[SRT Mike]

We have a part we're machining - it starts as a 2.5" cylinder of 6061 AL and it's machined to an octagon like shape. It's 1" high and machined to a final size of around 2.25. It's being machined on a bridgeport series 1 with a retrofit CNC control. It has mist coolant but we have not been using it - we've been machining dry.

The problem is that the exterior finish on the sides (where the mill is side cutting) is not as good as we'd like. Its rippled and has sort of twisting lines to be seen running vertically - like you can see the cuts the mill took out of the material. I can feel them easily when I run my fingernail over them.

We're running 1600rpm with a 2 flute TiN 3/4 inch mill. I will have to check the feedrate but I believe it is around 15ipm - we let MasterCAM choose the RPM and feed. The machine tops out at 4000rpm and 80ipm feedrate.

What can I do to improve the finish? It's a cosmetic piece and the problem is that if the finish is not good it requires a lot of sanding which ends up rounding over the corners and making it look not so good. I am hoping to do as little finishing as possible and get the best finish off the machine as possible. We tried doing a slow speed 4000rpm very light cut finishing pass without much luck. My assertion was that we should do the finishing pass at a relatively high feedrate to avoid overheating the mill, my coworker disagrees (were new to CNC machining) and kept turning down the feed on the high RPM light cut finish pass but it didnt really make it look any better.

Should I use a different helix angle? I dont know what it is on this mill, it was just a cheap mill we had lying around.

Would going to a solid carbide mill help? Maybe someone could recommend a brand for a nice finish? This mill was one we had lying around, came in a set from Grizzly so I know its a super cheap chinese import

Will mist coolant help? I would have to rig up something to do flood and it would be a hell of a mess on the open machine.

What should the feed and speed be and what about how much material to remove to best finish? The part is already machined out of the cylinder and we leave a little "meat" for a finishing pass, so we can do a finish pass at whatever amount of cut depth we want. We're doing the finish pass at the full 1" depth of the part but I mean we can adjust how much material we are removing in the finish pass.

Any other ideas to get a nice finish? I know this ain't a high-end Mori but it's all we've got until these parts start bringing in the $$ and we can get a newer fully enclosed machine, and I know this machine can do better, so anything you guys can suggest would be helpful!

[Verfur]

Mike,

3/4 sounds a bit big for a small mill, I would most likly use a 3/8 2 flute carbide mill for alum. Hertel (interstate I thinkit may be called now) makes a nice one that I favor. sounds like a rigidity problem. Ah yes coolant both for lube and mainly to remove the chips from the end mills path. If your machine has a tool changer on it I would use a Nuckle rougher and finish up with the 3/8 carbide mentioned above. I would try somthing in the range of 3000-3500 and 15-20 ipm and I like .005 to .010 for finish pass in a climb cut. Check with J&L tools

P.S. the feeds and speeds are from memory

feeds I mentioned are for the 3/8 em

But I am sure you will see a big diffrence

Please post results
John

[little bubba]

I would toss the 3/4 two flute. The main reason to use a 2 flute is for chip clearance, which shouldn't be a problem on a finish cut. With your feeds and speeds your taking better than .004 chip load per tooth, this is almost a guarantee of a crappy looking finish, I would back that off to almost half. Get yourself a 4 or better yet a 6 flute, I tend to like to finish with as small an endmill as I can so that I can feed as fast as I can and still keep the surface footage reasonable. Also make sure that you are climbing, a conventional cut tends to leave more burrs and is also more likely to smear the surface. Your running 315 surface feet, so you should be mostly ok with no coolant, though if you have a spray mister I would use it.

[stuart76]

i totally agree with the other posts, another trick to vastly improve the finnish of alum is to use kerosene instead of coolant. just an a hand held spray bottle or simmilar. i dont know why but works really well.

[Geof]

i totally agree with the other posts, another trick to vastly improve the finnish of alum is to use kerosene instead of coolant. just an a hand held spray bottle or simmilar. i dont know why but works really well.

Works very well but please remember that kerosene soaked aluminum swarf burns quite well. Actually it is horrifyingly well, I can still see the flames running up the wall behind the lathe in my basement workshop and spreading out across the ceiling. Do have a good extinguisher on hand like I did.

[widgitmaster]

I agree with all the above, but never use an endmill on steeel or other metal prior to cutting aluminum! Allways use a new endmill for best results, and keep them wet!
Eric

[nmachine]

You should run fast say 600 sfm if ya got it around 3000 rpm decent feed light finish cut and a sharp cutter. Give it alittle shot of wd-40 and it will be smooth.

[Kool Parts]

SRT Mike,
On a lighter duty machine I like to run carbide instead of high speed end mills. Make sure you are climb milling Use the max spindle speed, and the 3/4 shank is good. For the best finish I like to use a high helix 5 flute, and save it just for the finish work. This PDF is a good example but ignore the prices that's just retail crap.
Never and I mean NEVER use a flammable liquid for coolant. There simply is no excuse for it. There are hundreds of metalworking fluids available for the job.
Gary



http://www.niagaracutter.com/solidca...um_ss/s545.pdf

[nmachine]

Other than coolant what would ya use? If you mist it maybe but it has a low flash point, tap magic and others will flame to if in a high pressure mist. I've been using them for 10 or so years and never had a problem and will continue to do so. COOL PARTS

[Kool Parts]

nmachine,
Please, knock yourself out dude. Whatever makes you happy. Darwin's theory will be at work soon enough. And the fact that you have been doing it for 10 years shows you are a slow learner. But again as long as you are happy..go for it!
But it's irresponsible to tell somebody that is admittedly new to spray flammable liquid on a hot surface.
As a kid the diesel shop across the road from me used to love to grab-ass. One of the favorites was to light the grease rags in the back pocket of the coveralls with a lighter. Until they lit one that was soaked in solvet. Got to see a man burn to death that day. At the civil trail the foreman stated that "they had been doing it for years" That statement was on the front page of the paper in nice big print.
Now don't get me wrong, this is not a flame towards you, and I could care less if you flip steaks on the Barbe soaked in av gas. But the man had a good question and I just answered
Gary

[MILLMANM]

I agree with most Ideas,
But here my 2 cents,
1 Inch emill 2 flute@1000 sfm 3800rpm@15ipm has .002 chip load
this is about max rpm,
@500 sfm .5 emill 3800@15ipm .002 chip load
so a hss emill should do fine ,
But make sure the tool is sharp and leave.01-.02 on the wall to finish so the emill has something to get under
but it may just be the spindle bearing runout
anyway good luck
Brad

[nmachine]

You ain't worth the argument KOOL. Every good machinist I know does the same and if the part is hot as hell then don't. I didn't think I was babysitting the guy just giving him an idea that works. This is hardly comparable with somone lighting someones @#$ on fire give me a break. Not the same boat at all. OUT!!!

[ctate2000]

More flutes, .750 dia is fine. Climb cut if you can at 1600 RPM and 4 flutes you should run about 6.5 IPM to get decent finish. Use some type of cutting fluid. Kerosene works very well as stated earlier so does WD-40. Water soluable oils,ethanol and even the eco friendly stuff work well. Aluminum will adhere to the cutting egde of all tool materials except diamonds. Any oily fluid helps prevent chip welding. I have even heard of people using milk, veg oil and bacon grease these can stink up the shop I would think. Your problem is speed and feed. Mastercam, Surfcam and the rest were written by cmputer programmers not machinists. The feed and speeds they use are never correct.

[coonhunter]

Just wondering why some of you guys use 2 flutes and others 4flute or more? I know a 2 flute gives more chip clearance but on a finish cut there is not much left to cut? I've always used a 4 flute. Should I be using a 2 or 3 flute or does it really matter as long as your getting the finish you want?

Mike use some wd40 that will keep the chips cleaned of your endmills,chips kind of melt on the cutter and that will leave those swirl lines.

[ctate2000]

Rule of thumb: Two flutes for cuts which require full engagement. Four flutes or more when radial DOC is less than 1/3 diameter of tool. I like three flutes for aluminum they give adequate clearence for full engagement and an extra for finishing so you don't have to change tool same tool for both. The more flutes the faster you can run. Feed rate (IPM)= RPMxFEED (IPR)xnumber of flutes. Example 1000 rpm x.002IPR x 2flutes = 4IPM. change to four flutes and feed rate goes to 4IPM. Theoreticaly surface finish remains the same. Clear as mud?

CT

[ImanCarrot]

I've ben turning Aluminium for years, however I use an ultra precision air bearing CNC beastie but some of the following might be of use.
Tools: Single Point Diamond available from Contour Tooling in the UK and the States.
Tool Rad: 0.20"- 0.60"
Top Rake: 0 deg
Front Clearance 10 deg
Spindle Speed: 1K - 3K rpm
Depth of Cut: 10um, 8um, 2um (rough, pre and finish cuts)
Coolant: Light mist WD40 beneath tool so that it forms a light "bubble" at tool tip.
Extraction: Venturi to remove thin line of continuous swarf

Now, this will give you an optical finish on L111 Aly as long as it's not "rolled" which doesn't machine too well for me.

This is probably over the top for what you want, but as a previous poster said, Diamond Tools (mono crystalline, not poly) will get you a perfect finish on Aly, trouble is they are pricey and need relapping every now and again.

One tangential thought though... what if you machined it then sand- blasted it afterwards? it wouldn't give a shiny finish but would be a uniform and neat grey (obviously don't sand blast on machine- you could get grit under the slideways)...or how about lapping compund like Aluminium Oxide grit with water to hand grind it- that'd be cleaner than sand- blasting. Incidently, Brasso will polish up Aly quite well.

Hope this helps.

[Bluesman]

I have been cutting aluminum for the better part of 12 years and I find that the best way to get the best finish is high SFM I am using anywhere from 1200 to 3000 SFM depending on the aplication. for PCD tools I am usually at 3000.
But here is an acual setting for a 1"dia 4flt carbide EM I am using 1750SFM and a Chipload of .009in and definatly climb cut. This produces a finish of less than 62micro and on a brand new tool some times as good as 32 but I get about 25,000 cuts on it so twards the end it get a bit gummied up. Oh and it is a single pass about .200 deep.

If you need to convert SFM into RPM check out this sight it has a few converters in it and is quite usefull

BLUE

http://www.i-logic.com/utilities/sfm.asp

[MrWild]

I don't like six flute cutters due to the way they can do a sudden load up. With fast feeds you're almost certain to break it before you can hit the emergency stop. A large radius on the tool base at the tip helps with the finish. A sharp tip leaves more sharply defined furrows. Due to my distaste of fouyr or more flute small radius cutters, I slow my feed down so thejump betweein furrows is less.

A place to look for one problem is to tram the head. Out of tram heads leave bad finishes. Coolant is important but there are specific coolants for aluminum. If you have an exhaust to remove the smoke due to the high cutter speeds, I highly recomend a smear of A9 over mist coolant A9 leaves a very nice finish. Just dip a brush in a tin can filled with A9 from a bulk can and smear some on. If you must have mist coolng there are aluminum specific coolants you should try. Coolants are a science unto themselves.

[gibbsman]

The original post speaks of vertical 'waves' in the material this, to me, has nothing to do with coolant , although I do always use a water soluable oil when machining aluminum, the real problem is machine or set-up rigidity. Try using a smaller endmill with puts less side pressure on the part and spindle or try changing your approach to cut with the bottom of the endmill this also puts less pressure on the part.

[helix77]

Everyone Seems To Think The Problem Is The Cutting Tools , Or The Feeds And Speeds , Or The Lube , Or The Cam Software ........dude If You Cant Get At Least An Ok Finish On Aluminum Then Check Your Spindle Bearings Or Maybe Even Your Machines Servos. Because You Are Getting Ridges In The Cut Leads Me To Think That The Endmill Is Being Deflected Into Its Own Error ...and Theres Not A Feed And Speed In The World Thats Gonna Help If Your Bearings Are Bad.