6061 Aluminum Milling Help

Hi,

This is my first post, so forgive me if I commit a faux pas. For background, I am trying to mill holes in a 0.125'' thick sheet of 6061 Aluminum that spans 17'' by 14.75''. These holes range from 0.15'' to 0.2'', so the holes are relatively small. However, each time I try milling with my 1/8'' Carbide bits, they end up breaking shortly after. Could someone review my settings and try to identify the cause, because I've gone through about 8 bits and numerous forums to no avail albeit some improvement.

Bit Size: 0.125"
RPM: 24,000 or 400 hz. (Maximum for milling machine)
Feed Rate: 30 ipm
Plunge Rate: 15 ipm
Type: Carbide
Maximum KW: 0.8 KW

These settings came from cloudcnc's speeds and feeds calculator, so I'm not sure how exactly to fix it.

The cuts come out pretty clean, but they simply snap after some time. I've observed that when it snaps some aluminum seems fused to the bit. Any ideas? Thanks!

Use spray mist coolant and lubricant,
chip welding breaks cutters
chip load per tooth is .00? based on 24k rpm
practice on plexiglas.

you will get answers at the Zone

Kerosene or WD-40 for coolant/cutting oil. Spiral in, about 7° spiral angle. The rest of the settings should work depending on how stiff your machine is.

Quote:

---

Originally Posted by Jim Dawson

Kerosene or WD-40 for coolant/cutting oil. Spiral in, about 7° spiral angle. The rest of the settings should work depending on how stiff your machine is.

---

and how well your piece is fixtured down. If not secured properly something that long and thin will surly vibrate which will kill cutters that size pretty quick.

A piece that large could be secured with spray on contact adhesive. Just a couple stops or clamps should work to prevent any drift. Its not particularly strong, but its a large area, and the cutter you are using is fairly small. I use an 1/8 3 flute Alu Power end mill to spiral mill holes in 1/2 in 6061 just about every day with 24K spindles. I've tried spray mist and its "ok". I've stood there with a squirt bottle of WD40 and it works, but if you have to stand there you almost don't need CNC. LOL. I tried kerosene and found it worked better than WD and costs less. I tried transmission fluid and it works great. I even ran flood transmission fluid at one time. That resulted in very very long tool life and beautiful looking parts, but my shop smelled like a transmission shop. Finally I went to water soluble. Kool Mist sucked. It cut nice, but it stained the parts. The folks at Kool Mist just wanted to keep shifting the blame, but were no help. I was mixing it with distilled water and they still tried to blame the water. Finally I went to Master Chemical SC520 and run about 6-8% solution with distilled water. Parts are good. Cutters last a long time. The shop doesn't stink like burned up transmissions. And the parts come out nice and shiny like they should, I run thousands of hours on three high speed machines and one lower spindle speed machine milling 6061 and I won't go back to anything else. There are times when I have no choice but run an applied lubricant like doing a part on my router because its too big for my other machines where I can't run flood. Then I use Tap Magic (all metals) applied with a cheap flux brush, and I blow the chips away with a regulated blower clamped to the side of my spindle. Flux brushes come in bags of a BUNCH for around 3-4 dollars. I buy them for throw away use like I buy popsicle sticks for mixing resin.

Are you sure its 6061? I know you can get sheets of 6061, but sheets of 5052 are more common. Both of the local metal yards I trade with stock 6061 bar stock and 5052 sheet. 5052 is much pickier about machining methods and gummier and generally more of a pain to machine. It tends to burr more, and is really just miserable for a beginner. I know. When I was a beginner I had pieces left over from a boat repair that was all 5052 and I think the stuff held me back a six months in my learning curve. When I started machining 6061 it was like a weight had been lifted. Now oddly enough I use the same methods for 5052 I used for 6061, but I only use fresh sharp right out of the package end mills designed for aluminum. I am a big fan of 3 flute high helix 40-45 degree end mils, and in particular Alu-Power.

Coolant or atleast lubricant helps a lot to prevent chip welding, and getting the chips out of the cut helps even more. Might as well use one to do both jobs if you can.

Flood coolant is really ideal if you have it at least somewhat enclosed. Aluminum melts very quickly if not kept very cool.
We run aluminum all the time, but I have an enclosed NC mill, and use water based synthetic coolant at about 4 % ratio.