Machining Rc54-55 Steel

[triumph406]

Sorry for the double post, the title I revised to hopefully garner more answers.

I have an Aermet 100 maching question for the forum.

Due to a fatigue issue we are trying to avoid, we have made some parts from Aermet 100, and in the critical areas we have left .015" of stock to be machined off after heat treatment. This is so we can remove the de-carburised layer and obtain the best possible fatigue life in the critical areas.

We will be heattreating be Rc 53-54 (285'000psi)

In peoples experience what type of tool (I assume some grade of carbide) and associated speeds and feeds were used to machine Aermet in the heattreated condition? (I also assume that I'm not going to get very good tool life)

Thanks in advance for any advice

DC

 

[bugnut]

CBN is a product which all is recommend for hard turning. See the website below.

http://www.abrasivesnet.com/en/product/mbs/bzn/g.ht

 

[triumph406]

Thanks for the link Bugnut, unfortuantly we will be milling the part. We are looking at using coated carbide tools, I am wondering if there are specific grades we can use in our situation.

Thanks again dc

 

[tripleZ]

Pure carbide milling cutters, but you may have to play with the cobalt (binder) content to get the right mix for the material. I've personally never played with Aermet, so I can't help you there. Talk to the cutting tool manufacturers. Any hard milling I've done has also been on a machine with a high-speed capable milling head (with decent HP) to boot. I've never managed to get as good results with the standard CNC machine. Chatter and busted cutters can be commonplace.

Mikron makes a fairly decent machine designed specifically for tight-tolerance hardmilling of mold cavities. Check the specs on that machine and compare it to yours and see what you come up with. Without the rigid head and whatnot, the geometry of the part might require some creative dampening/clamping forces.

 

[swall]

Since you have a fatigue critical part, you need to be aware of the possibility of surface damage due to abusive machining. Never used to think it was a problem with milling, compared to grinding, until I saw some fully hardened 300M components fail the post machining nital etch inspection for "grinding burn". Subsequent metallographic examination revealed bands of softer material caused by the localized heat from milling.

 

[EdDanzer]

We have face milled hardened steels with ceramic inserts at a lower cost that 4140 annealed with coated carbide.

 

[tripleZ]

EdDanzer...any specific ceramic insert or cutter recommendations? I'm turning sintered powder metal parts. Macrohardness reads in the Rockwell "B" scale. Micro or particle hardness hits in the vicinity of 55 Rockwell "C". I'm getting away from TiN & Hardlube coating my carbide cutters/form drills and using some of the funkier coatings to increase wear resistance. Any other suggestions you have for testing would be much appreciated.

 

[EdDanzer]

For turning or milling Kennametal SNG443T K090 has worked for us. A rigid machine and setup are required. 300 SFM and .003” per rev. or .002” per tooth should be a good starting point.

 

[triumph406]

swall,

when you talk about grinder burn, were you cutting without cutting fluid?

We use a synthetic soluble cutting fluid, I hope we could avoid the same issues if we flood the part adequately. We will also be using small endmills (maybe 1/4 dia max) so I don't think we would generate that much heat. (I hope)

We probably ought to cut down the speeds and feeds to generate less heat.

Thanks for the heads up!
DC

 

[WIPLASH]

YG cutters have specific e/mills for harder materials I followed their recommendations and dropped cycle time from 45 min. to 22 min. on a part that was rockwell 55. I did use a lot of tools thow.Still the drop in cycle time payed for the cutters and I was done sooner than had alotted for machine time.

 

[WIPLASH]

http://www.Yg1usa.com