The multi-thread insert has a nose radius small enough for the finest thread it is suitable for; no choice...it has to be that small. This means of course that it is too small, i.e. the cutting depth will be deeper than a normal full profile insert for any thread coarser than the finest thread.
I have done a lot of custom 16tpi threads with this type of insert and I 'calibrated' the depth of cut.
The diametral difference between the OD and ID needed to be 0.065": in other words if I needed a 2.000" OD thread I would bore 1.935" for the ID.
The cut depth in both cases was 0.085" again on the diameter. On the OD the final cutting pass was around 1.815" and similarly on the ID the final pass was 2.020"
These figures do need a little playing around by a few thou depending on how loose you want the thread but I was able to thread mating pieces from scratch and have them fit very well.
Theoretically for 32 tpi you should be able to use 0.0325" and 0.0425".
I used G92 because I find it easier; just set the Z length, tpi and first cut in the G92 line then follow with multiple X values. I normally end with two or three passes at the same X for cleanup. The reason I like G92 is that it is dead simple to add smaller (or larger depending on OD or ID) X values to skim a little more off; normally I go three or five thou shallow at first so I don't overshoot. Never did figure out how to have the tool put metal back on.
EDIT:
My method to estimate the thread depth for any pitch is to just look a a tap drill chart; for instance 3/8"-16 uses 5/16" for a 75% thread so 0.065" diameter measure for the thread depth is a good start. I know someone is going to suggest going to the machinist's bible but my way works for me.
An open mind is a virtue...so long as all the common sense has not leaked out.