What is the pin pitch and width? If typical 0.5mm pitch, 0.25mm width, it's acceptable to "shave" pads down slightly to get better fit overall. For example, 0.23mm pad width allows 0.27mm gap, or for example 0.11mm mask web width and 2 x 0.08mm mask expansion.
Whether that's within the exact tolerances of any given fab, or they'll build it with the dimensions as given (risks lower yield), or they override that and build it to their own tolerances -- no idea. Ask your fab if in doubt.
Removing mask between pads isn't a big deal; the chance of solder bridging is lower with mask, but it's still pretty low without, when using proper pad dimensions and pasting. (And pasting doesn't matter a whole lot anyway as the rosin phase melts, allowing it to spread out during reflow; it does still help of course, just to say it's not as specific as you might hope.)
Ultimately, pad dimensions, shape, and positioning are a matter resolved by production. If you aren't doing thousands of units at a time, it doesn't really matter, and sticking to IPC or manufacturer recommended footprints is fine.
The one thing I would recommend at the EDA tool level is setting rounded pad corners, so that the soldermask is also rounded. For typical combinations of trace spacing and soldermask expansion, the trace can overlap the mask expansion region, exposing part of the trace (or if not all the time, then under worst-case alignment). Rounded expansion guarantees it's fine.