Footprint filters are used to help match appropriate footprints to a given symbol. This is important even for atomic symbols (symbols with only one matching footprint), as there still may be multiple compatible footprints with different variants or options (e.g.
Footprint filters use wildcard pattern matching, and allow the following wildcards:
*- Match zero or many characters
?- Match zero or one characters
:- Include the library name in the search (can only be used once)
Filters should end with a
*wildcard to allow matching of modified footprint suffixes
Filters should match the dimensional information (where required) to be as specific as necessary:
Filters should not contain the pin count if the pin-count in the symbol matches the pin count in the footprint. In those cases the footprint is matched by KiCad’s pin count filter. If not all pins are present in the symbol (e.g. NC-pins) the pin-count has to be part of the footprint filter (see requirements for NC pins). Then e.g.
SOT?23?5might be used instead of simply
By default, the footprint search does not include the name of the footprint library. To force the library name to be included, add the
:(colon) character to the filter. Text appearing before the
:will match the library name. Text appearing after the
:will match the footprint name.
Conn*:*Pitch?1.25mm*will match any footprint with '1.25mm' pitch, only in libraries that begin with the text 'Conn'
Footprint filters can be set in the Footprint Filter tab in the Symbol Properties window.