PCB Pads vs Components Footprints in PCB design
Land patterns are almost always larger than the size of the actual component pin, although in the case of 0.5mm pitch parts this is only true for the length of the pin in many cases.

Here is the component information for a 12 lead DFN from Linear Technology:



The pads themselves are 0.25mm wide and 0.4mm in length. Here is the recommended land pattern:



As you can see, the land pattern is 0.3mm longer than the actual component pad; this is so a proper solder fillet can form (and be inspected!).

On not quite so fine pitch parts, the land pattern is usually larger in both dimensions. Here is a typical 16 TSSOP package:



The land pattern is clearly larger in both X and Y dimensions than the actual pin. The actual pin width is nominally about 0.25mm and the recommended solder pad is 0.45mm wide; the length of the pin at the land pattern attach area is nominally between 0.5mm and 0.75mm, but the recommended pad length is 1.05mm.

There is a standard (IPC-7351) which is the basis of many footprint wizards. Not every footprint can be automatically generated (there are some unusual parts out there) but this covers the vast majority of parts.

There are a number of reasons that the land pattern is larger; one is that for these types of packages, component registration (the location of the part on the PCB) from the pick and place is never perfect so the actual part will not be truly centered on the pads.

Another reason is to ensure that the solder can surround the component pad.

You can read about the perfect 0402 footprint as well.