Having trouble cutting aluminum sheet

[fastturbovet]

We have an application where I'm cutting .020" 6061 AL sheet. We are doing it on a Bridgeport CNC which can go up to about 3500rpm or so. We're taking a piece thats 9" x 2" and I am cutting out a bunch of channels with a 1/16" endmill. The item is a heatsink and I need the channels cut out so that it will not touch any exposed traces on a circuit board when its installed, so they need to be accurately cut and with as good and "square" a cut as possible.

I am having a couple of problems. The first is that its extremely hard to hold down the sheet. Because I am cutting it, there ends up being small peninsulas of metal which are not very rigid. Any tips on holding it down? Problem is it will be bonded with epoxy to a PCB later, and if I use tape it can leave residue which is tough to get off (since the sheet is thin you can't rub it hard without bending/deforming it a little). I thought about making a custom adapter plate for a vacuum clamp? I also thought about taking a thicker piece of material (maybe steel) and cutting out the same channels in maybe 3/64 width and clamping that down over my AL sheet before milling. We also thought about stacking the sheets maybe 3-4 thick and clamping them down with a top-plate to help with the problems. Any other ideas? Which of these ideas sounds best?

Second problem - getting a pretty bad finish on the cuts. There are tons of burrs and hanging bits of shredded AL all along the edges of the cut. Is this a vibration problem? A tool deflection problem? A feed/speed problem? Or maybe a combination? I am cutting dry with no coolant, and the last time was full depth of cut (.02"), about 3,000RPM with about 4ipm feed. That was a "WAG" )wild-assed-guess) so I could be way off. What could I do to help with this? Different feed/speed? Fixture the part better? Carbide endmill? Less depth of cut? Is my DOC OK doing the full .02 at a time with a 1/16" endmill? Or should I try to take it easier?

And last but not least, I am not necessarily tied to 6061AL nor to .02" material (but I'd like to stay somewhat close). If I went to .05 or .06" thickness AL would it be easier to machine and fixture? I am also not tied to 6061AL. I can get 7075 in the same sheet size, so thats an option too. Being more brittle I wondered if it might flake easier and not burr up so muhc?

Any tips welcome - trying to get this figured out in the next day or so

[harvard5]

Try the 7075 we use it all the time repairing aircraft it finishes alot better than 6061. I don't know much about holding it down but I have used a vacum table to hold down balsa wood to use a router on it and it worked great!
Bill

[cbass]

Hey, you guys are tied for posts

Sorry, couldn't resist (its late, I'm tired etc..)

[Spezzaferro]

Harvard5 is right, 7075 is a lot better to machine than 6061
I cut thin sheet a lot and I use a double sided vynal adhesive that I pick up
at a sign shop supplier, It's quite pricey but it works great and leaves no residue.comes off all in one shot. I use a Carpet roller to roll on top of the sheet to ensure good adhesion.
Also I use a sacrificial piece of aluminum underneath and . with .020 material
i would go .050 deep, but cut your sacrificial first,

[mxtras]

This seems like a tough one, that's for sure.

5052 is an extremely common .020" coil and cuts well - another option, maybe.

How many of these do you have to make?

I think I would try a clamp plate arrangement to trap the material between two plates. You could run the part profile in the top plate with a larger diameter tool for clearance, then maybe even relieve the bottom of the top plate to increase the local clamping pressure around the windows.

Vacuum doesn't seem like an option, but I don't have a clear image of exactly what you're doing.

Scott

[little bubba]

For the burrs I would go with a carbide endmill, your probably bouncing all over the place. Are you climbing, conventional or full width? Generally climbing will keep you almost burr free, if your going full width is it possible to take a .002" or so clean up pass? You didn't say what quantity your making but if its only a few I would go with the double sticky tape, just drop it into a shallow pan of acetone after if there is some residue. If you have to do a whole bunch, a steel template over the top sounds like a good idea, a vacuum chuck sounds like even more fun.

[fastturbovet]

Thanks for the feedback. I am going to a local metal shop tomorrow to see if I can't pick up some 7075 and also some 1/8" stock to make a top-plate.

I have to make quite a few of these. Its for an electronics doo-dad we're making and we will probably need about 100-150 a month to start, and once we convert some other electronics products over to this new style we will need maybe 200-300/mo or so. Sticky tape would probably work but it gets expensive and its difficult when you consider how many we'd be doing.

I am going to go with the top clamp and 7075 and see how it does. The problem is, imagine if you were taking a 12"x12" square, and cutting (from the center) 5" one way, moving up 1/2", cutting 10" back, going up 1/2", cutting 8" back, etc, etc. You would have these thin slivers of material that were *extremely* flexible. Thats the problem I have - once the machining is done, the part is flexible as a sheet of jello. I will try the double-sided tape and use acetone to remove if the clamp idea doesn't work as hoped

Thanks!

Mike

[miljnor]

when making a sandwich style set up its best not to cut the channle in the top plate first... just sandwich the material inbetween to plates of material and cut everything at once. if your top plate and sub plate are thick enough and the sandwich is nice and tight this will also eliminate your burrs.

The other method is wax but you said you didn't want a residue. and you would still have to melt the wax off. the lower melting point wax melts in boiling water.

[Karl_T]

Considering how many you're making, look at sending this out to a laser. Tolerance on laser cut is around 0.010 may be a shade better, might be a problem for you.

Karl

[ViperTX]

If the backside of the aluminum doesn't need to be flat and in the quantities you're speaking off....I would look at some type of forming rather then machining....tool & die comes to mind as well as hydroforming....

[miljnor]

the company i use for laser can keep +_ .002 on that thin of material

[skippy]

As vipertx says, I would definately look at a tool and die set up. Considering you have a mill to make the tooling and the product quantities are not large, a manually operated set up would take no time to punch out 100 - 200 units. I guess first compare costs with contracting out to a laser guy.