PCB Pads vs Components Footprints in PCB design

Question

I want to understand the process of PCB design using a software like Altium. I have come across two approaches as follows:

Approach 1: While making the component parts library we make the footprints of the component slightly bigger in size from that given in the component datasheet. Later we use these footprints as the PCB pads in the PCB design. So in this approach if a specific part is used multiple times on the PCB then for each instance we will have the same pad on the PCB as we would be using the footprint of the part as its pad on the PCB.

Approach 2: While making the component parts library we make the footprints of the components of exactly the same size as given in its datasheet. We also make a library of pads of various shapes and sizes. Later when a part is used from the library in the PCB then at that point we get appropriate pads from the pads library for the pins of the component. So for each instance of a specific part that is put onto the PCB we can use different pads as needed for that specific position.

I want to understand which of the above two approaches are correct, especially for the case of SMD components and PCB design.

Answer 1

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.