F2.1 General footprint naming conventions

Each footprint is a .kicad_mod file (stored within a .pretty directory). The naming convention for a given footprint depends largely on the type of footprint, however a general guide is presented below:

Specific package type is written first, e.g.
- QFN - Quad Flat No-Lead package
- C - Capacitor
Package name and number of pins are separated by a hyphen
- TO-90
- QFN-48
- DIP-20
Packages with special pads add an identifier to the pin count field separated by a hyphen
- The field includes the count of uniquely numbered pads of this type.
  - For exposed pads (large copper pad below the part) [count]EP
  - For shield pads [count]SH (Unless such a pin is already expected for the part. An example would be a HDMI connector.)
  - For pads connecting pure mechanical mounting leads [count]MP
- Examples from the library.
  - DFN-6-1EP_2x2mm_P0.5mm_EP0.61x1.42mm
  - Samtec_LSHM-110-xx.x-x-DV-S_2x10-1SH_P0.50mm_Vertical
  - Molex_PicoBlade_53261-0271_1x02-1MP_P1.25mm_Horizontal
Unique fields (parameters) in the footprint name are separated by _ character.
Package dimensions are specified as length x width (and optionally height)
- 3.5x3.5x0.2mm
- 1x1in
- If necessary for clarity, footprint body dimensions may be prefixed with a leading B
Pin layout
- 1x10
- 2x15
Pitch is specified with a leading P:
- P1.27mm - 1.27mm pitch
- P5.0mm - 5.0mm pitch
Modifiers to standard footprint values
- Drill1.25mm
- Pad2.4x5.2mm
Orientation e.g. Horizontal, Vertical
Any modification to the original footprint, indicated by appending the reason
- _HandSoldering
- _ThermalVias
- _CircularHoles

Not all of the fields defined above are strictly required for a particular footprint. Additional fields may also be added as needed.

Edit on GitLab