tools for hard stainless

[67 Yankee]

Is anyone here cutting much 17-4 cond H900? I have a customer wanting a part that has to be cut from 17-4PH Stainless in the H900 condition, which looks like about HRC 44. The part will be cut on our Haas 5 axis VF5 machine from a 4"x4"x8" piece of barstock, about 90 percent of which will be milled away. Maximum tool reach required is about 2.5" and there are several .25" deep pockets with .125" inside corner radii and .125" fillets on the floors. The majority of the part could be done with a 3" face mill ( or 2" or 1" depending on what I find out), and the pockets can be cut with 3/8" and 1/4" solid carbide bull and ball endmills.

 

We don't do much stainless at all and have never cut from the hardened condition so I'm at a bit of a loss for tooling selection. Also it's only one part and I'm not eager to call in a bunch of tool reps to come and talk my ears off.

 

Thanks.

[Rick Henrickson The Boeing Co.]

duramill whispercut 3 and 5 flutes are great

[?Mark]

We do 17-4 ph daily but in annealed condition. I think it ends up as H900 after heat treating.

Tough to machine but have best luck with varimils.

It's been a long day here, but I think H900 is actually better for indexable tools then annealed.

anyhow, nice and sharp varimils should do the job.

 

hth

[Colin Gilchrist]

Data Flute has some pretty good cutters for Stainless. I would go with a 5 flute if you can. A good coating will go a long way towards helping your tool life. Call up data flute and ask them what coating they recommend for 17-4 H900. Don't ask them about cutters unless you need the info. That should keep the jabbering in your ear down to a reasonable level.

 

HTH

 

Colin Gilchrist

The Boeing Company

MR2 and Beta test site

[crazy^millman]

Look to the Hitachi Volecity cutters. I think you could get away with 650 sfm and 240 ipm with about a .06 to .08 depth of cut.

 

HTH

 

Varamills from Hanita, Data Flute, Fullerton, Calforina Tool, Dura Nill, G.W Shultz, and few other Carbide endmill makers have products that can cut this though some do better than others and though the good ones cost money they are worth every penny.

[heavychevy2155]

it is on a haas though.

[heavychevy2155]

cutting stainless can be a pain on a haas, I know I cut 304L on one all the time. Spend the money on the good tooling and it greatly eases the pain. I dont dry cut just good coolant flow, and Blaser coolant helps also.

[connormac]

Iscar coated carbide works well. My boss said he cut some 17-4 ph dry and got very good tool life.

[jeff]

17-4 will cut like butter with the right tool, and right speed/feed.

Since you only have 1 pc, just use what you have,and you should be fine.

save the money for future tooling.

But if you are looking for an endmill to do the job,I suggest the Varimill from Hanita like others have posted earlier,these things are awesome in many types of material.

and they run best when cutting dry.

 

17-4 is a remarkably stable material,I have cut many thin walled parts from a solid piece and when unclamped it didn't move .001

 

Although it was annealed.

[gcode]

The Sandvick Coromill 210 high feed face mill line

will blow your mind.

They work very well with Mastercam's high speed core roughing toolpath.

Suggested feeds and speeds from Sandvick's

Metalcutting Technical Guide

460-690 sfm

.016 to .059 feed per tooth (depedent on radial DOC)

.04 depth of cut

 

btw.. the Sandvick Metalcutting guide is an excellent refenece manual and deserves a spot of every programmer desk... and its free.

[67 Yankee]

I've done several small jobs from 304 and annealed 17-4PH but never the heat treated 17-4 and none that produced 30+ pounds of chips. I've used whatever I had hanging around and it has usually been a pain. Since this is going on our very busy and only 5 axis mill I need to buy the right tools to make the job as painless as possible. Of course it will be great to have those tools on hand for future stainless jobs too.

 

Looks like I'll be checking with the Sandvik and Hanita folks today.

 

Thanks a ton guys.

[Jean-Simon]

I do this type of material regularly. I had good results with sandvik 390 2" 7 inserts (11mm) and also variable helix end mills from Guhring serie 3114 or Destiny raptor dvh(double variable helix). I run around 120-130 sfm with 0.003/tooth to get a decent tool life.

HTH!

 

Simon

[ALEX888]

Check out the Mitsubishi AJX type high speed milling insert cutters.

We use one on 316 sst 2.5 diameter cutter 170 IMP .060 depth of cut 1.75 width

That will run for 1 to 2 days before we have to index inserts. We run it dry on a Haas vf3

And it is just amazing. You will need to run it slower for the harder material but you can remove a lot of material fast and cheap. I am sure a local rep would love to demo this tool.

 

 

Alex

[Gary]

I use yg alot cheap stuff taln coated nothing fancy they work well. I have a heck of a time slotting without coolant (tool loads like aluminum) so I use it with good tool life. We cut in the 37-40rc 17-4 daily

[Lars Christensen]

nosserøv, I do not hope that is your nick-name around the shop

[67 Yankee]

Haha, no Lars, that was just something I ran across one time that struck me funny and seemed easy enough to live up to. Besides, it has that cool ø in it that's not on my keyboard. Just makes me that much more a pain I suppose but I don't take things too seriously.

 

Thanks again for all the advice guys. I ended up talking to the Sandvik guy and the Mitsubishi guy. Looks like Sandvik is going to be the winner since the cutting specs are so similar and the Sandvik tool is a good bit less expensive.