Small hollow shaft with flats - best way to make?

[PStechPaul]

I wanted to make a small (0.312" or 8mm) shaft (I'll call it a pivot) that will hold a ball bearing and have flats on each end that will fit into 0.250" slots to keep the parts to which it is mounted from rotating. There will be a #10-24 bolt through a 0.203" hole through the pivot that will hold the parts together. Here is how I made it, but there might be better ways.

First I cut a 0.65" piece of SS shaft from a scrap printer. On the lathe, I faced the ends to the desired length of 0.625". Then I used a center drill to make a starter hole, and followed it through with a 0.203" (13/64") drill. It appeared to be concentric, and does not need to be high precision.

Next, I clamped the piece in the milling vise, using a partially drilled (mistake) portion of one of the faces to hold the part about halfway exposed, and I had marked a spot 0.25" from the end for the one set of flats. I used a 1/2" end mill and adjusted the ram so that the end of the mill met the 0.25" mark, and I adjusted the cross-slide (Y axis) so that the cutter just touched the part. Then I moved the table by 0.030 to take the first cut, and then I reversed the process and took a couple of cuts on the far side to get the desired 0.250 across the flats:



Then I turned the part over, and clamped it in the flat portion of the vise jaws on the flats of the part, and this time took only a 0.125" cut for the flats. Here is the result, and it looks like it is "good enough", and maybe can be touched up a little with a small file. It has always been difficult for me to figure out how to get an accurate depth for milling (Z-axis) because the only adjustments are the ram (which has a very rough depth gauge), and the table height (which is a very coarse rack and gear crank on the column). Here is the manual for the machine so you can see what I have to work with:
http://images.harborfreight.com/manu...2999/42976.pdf

Here is the part. Definitely just "run of the mill" ! [insert smiley here]







Any reasonable suggestions and constructive criticism welcomed. I want to be able to do things like this the "right way", given the limitations of the equipment I have. And possibly ideas of ways to achieve a more accurate way to set the milling depth. TIA.

[edit] I discovered one problem. The hole is somewhat oval, 0.209 x 0.198 on one end, and 0.217 x 0.219 on the other. And so the bore is somewhat conical as well. It's not really critical, but it would be good to know how to avoid the problem. Perhaps by milling the flats first, and then drilling? And of course a reamer would be better than a drill to make the hole truly cylindrical. I have a second part to make. Let me see if I can do better!

[Toolguy]

For something like that I would use a spin/indexer with collet or collet block in vise with the part in a horizontal instead of vertical position. You can touch off the end with the side of the end mill and move in with the x dial. You can take a cut across the part in the y axis, index the part 180 degrees and make another cut in y axis at the same depth. Then measure the part across the flats. Put a dial indicator under the end of the end mill and lower the cutter 1/2 the distance between the measurement you have and where you want to be. Cut both sides again and you're there.

[Jaakko Fagerlund]

Make a dial indicator holder that clamps to your mill column with a bolt or something, so you can see the depth setting at all times.

As for the hole, you said that you clamped the drilled part from those flats. That is where your ovality comes from, it crushes the part slightly. Put the drill or something a tad bigger in the hole before tightening against it, so it can't deform.

If you drill after milling, it might crush the part just when it punches through and the drill could then grab. But, I would test it out first to see what happens if nothing happens at all. On the other hand the drill might deform or rip those small walls easily if, as drills are generally like blunt force trauma to metal.

And please, do not use a centre drill for a hole start. It is, like the name implies, a drill for making center holes. Get or sharpen a proper spotting drill, thus prolonging your drill life and hole location accuracy.

[oxford]

Buy yourself a set of 6" digital calipers drill a couple of holes in it and mount it sideways to your quill. You will have to look at the numbers sideways but you will have a cheap DRO for your Z axis.

[PStechPaul]

Those are some good ideas.

I was able to make the second piece by milling first and then drilling. I used a smaller drill (#12 or 0.189") which is a close fit for the #10-24 screw. However, the hole varies from 0.196" on one end and 0.1875" on the other. At least it is smooth and concentric. I was able to squeeze the oblongated part back to nearly round.



I made a short video of the facing operation. Seemed to go pretty well for a HF lathe and carbide bit (that I touched up with a diamond file). The video title says 7 mm but it's really 8 mm. And it looks like the lathe is running backward:

[edit] I think a Spindex would be a very useful tool for small parts like this. I found one for about $70 including shipping:
http://www.ebay.com/itm/NEW-C5-SPINDEX-INDEX-FIXTURE-O-201-/181333281708

It looks like it might not be hard to make one. And I have an idea - among the parts I salvaged from the same printer I got the shaft from, is an indexing wheel with 12 cardinal points and some very fine graduations, which fit into an opto-coupler that should be able to read the transitions for angular position. The dial is labeled 1200CT and 200 LPI. There may very well be 1200 points per revolution, which would be capable of resolving 0.3 degrees. Or, perhaps the 72 tooth gear can be used, which would provide 5 degree increments. Hmmm...



[edit2] That's actually a 71 tooth gear! WTF!??

[Arthur.Marks]

You are finding why collets have a special place for those of us working with smaller work. A three-jaw scroll chuck will apply pressure at three points, and you're finding that it takes very little pressure to deform a thin section. In fact, it may take more pressure than the resulting thin wall can resist in deformation just to hold the solid rod to drill through it. One great benefit of collets is that the part is held equally on its full circumference. This greatly avoids deformation. There are other ways, of course, to achieve the same holding characteristics. "Pie" or "full grip" soft-jaws are one. Unfortunately, this is a scarce option on any chuck below 5" diameter.

Another method is to reinforce the workpiece either by the ID or the OD. For example, one might choose to drill the hole first on an oversize workpiece and then use a mandrel in it. One could also finish the entire job from first working with a solid. The OD is turned; the flats are milled; and the bore comes last. In that case, it would be possible to make a larger, stronger, split sleeve that the workpiece fit in. The sleeve is then clamped onto the OD of the work. Clamping the two in the chuck will then not deform the part. There is much more material to resist the three points of pressure from the jaws. You can think of the sleeve as a makeshift, DIY collet you've made specifically to fit your workpiece.

Believe it or not, I have started replying to this thread three times! The problem I kept running into is how to explain myself without dictating you need X piece of tooling or Y machine. One of the great things about machining is that there are so many various ways to make something. For example, I could imagine making this piece entirely on the lathe by using a file and a roller rest to create the flats. Equipment is often less the limiting factor in accomplishing projects than understanding the principles which achieve a specific result. Take, for example, drilling a hole. There are various reasons your hole may be tapered. One is deformation as already mentioned. Another is that a drill rarely makes a precision hole. Reaming or boring is necessary to ensure size and circularity. If positioning is paramount, boring is necessary because a reamer will tend to follow a drilled hole. A single-point boring tool, however, will only follow the spindle axis.

Tiny boring bars aren't always in everyone's shop. They can be made, of course, but at this size present something of a grinding challenge with only a standard bench grinder to work with. If the hole is made first and reamed, there is an easy way to assure concentricity. Mount the work by the bore for finishing the outer diameter. If the work is rotating on the axis of the bore, it is guaranteed to be concentric when other features are turned. A mandrel on which to mount the piece can come in various forms. A mandrel can be made from scrap turned to an interference fit with the bore. The work is then pressed onto the bore and retained by friction. A mandrel can also be made to be a close sliding fit to the bore. The mandrel may then have a step the work seats against and a thread on the end for a nut. The work is inserted on the mandrel. The nut is threaded tight against the work to hold it. Once again, the work is held by friction but this time by its ends.

Then we come to mounting the mandrel itself. It can be turned in-situ. This guarantees that the mandrel is concentric with the lathe axis. The mandrel could also be held in a collet. This makes for simple, fast and accurate mounting that can be changed among fixtures or machines. Lastly, the mandrel can be made to turn between centers. This also allows removal and accurate, fast re-mounting among machines and fixtures.

How to create an equal 180 degrees? There are a plethora of options here too. One way is with an indexer. Another may utilize a simple collet block held in the milling vise. If you have neither, a v-block will do. Clamp the work in a v-block. Place the v-block on its side. Mill one flat. Then place the v-block on its other side. Mill the second flat. A v-block has its angle central to its edges to a high degree of precision. I very rarely see this aspect of a v-block mentioned or utilized in images on forums like this. It is a handy fact, though, to keep in mind. As long as the clamp is not released, the block can be manipulated to create features accurately on the work in the same set-up.

So there you go I'm sure there is much that could be added to my reply. There are just so many "best" ways to make something that a short reply is hard to settle on. Hopefully this, my third try, will give you some details to explore.

[KJ1I]

Arthur beat me to it. I was going to suggest inserting a piece of snug drill rod in the bore (hole) before milling the flats. And I have seen the V-block idea/use illustrated in my old (1900-1920) machinists' manuals. I guess sometimes we forget the "old" ways in light of all the "modern" advances.

[LKeithR]

For me an appropriately sized collet and a collet block would be a "no-brainer" for a job like that...

[Doozer]

Clamp the shaft in the vise about it's length,
not it's diameter. That way you will not crush
the inside hole.

--Doozer

[PStechPaul]

Now I can see some of the special challenges and appeal of machining, where not only can there be many good ways to design something, but also many ways to accomplish the same (or similar) end result. I have similar problems in electronics, where I often design something that will work, but as I get into details I see other ways to do it, and I sometimes get caught in an endless cycle of redesign without ever finishing what I started. Just coming up with this simple little part was the result of maybe dozens of other ideas, some quite similar, and some quite different. This is part of a model steam/compressed air engine that was partially inspired by Brian's double opposed piston design. Since it is really just a "hobby project", and mechanical design does not come as easily to me as electronics, I have the luxury of working at my own pace, and learning as I go.

Other parts of this project will involve drilling holes and machining slots on a 2" diameter cylinder with 0.25" walls, a shorter 2" diameter cylinder with a 1" bore, and a 1" diameter rotating valve. I already had some difficulty drilling six-hole bolt patterns on both ends of the larger cylinder, getting them to match holes in rectangular mounting plates. But that may help position the cylinder in a way similar to the V-block method. I saw that in my "Technology of Machine Tools" First Edition textbook ca 1965, but I would need larger blocks than what I have.

Just as I found that many of the materials I bought for this project were no longer ideal after I made some design changes, I also see that many of the tools I have bought over the last ten years or so, are also not right for my purposes, and now I must buy even more, or improvise, or make my own. I can see why this can be an expensive hobby, and no matter how many tools you have, they are never enough.

Thanks for the detailed replies.

[edit] I just looked on eBay for collet blocks and I can see where they can be very useful for things like this. I had always assumed collets were for tool-holding, and not work-holding.

I'm not sure how well it would work to hold the part on the ends, since they can be damaged as well. I was going to drill a 5/16" hole in a piece of scrap material, and then cut it in half along the bore to get two halves that would grip the part without putting quite so much pressure across the bore. It would also reduce the amount of pressure needed to grip the part securely.

Now I need to mill some slots on the 3.5" flywheels:



I think I will use the holes already in them to bolt them to a piece of square stock in the vise. Or I might remove the vise and clamp the disk to the mill table. I have some step blocks I purchased at Cabin Fever along with other tools.

[fixerdave]

...A mandrel can also be made to be a close sliding fit to the bore. The mandrel may then have a step the work seats against and a thread on the end for a nut. The work is inserted on the mandrel. The nut is threaded tight against the work to hold it. Once again, the work is held by friction but this time by its ends.
...
There are just so many "best" ways to make something that a short reply is hard to settle on.

Then there's this guy... he takes a blank, bores it out to slip-fit a shaft, then "merely" Loctites it on. Then, he proceeds to thread said blank into a hob. Blew me away. Never knew Loctite could be that strong. So many options; so much to learn.

Using his approach, you could turn ridiculously thin-walled whatevers and then just heat them off. The only limitation is the part distorting from the heat. I wouldn't be surprised if you could cut a spring out... might be fun to try.

Arthur beat me to it. I was going to suggest inserting a piece of snug drill rod in the bore (hole) before milling the flats. And I have seen the V-block idea/use illustrated in my old (1900-1920) machinists' manuals. I guess sometimes we forget the "old" ways in light of all the "modern" advances.

Never occurred to me to use a V-block for that... way easier than trying to get something in a 5C block, especially if the size isn't right.

That's what I like about metalworking. You can learn and learn, and the stuff just keeps building up. In computing, you learn stuff, then you have to learn new stuff and try to forget that obsolete old garbage... from last year. A metalworking book written in the '50s (or even older) has lots of useful information, at least for a hobby machinist. Outside of basic theory, or support for obsolete stuff, a computer book with dust on the cover is garbage. Oh, sorry, let's say "due for recycling," but not a soul-satisfying workshop recycling way. You know, like gutting a printer for the ground steel rods

David...

[PStechPaul]

Very informative. As a relative beginner, I picked up a number of probably simple techniques. There are probably many ways to accomplish the same things, and perhaps none may be declared absolutely "best". If it gets the job done in a timely, safe, and effective manner, with the tools on hand or easily acquired, then it is a reasonable way to do it. I can see that it is possible to work fairly quickly when you know what you're doing and have good tools, but it is still a time-consuming process. I think I'm at the point where I recognize a tool doing a job well by the sound, shape of the chips and swarf, and the finish of the cut. Machining is as much an art as a science.