speeds and feeds for .013-.060 endmills

[2929]

Need to cut .030 deep slots in a hardened blade. not sure if ts or ss? max rpm our machine will go is 8,000. We keep breaking endmills. Any help would be greatly appreciated!

 

[mrainey]

Would need to have an idea about how hard the material is. In my experience, anything over Rc45 is a real challenge to machine with endmills. Material hardness is normally the major factor in determining appropriate RPM.

Are your endmills HSS or carbide? How many flutes? What is the flute length?

Are you doing any plunging with the endmills?

By my calculations, slotting feedrates for .062 endmills should be in the range of .0001/.0002 IPT (inches per tooth or flute).



Manufacturing Freeware and Shareware

http://mrainey.freeservers.com

 

[2929]

Thank You for the advice! Iam not sure of the hardness. That is one of our problems. Guessing i'm sure it is over Rc45. Probaly aroun Rc60. We have been using carbide endmills. 4 flute. We start with a .015 loc and go back over with a .030 loc No plunging. The blade is a perf blade set up at a 45 degree angle.Just cutting slots all the way down the blade. Thanks for your help. I just graduated 2 yrs ago from tool and die got a job at a small in house tool room for a plastics company and the only guy that was there quit! This is a great website. What would you recommend for sfm?

 

[EdDanzer]

I don’t think you will have much luck with carbide end milling anything over Rc50. If you must try, use a 2 flute coated carbide end mill at 100-200 SFM and about .0005 feed. The end mill should be as short as possible, 2:1 length to diameter ratio max. Try a shrink fit holder or standard end mill holder, they are more rigid than a collet.

 

[Nate101]

I'd use a TiAlN coated carbide end mill. If you can have corner radii it would help with the chipping also. I didn't see anywhere the diameter of the tool you're using, this is important because you may excede your RPM's, probably not in this case. SFM would be 30-50 with .0001-.0002 IPT for 50-60 HRc. The more flutes the better and a rigid setup. For most applications I'd rather sink it. It depends on what your customer will allow, though.

 

[2929]

Thanks for the suggestions everyone! We don't have an EDM. It's a relativly new shop. Still haven't gotten everything yet. The cutter diameter we are using is whatever the width of the slot needing cut is. .016 has been the smallest and .060 has been the largest.

 

[surfdog]

How about grinding it with a form wheel?