Cutting Aluminum on a CNC Router

Basic CNC tips for working with sheet aluminum. December 27, 2006

My company has asked me to cut sheets of aluminum 0.032" thick on my CNC in the shape of large diamonds. I am strictly a woodworking programmer and have no experience in metalworking. We have a Fagor 8025 router with a 48x48 bed. We use 3/4 birch plywood as a spoiler board. We create routes for 0.187 diameter rubber gaskets to fit into and drill holes for the suction. We do not have any coolant jets or any way to keep the metal cool when cutting. I am also concerned with how to hold down the 0.032 thick aluminum so as to not have it moving and not dent it. The aluminum is going to show in finished product. My company can not cut it on the laser engraver and will not purchase a punch for our press for this run. If anyone can give me suggestions as to what bits to use, feed speed and spindle speed and direction, this will really help. Also, if you think it can not be done, please let me know so I can take your response to my employer and let them know why we can not do this.

Forum Responses
(CNC Forum)
From contributor B:
If it were me, I would farm it out to a company with a waterjet (kind of like a plasma cutter but with water/ceramic abrasive instead). I think you'll not only have problems holding the material, but the heat generated whenever you machine metal must be taken into account.

From contributor G:
I'm a plastic guy who cuts aluminum once in a while for sign companies. I would suggest you try to use an Onsrud 62-622. The aluminum you're cutting is quite thin. I would skip the gasket and just create vacuum tracks. Aluminum has different grades, which I know nothing about. The aluminum that the sign companies send to me always cuts fine. I do end up filing the edges. I run 150IPM at 18000rpm (no coolants). It sounds as though you have a very similar machine to one of mine. As for as pricing, I take my normal plastic rate and then double it.

From contributor M:
The work you described doesn't even need to be done on a CNC. Why not farm it out to a local metal shop that has a shear? The .032" aluminum is easy work for a shear operator. The only caveat is that it probably needs to be accurately sized, so if you do send it out, choose the vendor carefully.

From contributor W:
If it's only .032, score it with an x-acto knife and bend it over for easy cuts.

From contributor T:
Sheet aluminum is actually very easy to cut on a CNC. Aluminum is typically very light and your existing vacuum should be sufficient if your finished parts are fairly good size. Use of a solid carbide endmill with two flutes and the smallest diameter you can run will give you a fairly clean edge and will minimize the potential for part movement.

As an example, if you use a 1/4" endmill with two flutes at 18,000 RPM's on softer grades of aluminum, you can run at 230 inches a minute. If you find that your material is harder, you can run the same endmill at 115 inches a minute. Check online for Tabletop CNC mills. Many of those machines run aluminum at the same speeds and feeds and some of the web sites have video of these machines running. It's very interesting to watch how fast and easy these machines cut aluminum. I have seen many CNC's run aluminum with no coolant in this method. About the only downside to this would be cutting tool life.

The comments below were added after this Forum discussion was archived as a Knowledge Base article (add your comment).

Comment from contributor A:
We machine aluminum every day on our CR Onsrud - the trick is using single O-flute bits. They work like a champ. The O-flutes leave a near mirror finish. We run about 15,000 rpm at around 120ipm, cutting no more than about 1/16" per pass. We use a downcut spiral for most applications. The only coolant we use is air. All the other supposed "aluminum" tooling has not worked for us.

Comment from contributor B:
I'll second the last commenter. The Onsrud 63-7xx and 62-7xx bits cut like a charm. I usually spray a little coolant or WD-40 on the piece but for AL that thin you shouldn't have any problem. If possible use 6061 aluminum; it's harder and you get more chips and less welded goo on your bits.