Library Conventions | KiCad EDA

Version 3.0.34

Library maintainer rules & guidelines

F5.1 Silkscreen layer requirements

The silkscreen is printed to the external surface of a PCB to aid in component identification and orientation. Typically this layer contains the component RefDes to locate components on the board after assembly.

KiCad refers to the silkscreen layers as:

  • F.SilkS - Front silkscreen layer

  • B.SilkS - Back silkscreen layer

The following elements must be provided on the silkscreen.

  1. Reference Designator must be drawn on F.SilkS layer

    1. Text size = 1.00mm

    2. Text thickness = 0.15mm

  2. Silkscreen line width is between {0.10mm and 0.15mm} as per IPC-7351C:

    1. Silkscreen line width should nominally be 0.12mm

    2. 0.1mm is allowed for high density designs

    3. 0.15mm is allowed for low density designs

  3. Silkscreen must not be placed over pads or areas of exposed copper

    1. Clearance between silkscreen and exposed copper elements is recommended to be 0.2mm.

    2. Clearance must be at least the silkscreen line width or pad mask expansion, whichever is greater.

  4. For SMD footprints, silkscreen must be fully visible after boards assembly (no silkscreen allowed under component)

  5. For THT components, additional silkscreen may be placed under component to aid in assembly process

  6. Pin-1 designator is provided on the F.SilkS layer

  7. Pin-1 designator must be visible after board assembly

Examples of silk for non polarized components

silk_non_polarized

Examples of silk for polarized components

silk_polarized

Edit on GitLab