The current version 5 footprints use fillet sizes as defined in IPC-7351B. We use the default placement and PCB manufacturing tolerances as listed in the same standard.
We use the component size definitions found in an old ipc document. (at least for the most common sizes.)
I checked them against a few components on farnell. Over all parts i checked (i think i checked 10 to 20 parts for 5 to 10 manufacturers depending on size) i got the same variation of component sizes as given in that old standard.
If you limit yourself to only one exact part you will most likely be able to get smaller tolerance ranges resulting in smaller pads and most likely larger pad to pad clearances. (So if you really need the space you will most likely make a unique footprint for the parts you plan on using.)
This is especially noticeable for 0805 as this has a smaller clearance than 0603. After 5 arbitrarily selected parts i was already quite close to the tolerance ranges used by us. Checking 10 further random parts even increased it on the toe side. (I found quite a few exactly matching the heel side) Nearly every single part could have had either a reduction on the heel or toe side. (Agrees with my suspicion that specialized footprints can help you out if you are pressed with space.)
The old kicad 4 footprints pads where too small for most parts i checked. (I could not find a single component that would have fit the old 0603 or 0805 footprints if you respect the tolerance ranges given in the datasheets. Even if you ignore manufacturing tolerances.)