How to get best "mirror" machined flat finish on 6061 aluminum

PaulT · Sep 8, 2009

We're working on a new product that starts as a long block of 6" x 1" 6061 aluminum.

The top of this block needs to be highly polished, after some pockets have been machined in it.

On the prototype, with the tooling we currently have we're using a 3" diameter APKT insert based face mill to make a 0.012" skim cut on the block, but with about 70% overlap it takes 3 passes and we're seeing some transition lines on the part, along with some fine machining lines.

We then go through a power sanding and then buffer wheel polishing procedure to get a pretty nice close to mirror finish, and this has been fine for the prototypes.

But I need to speed the process up for the real products. To reduce the amount of sanding and polishing required, I need to improve the finish quality of the facing skim cut we're taking.

Starting from scratch, what would be the best facing mill design and insert type to get the best possible finish on the facing cut we're taking?

Its ok if its a very slow pass, it will still pay off in reducing the sanding/polishing step.

Looking around a little it appears that a one or two insert based "fly cutting" type tool might be the best approach, is that true? (and if its that simple, I might just fabricate the tool)

I've never used and don't know anything about "wiper" inserts, would a wiper insert help?

Thanks,

Paul T.

706jim · Sep 8, 2009

I've read that diamond inserts make a lovely finish on aluminum and other soft metals.

There's never been enough money here for me to try it though.

Rstewart · Sep 8, 2009

Try the 3" Shear Hog facemill by A B Tools inc. I've been using them for about 2 years and they are The Ticket on AL.

Tonytn36 · Sep 8, 2009

Get a PCD insert, the bigger the radius the better.

Mud · Sep 8, 2009

Make sure your inserts have an 'up sharp' edge, meaning no edge prep to get the best finish. One insert in the cutter is the cleanest but will slow down the feed possible. A wiper will allow a faster feed but won't help the ultimate finish. A cutter wider than the material like a flycutter will eliminate the marks left by multiple passes.

We cut with Iscar E90AL face mills where possible with the APCR inserts for aluminum, they work about the same as Shearhogs. We feed fairly slow but not excessively so. Then we sand it with a DA orbital sander with 320 paper and buff.

You need some serious power to buff it economically, that might be what is missing. If you have a 3/4 or 1 hp buffer you'll die of old age getting it polished. Pick up a 5 hp min. buffing machine, get some big wheels and the right compounds and it will only take minutes.

John Welden · Sep 8, 2009

You'll need a cutter the width of the part to get rid of overlap marks. Might be cheaper to make your own.

I might do my finish pass on the block before cutting the pockets. The cutter may be happier with a less interrupted cut. Might not matter though, just something to consider.

stephen thomas · Sep 8, 2009

What you really need is a good tight shaper. M42HSS bit with 5% cobalt. Sharpen like for finish cut on steel, or (alternately) with some side sheer and a largish nose radius. Stone the edge to a good polish. Any DOC you want. Fine step over. Use ATF for cutting fluid, run shaper as fast as it will go without rocking. You'll get an irridescent polished finish looking better than ground. Nice thing is shaper will run unattended except to load & unload parts.

BTW, I've never tried it, but in a production environment it might be worth making a heavy stick holder to take APKT or similar high shear carbide insert, and experiment to take the "vagaries" out of who sharpens the bit.

smt

Limy Sami · Sep 8, 2009

''The top of this block needs to be highly polished, after some pockets have been machined in it.''

If it's got to be an optically good polished finish, polish it first then cover with masking tape and m/c,- thro' tape and all,..... IME mechanical polishing can/will round over thin sections, edges etc,....... which mightn't be what's wanted.

TonyOW31 · Sep 8, 2009

Make yourself a single point flycutter with a PCD tip that spans the whole surface ( it will need to be well balanced). Spin it up real fast, and do 1 finish pass. You will be able to shave in the reflection.

PaulT · Sep 8, 2009

Fellas, thanks a lot for all the responses.

Based on your suggestions, here's what I'm thinking.

Make an 8" diameter single point "fly cutter" style cutting tool out of a balanced length of 2" square 1018 steel (Stephen, this setup is the closest I'll be able to get to a shaper).

Use a CCMT insert lathe tool on the end of the fabricated cutter. I chose CCMT because you can get PCD tipped CCMT inserts from these guys:

http://amtektool.thomasnet.com/view...s-80-176-2/ccmt-pcd-inserts-80-176?&forward=1

If for some reason the PCD insert doesn't work out, I can use the extra sharp and polished CCMT inserts from Curtis at:

http://www.latheinserts.com/category.sc?categoryId=46

I'll use the largest radius I can get in that insert size, which is .031"

I know the single point method will be slow, but that's ok, while we're facing one my shop guy can be sanding/polishing on another one.

Does anybody see any flaws in this scheme or a better way to go?

Mud, thanks for the comments on the buffer, what we've found so far is that once we sand it to the point where the machining lines are no longer visible it buffs up surprisingly fast, even on our (ok, you nailed it) 3/4HP buffer. If we try to start buffing while the machining lines are still visible, you either can still see them or if you buff hard enough to get rid the lines, you get some waviness from the buffing.

So its the sanding operation that's taking most of the time right now, so I think if we can get the surface to a much smoother machined state, the sanding will go much faster.

I'm surprised with how nice a polished surface we're getting now though even with the prototypes, 6061 really polishes up nice.

Paul T.

PixMan · Sep 8, 2009

If you had enough work like that to amortize the cost of the tool, there is one new cutter out on the market that I've tried that is simply amazing for really fine finishes in aluminum.

It's a Valenite V650 "V-Flash" cutter. The only inserts available for them are PCD and CBN, and they are intended to be a "finish" face mill. With the full-edge PCD inserts you could do some serious roughing too. Be prepared for high speeds and high feeds. The 3" six-insert cutter a friend of mine recently bought is the "coarse pitch" version and he's running full out at 10,000rpm and 300 ipm feed and getting a consistent 6 microinch finish. He's now wondering what kind of finish he'd get by adding a wiper insert (or two, for balance).

If he had a 25,000 rpm spindle and the fine-pitch (9 insert) version, the cutter is rated for 28,000 rpm, but he'd have to feed it in rapid.

.005" fpt x 9 x 28,000 rpm = 1260 ipm. That's the 32m/m rapid rate of his machine! He got a little discount from his distributor that he bought it from, but the list price was $968 for the cutter and $108 each for the inserts (.13 max d.o.c.) He said he made his money back for the cutter in less than 6 weeks over the 45 ipm he was running before to get a coarser finish. No more polishing required. Machines the parts and ships 'em.

http://valenite.com/internet/4558/I...baa18ce858525759e006e0a28/$FILE/vflashcat.pdf

Hdpg · Sep 8, 2009

If you are doing a lot of these parts it may be worthwhile investigating a vibratory lap. Essentially a flate plate that oscillates in a random pattern, you place your part on it with some appropriate grinding/polishing media and it polishes it flat and shiny.

SteveinAZ · Sep 8, 2009

Paul, I was recently informed about APKT inserts and their tolerance...or not so tight tolerances. Anyway, was using an in-the-machine (with polished APKT inserts) stock one for facing and had a pretty poor finish. I had Curtis Payne send me a 3" Ripper, same feed/speed and the finish probably improved from a 125 to a 32, although I didn't check it. HUGE improvement.

I needed the 3" for another job so I call to get the big radius inserts that are cataloged at 0.355"R - well that's a misprint. The largest radius is 0.125"R, which was also fine for this job, but Curtis had told me of quite a few guys that needed the 1/8"R and he couldn't help them with the Ripper, now he can. There were actually quite a few catalog misprints on the insert radi - like 3 of 5 are wrong, give Curtis a call to strighten it out.

Back to the facing, I think the finish cut was at 0.050" doc and 0.002"/tooth on the last job, I would guess the finish is in the 16 range with no mismatch between passes, only a better finish on the overlap area. The Ripper is a fine product, but it is not for those who want to spend 2X on the body and 50% more for inserts. Down side, no PCD inserts.

Give Curtis a call.

Steve

CBlair · Sep 9, 2009

I have found that I get the best finishes when I have all my cuts go the same direction. That is I climb mill rather than go back and forth like most face milling routines. This may just be on my machine, I dont know if anyone else has the same experiance or not.

Charles

John Welden · Sep 9, 2009

CBlair said:
I have found that I get the best finishes when I have all my cuts go the same direction. That is I climb mill rather than go back and forth like most face milling routines. This may just be on my machine, I dont know if anyone else has the same experiance or not.

Charles

Yes, I always do that if I need multiple passes and a fine finish.

fmari --MariTool- · Sep 9, 2009

Nachi brand works amazing. They are DLC coated and they actually recommend using it dry on Aluminum. APET160508PDFRSN-DLC100. I made the mistake by using it to rough and take deep depths of cut, nut the best and it wore out quickly. I dont think it has the edge strength. But for fine finishing it is amazing. High rpms and fine feed the chips are like Aluminum dust. Hard to take a good picture from the reflection, inserts are blue in color.

IAMATT · Sep 9, 2009

Polished from milling I dont think this is possible. You can get a very nice finish from several cutters with high speed low feed. I havent ever heard of the above insert so maybe something has changed over the years. Polished means micron level ridges which you are not going to get milling.

PaulT · Sep 9, 2009

Thanks again for all the helpful tips fellas.

Frank, will those APET inserts you mentioned fit in an APKT face mill?

Thanks,

Paul T.

fmari --MariTool- · Sep 9, 2009

Paul,
As long as the other digits line up it should fit. 3rd digit is only a tolerance spec.

PaulT · Sep 10, 2009

Tool tip radius limits?

It looks to me that it would be best in this cut to use the largest tool tip radius possible, and the CCMT inserts I'm looking at now to use have a max radius of only .031"

But looking around I ran across some round RCGT-AK inserts that are also highly sharp and polished for aluminum.

They are available in diameters starting at .236" and going up from there.

I've never used a round insert before, will they work ok for this light (0.010") kind of finish cut in 6061, or is this too big a radius to get a good cutting operation and finish?

Thanks

Paul T.

How to get best "mirror" machined flat finish on 6061 aluminum

Stainless

Titanium

Stainless

Diamond

Diamond

Diamond

Diamond

Diamond

Stainless

Stainless

Diamond

Stainless

Stainless

Diamond

Diamond

Titanium

Stainless

Stainless

Titanium

Stainless

Similar threads