Library Conventions | KiCad EDA

Version 3.0.43

Library maintainer rules & guidelines

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:

  1. Specific package type is written first, e.g.

    • QFN - Quad Flat No-Lead package

    • C - Capacitor

  2. Package name and number of pins are separated by a hyphen

    • TO-90

    • QFN-48

    • DIP-20

  3. 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

  4. Unique fields (parameters) in the footprint name are separated by _ character.

  5. 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

  6. Pin layout

    • 1x10

    • 2x15

  7. Pitch is specified with a leading P:

    • P1.27mm - 1.27mm pitch

    • P5.0mm - 5.0mm pitch

  8. Modifiers to standard footprint values

    • Drill1.25mm

    • Pad2.4x5.2mm

  9. Orientation e.g. Horizontal, Vertical

  10. 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.