Getting a mirror finish in aluminum surfacing

[SRT Mike]

There are a bunch of threads on getting mirror finishes in aluminum and they all recommend monocrystalline diamond inserts when turning, or face milling with special wiper inserts for milling.

In my case, neither will work because this is a 3D surfaced part. Imagine a cavity like half of an egg shape, but larger, like the size of the palm of your hand.

I have a nice, new, Mikron Mill 600x with linear motors and 36,000 RPM in a temperature controlled environment. I have Rego Fix tool holding. I have the budget to buy necessary tooling. But not sure what to get.

I have tried brazed PCD diamond ball end mills from Harvey tool like this:

Diamond End Mills for Non-Ferrous Materials-PCD Diamond-Ball

www.harveytool.com

I was able to get a 16 finish but I need better. I know that's asking a lot, but I figure if there's any machine that can do it, it would be this one. I have seen monocrystalline diamond end mills but not sure if spending the $$ will really produce that much better results? Maybe a shot of WD-40? I've tried playing a lot with feed/speed... the best I got was 30,000 RPM, about .005 depth of cut, .005 step over and something like .0005 chip load per tooth on a 1/4 ball end mill. The PCD end mill didn't really produce a better result than a Helical tool 2fl ball end mill which surprised me. I also played around a lot with posting out arcs vs small line segments and my filtering settings in MasterCAM. In some test cuts I can see the facets in others I got them to disappear, but none of that really made the finish better... still topping out at a 16 finish.

 

[crossthread82]

You want your ipt to match your stepover so that way you don't end up with lines in the finish. I'd lower your stepover and increase feed so they're both around .0015"

As far as diamond ball mills go, I'm pretty sure Misumi and PHorn make MCD ball mills. $$$ but nice.

 

[Nmbmxer]

I've YT videos where they set the step over = to the feed per tooth. If one of those parameters is larger than the other then you can have a pattern you can see, either parallel to the toolpath or perpendicular to it.

ETA I see I'm too slow

 

[LockNut]

My thoughts. So, take it for what it's worth. 30K RPM is still too slow. But maybe you can't do anything about that. I would change the depth of cit to .002" and a .001"/.002" stepover. Use a .0001" surface tolerance in Cam and use lines only. Make sure you are using whatever smoothing/lookahead your Micron machine has. You are looking at 5000 SFPM for that PCD endmill. Maybe go to a larger endmill? Air blast? WD40 is a good idea. I just spray it on the part real good and use air through spindle.

 

[Mtndew]

Is that a 5 axis machine where you can tilt the tool and not use the center of the ballnose to get more sfpm at the cut?

 

[Milland]

You should check into post-milling diamond burnishing. Single crystal ball tip, filtered coolant, and just rub that baby smooth...

diamond burnishing - Google Search

 

[boosted]

That harvey tool sucks IMHO. You can just look at the brazed PCD, and know exactly how nice it's going to handle a small finish cut in aluminum. It's just a dull flat face.

These are supposed to be the best. I believe they also make a PCD. https://www.ns-tool.com/en/products/detail/15

We use OSG ABrand balls with DLC when it really matters, and have been fairly happy.

In my experience when you are looking for super nice surfacing, the best gains are done with the code. My Siemens machines like the point cloud to be really, really tight, with tight angular tolerances on the 5 axis moves too. Do you have the HSC/OSS/etc... setup correctly, and do you have code to match? If so, crank the stepover way down, put in a shiny new tool, and let 'er rip. It will be obvious once the edge starts to go. The big advantage to PCD or even the DLC is just how long that edge lasts at 36k.

 

[F35Machinist]

I would try it with an MCD tool and a .001 depth of cut and .0005" stepover. I buy my MCD tools from a company called Eurakryl in Germany.

 

[SRT Mike]

Is that a 5 axis machine where you can tilt the tool and not use the center of the ballnose to get more sfpm at the cut?

Yes it is and that's what I have been doing - but good idea.

 

[SRT Mike]

I would try it with an MCD tool and a .001 depth of cut and .0005" stepover. I buy my MCD tools from a company called Eurakryl in Germany.

Coincidentally I have their website open and just talked to them today - I wonder how much difference MCD makes over PCD? Is it quantifiable in Ra terms? The 6mm MCD ball mill from them *not* cheap!

 

[SRT Mike]

Thanks for everyone's replies. So the things I did are:

1) Changed the tolerance in MasterCAM to .0001
2) Made the IPT and stepover the same (.0015)
3) Sprayed some WD-40 on the part (the machine also has air/oil mister which we tried too)

With the above and the 2-flute brazed PCD 1/4" ball mill from Harvey, I was able to get a finish a little better than 8 Ra. You can see a rainbow of diffraction when you tilt the part to the side. It seems the hardest part is accurately measuring the surface finish. We don't have a laser interferometer so we're using a Mitutoyo profilometer and playing with the settings to get a result. But the finish is definitely better than 8 Ra. We'll probably send a sample part to the customer for correlation and see how they like it (they have the really fancy stuff to measure surface finishes).

 

[CarbideBob]

A pcd of the small grain should run up to and better that MCD.
Part of this depends on the tool grinding. Other is the PCD used. Course grains are easier to grind but at 500-1000x they look oh-my chipped due to pullout.
Second part is never use the tip for finishing. Easier said than done but a 5 axis (if you clear it) can keep the cutting away from the tip where you surface footage is poop.
8 Ra is not mirror by any thoughts or dreams.
You do not need a laser but the normal mits gives up down under 4 but 2 if a new stylus.
Once into this you get all sorts of readings depending on axis or number or tries. Normal check here is four runs with some twist.

WD-40.
Did this help by itself? Sort of magic dust on Al but says things about chip sliding, top rake and tool approach.

No help here as I do not know the fix or part.
2 cents and opinion from the peanut galley so maybe so very stupid post.