How would I do this? (pic)
I'm trying to figure out how I can make this. The center hole is only about 1/16" in diameter but it has a flat side for a "key." Perhaps a broach? I really just don't know. And of course, just to add to the complexity, it has to be perfectly centered. I thought about a very tiny end mill (1/32?), but the part I'm replacing has no internal radius on the flat part, and this wouldn't be ideal for preventing stripping (it would lose quite a bit of leverage if it had any radius in the inside corners).
I'm attaching a pic to help explain what I'm trying to do.
How many do you have to make? If only one, lay out the hole with dykem, drill a hole in the middle and get after it with a file. With enough care, you should be able to do a fine job. Especially if the shaft is available for trial fits as you go.
I'd think you'd need at least two small files: a half round and a traingular. You'd probably want to grind a safety edge on one flat side of each file.
1,000 +/- a few.
Way too many to do by hand and more importantly it has to be as precise and with the closest tolerance as possible. I don't have a specific figure for the allowable tolerance...just the tighter, the better. The part I'm trying to replace has a little slop to it and that's a major part of the upgrade I'm hoping to able to offer.
wire edm is the best, however slow. you could also adjust the corners with small u-cuts and then you could interpolate on a cnc mill. Any questions i am more than happy to send u a sketch of your part with my ideas added to it.
richard.brodeur@niagaratools.com
Punch it ?????
i would have to say based upon how thick that piece looks, deforemation may occur. ?
Wire or sinker
What's the mat'l.....how thick? If hard stack a bunch of plates and tack weld together, Drill some holes for threading and wire the complete profile. Or burn with a sinker EDM the center feature. I've done similar parts out of 6061 AL by steping down to a small diameter end mill. It's probably for a shaft, so a small undercut (over-extending the flat) would probably be permissable if the diameter is held tight.
My idea maybe not the way to go but I give it a try anyway. I think with the long rod EDM the center contour, hold in the chuck lathe face then cutoff .01 plus to length, then flycut cutoff end to length. With rod match the ID contour hold in the chuck, then turn OD.
Just my $.02
The best way to learn is trial error.
It's made from aluminum. It's dimensions are about 1" in diameter, about 3/8 thick and as much in-between material is removed as possible for weight reduction (similar to a billet wheel, but really small).
I'd like to be able to make them myself if possible. I guess I'm hoping someone makes a key broach in that shape. I don't have an EDM, but I do have a CNC and assorted other shop tools.
So I guess I'm adding a wrinkle to the design...I need the closest tolerances possible...but I need to be able to do them in just a couple minutes each for the lowest cost possible. You know, I want everything...and I want it for nothing
RE: New Texas
I like that Idea....Or how about finish turn a long section with a rough drilled hole (makes burning faster), then burn.....then part.....the only issue would be burrs at parting.
If the part thichness is within 6 mm, My opinion is to punch it out. for very precise job, u can make it with two punches, rough one, make 1 mm smaller then finish and finish it with another die. It will also reduce ur working cost. But dies cost must bear.
CNC VMC or just Lathe?
If you have a CNC VMC.....then have you ever stripped a job? I used to mount 3 Kurt Vices with aluminum soft jaws. then mill a .1 deep step on solid and moveable jaws. If I had 30" of travel I would cut a 28 or so long bar (In your case 1.125 X .5) face top, mill profile (as many times that will fit in 30"). Drill, mill center feature, step down to small diameter EM. Then deburr. Stack the strips up.
Then Op2.....Mill in circular pockets the same width apart as your parts in the strip, Clamp lightly, hit down with a dead-blow, tighten vice, Flycut, Deburr, parts complete......In fact, in Op1 I would pre-drill the corners of your "D" so you don't have to deal with EM deflection.
Strip
Clamping a longer bar allows you more holding pressure b/c the weight is distributed thus allowing you to crank! When flycutting op2 leave .015 to .02 for a secondary pass then .005 above finish conservitavley (so as not to "pull" the parts. Then your finish pass.
Any ideas where I can get something like that? That's probably more within my budget. I was thinking pre machine it, then punch it out...but I've really never done that before so I'm open for idea's.Originally Posted by Zaki
I know the right way to do this is with the EDM, but the budget on this project really doesn't justify it I don't think. These will only cost a couple dollars each in the end.
I'm not sure I understand how the "D" shape is formed. Small diameter EM?
Type of Equipment?
What type of mill do you have? Is it decent for roundness?
DImensions
You said a 1/16th diameter....Tolerance? Also how far off center is the flat?
the flat is maybe 1/64 off center (halfway between center and radius). The flat needs to have a sharp edge ideally.
Spindle Speed?
What kind of spindle speed do you have? Can you drill out the corners? There are many manufacturers of micro (circuit board drills) drills....Carbide holds up pretty good on aluminum.
Drill the corners 1st, then the center hole, then mill the profile in depth cuts....your time will be in the "d" but the rest is pretty fast.....how fast per part do you have to be?
The Only other thing I can think of is making them complete on a lathe.....Face, Turn, drill, then make a nibbler for the "D" shape, Then part.
Reply with Quote
