Working with Sheet Aluminum on a CNC Router
Advice, tips, and cautions on running aluminum on your CNC equipment. September 27, 2008
Question
I have a sign customer who wants me to cut some aluminum sheets. I have never done this so I'm wondering; do I really want to do this? I do have the oil/air mistor on a CNC machine (never used) but from machine shop/wood shop experience; wood doesn't like oil and oil doesn't like wood. I also do not want to contaminate my spoil board so as not to be able to cut wood, which is my primary source of cutting.
If I were to do this can you guys give approximate tool and flute/speed/feed rates cutting depths etc, do I need to do multi bits? Is there also a difference in the kind of aluminum that I might want to cut and what I would not want to cut? Could I cut the aluminum without lubricant with the proper bit and speed/depth cut? Any help is appreciated.
Forum Responses
(CNC Forum)
From contributor D:
You can do it. I don’t use flood or mist, just air. I made a small extension to my air nozzle to get it closer to the tool and it blows the chips away faster. Don’t use your dust collector (I think you know that). Depending on what you’re doing, you can pretty much use your standard solid carbide tools. Most of the tooling I use for solid wood I get from MSC - standard carbide metal working mills. In my experience a lot of the time regular end mills work better in solid wood. You can change feed rates and spindle speed and go from wood to aluminum, and back again. Just don’t forget to shut off that collector.
From contributor M:
How thick is the aluminum sheet? Anything over 1/4" I would say send it to a machine shop instead.
From contributor G:
Contributor D - why don't you want the dust collector on while you machine aluminum? I would agree with Contributor M. Thicker material can be a pain. Some of the grades of aluminum don't machine real well either, the chip tends to adhere to your tooling. The deeper the cut the more difficult it tends to be to prevent this. We just ran a job for a sign guy out of 3/32" sheet and we used a single O-Flute tool from Onsrud. It worked great with no problems.
From contributor D:
To contributor G: If you use the vac the aluminum will get caught in the filter bags, a cartridge type is better. You should only use you vac for one thing, either wood or metal - not both. Hot metal chips plus wood dust plus high air flow equals fire. As for the O flute, that will work better because its clearing the chip faster, but it won’t last as long. I use a stub length 1/2 inch roughing mill 3 or 4 flute 6000 rpm. 200-250 ipm.at.02 over then come back with my finisher.
We cut aluminum, brass and bronze up to1 inch thick. Taking shortcuts breaks tools, wears out spindles and results in bad work coming off the machine. It doesn’t sound like you’re doing any heavy machining, but you might want to look at your tooling a little closer. Changing things up may help you a lot.
You haven’t said what machine you’re running, but it really doesn’t matter. With a good spindle, the right tooling and a good programmer, a small machine can run just as good as a big one (just a little slower).
From contributor W:
I have a cabinet shop and a Techno LCX 60x120 table with 10hp spindle and vacuum pump. I too was approached by sign shops and no have second revenue source from them. We regularly do .040, .090 and .375 / .5 material. No oiler/mister as not to contaminate, I use oil can or spray lube and a single flute bit about 80 ipm, single pass up to .090 thick. On the .375 and .50 I went six passes leaving .020 for final pass. I use 1 inch ramp in, no overlap and no ramp out (learned this one after breaking several bits on .375) - also straight in on longest run, no angle drop in. Double sided stick tape for small parts and vacuum for everything else. We now run several jobs every week for sign companies out of lots of different materials such as aluminum, plexi, plastic and acrylic.
