Smitty, I think you accidentally unchecked diameter programming in your NC Post Output settings. However, it would appear that your nc code looks like it was done with diameter programming on.
So, where in your nc program do you tell your controller that you are using G90 absolute mode? If you say the lengths are right, it must be running in absolute, but the appropriate Gcode for the mode (absolute or incremental) should always be near the start of your program.
You also have not established a G92 work home which means we have no way of knowing where you are starting from. If you touch up to the end of the part, right on center, this is X0Z0 as you are already doing. Back off to X.5 Z.1 and then edit in this line near the beginning of your program:
G92 Z.1 X.5
S(spindle speed command, if you have a variable speed spindle drive)
M3 (spindle on, forward command)
All the rest of your nc program should then run in relation to this "virtual G92 home".
Second, you should not keep reconfiguring the default config, because it is a default. Configure it as you like, then click save as, and give it a meaningful name.
Apart from that, I looked at the last line of your nc code, which would be the finish cut, and it appears like the X diameter values are correct: .170" + (.02"tool radius *2) = .210".
So, I would think it is something you are doing in setting up your tools or zeroing. Do you know how your controller calls up tool offset commands? We do not rely on zeroing our tools all the time, in order to make slight (or major, for that matter) corrections to the all-over cutting diameters. This is what the tool offset tables are for. Chances are when the command T0909 is read, your controller software is checking for a value in an offset table somewhere, and adjusting your tool position. If you have a zero (both in X and Z) in that table right now, no adjustment will be made to the tool, but if there is a value in there, then you need to know if it is being applied or not.