I'm embarrassed to say that it was carbide CCMT.
(on retrospect I think that's the problem...)
Why be embarrassed? It is the tool you used.
I can tell you exactly why this is happening because I've been here before, and you can sum it up in one word - deflection. What is happening is that radial cutting forces are very large with tiny depths of cut like you were attempting. I don't know what the nose radius of your insert is but I will bet that a 0.002" depth of cut is less than 1/3 of your nose radius. If this is so then your tool is mostly skating over the surface of the work and will not provide a consistent cut, nor will it cut to the depth you dial in.
I went over this in more detail in my Boring Primer so I won't go into detail here but I encourage you to read it and try to understand how these cutting forces work. They are real forces and unless you understand them it will be hard for you to sort things out. Everything I said in the Primer applies to inserted carbide turning tools, too.
Okay, from a practical standpoint you need to hit a specific size, 0.875" OD and you're starting at 1.00" OD. Let's assume your nose radius is 0.015". Ideally, you want to take a minimum roughing depth of cut of 0.015 + around 0.005 - 0.010", so around 0.025" deep will work. Dial in that cut and measure the OD, then take another 0.025" and measure it. The SECOND cut should give you an OD 0.050" smaller than the first OD. Subsequent cuts at the same DOC should give you a consistent reduction in diameter. If this is so then the insert is responding as it should.
Next, you need to determine how small a cut that insert will allow. Most inserts will cut consistently (not accurately, consistently) at about 1/2 the nose radius, or about 0.008" DOC, without radial forces being too extreme. Go smaller than this and the insert tends to skate and not cut; go bigger and radial forces also rise until you get to about 0.005 - 0.010" beyond the nose radius. About 1/2NR is about the smallest you can reliably go and have the insert cut consistently. You will find that 1/2NR cuts will not cut what you dial in, though. Say you dial in 0.008"; you will not get a 0.016" reduction in diameter. It may be 0.015 or 0.018" but it will be consistently that number if you dial in that 0.008" DOC. Once you know what the minimum DOC your insert requires, write it down. Now you know that you simply need to rough the work until it is 0.015" or 0.018" away from final size and dial in your 0.008" DOC to come in on final size.
I hope this is clear. If not, say so and we'll break it down further. Practice until you know how to use that insert, then write down what DOC works for both roughing and finishing. Every insert is different so do this for every insert you use. Eventually, you will learn how each of your tools likes to cut and you'll be fine. Just remember that tip geometry for turning tools is important and the more you know about how that geometry impacts on cutting forces, the easier it will be for you to effectively use those tools.
Remember, too, that a properly ground HSS tool will usually cut what you dial in and is much easier to work with. One day, when you have the time, give them a shot.
