Several questions (glues, drill mills, molybdenum)

[BFGarrett]

So I've got an interesting project to try on my lab's Tormach. Basically we just want to cut some masks out of thin sheets (in the 1/16" ~ 1/64" range) of molybdenum, or failing that, aluminum. What makes it interesting is that the patterns in the mask have features fractions of a millimeter wide, and we might also need good alignment between different patterns on different masks.

So, first question - I'm thinking that milling it all in one setup is the only way to get the desired accuracy, which leads me to think I should glue the sheet to some sacrificial aluminum. That way I don't need to do any fancy edge finding, just roughly center the sheet, mill the patterns, cut out a circle around the patterns with an alignment notch, then release the mask from the sacrificial aluminum block. So, can anybody recommend a good glue for this type of workholding? Preferably it could be released with some acetone or heating.

Secondly - I have some really tiny end mills (0.02", 0.016", 0.01"), but I'm afraid of using and breaking them (haven't worked with them before). It occurred to me that since this is a mask, we don't care about having slots with vertical sidewalls, a \ / shaped slot would be just fine so long as the narrowest width at the bottom meets our specs. Hence I was thinking about using a drill mill like http://www.mcmaster.com/#3723a11/=22kwy5 pushed just barely through the sheet to make thin lines. Anybody do fine detailing work with these on a Tormach? I'm trying to figure out if there's some kind radius on the tip - I'd love to be able to make 0.004" wide slots, but 0.01" might do. I'm also a little confused about the speeds and feeds - it seems like since the tool diameter ranges from 1/8" or whatever down to effectively zero that you'll end up essentially dragging the point through the material rather than really cutting. Do you just set the speed/feeds based on the smallest diameter at which you care about the surface quality? Machining time is not important to us - if it takes us 10 hours to cut that part that's ok since the mask will save us a lot of time in the long run.

Finally, has anybody worked with molybdenum before? Anything important to consider with cutting it on a tormach?

[MichaelHenry]

I've used double-sided tape from McMaster-Carr (made by 3M) to hold thin plastic or aluminum stock to a sacrificial aluminum plate with pretty good luck, though the part sometimes comes loose near the end of machining. The likeliness of that happens seems to depend on a bunch of factors, inluding surface prep on the sacrificial plate, size, and features of the part, and the care with which the part is taped down. Ethanol or acetone can be used to assist removal of the part from the plate.

Mitee-Bite also makes a tape that is released with heat,. I've not tried that yet, though.

You might also consider a vacuum plate. Tormach sells one, but it shouldn't be too hard to make one.

Mike

[Don Clement]

Sounds like a job for chemical milling using a photoresist mask rather than using the Tormach. There are some kits that use a laser printer to make the resist mask. See: http://www.fullnet.com/~tomg/gooteepc.htm I bought a kit from Digikey for making masks using a laser printer to etch SS and BeCu thin sheets. I use Ferric Chloride or Ammonium Persulfate. However you might find what etches Molybendium.

Don

[justgary]

BFGarrett -

You might also try shellac to glue your parts to a plate. You can paint the plate with a coat or two of shellac and let it dry, then iron the parts down. Or, you can just weigh the parts down while the shellac dries (but it does dry quickly). Remove the parts with heat or alcohol, and more alcohol will clean them up nicely. I'm guessing that your coolant won't dissolve the shellac.

Definitely set your feed and speed based on the tip diameter of the tool, not the shank size. With a very small bit you'll be well over 25,000 RPM in a hurry, but you can scale the feed down proportionately by the RPM that you can achieve. Rough in whatever you can with a bigger bit to help limit the time running the smaller ones.

An auxilliary High-Speed Spindle (HSS) will get the RPMs up so that you can feed faster. I have used 0.025" and 0.020" dental mills with my Proxxon as an HSS, with good results. I am currently drawing a new bracket to use a variable-speed router as the HSS instead, since the router has a higher top speed and a larger collet (and probably better bearings). Others have posted their HSS mods in this forum.

I don't think I would attempt anything below about 0.060" or so with the main spindle. The feed just gets too slow. Changing to high RPMs will fix that.

Regards,

- Just Gary

[kn6za]

If cyanoacrylate adheres to molybdenum as well as it does to copper and aluminum it would be a perfect fit to this application. I have never actualy tried it with molybdenum, but its worth a try.

You can release the glue with acetone.

[zephyr9900]

BFGarrett, I've done both-- machined with the Proxxon high-speed spindle on my Tormach, and photoetched things like encoder wheels and monochromator slits in brass sheet with my spray etching setup (currently under revision).

If you machine, you definitely want to stay away from any double-sided tape or other adhesive that remains gummy, because that will clog your cutter the instant the two come together. Just Gary's recommendation of shellac or Andrew's ACC sounds great. I'd probably want to stay away from thermal release for fear of buckling the sheet before it fully released (unless you put the whole assembly in an oven or on a hotplate and heated it evenly--i.e. no torches).

If you etch your patterns (and I have no idea what acid you use on moly--like Don I've used ferric chloride on copper, brass, hard steel shim and stainless steel shim), for that size you definitely want to use a good photoplotted film, emulsion towards the work and all that. The best direct laser-printed line image still looks under magnification like it was spray-painted.

Randy

[RTP_Burnsville]

It would depend on what size the overall parts are...

For small parts the various superglues would never hold parts in my many attempts. Machining heats the parts just enough to break the bond.

I agree the double face tape makes a mess unless you can position it where it will not be cut.

I have had fairly good success using solvent based contact cement like that used to glue formica. There is also a product called Barge which is a flexible contact type cement that may work (available at most shoe repair shops).

Vaccum setups are great if there is enough surface area to hold the part. They do not work well on most small parts.

Tried 3M spray glue (super 77 or something like that). I think it would work of parts with a large surface area. It worked much like the superglue products on small parts, the heat and vibration would break the bond.

I am interested in hearing other solutions as well. I tend to do lots of small parts and holding them is a real challenge at times.

Robert

[Don Clement]

A method that I saw at Westec years ago to fixture delicate parts was a cold chuck that used ordinary water to fixture parts. The cold chuck was a thermally conductive metal plate connected to a series of Peltier (thermoelectric) devices. The chuck could instantly be made to be well below freezing or heated by control of electric current through the thermoelectric devices. A thin part is fixtured by spraying a layer of water between the part and chuck then making the chuck freeze. Thin delicate parts such as an eggshell or hard to hold parts such as a honeycomb composite can be fixtured with ease with a cold chuck. Release of the part is just a matter of reversing the current through the thermoelectric Peltier devices such as to heat the chuck above freezing. I have used Peltier devices before and they are simple and easy to work with using low voltage DC supply. See: http://www.apogeekits.com/peltier.htm or http://www.frozencpu.com/products/24...x_Peltier.html

Don

[BFGarrett]

Thanks for the responses everyone. One nice thing about molybdenum (I think) is that it has a very low thermal expansion coefficient, so it shouldn't buckle on heating (and we have hot plates for uniformity anyways). We may still work in aluminum or thin steel.

Originally Posted by justgary Definitely set your feed and speed based on the tip diameter of the tool, not the shank size. With a very small bit you'll be well over 25,000 RPM in a hurry, but you can scale the feed down proportionately by the RPM that you can achieve. Rough in whatever you can with a bigger bit to help limit the time running the smaller ones.

Right, what I was confused about was what the diameter at the tip of a drill mill is. It looks like it narrows down to a single point, which makes the effective diameter zero which makes the feed rate zero no matter what RPM you use. Hence I was wondering whether these tools actually have some small radiused tip on the end rather than a point (I couldn't find specs on what the width of such a tip was) or if it really does go down to an infinitesimal point too small to treat like a real cutting diameter and hence that tiny point ends up dragging through the surface.

As for size of the part - we need to cut out the perimeter of the mask (a roughly 3" diameter circle) and mill a small array of our very small patterns in the interior (each pattern less than 1/4" on a side, made up of little boxes and lines, lines as narrow as we can get, hopefully 0.01" or smaller).

I've certainly thought about using a lithography/photoresist/etch process, and we have lithography capabilities, however our lithography set-up is geared for depositing metal rather than etching, and it's not very good for precision alignment of small patterns over a 3 inch disk. With the tormach, on the other hand, if we can manage to cut the small features, controlling their location relative to the mask perimeter would be trivial.

I'll see if we have any chemical etchants that won't also attack our photoresist, and continue mulling that option. Our tormach is only occasionally used for fixing lab equipment and making one off specialized parts for experiments, so it's not a big deal to tie it up for one super slow milling operation.

[benji2505]

We mill/engrave thin sheets with the help of a vacuum table and a sacrificial MDF plate. We drill holes through the MDF plate and assure bonding of the sheets with the help of o-rings in grooves. One can reuse the MDF plate. We are milling the whole piece in one setup, which helps with the accuracy.

Another question was whether it would make more sense to lasercut this project. A good laser cutter should be ableto come down to 0.01" or smaller in width.

[RTP_Burnsville]

Don,

I find that Peltier element to be pretty interesting. Have you constructed such a chuck? If so did it work as expected?

Robert

[justgary]

BFGarrett -

The McMaster tool you showed will have a flat tip, similar to a drill bit, where the flutes meet at a cutting point. You would have to measure it since they don't specify. A shallower cutting angle would be much easier to control than that bit. I think it was Randy that pointed me toward Bits & Bits. This bit from them might be a good choice for you (especially if you rough first with a larger bit).

Every mill you use will have an effective end radius. If you use an easy to cut subplate such as MDF (or even aluminum, compared to Moly), even the dragging tip won't matter. Just set your feed to the smallest effective radius that you are using in your material on the taper. At some point the tip will drag, but at that size the cutter is strong enough to just go ahead and drag without breaking. You can also buy cutters with a specified tip radius. I never try to use the full feed rate with micro-sized cutters anyway, because I really want to just leave them alone and let them cut. If you back off the feed from the book value, you are more likely to get the part cut overnight without a tool breaking. Small cutters figure out how to break themselves without much help from you, so go conservative on the feed and depth of cut unless you have lots of cutters and want to babysit.

You may want to buy micro endmills and not worry about taper. Bits & Bits also offers straight endmills down to 0.005" from stock. This page lists their stock sizes. Generally, the cutting portion will only be three times the diameter, so you'll need to choose sizes wisely to get the depth of cut you need. They also offer engravers and other cutters that may work well for you.

By the way (and it really is none of my business; I'm just curious), why Moly?

Regards,

- Just Gary