Benesesso wrote:I attached a sketch in the first message.
Yes, it appears you did!
What's the preferred method for turning the 2.25" stock OD down to .875"? Should I take a lot of light cuts with a higher longitudinal feed rate, or take heavier cuts at slow feed? What's a good amount to remove in one pass?
A great deal depends on the tooling you have at your disposal. If that was my project, I'd rough with negative rake carbide, taking .400" off the diameter per pass. You can get the material off in a minute or so.
If you don't have insert carbide, negative rake, you can take the cut with a right hand HSS turning tool with a decent chip breaker, and take the same amount off per pass, but it would be at a much slower speed. I don't recommend you try that at this point in time, however. You should get familiar with your lathe and get a feel for its capabilities. A cut of that depth may (or may not) be a little too much for the machine to handle well. There's no need to put yourself in a position where things can go wrong.
When roughing, depth of cut and feed rate is how you get rid of material. I tend to discourage repetitive shallow cuts, which waste time and wear out tooling prematurely. There's usually no need for a finish of any description, so you use a coarse feed and appropriate speed. Judge speed by observing acceptable surface speeds for the material you'll use, and observe the color of the chips coming off. With HSS, if they are anything beyond a hint of yellow, you're running too fast. Brush apply cutting oil, to both lubricate and cool.
Considering this will be a refresher course for you, I'd suggest you take it slow and easy. Experiment with depth of cut and feed rate. Start with a feed rate of about .010" and a depth of cut of .075" (per side) and see how it behaves. As you alluded, you'll likely need to work in back gear, both for surface speed control and torque.
If I was to make the parts, now that I've seen the print, I'd make them on a common piece of stock, roughing both ends first. I'd rough turn the .875" diameter, leaving .03" for finish cuts, then drill the hole through. Drill it 9/16" through the entire piece. Turn the material over and rough the other .875" diameter. Cool the part, then face, turn the .875" and face the flange to proper length. Bore the .623" hole slightly beyond the finish length of the adapter, then bore the counterbore. Debur, then reverse the material and repeat.
When you have both ends finished, split the two parts. The finish bored .623" diameter will permit you to dial in the part, using a four jaw chuck and shims between the part and jaws, to prevent chucking damage. Hold the part by the .875" diameter, and leave enough room between the back side of the flange and the chuck jaws so you can run a DTI against the finished face, to establish perpendicularity. You'll chase the part a little, for as you tap it to get it perpendicular, you'll lose the concentricity. Work both features until they run true, then rough and finish the 1.249" diameter to proper length. Debur. Done. Don't be afraid to use a little abrasive strip to polish the turns if you don't like the finish, or if you're near size and want to bring size in. You can easily polish a half thou, and it can be difficult to take so little off when machining steel. It likes to tear and not cooperate.
Do NOT use a caliper (vernier, dial or digital) for your measurements. That's sure to get you in trouble*. Use a telescoping gage for the two internal diameters.
*There's no end to people thinking that a caliper is up to the task, but it clearly is not. Regardless of it's ability to read to tenths (some do), they generally don't reflect true size. When you're working with a thou clearance, it's most likely you'll miss the dimension when measuring internal diameters.
Hope this helps.