Hard-Milling

[Diedesigner]

Group,

 

I have a good friend who is working in a job shop for the first time. He isn't used to the aggressive approach the shop takes when it comes to milling (time is money.) He asked me for some guidelines for milling hardened die steels like A2 or M2. The hardness is Rc 60-62.

 

In my company we have always been on the conservative side with hard-milling. For uncoated carbide we always start at 50 sfm and take light cuts around .010 to .020 deep. Since his shop is much more aggressive than that, I am unable to give him anymore than that mentioned above.

 

Can anyone share some good starting points for aggressive hard-milling with uncoated, coated, flat, bull, & ball nose carbide end mills? I am looking for recommendations for feeds, speeds, and depths of cut for various diameters. The application is mostly 2D work on tool & die components though there may be some 3D contouring also.

 

I am not asking for any proprietary information, just some good starting points I can forward to my friend.

 

Thanks in advance for any help you can provide.

 

Regards,

 

Chris

[Guest CNC Apps Guy 1]

Well, Robb Jack, Sumitomo Carbide, Mitsubishi, Kobelco (sp?), make some outstanding Hardmilling cutting tools. If running Ball E/M's I usually run full throttle on the RPM and chip loads between .0005 and .002 depending on different factors (Tool Size, ROughing or finishing, hardness, etc...) DOC usually no more than 10% of diameter. Stepover depends. On flat tools 40% max usually. Bull nose and ball will depend on what I'm after. Coated E/M's have worked better for me than uncoated.

 

In many shops today MRR is the name of the game.

 

HTH

[Midwest]

An article I read a while back might help.

 

Magazine

 

November 2003 issue

 

The article is called "Cutting Tool Selection Impacts the Outcome of Hard Metal Machining"

 

Nice article with charts that might help answer a few questions on hard milling.

 

HTH

[Jean-Simon]

Hi Chris, I've machined A2 and D2 (60-62 rc) a lot and we were using OSG 60deg helix 5 flutes end mill and the chips were flying like if it was soft, full depth of cut but 5% (of tool diam.) for the radial cuts, I was following the feeds and speeds of the book (yes it's true), if I remember good, it was around 60 ft/min and around .001 chip load.HTH!

 

Simon

[Midwest]

Here is the

 

Article

 

Hope this works they want you to subscribe to get to the articles. It works for me but I am logged into the magazine web site.

[DavidB]

Hi,

I would deffently use coated carbide dry with air/oil mist if possible.If not just air.Removal of hardened swarf is number 1.

 

The part should be roughed and semi finished before hardening leaving around .4/.6 material depends on hardening process and part shape.

 

I would then take a another Semi Finsh cut leaving no more than .15mm even tool load for finishing is recomended.

Try using Ballnose and Bull cutters where possible,stay away from machining flat ereas with endmills oly use the side and use a high helex.

With good quality cutters machining this hardness it won't be a problem and the surface finish will be great.

 

Have fun

[DavidB]

quote:

---

full depth of cut but 5% (of tool diam.) for the radial cuts,

---

This is perfect and a great method.

 

When machining a pocket use pocket true cirle even if its not a circle this is the only pocket method that wont take a full Diameter of cut you will get some fresh air cutting but it works gr8.Go full deepth and step out 5%.

 

Try same method when soft and step out 10% watch the swarf fly.Always inpresses the boss.Run dry and plenty of air.

 

[Fig sign]

Y-G Xpower is very good for more then 60 HRc.

Iscar is not bad ,but better for 56-60 Hrc.

 

My speed is approx 45-55 m/min and feed is 0.01-0.025 per teeth .

For 8000 rpm I feel myself like my friend Pooh with an empty pot ,sometimes I need 12000-15000 Rpm and more .

 

HTH

[Guest CNC Apps Guy 1]

Run Dry +1000

 

Your tools will eventually shatter like fine china running with coolant.

[Hardmill]

Try starting @ 600-800sfm w/ .0005 - .0015

chip load, full depth about 5-10% stepover.

With a coated mill, "Just like my avatar".

That ought to get you started.

 

PEACE