Originally Posted by
sansbury
I rent a corner of a shared space in Boston, and my new next-door neighbor is working on commercializing his Ph.D. research in robotics, which works out well for both of us because he has a low-cost machine shop nearby, and I have a small but steady customer with very low shipping costs and reasonable expectations. He recently asked me if I could machine some pneumatic fittings for him, real simple job drilling and tapping three 1/8-28 BSPP holes on alternate sides of a quick-release fitting just like you have on your compressor to make a manifold of sorts. The first couple I did more or less manually in a vise and hand tapping because he needed them yesterday, but he wanted about 20 more done and said I could take my time with those so I decided to see how to do them more efficiently.
Putting them in the rotary table seemed like an obvious choice since that would allow me to do all three holes in one setup. Normally I like to fixture more than one part at a time, but I didn't have a whole lot of brilliant ideas for this one. The round surfaces are all larger in diameter and either move or are too small to clamp onto, so it seemed like any kind of multi-part fixture would involve a decent amount of material and engineering, too much to recover in 15-20 pieces. The rotary fixture I made was a simple doohickey that had a 1/2" section I could hold in a collet in the rotab, a couple inches to provide clearance, and a tapped hole the fitting could screw into. I counterbored about .050" of the hole so that the fitting's shoulder would seat firmly against the fixture to keep everything square. Since all I had to do was drill and tap, I thought I could get away without the part spinning and loosening itself.
The second nut I had to crack was that the tap had a .435" shank, and I have an ER-16 tap holder which maxes out at .375". Back to the lathe for another little piece of 6061 with a .375" shaft and a .435 bored hole. I added a set screw to clamp against the square part of the tap shank. It wasn't the prettiest thing but I figured at 500 RPM it wouldn't fly apart and the holes were very shallow so the torque requirement was low.
The one shortcoming of the fixture I made was that I had to align each part individually since the threads didn't align with the faces of the hex section the same way from one part to another. So basically after screwing a part in and tightening it, I used a dial indicator to align the face perpendicular to the mill. At first this was slow, but after a couple I was able to do it in under a minute. I would jog the indicator down so it was contacting one edge of the face, zero it, jog to the other edge of the face, and note the difference (say .010"). I'd jog the rotary until the difference was .005", and then jog to the other edge, lather rinse repeat. Usually one or two passes was enough. Then I would zero the A axis and start the program. However, I made another change because a couple times I indicated the part, but forgot to zero the A axis. Then as soon as I hit run I'd watch the table spin back to the old zero and I just wasted a minute. So I added a line to the program that zeroed the A axis before it started, so now all I had to do was indicate the part and hit go.
By the time I finished I was averaging a little under 5 minutes each, so at $5 each with customer-supplied material and tools it slightly exceeded the $50/hr machine time goal I aim for. Setup and fixture/doohickey-making took about an hour and a half mostly because i just got a new lathe and I still don't have all the tooling for that set up well, so I had to do some workarounds.