2. Choosing footprint type and metadata

2.1. Parametric vs. static file

For pcb-rnd there are two types of footprints: static file and parametric.

A static file footprint is a single data file that fully specifies the geometry of a footprint with all dimensions hardwired. This is most useful in two situations:

• generic footprint for hand soldering; for example the stock sot23 footprint in the footprint library shipped with pcb-rnd
• a special footprint designed for a single part of a specific vendor; for example unique footprints of thick modules, where the same footprint will not ever be used for any other part

A parametric footprint is a script or program that is executed parameters with parameters (on its "argv") and generates a footprint that is then printed to its stdout. The advantage of parametric footprint is that it can handle all presently known and future members of a whole footprint family. A parametric footprint can be used directly from the pcb-rnd GUI (library window), from the "footprint attribute" of a symbol in a schematics or can be executed manually from the shell with its output redirected to a static footprint file.

For high end footprints parametrics can be used to compute optimal pad geometry considering tolerances. This is especially important since different parts coming seemingly in the same footprint may have widely different dimensions, e.g. Texas Instruments has at least two SOT-23 variants whose footprints are incompatible ( DBV0003A and DBZ0003A ). One way to solve this problem is manually draw a few dozen variants of SOT-23 footprints using footprint recommendations from different vendors/parts. Another way is implementing a parametric SOT-23 footprint which gets main dimensions and tolerances as input and generates the optimal footprint e.g. using the RMS formulas from IPC-7351.

Bedrock prefers the latter and goes for static file footprints only for one-of-its-kind special parts.