My boss had a wild idea, which of course was placed on me to figure out. We have lengths of boxed 6061 T6 aluminum which is about 1/2 x 2 x 10' in length. The idea was to do a simple program to cut the ends to size and drill a few holes in the piece, so we did not have to outsorce this work. I reminded him that this is a woodworking machine, with no coolant, or adequate workholding for metals, but he insists on figuring out a solution.
I first tried a 1/2 solid carbide down spiral that we had a crapload of. I ran the tool at 15000 rpm which is our normal spindle speed, and feed at about 100 ipm. This did cut the piece, but it was real jagged on the ends (I believe it was moving the piece on the table) and played hell on the bit. We then ordered a 1/2 TiCN coated triple flute upspiral, which was recommended to us from our tooling supplier. We ran that at the same speed and feed, which just mangled the end and drug the head into the peice. We tried again with a fresh bit, this time as slow as the machine would go (3 ipm) this time it just melted the metal and made no chip formation.
We have the piece held down with the pins using the supplied clamps which holds pretty rigid, so most of the problem has to be with our tooling choices or our feed speeds. I was thinking of using a multi flute roughing bit but I dont know if that would make things any better. Any help would be appreciated..

I forgot to mention that the box tubing has about a .090" wall thickness.

You might want to try Onsrud router bits, made specifically for aluminum.

Couple of considerations ;
You will not achieve wood sfm (surface feet per minute) in aluminum. Your spindle rpms will drop what you would consider dramatically, however the cut quality will increase as you level out your chip load. Machining it "dry" does put you at disadvantages also, however not insurmountable.
I think you will find with a quality 1/2" diameter cutter ( high helix 3 flute style <duramill brands have always worked great for me dry> or a "ski" ground configuration made specifically for aluminum) your effective safe starting rpms will be down closer to the 7000 to 9000 rpm band. Remember, this is ball park, rigidity of machine and set-up, radial depth of cut and flute engagement of cut all figure into this. If say this recommendation were to work for you, the ball park feed you would be running at .003 feed per tooth would be 63ipm @ 7000 rpm. I ran some 6061 on a bridegeport style milling machine the other day dry....2000 rpm 14ipm...so as you can see machine type (in this case knee mill -vs- cnc router) can influence alot. Good luck ...and if you ahve anymore specific questions email me at ntek1@aol.com or visit my website at www.cnccustomservices.com and send email via there.

Honkey,

MarkT is on the mark, but I have 1 thing to add.
Be very careful not to let hot alluminum chips up into the dust system.

It is very easy to start a fire this way, and you really don't want to do that.

Either block the dust system to the machine, leave it off, or don't machine alluminum on the mahcine.

Blaine

Thanks for the replies. We finally got it working, which confirmed what I was suspecting in the beginning. We were turning the bit way too fast. I cuts smoothly now at 7000 rpm at 60 ipm. However thats just for the pockets cut in the side of the extrusion. We also experimented with cutting the ends with a slitting blade out of the agreggate head which worked extremly well, untill the teeth started chipping. We have a new blade made especially for this purpose on order. Now we just have to run production to see how our tooling life works out. By the way I recieved an e-mail asking the machine specs so for anyone who wants to know, this is on a biesse rover 30 with NC1000 software.