Hello Guest it is September 24, 2020, 11:50:14 AM

Author Topic: Bit for cutting 0.008"-0.02" (up to 0.5mm) aluminum/brass/steel sheets  (Read 9401 times)

0 Members and 1 Guest are viewing this topic.

I've been trying to learn the ins and outs of CNC routing and Mach3 (I just bought a license last night), and have been trying to mill a 0.02"/0.5mm sheet of anodized aluminum.  I've tried a 45°/'V' 3.17mm carbide bit that worked well on a piece of copper clad FR4, but it absolutely won't go more than about 0.1-0.2mm into the aluminum even if I put the z-depth on the cut to -1.0mm or higher, for example.  When I try to move the bit down manually (with the spindle on of course), it just won't 'enter' the metal.  I also tried a 0.2mm drill bit, but it did exactly what I expected ... snapped on first contact.  (If you even look at them the wrong way, they break though.)  I really want to be able to cut small holes out of 0.008"-0.02"/0.2-0.5mm aluminum, and didn't think it would be a problem, but I'm not really sure how to proceed now.  I'm assuming that it's just my drill bit, since I have a fairly decent spindle (Wolfgang precision spindle .... I forget the model number).  If someone can recommend a drill bit for cutting 'rectangles' out of this kind of thin metal (ideally that can be purchased online), I'd really appreciate it.

For reference sake, I'm trying to cut solder paste stencils out of sheet metal, and I have aluminum, stainless steel and brass to try, in 0.005"/0.02" (brass), 0.01" (stainless steel), and 0.02" (aluminum).

Kevin.

Offline RICH

*
  • *
  •  7,412 7,412
    • View Profile
Kevin,
How small of a hole do you want to cut?
How are you holding the thin sheet metal stock?

I would probably have the thin sheet attached to a flat sacrificial piece underneath the sheet as
this way it won't spring. The anodized Al surface can be real hard so you need to get below the
anodized suface. They sell small end mills ie; 1/64" ( .5mm ), are expensive, and break in a heart
beat if you put much force on them when milling deep, and by deep i would say greater than 1/2
the diameter of the end mill. If the plate springs up or axis velocity is high or jerky movement they
will snap off very easily. High rpm and and small chip load along with coolant / cutting fluid to keep
from galling up the cutter. SS and brass will  work harden. With real small size HSS end mills are
a little more forgiving then carbide ones. That spindle you have is nice and has a small runout.
Most of my experince is using a small end mill is to do engraving and and run at like
1- 5 inches / min at 28,000 to 60,000 rpm with about .003 to .005  depth of cut or less. When
drilling real small holes  ( below 1/32" - #80 / .013" and even less ) i use a sensitive drill press
which i made, 28000 rpm, peck drill the metal, and actualy watch the drill via 30X so i can see if
the drill is bending. Need to let the tool do the work.
Just some thoughts,
RICH 
Rich:

Thanks for the reply.  I have the metal pretty securely bolted to the base (to keep it flat), with some thick paper underneath to absorb any cutting past the metal (I have the Z limit on Mach3 set to -1.0mm ... great feature since I have no hardware limiters).  The holes are very small.  As small as 0.2mm for a 0.5mm pitch QFP footprint, for example.  Typically, the holes are more like 0.05" though.  I had no problem removing the copper layer from a sheet of FR4 with the same setup (though the copper was very thin), which is why I was surprised the aluminum wouldn't cut.  As per your advice, the spindle is quite high speed (25K RPM I think).  And I tried a 0.2mm endmill ... it broke as soon as it came in contact with the metal. :-(

I had hoped it was as simple as changing the bit, but reading your comments it seems not.  Can you recommend a brand/type of cutting fluid to try, or at least some characteristics to look for?  Given that I'm completely new to this, I'd rather trust someone elses judgement?  I'm sure I can find 100 recommendations on the web, but I may as well start with one that works with someone competent, and see how that works out.

Kevin.

PS: I've attached a photo just in case it help with any diagnosis, if anyone is willing to take a look.

Offline simpson36

*
  •  1,371 1,371
    • View Profile

Reading your post, it's unclear to me if you are wanting to drill, rout or do a thru cut in the material.

Adding to Rich's suggestion of a 'backer', I would add that if you can tension the sheet, that would also be helpful.

I have done a fair amount of machining tiny slots in 6061 aluminum with a .030 bit. For his I mount a 25k spindle on the mill head and use a HSS two flute center cutting end mill. In my application, the alumnum is solid enough that I can use spiral flutes.

For sheet stock, I would suggest that you will have no success with spiral flutes that will want to lift the material. Go with a straight flute and only one or two flutes. Straight flutes do not try to lift the material, but they also do not eject the chips. Most manuf today can give you the tooth chip load for the cutter. Calculate this out and folow it closely. For cutting all plastics and some aluminum, I find that compressed air is better than liquid coolant. With high spindle speeds, if you do not keep the bit cutting and remove the chips efficiently, the heat will go into the toolbit and with aluminum this will make the material instantly cling to and clog the bit. You need to keep the cutter cool and get the chips removed pretty much instantly to prevent recutting.

As Rich mentioned, this is going to get particularly dicy with materials that work harden. In the realm of yellow metals, I have only ever cut ampco bronze, which is not useful experience for brass cutting. However, I would be skeptical of success cutting stainless sheet at 20k plus, no matter what tool you use. You'll need to slow that down a lot and this is where you will likely need liquid coolant. Perhaps a high velocity mist where you could still blow the chips out. I'll be anxious to see other resonses and what you get worked out, though.


Offline RICH

*
  • *
  •  7,412 7,412
    • View Profile
Kevin,
Competent! Don't know about that!
When your breaking the surface of an anodized piece it's like going into a hardened piece of steel. That surface may be composed of pure carbon depending on the die used for the anodizing. So need  some time to break that surface.
The web of the drill or end mill is realy thin. Maybe a good way of expressing this is to say it's like playing pool
with a wet noodle for a cue stick. All it takes is for the drill or even the end mill to walk a small amount because of the surface, along with some run out, and maybe not entering perpendicular to the surface,  and you have a broken end mill or drill. So that particular time in machining can be very important.

Oh, BTW, backlash is a real killer on the small end mills.

As far as cutting fluid, well, there are books written about it and recomend taking a look at a Machinist Handbook for different materials. There is also a big difference between a commercial machining center and a what a hobbiest does. Depends on how your applying it.  Everybody seems to have their owne secret formula. There are cold air guns, misters etc. and in some cases you don't want to breathe mists from some cutting fluids. The whole idea it to get rid of the chips , keep things cool, extend tool life.

I use WD40 and also WD40 mixed with oil for AL. As for drilling real small holes,.........SPIT.......... human saliva / how gross,   ;D  but as a "starting" cutting fluid seems to work better than a lot cutting fluids i tried.   ;)

DO NOT USE A SYNTHETIC MOTOR OIL AS A CUTTING FLUID.

Best i can say, is experiment some for what you want to do, based on the equipment you have.  

RICH
Thanks to both of you for the very thorough replies.  Obviously I'm utterly new to this, but I definately don't mind doing some reading.  If you can tolerate just a bit more spoon feeding, though, would either of you be able to suggest a metal alloy that would be easy to work with (i.e., soft) when starting out?  I'm not terribly worried about longevity, etc.  I really just want to get to know the software and the machine, and have something thin I can easily cut and experiment with.

And just to clarify (Simpson), what I want is to actually cut right through the material.  I need a piece of metal with precisely positioned 'holes', and I spread some solder paste across the surface of the metal with a squegee, leaving paste in the holes.  Here is an example (though cut with a laser):

http://www.gsiglasers.com/UserFiles/Images/Market%20Sectors/Electronics/precision_cutting.jpg

Kevin.

Offline simpson36

*
  •  1,371 1,371
    • View Profile
Let me second what Rich said about breathing in the mist . . . not a good strategy.

Incidentally, I have been having good succes with a new Aqueus all pupose non staining cuting oil from Tapmatic (my favorite oil). They don't say you can cut it, but I've cut it half and half with water and it's working great so far, even for threading.

For metal test material, avoid the anodized stuff and don't imagine that soft material is easier to cut than harder stuff, epsecially in the world of aluminum.

Forget about any 3000 series. 6061 is good stuff, but tricky in sheet form because it is still a little on the stringy/I'll clog your tool just because it's Thursday type of stuff.

You might try 2024 sheet. This is free machining screw stock stuff. You want a nice clean individual chip.   www.onlinemetals.com