Hard milling

[Peccator]

Can anyone shed some light on hard milling? I have a job coming up and I don't know a lot about this area of machining.

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

The material will be 440C stainless hardened to 52-55 Rockwell.

The Min Z will be -.145.

Tooling... .0625 to .0156" ball and flat end mills.

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

With the research I have done I have found that for hardmilling you need to use TIALN end mills and run them dry.

The last time we ran these parts they were 416 stainless at 28 rockwell. The boss said they were the best he has seen in his shop. But, they need to be better. We are looking at fixturing with electromagnetism because the parts will be half round.

 

The yellow, orange, green and red surfaces are to be machined on this particular part.

 

I can't save to the FTP. If anyone is interested in looking at it.

 

[JAMMAN]

I use TIALN coated carbide end mills in the range of .012" to .035" (mostly for glorified drilling) and get 5 times the life of uncoated end mills. Run e'm dry, lots of RPM, blow them with air.

 

My opinion.

[Peccator]

Failed to mention we will be running a speeder head upwards of 20,000 rips. Looking into every option for speed. Even perhaps buying a new machine.

[Eazy]

+100 for TIALN. We use coated tools for all our finishing work. I've cut up to 60 Rockwell without a problem. I run them with coolant and dont appear to get any better/worse tool life than running them dry.

[Peccator]

This part has to have a mirror finish after machining. There can be no polishing after machining! Can anyone help me in the area of toolpath types to use to achieve mirror finishes? Stepovers? Stepdowns? I'm not clueless. I just need a little help.

[Jack Mitchell]

I would suggest a 10% stepover and a 10% stepdown in regards to the cutter diameter.

Instinct sort of guides me on projects such as these. Go with the shortest and largest cutter possible, the smaller ones will deflect.

 

I know that I am not helping you much with your apprehension so just follow your best guess and learn to live with the results.

 

The path from orange to yellow is my only concern (the differing diameters) and maintaining an even but accurate flow.

 

The red overflow pockets are trimmed off afterwards anyways so I wouldn't really be concerned with finish or dimensional accuracy in those areas. (assuming an aluminum or plastic injected part).

 

The above is my suggestion for roughing only - I might suggest a .001 or .002 finishing cycle as well.

 

 

Regards, Jack

[Hardmill]

Send me your part, i'd be happy to help you

out. Your generally going to be in the neighborhood

of 800-1000 SFM (if you got the RPM)

Chip load will be .0005-.001.

What brand of tool are you buying, thats what is

going to dictate your speeds and feeds, as well

as the machine and holders.

 

PEACE

[Code_Breaker]

Rookie 1,

 

Send me the file via e-mail and I will take a look and give input. We do all our hard milling on the Yasda -- holding .0002 tolerance -- using OSG TiAlN coated tooling.

 

I also us 10% DOC for 30-40 HRc, 5% for 40-50 HRc and 4% for 50-60 HRc. Chip load varies with size and type of cutter.

 

All the above, and more, plays in speeds and feeds.

 

HTH

 

Code_Breaker

[crazy^millman]

I think the speeder might give you trouble in my opinion. I say this becuase it is a hunk of a thing in the ones I have always seen. You are going to want maxinum rigidity for harmilling if tryign to achieve a good finish. If you have your tool hanging out of the spindle the distance plus the speeder you are out there a ways would problay work but I think you are only gaining rpms and loosing alot in rigidity. I have read many articles on hard milling and have done some but been a few years now. I would think if your compnay is looking at a new machine I would go by the recommedations of Hardmill(and yeah he does hardmill parts all the time), and some of the others who do it on a regular bases. I would want a very rigid, high rpm, high accuracy, and highspeed maching to make it pratcial if this is going to be a production job. If you are doing one or 2 I would try it on just about anymachien just take problay 3 to possbily 10 times longer but be cheaper in the long run if looking at a new machine.

 

Just my 2 cents worth not an offical commnet just my opinion is all. So please no

[jeffl]

Hardmill

How fast can you push your SFM if you have the RPM?

Example:

H13 RC 50

 

Carbide.

TIALN Coated.

Ceramic.

 

I've had near mirror finish results with a 5/8" uncoated carbide at 1400 SFM and .003 fpt.

[Peccator]

Thanks for replies guys.

Millman, no flaming here. I agree with you on the matter of the speeder being big and bulky. We are looking at production runs in the 100's. I think this speeder will puke on us. If it were my money I would purchase a machine to strictly hard mill. With the speeder we have, I know we can,t get to the 800-1000 SFM.

 

Which leads me to these questions.

 

Code_Breaker,

How big is that Yasda in X, Y and Z? What is your top spindle speed? At what limit is rated for IPM?

What is the rapid? Just curious.

[Code_Breaker]

The Yasda model YBM640V is 600mm x 400mm x350mm.

Spindle goes to 20,000 rpm, but anything onver 15,000 requires 20 minutes of warmup. The max feed is 400 IPM and, I believe, max rapid is 600 IPM.

 

 

HTH Code_Breaker

[jbel]

Rookie,

 

These SGS Turbo Carb ball mills are the shiznit for milling hardened steel. There are speed and feed recommendations on the last page. We mill Rc 42-46 all the time with the 3/8" and 1/4" balls and can get mirror finish results when we need to. Definitely go with the TiAlN coating. It has tripled to quadrupled our tool life with a better finish to boot. You should see better finish with air blast.

I don't know about the OSG stuff but if it is as good as their other products they should work well too.

[jbel]

One more thing.

USE THE SPEEDS AND FEEDS RECOMMENDED BY THE MANUFACTURER.

They may seem high at first but when you apply them correctly and see the results you'll never go back again.

[Hardmill]

quote:

---

Hardmill

How fast can you push your SFM if you have the RPM?

Example:

H13 RC 50

---

Depending on your application 1200-1500sfm

is not out of the question.

 

PEACE

[Hardmill]

Rookie,

The Yasda is the best mill out for hard milling

in fact I used to run the two at code-breaker's

shop. I currently have a 640 w/ a 4th axis.

.00001 inc. This is without a doubt the best

machine (accuracy) out, with a price tag to

go along with it. And no I did'nt add too many

zeroes for the inc., it does move in 10 millionths

increments.

 

PEACE

[JAMES GABEL]

I run the yasda's at the shop the code breaker works at and I agree with hardmill, they are the best machine out there. I will back them up one hundred percent.

[Hardmill]

Jimmy whats up??

Good to see you here.

 

PEACE

[Code_Breaker]

Rookie1

 

Based on my review, I have a few suggestions:

 

[*]ops 15-16 & 22-25, your tolerance setting is .002 and step is .0003 and .0001 respectively. Your tolerance setting is defeating your purpose of a mirror-like finish. I suggest you use the same settings as ops 17-21 of .0005.

[*]Also, you are running all these tools at 2500 RPM, making your SFM between 10 an 20 for a 2 fluted tool. Your SFM for 440C stainless is 700. What RPM does your "speeder" increases it to?

Outside of these coments, I think with the proper tool selection (as stated in this thread by several persons), you will have a great part.

 

(Remember, this is just my view point. I reserve the rights not to be )

 

HTH

 

Code_Breaker

[Peccator]

Like I say no, intended here. Why should the student the master?

 

Jbel: It looks as though we are going to use OSG end mills with TiAlN. Thanks for the suggestion though. I'll keep those in mind.

 

Hardmill: Thanks for your input on the machine specs. I looked at these online. Suhweeet!

 

Hardmill / Cobe_Breaker:Thanks for all of your input on the operations of the file that I sent to you guys. The input spindle speed of 2,500 rips outputs 20K thru the speeder. The smallest tool will be a .015 ball end mill. Thanks for the tips about tolerance settings in surfacing. Thanks for the edification.

 

Shane teh student.

[Peccator]

Just got out of a meeting with the Senior programmer, V.P. and the salesman for Yasda.

 

I am impressed!!

 

Shane

[JAMES GABEL]

You can't go wrong with Yasda. I am here also if you need anyhelp with hardmilling or if you have any questions about Yasda's.

[JAMES GABEL]

What's up hardmill, I will be on this forum more often.

[Peccator]

Thanks, James.