Milling Aluminum

[InventIt]

I am curious about milling alum. with my cnc router. I am still in the build process and I would like to incorporate the needed requirements into the design so the machine will perform as expected on harder materials like alum.

Can you guys who have experience will this give me some help.

What problems did you have when you milled alum in your router?

Thank You
Rob

[balsaman]

I have had the endmills plug up and break. This is because of no coolant mostly. I also had trouble because my spindle was underpowered at 7 amps.

If you want to do it the machine needs to be stiff, and you need to take it easy. I had the most luck with a 1/4" endmill.

E

[Hobbiest]

End mill may have also been plugging up from too high a spindle speed. It ends up almost melting it instead of cutting off chips. Don't know what proper speed is, Hu and Ballendo say that it depends upon the situation.

[balsaman]

That's where the coolant comes in. Keeps things cool and provides a lubricant too. All I know is my router had to be on max to get enough power to keep it from stalling.

The 1/4" bit has bigger flutes so the material could get out of the way better. In hind sight I was probably cutting too deep in one pass too. .200"

E

[strat]

All wrought aluminum alloys, 6061-T651, 5000, 6000, 7000 series
carbide .....opt f 15 s 620 avg f 8 s 2020
hss............ opt f15 s165 avg f 8 s 850
f= feed .001/tooth s=speed ft/min
this is from machinist handbook

[ger21]

To mill aluminum with a ROUTER, you need tooling designed to be used with a ROUTER. The feeds and spindle speeds you listed are useless to someone using a router with 10x the spindle speed. (unless they can cut at 150+ ipm). Spend the money and get router bits designed to cut aluminum. As I mentioned in another thread, check out http://www.onsrud.com .they have a huge assortment of aluminum cutting bits designed to work at router rpms. One other thing to consider, as was mentioned, is coolant. If you dont want or can't use a liquid coolant, try setting up an air line to blow into the cut. This will help keep the chips clear and keep the cut a little cooler.

Gerry

[steveald]

Hi,

I cut aluminum with a 3.25 hp router at work and with a 2.25 hp router at home. I use a water and oil mist coolant at work, but it's messy so I went with a Lenox Micronizer Jr. oil mist coolant system for home that works just as well. It blows compressed air at the bit, and adds 3 to 6 drops of cutting oil per minute to the air.
I use a 1/4" 2 flute up-spiral endmill TiN coated carbide router bit whenever possible, and 1/8" when I need sharper corners. I have heard of people using a 1/16" or smaller bit with aluminum, but I haven't had any luck with those bits.
The speeds and feeds I use are 10-15 ipm depending on the edge finish I need, 16,000 rpm for 1/4" bit and 19,000 rpm for 1/8" bit.
I cut up to the diameter of the bit per pass, and between 50 and 75% step-over for surfacing, again depending on the finish I need.
I use 6061-T6 whenever possible, increase the feedrate for utility grade to avoid melting and plugging up the bit.

Steve

[peter]

hi guy's
don't be using endmills to many flute's
will cause it to clog up
use slotdrill's 2 flute 3 flute max
this will allow it to clear swarf in between cut's
just input
best regard's
peter

[InventIt]

So it sounds like coolant is the biggie.
Do you guys have problems with the bit grabbing the work piece or a lot of chatter?

steveald
Are those the "alum cutting" end mills. the ones that have a different helix designed for soft metals? If not have you tried them?

[steveald]

Hi,

The bits I use are general purpose router bits. Everyone I have dealt with in the sign industry refers to them as endmills, but they aren't like milling machine endmills, so they probably should be called a slotdrill.
I haven't tried any bits that were specifically for aluminum.

Steve

[azsigns]

I cut out aluminum lettering all day long.
Here's what I do using a 3.25hp router on a medium built machine.

5052 Aluminum
1/4" Single Flute Carbide (Belin Yvon 33635)
Depth/pass 0.080" to 0.090"
Feed Rate 35 - 38 ipm
Spindle 13000 rmp
Mist Coolant (Oil Based)

This gives me a mirror finish on the edges and good tool life.
The Belin Yvon cutter is by far the best I've ever used.
Nice clean cool little aluminum curls for chips. Not those short sharp slivers you pick from your fingers for days.

The cutter being single flute has an extra large clearance for the chips so it never welds up. Expensive bits but worth every penny.

Just feed the Z axis slow around 10 ipm. They don't like to plunge.

Chris

[ballendo]

Thank you for this info!

What is the typical total thickness of your part and/or cut depth?

Ballendo

Originally posted by azsigns I cut out aluminum lettering all day long. Here's what I do using a 3.25hp router on a medium built machine. 5052 Aluminum 1/4" Single Flute Carbide (Belin Yvon 33635) Depth/pass 0.080" to 0.090" Feed Rate 35 - 38 ipm Spindle 13000 rmp Mist Coolant (Oil Based) This gives me a mirror finish on the edges and good tool life. The Belin Yvon cutter is by far the best I've ever used. Nice clean cool little aluminum curls for chips. Not those short sharp slivers you pick from your fingers for days. The cutter being single flute has an extra large clearance for the chips so it never welds up. Expensive bits but worth every penny. Just feed the Z axis slow around 10 ipm. They don't like to plunge. Chris