[Alex, Daniel]

I tried to make the stainless steel bushing today with some improved G-Code and methods from this. 

According to FS Wizard, I should use a spindle speed between 991 and 1322 rpm and a feed rate 4.73 and 6 in/min, depending on the radius of the cut. I ended up using a spindle speed of 830 rpm and a feed rate of 5 in/min, with a finish feed rate of 2.5 in/min. I took 10 thou (0.01") per cut; I could be more aggresive here but it would not save very much time considering how long everything else takes.

The program ran well and the diameter matched the existing bushing to within 1 thou. There may have been some bumps, so lowering the lead-in feed rate would be appropriate.

The program did take off some of the inside instead of letting the drill do all of it, leaving a nub, so used what I thought was a spot drill but what was a tailstock support. The drilling (at 640 rpm), partially because of this issue and partially because the drill got way too hot, did not go very well. The diameter was around 0.244" at the start of the part and down to 0.237" at the end of the part. The drill bit may be damaged.

Chamfering/countersinking (at 120 rpm) was "too easy" and I took a bit too much material, but this is a mostly cosmetic concern.

Tapping the part was very exhausting. There are 100 threads per inch (tpi), meaning Alex and I would have to do hundreds of total turns to tap the part while breaking the chips. I eventually had to redrill the part.because of the reduced diamter issue. I was able to tap the part almost to completion, leaving only a few threads left on the tap before the part.

The parting operation (at 170 rpm) went very well. I used a pencil-like tool to catch the part so that it didn't fall, of course ensuring this tool did not extend too deeply as to be cut. I could potentially go even slower with the spindle next time.

The parting operation did leave some material, so I clamped the 0.374" diameter portion and took off the material with the carbide insert and faced off the surface. The 1/4-100 screw we had did not go into the hole all the way or the "back way" at all. I tried to clean up the thread from the back outside of the lathe, but this ended up ruining the thread.

Things to change for next time:

Drill better, potentially in the Haas VF-2 CNC Mill. This mill will allow for constant pressure and more importantly, a ton of coolant direclty on the part and drill bit

Tap the part from the "back side" so that we are tapping a thru hole. I don't know why I think to do this today.

Instead of using a tap, I could use a thread mill. A thread mill that can make a 0.7" deep, 1/4-100 thread does not seem to exist.

Another option is to have someone, like Thorlabs, 3D Hubs, or Xometry make the part. Newport will not make this part. Some people in Nick Hutzler's group recommend silver (or gold) plating.

Another note: we also are considering making this part out of copper. Copper is difficult to work with as it is gummy and it will be weak in the end, considering how little material makes up the threads.