Why would metal from a pad be *underneath* the solder mask in a footprint specification?
There are two ways of defining the "active" area of a surface mount footprint: SMD and NSMD - that is Solder Mask Defined and Non-Solder Mask Defined.

It is unusual to see both in one footprint, but certainly not impossible. 

SMD pads effectively have a raised lip around the edge of the pad. This at times can have an advantage over NSMD pads for a couple of reasons:


It can create an insulating seal around the pads reducing the possibility of solder bridges forming during re-flow
It increases the mechanical strength of the pad since the mask helps hold it down
It limits the surface tension pull-down of the component on large pads


It is only the larger pads that are SMD in that footprint. Those pads will typically have more solder paste on them, which means the possibility of that paste oozing out sideways and forming bridges. The solder mask basically forms a barrier around the pad reducing the possibility of those bridges forming and making the solder paste remain within the area of the pad during reflow. Also when the solder paste melts the surface tension will suck the component down towards the pads. The larger the pad the more force it exerts. With large pads it is possible for them to exert too much pressure thus pushing the solder paste out of the normal pads and making bad connections. By using SMD on those pads you limit how far down the chip can be pulled by those pads. The mask forms a cushion on which the chip sits so the other pins can then reflow properly.