[RP Designs]

So I am still waiting on my mill to arrive so I have to entertain myself by trying to pick the brains of the many experienced pro's on this site. I have tried a search and not really come up with a great answer. I have been watching youtube videos of different milling operations. I have seen many machines produce a near mirror finish on aluminum straight from the machine. Of course these where VMC's and I have no idea of what RPM they where turning. I will be running a kneemill which currently can turn the spindle at 4200rpm max. My question is what spindle speeds do I need to produce these types of finishes right off the machine, assuming the set-up, tooling and coolant is all perfect?

[Jason3]

Hi there,

Were you looking for a mirror finish from face milling, or on a 3d surface? Are we talking about a CNC knee mill? You have plenty of rpm to get a good result from a face mill in alu, but that would take some time on a 3D surface.

For the best finish on Alu with a face mill I like the 45° insert type - this is the one I use: Maritool 45° face mill I also use this face mill (with different inserts) in steel, with a near mirror finish too - take a look at the video on that page, I'm getting comparable results on my (manual) knee mill. Take a light finish cut after your roughing cuts - knee mills are comparatively flexible, and you won't get a brilliant finish with a heavy cut.

If you need to mill up to a shoulder, I find this one gives nearly as good a finish: Maritool 90° face mill

In both cases you'll get the best results with the inserts designed especially for aluminium (usually very sharp, polished inserts).

You can get a nice finish with on a flat surface with a decent sharp end mill, but generally the swirl marks will mean you wouldn't consider it 'mirror' finish. On a 3D surface more RPM would greatly speed things up, but generally you'll want a very small stepover and stepdown, and your CAM software will need special 3D strategies to get the best results. I get good results with a 1/4" EM @ 25,000 - 35,000 rpm and feed rates around 100 ipm. With a 4200 rpm max, just drop the feed back proportionately and keep the coolant on - either flood or an air/mist blast. The important thing is to keep the chips out, and the cutter cool.

You can also often add a VFD to get more speed from your standard spindle motor - several others are doing this with good results, some are getting as much as 8500 rpm that way. I don't know what effect this might have on the longevity of your spindle bearings though. I use a VFD on mine, but haven't needed to turn it up past 4200 yet.

Hope that helps

Best regards,

Jason

[stag53]

Getting all the way to true mirror by machining won't happen... BUT, diamond tooling will get you the closest. PCD (Poly Crystalline Diamond) will get a very shiny surface, and Mono-Crystalline will get you a little closer. High speed, high rigidity, lots of coolant needed...

[MrWild]

You will never get a polished look. For that you need to buff, and mahcines that buff, don't use tooling. They use cloth and rouge.

[ImanCarrot]

To get a true optical mirror finish you'd need to diamond turn it. There's lots of companies that'll do it for you, but they aint cheap!

[LeeWay]

I started out polishing my aluminum parts before I learned how to powder coat. It worked pretty well.
Sand progressively from 150 to 600 grit. Then polish with compound. Finish up with hand rubbed Mother's.

[RP Designs]

By mirror finish I mean a very shiny surface with minimal swirl marks. Mostly I would be concerned with the flats, so face milling and edge milling.

[PixMan]

With the top speed of your milling machine, the best benefits of using polycrystalline diamond (speed!) may not be seen. However, if you want your aluminum parts to come off the machine with the best possible finish and minimize polishing, look into a Valenite V-Flash V650 mill.

While you can't take advantage of the 2" cutter's 35,000 r.p.m. maximum speed, you can really use the fine adjustment of the inserts to get a near-mirror finish. The inserts in the cutter can be adjusted to within a micron or two, with the insert already snugged into the pocket. Use a wiper insert on it and the results on aluminum are stunning.

I've never seen insert sizes held to such tight tolerances, so having the adjustment of the inserts in the cutter is the only way to assure perfect alignment. Older designs had you snug down the insert, measure the deviation from tip-to-tip, loosen them, adjust, tighten and re-check. It would often take so long to do this that many people would just resort to using two of 6 inserts. Now with a cutter you can adjust with the inserts in tight, you'll get all 6 (more or less, depending upon the one you get) inserts cutting perfect in short order.

[mc-motorsports]

To get a true optical mirror finish you'd need to diamond turn it. There's lots of companies that'll do it for you, but they aint cheap!

What material is that?

You even have a perfect finish around the bolt holes where it's an interrupted cut, nice!

[Geof]

But he only takes off half a gnat's whisker DOC with a machine that weighs in at tens of thousand of pounds I think.

But it is nice, much much betterer than I can get on my TL2.

While I am posting I guess I can make my comment to the original query: In my experience 4500 rpm is far too slow and you need to be up around 8,000 or more with cutters around 1/2" to 3/4". On side milling I have even noticed a difference between 8,000 and 10,000 with the finish being much shinier at 10,000.

But it is not just the rpm it is also the feed and machine rigidity. Look at the parts in this picture:
http://www.cnczone.com/forums/attach...4&d=1183321427

These were faced using a 5/8' corner radius two flute mill at 10,000 rpm, about .05" depth and 100 ipm. Swirl marks are visible and they are most pronounced at the locations were the cut has started or changed direction. My explanation for these is that the entire head bobs slightly when the machine shakes due to the table rapidly changing direction. The radius around the perimeter is done with a large two flute carbid router bit in one cut again at 10,000 rpm but the feed is only 50 ipm and there are no ripples visible in this. If the facing feed is dropped down to around 50 or less the swirl marks are barely visible.

[mc-motorsports]

I made this many years ago, 3" facemill 3000 rpm on a conventional BP. The head was perfectly square, possibly leaning .0005" towards the front, spraying WD40 inbetween the inserts to reduce dragging on the back side. It's as good as I could get with the equiptment I have.

Something with more of a mirror finish that you want to read a newspaper in the reflection requires more RPM and ridgidity. If it needs to be a mirror finish, I achieve it by polishing.

MC

[PixMan]

It's a good-looking part, but the V650 mill would get you a MUCH nicer finish by virtue of those adjustments for the inserts. A 3" one is available in course pitch (6 inserts) or fine pitch (9 inserts). Use 2 wipers in the course, or 3 wipers in the fine, adjust to within a couple of microns, and you'd easily get down to an 8 microinch (or lower) finish even at 3000 r.p.m.

The auto industry uses those cutters for that kind of finish on aluminum cylinder heads and gets finishes like that on the bi-metal surfaces across valve seats. Of course, they're running closer to the cutter's maximum speed, but the results are more a function of having all the inserts lined up perfect rather than pure speed.

[Geof]

That is very good; 3000 rpm at 3" is of course faster at the periphery than 5/8" at 10,000 rpm. I am guilty of wearing blinkers because nearly all our parts are faced with solid cutters 3/4" or smaller.

Rigidity and better quality bearings are the key. I have a Bridgeport clone that can do pretty good but there are regular imperfections which I suspect is due to the spindle bearings introducing a minuscule wobble.

[Cartierusm]

I just got a Shars 2" Face Mill 90 Degree 5 Inserts and have been squaring up aluminum stock all week. 3000 rpm and about 3-4 spring cuts after the initial roughing and they did have swirl marks but the aluminum itself was very shiny. I can take pics and post if you want to see.

[Musick7]

By mirror finish I mean a very shiny surface with minimal swirl marks. Mostly I would be concerned with the flats, so face milling and edge milling.

I did just the Edges/ends as you can see the difference. I used a Fly Cutter on a Jet knee mill Had it on the Highest speed and first cut I took maybe .125"1/8 and the last cut used a little oil and took .0625"1/16. I had automatic feed on the Z axis only and used #2 or 2.5 so it was slow. I did some others and bumped it up to 3.
I didn't use any buffing stuff. This was only the FlyCutter and nothing else.

[mc-motorsports]

That is very good; 3000 rpm at 3" is of course faster at the periphery than 5/8" at 10,000 rpm. I am guilty of wearing blinkers because nearly all our parts are faced with solid cutters 3/4" or smaller.

Rigidity and better quality bearings are the key. I have a Bridgeport clone that can do pretty good but there are regular imperfections which I suspect is due to the spindle bearings introducing a minuscule wobble.

I actually cut the top of that part on a $300 Excello (XLO) knee mill It was actually the first machine I bought 10 years ago when I was doing fab work after my day job, that and an engine lathe that was scrapped and replaced. I still use the machine every day for secondary opps, it just won't die! Good Canadian stuff

MC

[cncjunky]

Those high speed mills sure do sound nice, but to pricey for the amount of work thats flowing. If you can justify the means of spending that much money on a machine then I guess it's worth it, but I do what many of you do, buff it. I have a horizontal buffer and a hand held buffer and I get nice mirror finish results "no tool marks", you can see your self in it, good looking finish. The only problem with buffing is your taking away small amounts of metal, so I guess it depends on the part and tolerances.