Answer to your questions:
I work with version 043.066, where the M1076.m1s file is in the root folder (not in /macros !! )
There is in the menu under Options/Parameter the X-Axis mode switchable between Radius and Diameter mode. (Documentated in the help file)
As for the G-Code header, take what you normally prefer for your work. For example, on my lathe with my tooltable the M10x0,75 program will look like (in radius mode):
g18 g21 g40 g90 g94 g80
t0404
s700
f85
m3
G77 r5 x4.953 k0.0 z-20.0
m5
s120
m0
f40
m3
G76 p0.75 r4.953 x4.396 h0.2273 i29.5 k-1.631 z-20.0 l360 q0
m5
m30
This will first bring the diameter down from 10 to 9.9 mm with a normal cutter, then request a tool change, and then cut the M10x0,75 with 6 passes (the first is 0.22 mm deep, which is okay even for a small HSS 60° cutter with a sharp edge. With some other tool you can probably cut it in only two passes ...). But the surrounding lines of code are very different for everyone, depending on the setup of the machine. The purpose of my software is in finding the initial dia (9.9 mm in this case), the depth based on the tolerance (0.2273 mm in radius), and to check the number of passes needed, which gives the depth of the first cut.
In Diameter mode, the two lines will change properly to G77 rXX x9.906 ... and G76 p0.75 r9.906 x8.792 h0.4546 ... that looks okay.
I found a bug, too - the steps for five passes aren't displayed properly, but that doesn't change the output.