Wire EDM Small Slots in Aluminum

I am mechanical design engineer. One of my current design concepts involves small "U" shaped/profile slots around a hollow cylinder and along its length (similar to splines on a shaft). These slots would be on both the ID and OD. The cylinder would be made of 6061-T6 up to 2" long. My question is from a practical perspective what is the smallest slot width possible using a wire EDM? The depth of the slot would be equal to the width. Are there any "rules of thumb" I should use? Just want to make sure what I draw up can be made.

Thanks in advance.

I know of EDM Wire that goes down to .0008" dia. Thank goodness I've never had to work with it. There are specialty shops that deal with super thin wire. More common sizes are .008, .010, .012". Think about your application too. The smaller the wire, the higher the price to machine. Maybe you could get away with a standard .010" wire slot+overburn (about 20-30%).

Keep the EDM process in mind too. If the entire OD needs slots close enough together to hinder any possible clamping, it may need to be done in two set ups. If that's the case, the operator will need to have a way he can time it rotationally to pick it up the second time. I call this 'whole perimeter machining' and EDM operators are often left wondering how the heck they are going to hang on to a part like that. Think about drawing vertical lines all around a bar glass with a sharpie without moving it. Now think about doing it while HOLDING the glass! That is the nightmare of EDM operators trying to cut a poorly processed part.

A shop may also be able to make an arbor attached to a precision indexer (more $$$ and not all shops have that capability). It all depends on how much you want to spend to get it machined.

Hope this helps.

Where in North Carolina are you? If you are looking for a vendor with a lot of wire EDM experince, give me a call. A sketch of what you need will make suggestions a lot more meaningful.

336-664-113zero
Progressive Tool @ MFG. INC. Greensboro, NC

Tasdau,
Thanks again for the reply. The 0.010 wire + 30% overburn would work for the moment. I understand traditional milling & turning operations but I have no background on EDM other than seeing them in operation once or twice. Work holding is a topic that is always in the back of my mind when I design. Is there anything specific to work holding in the EDM world that would be helpful?

I'm not sure if I understand your question about "anything specific", but keep in mind Wire EDM is different from any other machining in that all parts have to be hung over an edge and suspended by some mechanism.

Another option for your part would be to cut the entire thing from a solid block so the slots could be cut by the wire while it's cutting the OD after all the ID stuff is done. If you needed multiple parts you could nest them in a block and make set up a breeze. Tolerances for size and surface finish need to be considered too before prepping the block if you go that route.

That sounds like a good candidate for EDM and is probably the best way to go. Keep in mind that for anything done in large quantity, EDM tends to be expensive compared to other cutting processes. I can envision something like that being broached on the ID, then finished to diameter and milled on the OD.

I was thinking of the solid block approach also. These are for prototypes where each prototype may have up to 4 parts that require this type of profiling; so the numbers are small. What are typical surface finishes post EDM without additional processing? Thanks again for all the information.

Since these parts are only a couple of inches long, you might consider sinker EDM as an alternative to wire EDM. Fixturing might be easier plunging into the side of the part.

Any reason you're not considering laser? UV laser is, in my opinion, the go to technique for really thin stuff (PCB stencils are .003 to .006" thick stainless and you can get tens of thousands of precise cutouts done for about $150 on a laser) and fiber is pretty good for the .015ish range that you're talking.

A UV laser will easily make a .001" kerf if you need to. For low volume stuff, a fourth axis works fine, and there are dedicated tube lasers for high volume stuff.

Oh yeah, and laser is much, MUCH faster than wire.

Roughing only on aluminum will give about a 90-100 Ra finish. That can be improved with skim passes. You can get down to a 35-40 with multiple skims (manufacture's specs will vary from machine to machine).

If skimming, your kerf will be wider because the rough passes will need to leave stock for the skims to remove. Your slots can still be programmed to just go 'in & out' to keep them smaller but you will get only the rough finish.

If you go with the block set-up, the OD skimming will need to be done 'in the gap' and will require additional considerations for processing like number and location of start holes.