Oh venerable master machinests, I beseech you!

February 23, 2009 1:30 PM

Designing a COMPUTER CONTROLLED MILLING MACHINE, small, very precise, and specialized to one type of task. Help me understand the bits and drills that will do the actual carving of the metal.

This machine will take flat slabs of metal about the size of an index card, and carve dimples and grooves into the horizontal surface.

The dimples are small, precisely hemispherical, at a depth of one radius of the sphere, and in any case never deeper than the diameter of the sphere.

The size of the hemispherical removal of the metal must support a diameter of 1/25" at the largest, and 1/250" at the smallest, although I'd go to 1/1000" if it wasn't too much extra trouble.

I have a positionable X-Y stage to serve as a table (top of the line Aerotech, already have it lying around.) I imagine a drill bit at a fixed location that can be raised and lowered with precision, the metal blank is on the table and is moved around under the drill to locate the contact point.

QUESTIONS:

1) A drill with a precisely shaped tip could repeatedly drill a vast number of hemispherical dimples to create a channel, just operating up and down. (time is not an issue) What kind of half round bit could cut the channels laterally, like a router?

2) Can I purchase such bits off the shelf? Can I sharpen or reshape the bit tip if it becomes deformed with wear? What would it take to make my own bits, or can I get a blank, say cylindrical bit, and shape the hemispherical business end myself?

3) The specific metal being carved is not so important, what would be a workable metal soft enough to go easy on the bits?

4) Should I ditch the whole bit idea with a laser or some such? The X-Y stage has an MSRP of about $75K, I wouldn't want to go into that ballpark again. And I'd also like to have some way of tinkering with surplus parts that I could get a deal on, during the early development.

posted by StickyCarpet to technology (24 comments total)

Lasers seem like they'll burn holes, not cut spheres.

Would a press work better for your application?
posted by jenkinsEar at 1:52 PM on February 23

If I'm understanding the application correctly, I'd use various ball end-mills and a tool-changer. Something like these.
posted by aramaic at 1:55 PM on February 23 [1 favorite]

Oh, and I just realized: do you intend for the dimple to have an "interior" diameter which is larger than the "throat"?

With an end-mill, if you have the depth nearly equal to (or greater than) the diameter, you end up with what is essentially a cylindrical hole with a curved bottom -- not a "hollow sphere which impinges upon the surface". That latter one is inordinately difficult to machine (well, *I* can't manage it, anyway).

The distinction that I'm trying (and likely failing) to convey is rather like the difference between a U and an O that's got a little hole at the top (vaguely like an upside-down Omega). The U is easy -- the O is nigh-impossible.
posted by aramaic at 2:06 PM on February 23

I think that you'd do much better to buy a numerically controlled mill than to try to design one for yourself. It'll be cheaper, take less time, and be more reliable.
posted by Chocolate Pickle at 2:21 PM on February 23 [1 favorite]

Use abrasives. Diamond coated ball shapes are very common and inexpensive, coolant and sensitive feed rate insures tool life and surface finish.91246 DIAMOND POINTS,
posted by hortense at 2:24 PM on February 23 [1 favorite]

aramaic, what's the problem? A ball-end mill will create a dimple to have an "interior" diameter which is larger than the "throat". I own several of those; ~$8-$20 apiece.

The smaller sizes listed by StickyCarpet (1/250" = 40 tenths) are going to be nigh-on impossible to find, however. I think my smallest ball mill is 1/64", and I was specifically shopping around (McMaster-Carr, etc) for small ones to do fine relief on a seal matrix mold.
posted by IAmBroom at 3:08 PM on February 23

Those holes are pretty damn tiny. I don't think you can find any end-mill or drill bit with a 1/250" diameter. 1/250" is roughly the diameter of a human hair (though there is about an order of magnitude variation in human hairs). 1/125" is about the thickness of standard aluminium foil. Steel is only a few (4ish?) times stronger than aluminum.

1/50" is a #76 drill bit. A #80 bit (smallest "standard" size) is ~1/71"

I'm having fun trying to imagine what you could possibly need them that small for. Can you tell us more?
posted by aubilenon at 3:21 PM on February 23 [1 favorite]

Brackets to hold the piece of metal in place and prevent it from being thrown (reinforced with a magnet if the metal being cut can be magnetized).

Next two sets of X,Y,Z adjustments, one to rough and the other to tune your zero(0,0,0) or home position. Milling equipment generally works off of screw threads to calibrate.

From what you have described, the Z access seems to only have two positions, an up and down. Given that if you dig too deep in a single pass that you will throw your material, you probably want to have more than one depth of cut setting. In otherwords, plan on 3 axis you will need to send commands to.

And you will of course need to set the speed of rotation - thinking that one speed will cut anything may be a bit impractical. Certain speeds are better at certain things than others... this gets into torque, gearing and a wide assortment of ways you too can program a computer to break your fingers and maim you for life. Talk to your local shop teacher, there's all kinds of formulas on how fast you cut based on what you are cutting and what you are cutting it with.

From my experience in cutting stuff, depending on how much you are cutting and how fast you are cutting it, and how often you want to replace your tools, you may need coolant, so when the tool is in motion, you may want a pump lightly soaking your piece with coolant (spray it on too hard and you'll spray filings into the air) That might not be necessary, your mileage may varry.

Next you need an E-STOP - not just a software E-STOP, a hard fast oh-my-god-it-just-took-Jim's-finger sort of E-STOP which someone else can reach incase of emergency...

Now for the C&C part, you need a microcontroller, a few A-D, D-A converters, position sensors, etc, whatever you'll be doing to controll this.

Routines
Set tool Speed(integer value), Spin tool (on/off), move tool X(integer), move tool Y(integer), move tool Z(integer), Coolant(on/Off), ESTOP(on/off).
posted by Nanukthedog at 3:30 PM on February 23 [1 favorite]

EDM is an option. (electrical discharge machining.) Details good to a 10th or better (i.e., .0001 inches). If you can't do it with that, give up. If, as you say, you have a lot of time, you'll use it for this approach. The positioning stage is still potentially useful.

An improvement would be to machine the gross details with a rotary method as you propose, then finish the final details with EDM.
posted by FauxScot at 3:47 PM on February 23 [1 favorite]

Thanks for the interest! Let me clarify:

* the hemispherical dimples have no undercuts, if the the depth exceeds the radius, it will be a cylindrical hole from there up.

* Th Areotech X-Y stage I have is the whole package, power supplys, conrollers, software. I even have an LED display motor emulator. I've done motion control before, and I'm all set up for that.

* I actually have two of the X-Y stages, I'm thinking of taking the second one apart
into two 1 dimensional stages, and use them to raise and lower the cutting tools.
So I could have two different cutting tools. And very precise up-down positioning.

* I was really hoping to pick up chicks by mentioning the top-of-the-line Aerotech. If you know that brand you'll appreciate this has extreme accuracy and repeatability.

*I'm aware that a coolant will be applied, I also have a little gizmo that focuses cooled and compressed air, so I'll try that before getting messy.

*Using a press? I'm making dies for a press.

*What am I doing? I'd rather show you than tell you. Stay tuned.
posted by StickyCarpet at 5:18 PM on February 23

EDM was my first thought, though I don't know a lot about it. I can't see the smaller dimensions you're contemplating being cut with rotary tooling, at any price. A channel .004" across and .002 deep is a rather fine scratch. The mechanism to do neat work at that scale would have to be improbably perfect.
posted by jon1270 at 5:29 PM on February 23 [1 favorite]

Hey Aramaic! The page you linked to, has a further link to nano tools!
posted by StickyCarpet at 5:30 PM on February 23

aramaic, what's the problem?

You machine microscopic overhangs on a regular basis? My hat is off to you. Personally, I can't really manage an overhang if the opening is smaller than the shank of the mill.
posted by aramaic at 5:42 PM on February 23

Oh hey, I located an article you may find useful, discussing the use of 0.001-inch end mills. It actually gets mildly specific as to techniques used.
posted by aramaic at 5:50 PM on February 23 [1 favorite]

I find it hard to imagine meeting all your requirements with the same tool. Drilling a 1/4" hemispherical groove with a ball-end mill is really not that tough, but 1/250"? That's a mighty fine bit.

If the very fine lines don't need to be precisely hemispherical, could you do chemical etching? You can achieve quite impressive precision if you do etching work carefully, and all you need is a very fine, hard stylus to scrape away an inert coating over the material. That might let you take advantage of the X/Y stage and wouldn't require a ton of additional equipment.

Although, come to think of it, there's really no reason to use the X/Y stage at all; if you can make etching work for the depth precision and shape that you need, you could do the layout photographically. 1/250 or even 1/1000th of an inch ought to be well within the range of easily available PCB etching chemicals, so you'd be set if you were okay working with copper.

Apparently some CO2 laser systems can do engraving and ablation; I don't know whether putting together a DIY laser-engraving system with the 2-axis stage you have is really going to be easier than buying an off-the-shelf one, but a laser seems like it would accomplish most of your needs. Supposedly they can cut a channel as narrow as 0.006", although that would be with vertical edges; you'd need to get creative and mount the laser at an angle to get chamfered or angled edges.
posted by Kadin2048 at 6:22 PM on February 23 [1 favorite]

Kadin2048: from your link,

CO2 laser: Initial capital investment required $300,000 with a 20 kW pump, and a 6.5' x 4' table

Your idea of scratching the resist with a sewing needle before dipping the piece in acid is sounding better all the time!
posted by StickyCarpet at 7:07 PM on February 23

For those following along at home, EDM on wiki.
posted by StickyCarpet at 7:31 PM on February 23

Although I have not personally tried the device, you may wish to look at books on home-built EDM. It might be interesting to machine a reverse-match electrode, and then use EDM to mass-produce the subsequent parts. I say this having zero idea how fast the electrode will degrade, so YMMV (in a big way).
posted by aramaic at 7:43 PM on February 23 [1 favorite]

Just FYI, y'all, the Aerotch has a cumulative error over the entire excursion of .00001 inches.
posted by StickyCarpet at 9:41 PM on February 23

(Any more input still welcome. )

hortense: Diamond coated ball shapes are very common and inexpensive,

FauxScot: An improvement would be to machine the gross details with a rotary method as you propose, then finish the final details with EDM.

Kadin2048: if you do etching work carefully, and all you need is a very fine, hard stylus to scrape away an inert coating over the material.

aramaic : look at books on home-built EDM

That's some pretty good brainstorming there, THANKS!
posted by StickyCarpet at 1:42 PM on February 24

Just a side comment, but it does look as if those ball end-mills aramaic cites could cut a slighlty overhung channel, if they entered from the side or through a hole.
posted by StickyCarpet at 1:50 PM on February 24

Just to follow up on a couple of ideas:

First, ball-end mills don't cut as well as square-end mills, period. Square-end mills do all their cutting at the very perimeter of the cutter. If you read the linked article on JPL's micro-machining you'll have noticed that the centers of the tiny end mills they use cut flat-bottomed channels are relieved away from the surface being cut. You can't do that with a ball-end mill because the center of the cutter is part of the round shape that you want to cut. The problem here stems from the fact that the centerline of the cutter is essentially stationary, no matter how fast the cutter is spinning, so even if the toolmaker is able to grind cutting edges that go all the way to the center of the mill, they will still cut poorly because they'll barely be moving. Take, for example, a .010 mill that's spinning at 90,000 RPM. The perimeter of that mill is moving at about 235 feet per minute, while a point .001 out from the centerline of the mill is only moving at 47 feet per minute, etc.

The other thing is in regards to this idea of being able to cut an overhung channel. This is not impossible, but it's extraordinarily difficult. You've got to remember that when the cutter does it's cutting, it's not vaporizing the metal; it's scraping material away from here, and dropping it off over there. All those metal shavings get fluffed up (they don't fit together like a puzzle; there are inevitable air spaces between them), so they take up more room than they did before the cutting took place. An overhung channel makes it extremely difficult for the cutter to lift the shavings out of the channel to get them out of the way. If the cutter can't evacuate these shavings from the channel its cutting then they just get packed into the channel behind the cutter. Very soon, the compacted shavings are piled up so close behind the moving cutter that there's no room for the cutter to put more shavings. The cutter itself becomes clogged and can't cut anymore, but the machine can't tell that this has happened. The bit (or the workpiece) keeps moving, and the cutter breaks. Now you've got a short section of channel that is compacted with shavings and the end of a broken tool, all of which are difficult to clean out. In other words, you've just made a piece of scrap.

Maybe that's more than you wanted to know about penguins, but I hope it sheds some light on why what you're proposing is so difficult.
posted by jon1270 at 3:40 AM on February 25

I didn't initially see a need for undercutting, but since it came up I can see how just a bit of that might be useful, such as making a slot that the piece could slide into like a cartridge. But that's just a frill.

As for the shavings, I've been playing with these Vortek nozzles that can focus compressed air like a lense, with a point away from the nozzle. I can see going totally overbuilt on the blow off, with 6 nozzles or something. Since speed isn't a priorty, hell I won't be able to afford an unlimited number of blanks to work, I could lift the cutting tool
periodically so it would blow clear.

Looking at what steel alloy to cut, I'm seeing that one type of steel, just for this purpose, has the special property of shedding clean little chips that don't tangle.

I'm liking an alloy called Maraging Steel because it is softer than carbon tool steel, but after you work it you bake it at 1000 degrees or so and anneal it and it gets a lot harder after the fact.
posted by StickyCarpet at 11:28 AM on February 25

jon1270, it seems your point about tool rotation speed is well taken, and at these tiny dimensions people are talking about 500K RPM being the target. A dentist's drill can hit 300K RPM, but still it's another factor to consider. Luckily, the more dangerous high energy forces that are required, the more free testosterone as a bonus.
posted by StickyCarpet at 2:44 PM on February 25