Advice on cutting aluminum?

[myxpykalix]

I have someone who needs a piece of 3/8" thick aluminum that is approx. 24"x36" that needs a relief carving done cut .25 deep in it..SO

since i've never cut aluminum on my bot i need advice on the best bit, depth of pass, feeds/speeds stepover and whether i need to have some type of cooling?

Thanks for the help.....:rolleyes:

[bleeth]

solid carbide ball nose as short as you can use, 8-10k spin, cut in passes .07 deep or so. Use tapping fluid. Blow your chips away regularly. Move slow (.75-.85 ips). Most issues will come from not having the piece properly secured. I don't recall whether you have a router or spindle.

[Brady Watson]

Don't plan on it turning out as well as you think it should. You need a really tight machine, tweaked ramps, small stepovers and correct tooling to do even a marginally good job. The Bot really isn't the right tool for this type of work. Not saying it is impossible...just that you shouldn't be fooled into thinking that it is going to be a walk in the park. I would not be surprised if it took several days to rough out and 3D machine.

-B

[bleeth]

And since BW taught me everything I know about machining aluminum I would believe him!!
And don't even think about milling the hard aluminum!

[knight_toolworks]

Don't plan on it turning out as well as you think it should. You need a really tight machine, tweaked ramps, small stepovers and correct tooling to do even a marginally good job. The Bot really isn't the right tool for this type of work. Not saying it is impossible...just that you shouldn't be fooled into thinking that it is going to be a walk in the park. I would not be surprised if it took several days to rough out and 3D machine.

-B
very true plus the best bits to cut aluminum with a cnc don't leave the best surface.

[myxpykalix]

I was incorrect in my depth. It only needs to be cut .10 deep. How many passes would i need for that? Does that alter the feeds/speeds mentioned above?:eek:

[John Rucker]

I think we have cut more aluminum than any other material with our ShopBot. Works very well!! We use it to create faceplates and custom outside enclosures. I have found the best results with Onsrud 65-xxx series bits. They have one flute and create an excellent chip to dissipate the heat. The bits are warm to the touch after a multi hour cut in marine grade aluminum. I don’t use any oil or forced air since the aluminum chips carry away all the heat. We have a router and cut at 10,000rpm.

I have included a video I made that use to be on the buddy’s home page.
http://youtu.be/Nc5fMqJf6DE

http://www.solar-current.com/images/ToolCfg65-025.jpg

[myxpykalix]

dave,
"Move slow (.75-.85 ips). "

don' you mean IPM?

[Brady Watson]

It depends on how much detail there is in the relief. The smaller the bit, the more precarious it gets. You can't machine it like you do wood. You can't just rough out with a 1/4 or 1/2 and then go right in with a 1/8 or 1/16 without first running a 'rough finishing pass' to clear out as much as possible before doing final finishing.

Get a sample piece of AL, a pile of bits and machine a snapshot portion of the actual relief. That will get you in the ballpark.

2D cutting of AL is WAY different than 3D relief machining of AL.

-B

[myxpykalix]

john,
your video was very informative and i want to look more at your solar stuff later. Based on your settings and advice the best time i could get was over 30 hours but it is a fairly big file so it is what it is..:)

[myxpykalix]

brady,
i might have mis-stated what i want to do and is more like 2d cutting out of a shape with a flat face (as you talked about) as opposed to 3d relief carving of the surface of the piece.

using his settings above and the advice from you guys my cutting time is is still in the 30 hour range.:(

[John Rucker]

Yea for a big job this may be a very slowwww process. I have bumped up the speed with bigger bits but i bet it still is way too slow for what your wanting to do.


john,
your video was very informative and i want to look more at your solar stuff later. Based on your settings and advice the best time i could get was over 30 hours but it is a fairly big file so it is what it is..:)

[knight_toolworks]

with a 1/4" bit I can cut .09 in a single pass at 1 ips.

[bleeth]

I meant .75 to .85 IPS Jack. I don't think in IPM. In otherwords; slightly less than 1 inch per second. This is assuming a good quality 1/8 ball nose, ramping in, and the other good advice you have received from other posters and the other things that I wrote previously. This is a starting point considering that there have now been a couple different explanations from you of exactly what you are planning! A picture is worth a thousand words.:)