Aluminium Question :-)

[dubliner]

I have to cut anodized, 1/6th in Al with an 1/8th bit. The cuts will be vent slots, a logo etc, so they have to be clean and look like they were done on a CNC, glad I have one, they plate will be about 40x24, with the pattern cut into it, then it will be bent to be a cover over some electronic gizmos. What bit, what feeds and speeds would you use to get a pretty flawless edge in that material. PRS Alpha, 4hp Spindle, 15hp blower. Thank you kind chaps in advance, Nev

[knight_toolworks]

as long as it is hard aluminum like 6061 you can cut it at 1ips 14 to 16k and .09 or so depth of cut I use .5 speed on the z a good 0 flute makes a world of difference though you are limited on what you can find in .125. well my speeds above are for a 1/4" bit so you may have to take less per path and or go slower. also you want a climb cut that will give you the smoothest cut.

[cabnet636]

do you know the grade 6061, 3003 etc, the higher the harder and harder is better for machining, lower is softer prone to rewelding. that said

i have never done anodized, yet i would start 12- 14000 rpm 60 or less ipm at .0625 deep on a test piece if it chips cool. then you might up it a bit.

hope you have some test material and use an "O" flute bit

[majohnson]

some coolant would help, fresh new not resharpened cutters another plus.

[lcolburn]

I've done some .04" thick anodized before with pretty good results. 1/8" solid carbide two-flute end mill (from McMaster or the like), 10k rpm, 100 ipm, .015" pass depth, climb cutting.

Hold down is a pain- if you have some scrap acrylic I find it helpful to use this under the AL, and just spray-adhesive the AL down to it. Got to watch out if you're using coolant or oil as these will compromise the spray adhesive. In my experience the thin stuff deflects down away from the tool when cutting, so I have to overcut a lot if I'm using an MDF spoilboard. Harder stuff like acrylic alleviates this problem slightly.

Also if it helps, I usually leave the protective plastic film on the AL until after I'm done cutting it.

[dana_swift]

Neville- I dont use any cutting fluid when I work metals, I just use compressed air blowing directly on the bit. It clears the chips and cools everything quite adequately. When a cut is finished, the bit is hardly warm.

The air regulator is set for about 40psi when there is no flow, coming from a 120psi feed. The flow rate is pretty high, pretty much what ever your air compressor can maintain.

Beyond that, follow Steves advice. I use 0.125 dual flute upspiral bits and they work good enough. It does eat the cutting edge on bits, so prepare to pitch the bit(s) when you are done. Add that to the cost of the job, but 0.125 bits are inexpensive. The ones I use dont have any special coatings either. That might help, but I have not tried it.

Good luck! If you have any extra material, make some test cuts to raise your confidence.

D

[dhunt]

some coolant would help,
fresh new not resharpened cutters another plus.Would the occasional squirt of WD-40 (via the thin red tube for accuracy) work?

We use Amana solid tungsten carbide spiral upcut bits almost exclusively..
T.Carbid has a hardness rating of 9. --Aluminum has to be way less than 6 or 7.

How does all that factor in? ..with a squirt of WD-40 every half-inch or so?
Crazy?

.

[cabnet636]

neville if you are gonna do a lot of this try a cold gun,, this will do the trick

http://www.airtxinternational.com/cold_air_guns/

[Brady Watson]

Anodized AL at that thickness is no more difficult to cut than non-anodized AL. Single spiral-O flute, 3/16" dia or greater will work just fine.

No coolant or lubricant required. You can if it makes you feel better, but the cut won't look any better. Just get your chipload right and Z-ramp into your cuts.

-B

[br928]

I have used 1/8" single O-flute on aluminum with good results. About a 1/16" per pass. I do use a cold air gun, because I have one, but compressed air to clear the chips is all that is needed.

[dubliner]

Thanks all, yes I have to use .125 bit on this one. I guessed I could cut that in one pass, just want a "finished" look as it's part of a musical instrument so appearance and fit of the other parts are critical. Being such thin material I thought a neg or pos shear would bend/lift the edges so I thought zero shear. Any thoughts on that?