Fast machining of aluminum

D

Dave K

Diamond

Joined

Mar 21, 2004

Location

Waukesha, WI

• Dec 4, 2005

• #1

You all have seen the super high feed rates of roughing aluminum in a machining center, and I'm sure some of you are doing it in your shops. My question is, what kind of end mills are they using? I'm talking about when they're running at 100+ inches per minute. I've seen 3 flute carbides being used for this but are there certain degrees of helixes you should use to accomplish these types of feed rates?

 

B

Boris

Titanium

Joined

Oct 4, 2005

Location

England

• Dec 4, 2005

• #2

Fastest thing I've done in Aluminium is 20 mm dia 3 flute fine pitch carbide ripper

10 mm DOC 7500 RPM 750mm/min feed
that was roughing out the 3 channels in a block of ally that was going to form 4 components
These were profiled at 1250 mm/min at 20mm DOC with the same ripper
The cutter lasted 4 maybe 5 shifts before it needed sharpening ( or barely 1 shift when the management decided to save money by turning the coolant concentration down to 2% to save oil... D )

Boris

 

H

huskermcdoogle

Stainless

Joined

Nov 11, 2005

Location

South Texas

• Dec 4, 2005

• #3

I have been running around 120ipm with a 3 flute 3/4 inch carbide insert mill takeing .200" DOC can't go any faster with my machine becuase it is old and feeble. Tool doesn't seem to care, and parts aren't moving.

 

H

huskermcdoogle

Stainless

Joined

Nov 11, 2005

Location

South Texas

• Dec 4, 2005

• #4

oh 7500 rpm

 

D

Dave K

Diamond

Joined

Mar 21, 2004

Location

Waukesha, WI

• Dec 4, 2005

• #5

So, you guys basicly do this with carbide indexable tooling only? I guess I'm wondering if these kind of speeds are achievable with solid carbide end mills. I'm thinking 3/8 or 1/2 diameters, with 3 flutes. I figured 3 flutes gives more cutting edges, with still plenty of room for chip evacuation. I just don't know if I should be using a higher helix than standard.

 

N

Natchamp

Aluminum

Joined

Aug 29, 2004

Location

So Cal

• Dec 4, 2005

• #6

The best 2 tools I have for aluminum are;

Destiny carbide roughing endmill:
.500" diamter, 3 flute
8,000 rpm
100 ipm
.500" doc!
.250 step over

ShearHog 1" single insert cutter:
10,000 rpm
400 ipm
.080 doc
.800 step over

Mark

 

Bobw

Diamond

Joined

Feb 8, 2005

Location

Hatch, NM Chile capital of the WORLD

• Dec 4, 2005

• #7

If your going to stick with solid carbide endmills, think roughers. They may cost a bit more, but they surely can haul ass. 1/2" rougher 4flt(I was just playing). 12000 rpms, .2 DOC, .25radial, 700ipm. I found this only works on the front side of the part where the coolant is hammering the endmill. I don't see a reason why you shouldn't be feeding near or well over 100ipm with a solid carbided endmill, even with a lower max spindle speed, as long as you have the coolant.

Some of the inserted cutters with their more advanced geometry are really really impressive, then you can really have fun.

 

D

Dave K

Diamond

Joined

Mar 21, 2004

Location

Waukesha, WI

• Dec 4, 2005

• #8

Ok, thanks guys. Natchamp, I'm not sure what a destiny cutter is.

As far as the shear hog, I have corner radii that don't allow me to go that big in dia. 1/2" is the biggest I can use.

 

J

Jamie

Hot Rolled

Joined

Oct 14, 2005

Location

Ont. Canada

• Dec 5, 2005

• #9

Rippa 3Flute 17deg Hi Helix

 

3

3t3d

Diamond

Joined

Nov 1, 2004

Location

WI

• Dec 5, 2005

• #10

An old job I used to run was a three flute 37 deg. helix 3/4" solid carbide EM 10,000 rpm .125 DOC .75" width of cut at 400 ipm. It was a real aluminum blizzard in there.
Pushing a 1/4" 3 flute at .25 DOC .25 width of cut, at 10,00 rpm anything much over 130 IPM and it tends to snap off the toolbit.
I also run 3/16" 10,000 rpm .25 DOC 3/16" width of cut at 70 ipm and again 10,000 rpm. The tool last for weeks. I can't go faster there, or the part is shoved off the vacuum chuck.

Are these the sort of number you are curious about?

Pete

 

smallshop

Diamond

Joined

Jun 2, 2005

Location

North Central Montana

• Dec 5, 2005

• #11

ShearHog 1" single insert cutter:
10,000 rpm
400 ipm
.080 doc
.800 step over

Click to expand...

Yep. I can't feed my machine that fast. But that is the tool I use when I have lots of material to remove. Paid for itself the first job I used it on and they're not cheap.... Tool sounds kinda like a go-ped at full throttle....

 

M

michael

Cast Iron

Joined

Oct 4, 2004

Location

hangtown, california

• Dec 5, 2005

• #12

Get a Shearhog. Follow the suffested cut parameters. Use your horsepower. You *will* be happy. Seems pricey at first, then you use it and wish you had gotten one sooner.

 

dkmc

Diamond

Joined

Jan 13, 2002

Location

Upstate NY -In the Flats next to the corn fields

• Dec 5, 2005

• #13

Very interesting info guys.
Any ideas as to Horsepower requirements on your posted feedrates/DOC..?????

dan k

 

D

Dave K

Diamond

Joined

Mar 21, 2004

Location

Waukesha, WI

• Dec 5, 2005

• #14

Pete,
Yes, that's what I'm looking for. So it looks like your using a pretty steep degree of helix, and that's what I wasn't sure of.

As far as the shear hogs, I want to get one of those because I've heard about them in a previous thread, but like I said earlier, the corner radius only allows a max .25 radius, hence no bigger than a 1/2" cutter.

 

P

PBMW

Titanium

Joined

Aug 13, 2005

Location

Bremerton, Wa

• Dec 5, 2005

• #15

so ...what's the problem? rough with the shear hog and finish with something smaller to drive the corners....
Jim

 

D

Dave K

Diamond

Joined

Mar 21, 2004

Location

Waukesha, WI

• Dec 5, 2005

• #16

PBMW,

That's a damn good question. Don't know where my head was at. Just a brain fart that wouldn't quit, I guess.

 

P

PBMW

Titanium

Joined

Aug 13, 2005

Location

Bremerton, Wa

• Dec 5, 2005

• #17

No problem Dave...I brain fart all the time...
Just the other day I needed to do a part that I had to finish the inside first as it had .125 thick walls. cut thru top to bottom. then hold in form jaws on inside and finish outside.
Started pocketing the inside and got 3/4 done when I realized that if I had punched a couple holes in there first, I'd have had a path for the chips to flow out of.....
instead of me standing there with the air gun....
Jim

 

smallshop

Diamond

Joined

Jun 2, 2005

Location

North Central Montana

• Dec 6, 2005

• #18

ok Jim, How many parts before you that little "ah-HAH".....

 

P

PBMW

Titanium

Joined

Aug 13, 2005

Location

Bremerton, Wa

• Dec 6, 2005

• #19

Well, see.....(Shuffles feet..) that's the real Bi*ch.
I only needed one....

But I'm ready next time!

Jim

 

P

psychomill

Titanium

Joined

Mar 12, 2005

Location

Silicon Valley, California... + other states & sev

• Dec 6, 2005

• #20

So, you guys basicly do this with carbide indexable tooling only? I guess I'm wondering if these kind of speeds are achievable with solid carbide end mills. I'm thinking 3/8 or 1/2 diameters, with 3 flutes.

Click to expand...

Yes you can do this with solid carbide tooling. As some others have mentioned, Destiny Tool does make some nice ones in their Viper series, 2Fl or 3Fl. Here's a link Dave. Several other makes will also handle hi chip loads. Generally, these helix angles on the tools hover from 36 deg to 45 deg. give or take a couple. Hanita Javelin hoggers can rip it up too. I've gone over 1000ipm with their 3/4 and 1.0" hoggers.

If you need "endmill" style" cutters (as opposed to knuckles on a hogger), then check out Dataflute's stuff. In particular the HVM and ALDH series. I tested dozens and dozens of these cutters for them before they were marketed. Amazing cutters. Had the 1/2 ALDH cutting at 900ipm (12k rpm). And for note, a 1/2 ALR (which is hogger and a BIG improvement over their older ARO design) was able to push at 1180ipm, .200 DOC and didn't bat an eye. Same endmill at .250 DOC (Full slotting pass) at 800ipm (you'll need some HP and GOBS of coolant). Thats moving 100 cubes with a 1/2 em! And most of these test cutters were uncoated. The coated ones definately improved tool life and HP consumption though.

With the right tools (and there are others out there), the 'sky is the limit'. Oh, it helps to have a good machine and set up as well...