Library Conventions | KiCad EDA

Version 3.0.43

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}:

    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. Polarity marking / Pin-1 designator must be drawn on the F.SilkS layer

  7. When components are expected to protrude past the board edge (e.g. connectors), silkscreen should not be placed such that a reasonably-placed component has silkscreen outside the board

    1. Clearance between silkscreen and board edges should be at least 0.5mm

Polarity marking / Pin-1 designator

  1. The prefered style for SMD packages is a filled chevron

    1. It should positioned inside the courtyard to prevent silkscreen overlap

    2. It can be rotated by 45° for a better fit

  2. Examples other established and acceptable styles

    1. for SMD devices

      1. shape for SMD diodes

      2. For small packages (0201 diodes, …​) a 0.25mm dot should be used.

    2. for THT and SMD packages

      1. corner bracket or extra line for connectors

      2. + sign for SMD capacitors

    3. Follow established styles that already exist in the target library

  3. If the device has a marking that is not on Pin-1 (popular on digital LEDs), the marking needs special attention

    1. The digit 1 is put on the silkscreen marker next to the pin numbered 1

    2. The silkscreen polarity marking is placed according to the physical marking on the device

  4. The marking must be visible after board assembly for inspection and debug purposes

    1. It also should be visible after connector mating


Examples of silk for non-polarized components

Examples of silkscreen for polarized components

Example of a connector with silkscreen that is "pulled back" from possible board edges: