What bit and setting do you use to mill aluminum?
I have to make a part out of aluminum on my machine. It's rigid enough, But I have no idea of where to start with the bit and the settings.
The material is 3/4" thick 8020 aluminum (That's what's printed on it anyway.
I will need to mill a few slotted pockets 1" long 1/2" wide, with the ends 1/2" in diameter, and though hole slots about 1" long 1/4" wide, with the ends 1/4" in diameter.
I will also need to mill clearance squares triangle shaped 1 1/2" x 2" x 1/4" deep.
My machine has a 5hp spindle, ER 32 collet, 12k-18k rpm
I would like to dry cut, but can manually spray with rubbing alcohol from a spray bottle if needed.
Can anyone recommend a bit and the settings they use for it, as well as some tips?
Similar Threads:
Re: What bit and setting do you use to mill aluminum?
Although I am no expert, my experience milling aluminum and what I have seen in other shops leads me to suggest a single flute bit and high RPM. I did some L shaped brackets milled from some 1/2 inch plate on my machine (small machine with a Bosch Colt as a spindle) with the spindle at max RPM (35,000) and cut 40 pieces 1 1/2 by 1 1/2 inch from a single plate. At lower RPM the feed rate had to come WAY down.
Re: What bit and setting do you use to mill aluminum?
The base recipe I'm using to cut dry.
Onsrud 63-610 or Yonico 31011-SC. Both Single flute, 0.125dia, 0.5 LOC and 0.250 shank.
0.002 chip load. Usually around 12000-13000 rpm.
I try to use trochoidal tool path whenever possible.
Re: What bit and setting do you use to mill aluminum?
I've been using a single flute spiral upcut bit to mill 6061 aluminum. I don't recollect feeds and DOC, but they're very conservative...probaby less than 30ipm feed. I've had no issues with breaking bits, or even gumming up the bit.
Originally Posted by TTalma
Re: What bit and setting do you use to mill aluminum?
I run a two flute 1/4" carbide endmill at around 16,000 RPM and 80 IPM, about a 3-4mm DOC, but my mills only flute for 1/2". Important to go hard at it because *****footing around means you tend to rub rather than cut, which creates a lot more heat, which leads to chip welding, an "ohno" sound and bits of your endmill flying around the shop.
I've never had a lot of luck cutting dry, especially when slotting - swarf left in the channel also causes issues with both re-cutting and welding. A continual air stream to blow swarf out and a mist of 80% water, 20% methylated spirits (aka denatured alcohol in some areas?) helps enormously and doesn't leave a sticky coolant mess at the end of the job. Just let it dry out and then blow out the dry swarf.
As Biggs427 says, trochoidal paths when you can. Just checking FSWizard, a full depth climb cutting trochoidal path with a helix in and say 0.3mm stepover, 18000RPM and about 200 IPM with decent chip evacuation and a bit of sprayed coolant with a carbide tool would do you right. HSS instead of carbide, to me, is a false economy - but if you go that way drop the feed rate to about 160 IPM.
Important - with aluminium, DO NOT use coated (AlTiN etc) cutters. The coating ever so slightly rounds the cutting edge and what you need more than anything else is a sharp edge. Uncoated HSS or carbide tooling is cheaper and, ironically, will last a lot longer.
Whatever you get, make sure you buy at least 3 cutters. You'll likely ping a couple as you tune things in.
Re: What bit and setting do you use to mill aluminum?
Thanks for the tips. I'm going to order a few of the bits and see how it goes!
Re: What bit and setting do you use to mill aluminum?
Also, if you want to dry cut, a small amount of constant air pressure in the cut path to help clear the chips and cool the cutter helps a lot.
Reply with Quote
