What's new
What's new

Surface finish issues while sidemilling aluminum.

CoolHand

Hot Rolled
Joined
Sep 6, 2005
Location
Missouri . . . Near the Middle.
Title says it all, I am side milling aluminum in a small VMC and I am getting a less than satisfactory surface finish.

The machine is a box way C-frame 3 axis VMC made by Moog/MHP in the early '90's. 5000 RPM spindle, BT40 taper, 5/7.5 HP belt driven two speed gear reduction head (IE belt drive from motor to spindle, with a two speed shifting head. Low speed has a single counter shaft for reduction, high speed is straight through).

This is the part in question, machined from a 6063 T-6 extrusion:

SuperULERail2.jpg


I am currently just worried about the sidemilling finish on the final contouring pass around the outside of the piece. Surface finish here is the main concern.

I removed most of the outer material with a two insert carbide cutter 1" in dia, running at 5000 rpm, 0.35" DOC, 90 IPM feed, no coolant. That runs fine, quiet and fast, all is well. The first pass leaves 0.015" for a finish pass, which I take with a 3/4" dia 5 flt gold coated (no idea what the coating is, though I suspect it is TiN) solid carbide EM with a 50 deg helix and 1" LOC (IE super stiff) in a Kennemetal 3/4" ID milling chuck. The radial DOC is 0.015", the axial DOC is 0.655", spindle speed is 5000 rpm, feed is 90 IPM, and this time I have the coolant on. It cuts fine, quiet and fast, but I am left with this surface finish:

SideMillingFinish1.jpg


SideMillingFinish2.jpg


I can just barely feel the marks with my fingernail. Other than that, I have no idea how deep they are. They take a while to sand out, which is what brings me to you all. I'm tired of running the sand paper. lol

So, here's the question:

What can I do to improve this finish? Is it my spindle? Everything I cut (sidemill) ends up with this finish on it, but I tend to cut everything with the same data, so that doesn't really prove anything. Also, end milling surface finish is excellent, so I would tend to think this is not spindle or tool retention related, but WTH do I know? Is my cutting data off? Am I using the wrong cutting tool? The problem is not chatter, the thing didn't make a sound while it was cutting.

I'm not opposed to spending money on new tooling if needs be, but I'd just as soon use what I have if I can. I also have quite a lot of stuff on hand here as well, so if the cutter is at fault do feel free to suggest a better tool, I might have one in the drawer already. ;)

Even with the less than stellar sidemilling finish I'm pretty happy with the way this part turned out. As a test I ran the feeds and DOC's at nearly double what I had ran them at in the past, and everything cut beautifully, so I'm gonna call it a win. Cycle time was down by over half. Right now it's running at about 3.5 mins with five (5) tool changes.

Bear in mind that this is a second op on a cut to length extrusion with a few holes drilled in it, so not every single operation in that piece was done in this set-up. This go 'round first takes the outside contours, then it opens up the big pockets on the inside. The outiside contour is cut while the piece is full cross section, the thin walls are created afterwards when the pockets are cut.

Any assistance you all can offer would be greatly appreciated. I'm getting awful tired of sanding.


[ 05-21-2007, 01:46 PM: Message edited by: CoolHand ]
 
CoolHand.
you can try reducing your chip load,on the finishing tool at the moment it seem's to be 3.6 per tooth .
I would start the finish cutter @ 3100 RPM/24 IPM and move up from there if all was OK, but then I'm on the conservative side.
Some times I find new ie; sharp HSS cutters give a very good finish.
I'm sure you will get it rather than sanding
Forrey
 
Put a scrap peice of aluminium in a vice or clamped to the bed and take a very small pass on one side under the same circumstances as this part.

Perhaps the marks you get are not from the finishing pass but there already from the roughing pass and there simply isnt enough stock left to skim.

Other than that, check tool retention knobs for tightness and the cutting tool also.

All i can say is, i've never seen a problem like this if there is enough stock for a finish pass and you keep that pass at a nice feedrate.

One thing I would suggest is to experiment with the spindle speed on thin walled parts. Full RPM is not always the best way to approach these jobs for finishing. Possibly try 1400rpm with a 3/4" 4 flute end mill run nice and slow with some coolant.
 
I'll second Forrey45.... a new / very fresh HSS cutter can often leave better finishes on aluminium than carbide. It grinds to a sharper edge. I often use HSS to finish some parts....looks odd using 'old tooling technology' in a new machine with an expensive job on the table, but I know it works reliably.
 
Coolhand,
Time to start checking everything for being loose. I mean end play in the axies at least X and Y. I would also check spindle end play as well as tool clamping pressure. If nothing shows up, check your fixturing. Put a couple indicators on and around the part, fixture and or axis and try to determine what is moving.
Then and only then after you have exhausted tremendous amounts of money, get a tube of hyspot bluing (non drying) NOTICE I did not say layout dye. Blue up a tool holder, no, no, no, not with a butter knife. Just a light even coat and clamp the holder in the spindle. Remove the tool holder and look at the contact. The blue will be squeezed out and thin where the contact is made. The bluing will not be touched where the bluing is undisturbed where the contact is not being made. We are all waiting with great anticipation to see the outcome. Well at least I am.
Regards Walt.
Spindle Grinding Service Inc.
'Have Grinder Will Travel'
We would be glad to come and show you. "grinding"
You know Missouri and all.
 
Yeah Coolhand I think these guys may be on to something.I used to cut a lot of Aircraft parts that look similar to that one.I had the same sort of problem.What I would do is use a 2 flute HSS endmill and slowdown the RPMS and Feedrate and that seemed to work a whole lot better.See how that works and if its better but still not as good as you want it try leaving a little less than .015 for finish.
 
Why are you using a 5 flute cutter for finishing?

2 flutes work really well in aluminum for finishing, and you can still move pretty fast as there is almost no tool pressure.
 
Do you have any runout with the finish EM?
Aslo, three flute for cutting, instead of two. That way, the engagement, and leaving the cut is more uniform, instead of two flutes banging into and out of the cut. Much smoother.
Also, I question how rigid that setup must be.
 
On coatings. I think ZrN has a little sharper edge compared to other coatings. I have found ZrN to work very well in aluminum.
 
I'd 2nd a 2 flute HSS and also ask;
Is the part held tight in the fixture, any chance there is a harmonic from having the interior partially removed(try placing a pc of foam in the cutouts).
You are climbing, right?
 
I've seen this EXACT same problem before. Basically identical.

You don't have enough chip load for the endmill to actually take a cut, and the endmill has the wrong geometry for aluminum. Sometimes slowing down the feed has the opposite affect of what you want. Those marks in the part are from the tool "pushing" the material instead of cutting it.

Get yourself an aluminum specific 2 or 3 flute carbide finisher, run the recommended chipload, (at least .006 per tooth), and all of your problems will be solved.
 
First off, let me say that if the insert mill I was using (brand new BTW) has over 0.015" TIR, I will eat it. I left 0.015" of stock for the finish pass, which is half again what I usually leave. I don't see any way possible for that insert cutter to sneak through that much stock and make all those marks, especially since I get this finish on most every finishing op, not just ones following that insert mill.

I used the 5 flt cutter because it was new, sharp, very stiff, and the extra flutes allow me to keep the feed up while keeping the FPT down around 0.001" (once you take chip thinning into account that is).

I cut the outside contour before I open up the inside pockets, so the piece is full cross section the entire time this cut is happening. I do this specifically because cutting the pockets first would cause a stability issue with the thin walls. I heard no chatter, not even a hum out of the piece while it was cutting. I also get this finish on solid stock clamped directly in the vise too. This (along with the fact that it didn't sing at all) leads me to believe that it is not the fixturing that is at fault here.

I'll have to dig out a 2 flt HSS EM and give it a try. Probably go up to a 1" OD cutter and down to say 5-10 thou of stock. Say 1600 RPM (~400 SFM) at 10 IPM with a DOC of 0.655"? Sound aboot right for regular length HSS?

Walt, no offense intended, but I hope I don't need to see you. ;) That said, what kind of coin are we talking about to grind a 40 taper spindle? What about bearings? I'd have to get out the maintenance manuals to tell you how many and what kind though. End play in the axes could be an issue, I will have to get out ye olde indicator and see what I can find there. What course of action do you recommend should I find something? Bear in mind that this machine is quite old and may not be worth spending $10k on. I will also check the TIR of both the rough and finish tool while I'm at it.

I have tried 3 flt tools in the past and they gave me fits (1/2" and under). Chip packing city. The gullets would weld full of chips and then KABOOM (Firestone!), end o endmill. Though, at the time my coolant pump was woefully underpowered. I have since replaced it with a much more powerful model, so maybe they'll be OK this go round. I've been wanting to try the ZrN coated three flutes that MSC sells. They supposed to be specifically for aluminum at high feeds, so I've been eyeing them for a while now. Worst case, I break a few and learn something. What's a few broken cutters between friends, eh? :D

I am climb milling, this ain't my first rodeo.


Joe - That's what I like to hear. Faster is certainly easier to tolerate than slowing down to a crawl. Sanding doesn't take but about 10 mins per piece, so once the feed goes below about 15 IPM or so, I'm better off to just sand the damned things. lol I will purchase a couple of two or maybe three flute ZrN coated carbides made for finishing and push 'em as hard as roughing. How much stock would you leave for a 3/4" tool? I left 0.015" this time, but I suspect that may be too much. Whatcha think?

Thanks for all the advice so far guys, every bit of it helps.
 
CoolHand,

As far as the 2 flute cutters go, I use 1/2" uncoated carbide 2 flute end mills quite a bit. The max RPM on my mill is 4500, so I run them at 4000 RPM and 40 IPM leaving .010" stock, and get a great finish every time through hundreds of parts. This figures out to 523 SFM and .005 chip load.

Someone on an earlier thread here spoke of 2 flute cutters banging against the part? I guess it really doesn't matter what the tool does as long as you get a great looking part, and the tool life is up there. Besides, usually a finishing endmill is going to last a long time in aluminum no matter how many flutes it has. :D
 
Coolhand, .015 is fine. Anything between .01 and .040 should do well.

When I ran into this problem, I was using an MA Ford, 1.0 diameter 3 flute aluminum finisher, with a 4 inch length of cut. It was a contour cut with a 4 inch depth, so I used every last bit of that length.

I simply COULD NOT get a good finish. I kept going slower, and slower, and slower. I finally realized that I needed to feed heavier so that the tool could actually get into the cut and stabilize. I had started at 15,000rpm and 100ipm, and kept turning the feed override lower, and lower, and lower. The finish looked just like what you've got here. I ended up with 10,000rpm and 150ipm, getting a PERFECT finish.

At your depth of cut, even a .500 dia 2 or 3 flute, solid carbide, aluminum specific endmill will give you a wonderful finish. You can get a .500 Destiny, Hanita, MAFord, etc. with a 1 inch LOC, for less than $50 bucks. The .750 diameter will be over $100, and the 1.0 will be over $150. I use a .500 Destiny Viper 3 flute with a 1.5LOC in a shrink fit holder for any finishing operation that's less than 1.5 deep.

Just go 5000rpm and .005-.008 per tooth.
 
Yeah, it' takes a lot of 0.010" cuts in alum to take the edge off a carbide tool.

This last weekend I replaced a 1/2" 2 flt that had been in it's holder and in the tool changer for over a year. It just wouldn't give up. Finally lost a corner on one of the flutes (I suspect due to recutting chips in a pocket I couldn't get enough coolant into) and had to be retired, but it was a good soldier to be sure.

When I rough with the 1/2" tool I run it at 5000 rpm, 0.004 IPT, at 0.25" DOC with half to full width engagement. They cut almost forever at that data, and leave decent enough finish that I don't even take a finish pass on features that won't be polished to a gloss later on.

That's why I have to sand the current finish, if I let the anodizers loose on it like it is, they destroy the part dimensions leaning on it with the buffer trying to take those marks out in 5 secs. Don't get me started on anodizers, that ain't a pretty picture. ;)

Joe - Sweet, it gets better and better. I was not looking forward to spending $100+ on that finisher, especially since it's not a lock that it'll work. $40-$50 is easier to swallow, and I use the hell out of 1/2" tools anyway, so it'll have friends. :D
 
Thanks Walt, I'll get back to you when I get home from work (the machine shop is not my primary income generator anymore, and my personal computer with my email is at home now).

Thanks much for all the assistance guys, every bit of it has been useful.
 
Someone on an earlier thread here spoke of 2 flute cutters banging against the part? I guess it really doesn't matter what the tool does as long as you get a great looking part, and the tool life is up there.
That relates to the tool engaging, and then leaving the cut before the next flute starts to cut. If you have one flute always engaging before the last flute leaves, it will run smoother. When I swithced from two flutes to three flutes, the cutting got a lot smoother.
 
Try a two flute cutter and grind one cutting edge to have several thousanths clearance. Now you have a one flute cutter.

At 5000 RPM you have 83.3 RPS. At 20 IPM you move 0.333 IPS. Thus, 0.004" pitch for the surface pattern. A 3/4" 0ne flute cutter with the above speed and feed produces less than 0.000,1" peak to peak variation.

Do consider the possibility of resonace of the thin side wall.

Do experiment on solid stock and see if you get the same result.

A photo of good surface finish in 6061 is my photo P8 on the MISCELLANEOUS PHOTOS page at www.beta-a2.com . This was done with a 2 flute uncoated carbide unknown speed and feed with very light finish cut. Basically the final bore is made by multiple spring pass cuts. The last cuts take a few tenths.

.
 








 
Back
Top