I need to make this part. It's a lower bearing race; this piece is welded to a bike fork, so the crown from the headset bearings can be pressed on(normally a .001-.004" press fit). I've talked to two machine shops, and both of them say the wall is too thin to machine(about .025"). I only need to hold half a thousandth of an inch tolerance, +/- .0005. I am looking to make two versions out of mild steel and the other being out of 6061-T6 aluminum. My idea for the steel one was to buy a 5/16" thick mild steel plate and just cut them out with an end mill. I guess that won't work? How can I do it?!?

Sorry about the dimensioning and such

 

first, a half a thousandth of an inch is .0005", not 5 thou like you typed (.005") you need to add an extra zero there. that is a pretty tight tolerance and a very big difference between that and .005" tolerance.

second, i'd turn that on a lathe, not a mill. and maybe finish it on a cylindrical grinder.

 

Sorry, just a typo. I was hoping cutting them on a mill could speed up the process and keep setup time to a minimum. I did get recommended to turning on a lathe and finishing on a cylindrical grinder. One of the guys I spoke to thought that would be the only way to get the tolerance I need. I guess I'll think about heading back there then. I was really hoping to cut down on cost. I appreciate your response!

 

I could make that. I would use my lathe though (not my mill). On a tight tolerance job like that one, I would bore the ID first, don't hit the size yet, maybe leave .030 or so for a finish bore. Turn the OD to finished size, then depending on how important that ID is (but probably not neccessary) i might make a sleeve that would slip over the OD to keep the ID from deflecting when finishing its bore. If you take your time and what i call sneek up on the size it should work out. Overall a easy job, the .025 wall thickness is being the tricky part.

If you do make that sleeve for the OD like I mentioned, it will probably help out a lot when it comes time to press that bearing in ;-)

 

Hmmm, ID just slides over 1-1/8 OD tube. Unfortunately, 1-1/8" is never exactly 1.125, the 4130 I order is ~1.3025". By the way, I'm looking to make about 60 of these pieces.

 

1.125 is exactly 1.125 if you can hit the size with your equiptment. Though you would want to leave 2 or three thousandths clearance between the sleeve and part.

 

Yes, I can make the tube 1.125. I'm saying when I order it, the actual OD of the tube is ~1.130.

 

given the application you should be fine with 0.001" tolerances. Turning may be cheaper depending on the shop, but I don't see a reason these can't be done on a mill. 0.025" is thin but there is no reason it can't be done. The devil is in the fixturing.

 

Good luck holding half a thou tolerance on that part if it were made on a cnc mill, It is a job for a lathe (manual or cnc, doesn't really matter)

Why would you need to hold half a thou on tolernaces?

There is no such thing as a CNC Endmill

 

lol @ CNC Endmill

 

Crown rings are usually made with a thicker compression area and then a special cutter is used to chase it down and face it (I have the machine that does this) . I have some that are already welded to butted steerer tubes and finished if you need one. I have crown ring blanks also. You can finish them on the lathe (if you have one) when the fork is done. On the aluminum part, machine the riser directly in to the steerer rather than using a sleeve. The aluminum sleeve has been used in the past and seems to be pretty fragile.

 

You can do it with an cnc mill but it will be a 2 step process. Do your 1.180 and .188 dimensions. After that call a EDM machine shop and they can wire cut it all out for. And hold that tolerance.

Using a lathe will be cheaper..

 

For as simple of a part as it is, they are pretty complicated. The ID and OD are not really relevant. The thin part is a shim that will be compressed with installation of the bearing race. Production parts, cut to size are used on BMX forks and the ID collapses a bit, they are then pressed on the tube and welded.

I will throw up some pics later.

 

 

Yeah, first.. this is not something you'd make on a mill, not saying it couldnt be done, but thats just nonsense.

This would be a very simple part to turn.. holding half a thou tolerance would be tricky, but not impossible, emery cloth works wonders on one-off jobs like these

Start with >1-3/8 dia. shaft or tube, chuck it in the lathe leaving an inch or so out of the jaws, bore your i.d. first, then turn the 1.180 shoulder a thou or two oversize and hit your target size with progressivly finer grit emery cloth. Part it off to your desired length. When your working with tight tolerances, be sure to let the part air cool before measuring/taking a finish pass, and do not try to chuck on the .025 wall, especially the aluminum.. if you part your piece off, you should be able to finish this in one operation without flipping it in the chuck. Bleh

Ive done a few thin-wall hub centering rings out of aluminum for my car.. very similar.

If your going into production with these, then cnc is the only way to go (turning center that is.. not a mill).. no emery cloth required , and this part would take 10min to write in g-code.

 

So the correct process is to order blanks, finish the fork, then use a crown race cutter to put the finished dimension on? If I can order blanks, I could probably finish the forks and have a bike shop cut them to the finish size. Do you mind telling me where you get yours? I'd be interested in buying a blank from you to check it out.

Sorry for all the confusion. I'm doing my best to learn. Thanks for all the help guys!

 

the procedure you describe is correct, PM sent