Cutting aluminum sheet

[Zach Froble]

Can anyone give me some help with cutting and drilling aluminum sheet. I have 3 pcs of 6061 about 38in. x 38in. x.190 to cut and drill.

Looking for some recommendations on feed speeds and cutting parameters. I have a 3/8 low helix cutter that is supposed to be for aluminum and cobalt drill bits for the drilling.

Thanks,

Zach

[Georgi Baltov]

Zach,

I tried it once and it sucks. There are special machines that do that and they have cooling liquid that help a lot. Without cooling it's just waste of money. I would never do it again. My recommendation is get the job done outside in a proper metal shop. That's why there are metal CNCs and wood CNCs. It's up to you.

From my experience the heat will destroy the carbide really quickly and from there one it's not cutting it's forcing its way. I bought some expensive tools from harder carbide but it still didn't work. The soft MDF bed will not help you much when drilling either. You will get a bulge on the back of the material. The drill will probably make a few holes and then it'll overheat, dull and destroy your material on the bottom.

If you are still willing to do it get upcut tools that would extract the heated aluminum out of the cut groove. If possible try to blow air so it helps cool the bit somewhat. Other than that I have no more encouraging advices to tell you. It's up to you.

If by any chance it works, I would love to get some feed back on your success.

Cheers and good luck

[Ryan Hochgesang]

The following is general information on where to start, however your Thermwood is definetly capable of cutting Alum.

First of all, coolant is definetly going to be needed in order to keep your cutting tool cool and free of chips. A low helix, up spiral type tool, containing 3+ flutes will be best. It will also be a good idea to slow the spindle RPM a bit slower than what you typically use when routing other wooden or plastic parts. You will NOT want to go slower than 7,500 RPM during cutting. Below this RPM, the HP curve starts to drop fairly quick limiting rotational power at the tool tip. Light depth cuts (Approx .03") are generally a good idea when removing material with full dia. of tool. Feed speeds are likely going to be around the neighborhood of 50 - 75 IPM. There is a solution call Acculube that works nicely for cooling and lubricating tool for the cutting process and it is more sticky which helps contain the coolant, as compaired to other liquid type solution which may tend to flow from your part to other areas of the working envelope. Eitherway, you will have some oily residue from this type of process. You may want to consider additional Table/spoilboards when cutting with coolant ON.

Hope this info. at least gives you some ideas on where to start.

[Georgi Baltov]

As I said, cutting it will not be an issue. Aluminum from my experience might cut better than some oily hard woods. Cooling however is the main issue. The heat destroyed my tooling. Using coolant is an option, however when I did it I didn't want to soak everything with it and didn't want to make any retrofit to allow constant lubrication of the bit. Plus if later I decided to cut wood again I needed to make sure there's no residue left over because it might stain the wood.

I've cut plenty of plastics and aluminum is in a league of it's own. If you can solve the heat issue then by all means go for it.

[Brad McIntosh]

As an alternative to liquid coolant, some of our clients have had success by using a combination of an "air chiller nozzle" directed at the too/cutting area and and special tooling that was dipped in a kind of non/low stick coating.

The "air chiller noozle" was similar to these:

http://www.arizonavortex.com/vortex-tube/
http://www.directindustry.com/prod/nex- ... 54875.html

And here is en demonstration of one working: http://www.youtube.com/watch?v=rVCq-V0GzBQ

I can try and get more spec's on the type of coating used in the tool "dipping" process.

[Zach Froble]

I just wanted to thank Ryan, Brent and everyone else for their suggestions and help. I ended up getting the tool that Brent recommended (Onsrud 63 series o-flute). I didn't cut it one pass like everyone said I could, I was a little conservative. I figured I would post my setup in case anyone else ever needs it.

Onsrud 63 Series O-Flute Upcut bit .25 Dia.
150 ipm. 16000 rpm
.03 depth of cut per pass

Cut like butter. I did squirt a little coolant on in the path every so often.

I could have taken a larger depth of cut, but it was cutting so smooth and I didn't want to take any chances since I only had 3 pieces to cut.

Thanks again,

ZachF

[Ryan Hochgesang]

Thanks for the update Zach. Sounds like you just added another tool to your toolbox