Aluminum Speeds and Feeds

[Brian B 74]

I have (2) T-6061 aluminum blocks (5" x 12" x 63") that I am cutting a half round cavity into. Cavity is R2.813 56.875" long. I am cutting these in my high speed machining center (24k rpm, Siemens 840D control).

 

I ordered a few YG Alu-Power 1/2" ball endmills that will be in tomorrow.

 

My experience is in pre-hard material. We very rarely cut aluminum so I am a bit lost with starting feeds, speeds, and depth of cuts.

 

Any help is greatly appreciated.

[Dave.L]

Alway start with the tool mfg recommandations.

[Nick Eaton]

I would rough the part first with a minimum rad tool (.02-.03). Ballnose endmills are not very efficient chip makers and you really want a uniform chip with as high a chip load as possible (.006 or higher) to keep the heat in the chip and avoid distortion.

I am roughing 18" long slots in our Kitamura 20k with plus head at 19000 and 650 ipm with a .17 cut depth with a 3 flute .375 cutter.

Ultimately your feedrate and depth of cut will depend on your horsepower and system rigidity.

To get proper speeds and feeds for ballnose finishing you will need to calculate effective surface footage and chipload. Again keeping the effective chipload at .003-.004 will save time and avoid distortion. You will have to make several calculations as the effective surface footage and chip load will change as you work around the radius.

As an example with .5 inch 2 flute ball,.02 depth of cut and .01 step over 18000 rpm and 650-700 ipm on a 45degree angle gets you in the ball park.

Twice as much feed on the flat (bottom of your channel).

Keep an eye on your load meter when roughing. If you are not running a 70% load you can probably go faster or deeper.

 

Hope this gets you started

 

Nick

[crazy^millman]

24k and 600imp to 800ipm would be my starting point, but people always all me crazy. Might start on the slow side with 18k maybe 400ipm to 500ipm.

 

HTH

[workmantm]

What Dave said, but if you can use square Endmills then I would reccomend looking at the OSG Blizzard line. For pure metal removal rates in a full slot they can take a cut that looks insane on paper and keep asking for more. Its my choice rougher for Aluminum.

[Josh T™]

I would start around 12K and around 400ipm depending on the depth of cut. This should give you a "jumping off point"

 

HTH

Josh

[jeff]

quote:

---

I would reccomend looking at the OSG Blizzard line. For pure metal removal rates in a full slot they can take a cut that looks insane on paper and keep asking for more. Its my choice rougher for Aluminum.

---

I use these almost exclusively for Aluminum,sometimes I will use the Hanita Javelin.

Amazing how fast they can cut.

[Brian B 74]

So my understanding is that with aluminum you want to ruff with a square endmill? OSG is 2 miles from my shop so getting a cutter is no big deal. If I was to get a 1/2" blizzard (List 2021) with a .060 CR, should I invest in the DLC coating? Should I stick with the recommended speeds and feeds (9100 RPM 225 IPM))?

 

Thanks for the all the info!

[workmantm]

The Blizzard line is mainly designed for shops like mine, 10K max RPM Haas machines. Compared to your standard EM they have 200%+ performance gains. You can call OSG to see if you can run them faster, but I can't get above that so I've never looked. The key to maximizing the tools is the 1/2 diameter DOC on a full slot. That is how they keep things running with the high chip loads. I can't really speak about running anything above 10K as we don't have the capability here in the shop, though I wish we did.

[gavetta]

You also need to know the horse power of your machine. If you don't have enough horsepower, you may stall the spindle. Check here

 

http://www.mapal.us/calculators/milling/Ca...atorMilling.htm

 

Scroll down to where it says "To Calculate Machine Requirements Enter the Following Known Data:"

Hope that helps.

 

P.S. You can also google "material removal rate", lots of good info out there,...google is our friend

[jeff]

quote:

---

If I was to get a 1/2" blizzard (List 2021) with a .060 CR, should I invest in the DLC coating? Should I stick with the recommended speeds and feeds (9100 RPM 225 IPM))?

---

I don't have the book in front of me so I don't remember what the 2021 series is... but I found that the 3 flute Blizzards work a lot better.

Bright finish is the way to go.

 

I would go with the reccomended RPM's, but the feedrate is subject to your application of course.

[Joe788]

For only two parts, I wouldn't get too carried away trying to maximize metal removal rates. The last thing you need is to pull an endmill out of it's holder and gouge the $1100 billet because you wanted to save 10 minutes.

 

Use any aluminum specific 1/2 inch three flute bull mill to rough, and an aluminum specific two flute ball mill to finish. I'd recommend a 1 inch ball if you've got one, but they are about 4X the price of a 1/2 inch ball, so you have to decide if the cycle time difference is worth the two extra parts.

 

I don't know how much horsepower you have, or how fast you usually run the machine, but 24,000rpm and whatever chip load you're comfortable with will be no problem. (Assuming you're using balanced shrink fit or milling chucks).

[Bob W.]

It sounds like a great part to run a Volumill demo on (15 day trial license). I ran a demo before I purchased a license and they had me running a 3/16 bull mill at 500 IPM, 25% stepover, and .18" depth cut, @ 12k rpm to rough a cavity. With a 1/2" end mill you should be able to cut as fast as your machine can feed with a 1/2"+ depth cut & 25% stepover.

[Brian B 74]

I just uploaded a file to the ftp site called aluminum.mcx. Pretty basic part. You can see the speeds and feeds I am running (nothing crazy). Thanks for the help everyone!