Location
New Jersey, USA
We suggest to try increasing your concentration to 8-10%. That will help performance and, ultimately, the finish. You can always reach out to your Blaser rep, or feel free to private message us and we can connect you with your local rep.
Hey thanks for responding to my post. I actually did bump the coolant from 5% to 8% the first day we started having issues with the job. We finally got through the first op and currently working on 2nd op. So far this op seems to be going well.
 

TommyGunzz

Plastic
Joined
Apr 30, 2010
Location
New Jersey, USA
Not sure why I didn't think of this earlier: :o

You don't mention if you have a through hole or not.
Cutting to X0 in Stainless in general is hard on cut-off blades.
The tool will last a LOT longer if you cut to .1 to .07 and then twist it off - somehow.
If you are picking off with a sub - this is a none issue - just shut down the sub for a second before pulling away.
Otherwise you may need to program a break-off move, or manually twist it off by hand.


-----------------------

Think Snow Eh!
Ox
Hey Ox sorry that I'm just getting back with you, but I definitely appreciate you responding to me and giving suggestions. We just finished the first op on Monday and now we are on 2nd op. We are running blaser coolant and I have increased the concentration from 5% to 8%. We were parting to centerline and I actually had thought of doing what you said and parting to .1 and breaking it off. We ended up parting to like .500 with a kennemetal A4 style insert and then came I with the A2 style insert on a blade the rest of the way. It went really well once we did that and had the speed and feed right. This was some of the nastiest stainless i have ever cut. As far as roughing the face and OD I decided to use a wnmg 432 to get underneath the skin of the material which I felt was the worst part of it. The cnmg432 seemed to last much longer afterwards. I figured that adding a preliminary roughing tool and using two part off tools was better than trying to change inserts every few parts. Currently running 2nd op in an emergency collet. We rough the face which only has .02 from first op but has a little nub as well, then we come in with a .562 insert drill and then rough bore, finish bore and finish face. So far so good.
Thanks again for your help.
 
  • Like
Reactions: Ox








 
Top