It seems the opposing factors that influence this decision are routing
traces between pads (favoring LMC) and manufacturability or fabricator
capabilities (favoring MMC).
Is this assumption correct? If not, what are the reasons to choose
MMC, LMC, or specify a percentage reduction for BGA landing pads?
Yes, that assumption is correct. It is up to the designer, but there are tradeoffs associated with SMD vs NSMD.
With SMD the silkscreen surrounds the pad and this makes it harder for the BGA to pull the pad up if the package warps (thermal expansion). Having the pad more secure also prevents cracking (if teardrops are not used).
NSMD has the silkscreen and soldermask removed from the pad, the solder can extend all the way down around the pad, which allows for a smaller pad. The problem with this is there is less material holding the pad to the PCB and it can pull up easier. The good part is less copper means more space between pads. NSMD can also create problems with high volume runs.
Opening up space allows for easier routing and less restrictive PCB requirements which can have cost ramifications (like 3mil traces vs 4mil in some cases).
It probably wouldn't be worth worrying about in low volume production runs. In high volume production runs it could affect yields so SMD would be better. Some manufacturers also have reccomendations on what process to use and the pad size. At the end of the day after using altiums wizard the most important numbers I care about are the pad size and the soldermask size. I haven't used the BGA wizard myself because I don't do the footprint creation, but I'd be worried about the pad diameter and the design rules concerning the silkscreen. In the past I have had to edit the footprints and change the pad diameters after part creation.
I think micron has the best explanation in this table and document.
PCB design guidelines depend on many variables, including ball pitch,
ball diameter, and PCB metal land pad type. Solder mask-defined (SMD)
pads have a solder mask that partially overlaps each metal land pad
and defines the opening diameter. Non-solder mask-defined (NSMD) pads
have a solder mask clearance area away from the metal land pads so
that each metal land pad diameter is defined by the edges of the
metal. Figure 4 illustrates the difference between SMD and NSMD pads.
With SMD pads, the solder flow is restricted to the top of the
metallization, which prevents the solder from wetting the sides/wall
of the pad (contrary to the NSMD case). Some of the advantages and
disadvantages of the SMD and NSMD are listed below. Application should
determine selection of pad type.
I usually size bga off of something that has already been build like an evaluation kit pcb file and also look at the fanout to see what clearances they used because I know it's manufacturable. That isn't always possible