How to hold this part for milling?

Mill the flat first, then round the ends. If the flat is half or more of the diameter, you can do two pieces at a time in the lathe, with an extra flat piece between the pieces! If less than diameter, use an extra piece, or try how well the collet holds the piece with the flat missing..

Kristian Ukkonen.

What is the advantage to milling the flat first?

"Chief McGee" wrote in news:gKCJc.98543$XM6.80942 @attbi_s53:

Because you can hold it on the mill then, and access the entire length.

What is the finish dimension of the "D"? Do you have to mill below center line?

Greetings Ed, For sixty parts I'd just do them one at a time. 303 machines easy so cutting time will be short. Making a fixture to do only 60 parts this small would probably take more time than you would save. If the rounded ends need to be spherical then a form tool in the lathe would be fastest. You can buy a tool made for the lathe to do this or you can buy a "corner rounding" end mill and use it in the lathe. This way you will have 4 cutting edges so if one gets dull there are still 3 left. With 303 the edges won't get dull with only 120 ends cut. A ball turning tool will be slower than a form tool. If you are determined to use a fixture here's an idea that will work: Mill an aluminum block 2 x 3.5 x .75 thick. In this block mill 6 grooves .187 wide and with the depth the same as the "D" dimension. With a thin (about .032) saw blade mounted in your mill and the block on it's long narrow edge in the vise make a saw cut in each groove close to the side of the groove and about .450 deep. The saw cut must be off center because the rods will be sitting in the groove and locating off the bottom. If the saw cut is on center the rod will sit deeper in the groove and the location will be off. Now, since the grooves you milled were just wide enough to let the rods fit in, then when the fixture is clamped in the vise the fixture will not have to be squeezed too much to clamp all the rods in place. If it moves too much the bottom will curve up off the bottom of the vise and the parts may not all be the same when milled. All the slots must be filled when milling or they won't be clamped tight enough. Cheers, Eric

Don't make a federal project out of a short & simple job. Round the ends in the lathe with a form tool. You may be able to leave the spindle running when changing parts. For the flat, if you have a 6" vise, just put in 2 at a time. Each pass will get 2 done. That is not many repititions, you'll be done before you know it. If you should need to do a couple hundred or more, then you might make the fixture work pay off. You're cutting butter, afterall.

michael

Rounding the ends is easy, if you have a lathe with a 3/16" collet and a form tool. Milling the flat is more involved-- Eric's "flat collet" idea is neat but I'm in favor of the easiest solution in the least amount of time. I would use hard maple as a fixture plate with 3/16" grooves as in Eric's idea, but bed them in with a small gob of epoxy about 1/3 of the way in from each end. Make the block about 3/8" narrower than the desired length of the rods, to allow miking of each end. The maple block is surfaced, then 3/16" wide x 3/32" deep slots are cut, and the glued-in rods flycut or endmilled. Heat them just enough to break the epoxy bond (soldering gun, to avoid heating the wood too much). Of course, if you need better than +/- .002, this probably won't be accurate enough.

Or cut the slots with a 3/16" ball end mill, and superglue the rods in the block.

Ken Grunke SW Wisconsin

The flat can be to the centerline of the bar, or slightly above (dimensions are not critical - these are decorative pieces). I do not have a large vise for my Taig mill - the table is small. The issue I need help with is how to hold the bars in order to mill the flats. I'm milling a large enough quantity that I can build a fixture if nessary. Any ideas?

Ed

If you leave them over length for clamping purposes and mill to the centerline, you could then round the ends by machining them in pairs in the collet lathe...

Joe

No fixture needed, just a parallel under the part so the center line is just below the top of the vise jaw. Mill the flat to the desired depth, repeat

To be clear you are gripping the bar in the vise the short way.

I fully agree with those that suggest you do them in a vise, one at a time. If the project was mine, that's exactly how I'd do it on my manual Bridgeport. You're not removing enough material, nor do you have enough parts, to make this a job worth your worries. If surface finish is important, you can make your cuts with a fly cutter. Make a parallel from a piece of 1/8" aluminum that holds the part at the precise depth in your vise that permits machining it without cutting the jaws. One caution: These parts may not stay straight when you machine the flat.

Harold

I agree, Roger I have parallels for all the most common sizes of stock already made to allow me to do this. The heigth of the bars is right to allow milling at center, and the width is right to allow biting the part without stopping the vise jaws. You will be cutting so close to the vise it may scare you, but I do a LOT of stock this way. A good vise will hold round stock a couple of thousandths below center with a camming action. If you don't need centerline cuts, just make your parallels a little shorter.

RJ

Thanks to all for the ideas. The keyword here is "Taig mill" The table is only 19"x 3.5" and my little vise is only 2.5" wide.

I'm going to make a custom parallel 3.5" long and slightly thinner than the 0.187" bar to be milled, and mill one bar at a time to centerline, with 0.5" of the rod and parallel overhanging each end of the vise. I'll write some simple G-Code to do the work (the Taig CNC has no handles).

Then I'll place two at a time in the 5C lathe and form the ends.

Regards, Ed Ferguson

Ed, That won't work very well. If the parts are milled exactly to center then they'll come out of the vise. If milled to .005 above center the'll stay in but that means two at a time in the collet will be out of round .010. Your collet may not even expand that much. Though twice as many ends will need to be done doing them singly before milling them will work much better. The milling will take longer than the turning so after the first one is turned you can load it in the mill and start turning the rest. ERS

A 6" vise on a Taig? The Taig would proably fit *in* a 6" vise. :-)

Enjoy, DoN.