What's new
What's new

Can the Precision Matthews PM-728VT CNC kit able to do micro machining?

rajhlinux

Cast Iron
Joined
Jul 17, 2020
Location
USA
Hello,

I'm not sure if the PM-728VT ultra precision bench mill bought with the ultra precision CNC kit is able to use 0.2mm (~8 thou) flute Flat Square End Mill spiral bits.
Example:

My objective is to make custom CPU/Chip Die water cooled cold block plates, which requires micro fins to extract heat efficiently. I'll be using copper blocks since it has excellent properties of the highest thermal conductivity of any engineering metal.

Generally the micro fins have a gap channel which are milled of a width of 300 microns (~100 thou), and the standing remaining fins/walls are about 100 microns thick (~4 thou).
The PM-728VT is an ultra precision bench mill, it should hold 2 thou all day and I believe it is more than capable of coordinating at this mechanical accuracy and repeatability.

Question is what type of spindle do I need to make this work? Spindle as in what type of motor for high RPM that will work for the PM-728VT

Another question is can I use stepper motors with closed loop to do this, it should provide enough resolution and keep track for the task?

To further clarify what I'm trying to machine, I have attached some photos.

Thanks.
 

Attachments

  • cpu_fin_cold_plate.jpg
    cpu_fin_cold_plate.jpg
    211.2 KB · Views: 96
  • cold plate cpu.jpg
    cold plate cpu.jpg
    1.1 MB · Views: 95
  • Optimus Cold Plates - Optimus Water Cooling.jpg
    Optimus Cold Plates - Optimus Water Cooling.jpg
    2.1 MB · Views: 94
Last edited:
Very roughly, the basics are that metal wants to be cut at a certain velocity, ie if you imagine a stationary tool, you want to bring the work across the tool at a velocity that is optimimal for the material. Since with a mill, the tool rotates and the work stays still, then as the tool gets smaller, it's velocity is getting lower and lower for a given RPM. So for micro mills like this you will generally want huge amounts of RPMs to get anything done

There is also a maximum size of "bite" that you can take for each RPM, so more flutes or a larger tool can take bigger "bites" or more bites per RPM. However, your tool here is constrained by the size of your slot. So again, this is going to want as many RPMs as you can.

For sticky materials like aluminium or copper, you need to find ways to stop the chips of material sticking to the tool itself. So a cutting fluid, coolant, pressure air blast with MQL or similar is pretty essential.

Broadly endmills want to cut up to a few times deep their diameter. As the ratio of length to diameter gets large, then the stiffness of the tool goes down significantly. You will need to take cuts which are shallow relative to the diameter of the tool, which gives you a sense of time that will be needed to make such a cut.

Possibly the easiest thing to navigate is precision in placing the tool in a given X/Y/|Z plane, although your requirements here are starting to get reasonable precision for a small hobby machine

Have you considered a saw or laser cutting? The saw can have a very fine kerf for a large diameter, so can cut certain types of shapes far better than a spinning end mill? A laser could be relatively more expensive, but if you were happy with lasers which will give an angled cut, then you can look at one of the off the shelf fiber lasers with galvo heads. This is a point source downwards, so the cut is in the shape of a cone, but it's not so pronounced across a small distance. The benefit is that you have a tiny kerf and no tool to break, you are literally ablating away the material.

I think if you start with the free FSWizard and have it suggest a cut for some tools. Then run up a quick design in the free version of Fusion and create a program. The end result might surprise you how long this could take to run? Iterate from there while you figure out what your requirements are?
 
Yeah, sadly I'm with GENERALDISARRAY on this one...you don't have a prayer of cutting these cooling fins with an endmill in copper on this machine.
You need much better than this tool will give you and even with a top of the line CNC mill worth a million bucks, it's still a hard part to cut in copper with a 0.008" endmill.

As hi-fly-cnc suggests, sawing these slots gives you a better chance at success, but it's still not going to be easy...the problem is copper is both gummy and abrasive, and your fins are only 0.004" thick so they will be fragile as Hell.
One stray chip lodged between the saw's teeth and it will rip the shit out of your array.

So I'd wire EDM them if I could and I'd try to saw them (and clench my sphincter a lot) if I couldn't wire them.

Don't let the "ultra precision" hype of the PM advert fool you...it's marketing bullshit.
This machine may be better than the average benchtop mill/drill, but it's still not a precision machine.
Look up a Kern Nano or a Hermle if you want to know the specs of a precision machine.
Try to guess at the price too...there's a reason why they cost as much as an executive home here in Vancouver.
Even if I had one, I still wouldn't try to mill those with an endmill.

Cheers

Marcus
www.implant-mechanix.com
www.vancouverwireedm.com
 
Very roughly, the basics are that metal wants to be cut at a certain velocity, ie if you imagine a stationary tool, you want to bring the work across the tool at a velocity that is optimimal for the material. Since with a mill, the tool rotates and the work stays still, then as the tool gets smaller, it's velocity is getting lower and lower for a given RPM. So for micro mills like this you will generally want huge amounts of RPMs to get anything done

There is also a maximum size of "bite" that you can take for each RPM, so more flutes or a larger tool can take bigger "bites" or more bites per RPM. However, your tool here is constrained by the size of your slot. So again, this is going to want as many RPMs as you can.

For sticky materials like aluminium or copper, you need to find ways to stop the chips of material sticking to the tool itself. So a cutting fluid, coolant, pressure air blast with MQL or similar is pretty essential.

Broadly endmills want to cut up to a few times deep their diameter. As the ratio of length to diameter gets large, then the stiffness of the tool goes down significantly. You will need to take cuts which are shallow relative to the diameter of the tool, which gives you a sense of time that will be needed to make such a cut.

Possibly the easiest thing to navigate is precision in placing the tool in a given X/Y/|Z plane, although your requirements here are starting to get reasonable precision for a small hobby machine

Have you considered a saw or laser cutting? The saw can have a very fine kerf for a large diameter, so can cut certain types of shapes far better than a spinning end mill? A laser could be relatively more expensive, but if you were happy with lasers which will give an angled cut, then you can look at one of the off the shelf fiber lasers with galvo heads. This is a point source downwards, so the cut is in the shape of a cone, but it's not so pronounced across a small distance. The benefit is that you have a tiny kerf and no tool to break, you are literally ablating away the material.

I think if you start with the free FSWizard and have it suggest a cut for some tools. Then run up a quick design in the free version of Fusion and create a program. The end result might surprise you how long this could take to run? Iterate from there while you figure out what your requirements are?

Thanks for your detailed advice.

Are there any type of low cost or used air driven spindle adapters that can do this or recommended? I have considered laser cutting tool however it is expensive and only useful for specific projects. I'm also considering to use the PM-728VT to help me make parts for making a precision laser module.

Also the end mill can do precision laser work by simply attaching a laser module to the spindle, great for making PCBs from photoresist. With that said it seems a precision bench mill would provide more project use. I also work on wood.

I saw some people using a precision air die grinder for high RPM micro machining, is this a good idea? How can I attach this to the spindle.

As for a saw, not sure how this could be done. Like using a dremel by hand? Would like to do this in an automated calculated way, such as using a CNC of some sort.
 
In 2 of the photos you posted the slots appear to be made with a saw of some sort, there may be a hint in there
If I was going to do this at home I would use a slitting saw, that will get you to or closer to the needed sfm without needing a 50k spindle.
 
Hi rajlinux:
You wrote:
" so what better machines are there for $6K brand new "

Probably none.
So what?
It's still not a precision machine, and invoking its "tolerances" will not make it so...no matter how hard you wish.

Spinning and cutting with small cutters is not that simple...the details do matter.
Just the thermal growth on your machine as it warms up is going to move the position of the cutter a lot...potentially half the cutter diameter.
Proper micro milling platforms take this and many other variable into account, and EVERY ONE is necessary to control in order to be successful.

Never mind the aspect ratio of the sample (photo #2)...how do you propose to keep the cutter in one piece when it's sticking out 10 times its diameter or more?
If that cutter wobbles 0.0001" it's already a big problem at this scale...were you hoping your $6000.00 mill has the bearings necessary to spin a cutter at 60K RPM for days and hold a tenth?
Just the spindle on a real machine costs easily ten times what you're hoping to spend...in fact I'll bet if you smashfucked a Hermle spindle you wouldn't have any change left over from a hundred grand to get it fixed.

That's the reality...having a boner for a bottom end machine on Amazon will not change it.
And yeah...it's a bottom end machine.

BTW; to answer one of your other comments:
If you want to saw these, you mount the saw in an arbor and put it in the mill spindle.
You clamp your job so it's sitting vertically on an angle plate.
You use your machine to traverse the work past the saw.
Once one slot is done, you move the saw in Z and make another slot.
No Dremel, no hand work.

Cheers

Marcus
www.implant-mechanix.com
www.vancouverwireedm.com
 
Easy, put the .0075" start holes in with an edm drill, then wire the slots with .004" wire. Total investment 400k+ dollars and lots of dicking around. Anything short of that will leave you with nothing but disappointment and parts that aren't worth the copper they're made of.
 
Hi crossthread82:
I'm confused...start holes...what start holes?
0.004" wire? Huh?
Did I miss something important?

Cheers

Marcus
www.implant-mechanix.com
www.vancouverwireedm.com
I'm referring to the fact that the only realistic way to get those in reliably is with wire edm and given his dimensions he'd have to use .004" wire and some needle sized start holes. Eluding to the fact that without a small fortune in machinery he's not going to get what he's looking for... that is of course if I were to do it.
 
Ok, I looked up their website:

If you scroll down a bit you can see an image showing the tooling marks that reveal how they're made: they're stood up on edge and cut with slitting saws.
 
I wonder how much those thin fins actually contribute to better heat transfer to liquid, since the finer you go, the less tall they can be till you simply don't get any heat transfer from extra surface area that is too far from the heat source to actually conduct anything
and I also think that cutting them with rotating tools is a big waste of time, skiving seems just way more economical, especially if they retail for 50$
 
If they are making those for $50 material & tooling costs included, then it is probably a gang tool/stack of saw blades and spacers in a horizontal.
With or without numerical control.

think that cutting them with rotating tools is a big waste of time, skiving seems just way more economical, especially if they retail for 50$

Gang tool in a shaper?
Especially if it is a Klopp?

:)

smt
 
If they are making those for $50 material & tooling costs included, then it is probably a gang tool/stack of saw blades and spacers in a horizontal.
With or without numerical control.



Gang tool in a shaper?
Especially if it is a Klopp?

:)

smt
They're selling for $50, which means they're making them for less than $25 each.
 
Hi again crossthread82:
I don't think you need start holes...looks to me like you could just wire in from the edge.
Also, the ribs that are left over are 0.004" wide...I think you could sneak a 0.008" wire between them or maybe a 0.006" wire.
That would make it a straightforward job to cut on the wire.

Probably the biggest challenge is achieving the depth of the cuts without having the ribs fold.
I'm guessing they are 20 times as long as they are wide, so maybe 0.080" deep.

Gang sawing is probably going to work so long as you don't pick up a chip and massacre the ribs.
I doubt you could shape or skive something like this in copper, but I could easily be wrong on that.
Wire EDM is easy, cheap, and safe, so long as my dimensional guesses are good and the OP can live with a full radius at the bottom of each slot.
I'd really like to see someone try this with a skinny endmill...that's one LOOOONG stickout, and it would be fun necking down a cutter that small too.

Cheers

Marcus
www.implant-mechanix.com
www.vancouverwireedm.com
 
Pretty sure skiving those fins is the best option if any kind of production time is expected to be held.


Milling those with an end mill is a fools game.
 








 
Back
Top