Milling sheetmetal - fixturing tips?

Ken Gracey

Hey all, the laser cutter and Delrin have been a fantastic choice for my quadcopter, but I'd like to take a whirl at CNC machining some sheetmetal for some airframe chassis parts. Normally sheetmetal is machined on a CNC punch and it's not too practical to mill it due to fixturing issues.

But I know many of you have done this successfully. I suppose the absence of coolant makes it a whole lot easier to secure but results in a poor finish.

The kinds of pieces I'd mill would be 6061 0.063 aluminum, about 7" square or smaller. What kinds of tricks do you have for securing this to the table? Any special double-sided tape? Are you drilling the holes first and then securing with screws into a fixture underneath? I'd really enjoy a hassle-free approach if one exists. Bonus points if the setup can accommodate coolant. No magic please.

Thanks in advance for the tips!

Ken Gracey

kwinn

How about using a vacuum table to hold the sheet metal and recirculate the coolant/cutting oil.

Phil Pilgrim (PhiPi)

Ken,

The way I do it is to clamp the sheet metal to a sacrificial piece of MDF, as shown in the photo (which shows G10, rather than aluminum):



Don't overtighten the clamps, because the aluminum might bow upwards. You also have to be careful planning the cutting path, since a spiral-flute mill will tend to pull the sheet metal upward, and you don't want it flapping around while it's being cut. (I've sometimes resorted to pressing down on the metal with my fingers while it's being cut to keep it from vibrating -- but you didn't read that here!)

Another method I've used is to clamp the sheet suspended between two metal blocks. I don't have a flood cooling system, though, so it's hard to keep coolant pooled where it's needed, since it runs away through the cut slot.

In any case, vibration and flapping around of an almost-finished piece are the biggest issues. But I've only ever used spiral-flute mills. You might have better luck with a milling cutter having vertical flutes, since it won't tend to pull up on the material.

-Phil

Ken Gracey

@kwinn, hmm. At home I have a desktop CNC with no vacuum hold-down table. But at Parallax we have a CNC router with vacuum hold-down. No coolant is used on that machine, however.

@Phil. OK. I think I could give this a try. The biggest problem is lifting the sheetmetal up off of the MDF as you pointed out. I'm not familiar with vertical-flute cutters, only spiral cutters. That's another good idea to try. Any luck with adhesives of any kind? I realize it's a hassle to clean them off of the metal afterwards, but I'm happy trading that labor for other headaches like making a fixture.

Thanks for the tips so far!

Ken Gracey

Phil Pilgrim (PhiPi)

'Never thought about it, but a spray low-tack contact cement or double-sticky carpet tape, combined with clamping the ends to the MDF might be enough to quell the vibration and lifting. I wouldn't rely on it in lieu of the clamps, though. And you don't want an adhesive so aggressive that you end up bending the parts prying them off. BTW, WD-40 is good for removing adhesive goo.

-Phil

Ken Gracey

Maybe we need a waterjet at Parallax, or a super high-powered laser cutter. . .

Ken Gracey

Phil Pilgrim (PhiPi)

Ken Gracey wrote:

Maybe we need a waterjet at Parallax, or a super high-powered laser cutter.

Now you're talkin'!

-Phil

Roy Eltham

If you use a slow feed rate, then cutting thin aluminum sheets shouldn't be that problematic. Just do what Phil does with a piece of wood/mdf under it and clamps around the edge.
Also, depending on what you are cutting out, you could leave little "break away" spots that you can snip out after it's done.

RonP

Ken,

If the design is similar to your other designs with a hole in the center, you could drill a hole in the center first and bolt it to MDF or whatever that might keep it from lifting but then you would have to cut out the center last. Just a thought.

-Ron

Phil Pilgrim (PhiPi)

'Nearly forgot: Another thing I do with thin stuff is to tape the top and bottom edges to the MDF (top to over-the edge) with masking tape. This helps to quell any vibrations from the piece as a whole, before the part is nearly free.

-Phil

Ken Gracey

@RonP. Yep, that seems like a possible approach. I could use the existing holes to secure the material to a substrate underneath, and mill them out last.
@Roy, this stuff climbs up end mills something terrible. An inch away from a hold-down of some kind can be too much with 0.050" aluminum. The break-away spots could be useful in combo with Ron's suggestion.

Thanks for sharing the ideas.

Ken Gracey

Phil Pilgrim (PhiPi)

Here's a wild-haired thought and something I've never tried, but I wonder what would happen if you clamped a collet onto the milling cutter to keep the metal from climbing up it? Probably a bad idea, on second thought, since the chips would be trapped under the collet.

-Phil

W9GFO

I just clamp it on top of sacrificial material, either PVC or mat-board and use my fingers like Phil (or the end of the vacuum that is collecting the chips) when it starts vibrating. Can't say that I've had much problem with climbing up the end mill. Maybe higher rpm or slower feed rates would reduce that?

Roy Eltham

Ken, you might try a harder aluminum, like 5052, instead. I've read that it actually works better because it holds the sheet shape better when cutting. Of course you have to slow down the feed rate a little for it.
Another thing I've read is that you can stack a few sheets and cut that and only the top one is "throw away".

Ken Gracey

Roy and W9GFO - excellent points and I shall put them both to use on the trial run.

Didn't think about using 5052 but I'll take a look at the metal properties. As long as it's not too gummy it should work great. Thanks for the tip.

Ken Gracey

Phil Pilgrim (PhiPi)

I've always used 6061-T6. It machines nicely, but it doesn't bend very well, tending to crack. 5052 is not as brittle as 6061 and is less liable to crack when bent sharply, but it has a reputation for gumminess when machined.

-Phil

Paul K.

I use clamps like in Phil's picture but use one on each corner. Since you don't want to make a fixture just leave tabs holding the part in the main Al sheet. One on each side 1/8" is plenty. Then you table saw cut the part out of your stock at the end and sand the tabs down. Then use a SOS pad to brush the final piece.

I would use 6061 it machines the best. Use a carbide 2 flute end mill 1200-2000 rpm at about 2-3 feedrate. Play with the rpm till you see chips coming off not dust. Take about .035 of at the most in one pass. I use these rates with a 3/32 or 1/8 endmill.

Do a rough cut first at the rates above. Cut you piece out about .01 - .015 larger than it should be and then do a 2nd pass at the correct dimension same rates as above but at the whole depth of the material (.063). Then do a final pass at 10-15 in/min at the whole depth of (.063).


Heres a link to my last project. The wings are from .032 and the body is .063
http://forums.trossenrobotics.com/showthread.php?t=4561

DukeJCDC

Depending on the size of the piece, you could also tape it to a clean piece of aluminum. Clamp a piece of aluminum and skim it clean. Use a pretty strong double sided tape to tape it down then cut it with maybe a 1/8 or 3/16 endmill at a slow feed rate. If you want a nice finish on the edge, leave .02 extra material on all sides then make a second pass to clean it up. Also, leave .005 stock on the floor. That will keep the mill from getting tangled up in the tape and help leave a nice clean finish.

Ken Gracey

DukeJCDC wrote: »

Depending on the size of the piece, you could also tape it to a clean piece of aluminum. Clamp a piece of aluminum and skim it clean. Use a pretty strong double sided tape to tape it down then cut it with maybe a 1/8 or 3/16 endmill at a slow feed rate. If you want a nice finish on the edge, leave .02 extra material on all sides then make a second pass to clean it up. Also, leave .005 stock on the floor. That will keep the mill from getting tangled up in the tape and help leave a nice clean finish.

Thanks Duke - I think your approach is ideal if I can make it work properly I'll do it. I'm planning ahead to do this project in about 10 days, not a minute sooner because of obligations elsewhere.

Most importantly: WELCOME TO THE FORUMS! The welcome committee would like to make you right at home. We're glad to have you as part of the ongoing, 24/7 action. You'll find lots of qualified people on this forum - I'm more of a learner than a contributor but I have tremendous respect and appreciation for those who can answer the real technical questions.

Ken Gracey

DukeJCDC

Thank! I'm spanking new to the world of robot building. It's something I've always wanted to do and am hoping to do as a career here pretty soon

If you have any more questions or anything, feel free to ask. I'm a lead CNC machinist at a full service engineering firm. And once I get my Boe Bot here in a few days, I'm sure I'm going to have tons of questions to get it up and running.

Tubular

We use a special Tesa 1" wide double sided tape for this purpose (machining 3mm acetal, taped to 16mm mdf).

Since you're 10 days out I'll post you a roll tomorrow. I owe you a roll of tape anyways

Capt. Quirk

So long as you are not cutting a large area of sheet stock, Why not just make a fixture out of some rem stock steel or aluminum.
It would certainly make your efforts more safe and repeatable.

Besides, making chips is fun!