[geoffw]

Iam having issues with a Cloudy Aluminum Finish, cant seem to figure out what it could be, here is my setup:

-1998 Haas VF2 (Very Low Hours)
-BobCad V26 Build 1335
-Lakeshore Carbide 1/2" 3 Variable Flute Aluminum End Mill
-7500RPM @ 50IPM, .007" Finish Pass
-Tullco PolyCut Coolant

At first I thought that maybe the coolant was too rich, but its exactly where the manufacturer wants it, ~2.25

The finish on the inside bore of the part is perfect, but the outside profile has weird cloud lines as you can see in the picture.

Any help would be greatly appreciated!

-Geoff

Attachment 258920

[G59]

I hate to say it..................but this looks like the typical surface finish of carbide tools. I'm sure others will disagree, but for aluminum, it's hard to beat HSS.
Carbide tools aren't as sharp as high speed cutters.
They last longer and are 2.5 times more rigid, but the molecular structure of carbide limits it's overall sharpness.

[mmoe]

What kind of aluminum? If it's 6061 straight off the machine, I don't think it looks that bad really. How was the inside bore done in comparison to the strategy for the outside profile?

[geoffw]

So what would you recommend finishing with? 2Flute HSS?

[geoffw]

What kind of aluminum? If it's 6061 straight off the machine, I don't think it looks that bad really. How was the inside bore done in comparison to the strategy for the outside profile?

Exactly the same strategy, feeds and speeds.... Hole was roughed and then finished with .007"WOC, Exterior was roughed and finished with .007" WOC.

[G59]

It could be the coolant. I know Koolit coolant doesn't leave as bright a finish on 6061 especially if you let it sit and dry up after machining. Did you try just wiping the part off with WD40 after machining?

[geoffw]

It definitely doesn't come off with WD40, tried that plenty of times.

[G59]

try a different endmill. That may be all it is.

[geoffw]

I fixed the problem by increasing my DOC from .005" to .020" and from increasing my feedrate from 50ipm to 67ipm.

Does anyone see the benefit in running slower feeds and speeds to get a better finish?

Attachment 259158

[G59]

Less rubbing of the endmill on the surface. But from your pictures,I'm surprised the Hass doesn't leave a better finish. You definitely can tell it wasn't a turn part.
Glad you found a work around it though. I still would of tried a HSS endmill.

[geoffw]

Less rubbing of the endmill on the surface. But from your pictures,I'm surprised the Hass doesn't leave a better finish. You definitely can tell it wasn't a turn part.
Glad you found a work around it though. I still would of tried a HSS endmill.

The finish is amazing (i only finished the upper portion of the cylinder), Ive seen a lot of billet parts and this is definitely up there with the best finishes Ive seen.

I plan on experimenting with HSS end mills this weekend.

Would you go 2, 3 or 4 flute for finishing?

What feeds and speeds and DOC?


-Geoff

[G59]

I would go with 3 Flutes HSS. Usually you run them at 1/2 the speed and feed of Carbide.

If you think the finish is great, then just carry on. I'm just making a suggestion here. I'm certainly not telling you to retool your whole setup.

I think you'll like the fact that the end mills are more than half the price of carbide, and surface finish is usually better and lasts just as long.

HSS is great, but anything under 1/4", stick with carbide. That's where the extra rigidity really pays off.

Try this link, great stuff for calculations of feed and speed. FSWizard - Free Advanced CNC Speed and Feed Calculator



So as you can see the rpm 4968 with 50 ipm.

[geoffw]

Im just learning what tooling i need so its not a big deal to buy what I need.

Ill try it tomorrow.

Ive heard some people say that a 4 flute HSS leave a great finish on aluminum when finishing....do you have any experience with that?

[G59]

4 flutes are good, but I've seen quite a few leave a ripple finish on the part due to harmonics. I know I've experienced it, although the ripples were barely noticeable, with 5 thou vision, you know they're there.

3 Flutes seem to cancel out the harmonics I had through the spindle and tool.

It's really up to you and what works best on your machine. Every machine is different, so hard to make a call on that one.

[zero_divide]

An aluminum-specific Carbide tooling is not worse than any HSS tool in surface finish.

With a proper tool i normally get mirror-like surface finish at about 0.0025-0.003 ipt chipload

Whatever marring you see is because of the dull tool.

These pockets were done at full 1.5" depth of cut with a .5" 2" long 3 flute Niagara Elite endmill. Even at 0.010" chipload and significant scalloping because of very hight feedrate, you can still see reflection of the tool.

For aluminum when tolerances do not exceed 0.002" i do not even bother to use a separate finishing tool.

Btw 4 flute endmills are most often designed for anything BUT aluminums. This means they have different rake angle that affects how the chip curls and needlessly increases cutting force, which in addition to higher number of flutes leads to a lot of chatter.

Sometimes even with very stubby cutters, tool with improper geometry "shivers" or causes more shearing than cutting and produces cluoudy finish.

Long and boring story short: Use tools designed for the purpose. Generic endmills that claim to work for all meterials tend to not be very good for anything.