KLC 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 must not be placed over pads or areas of exposed copper

    • Clearance between silkscreen and exposed copper elements must be at least 0.2mm or more than the pad mask expansion (whichever is greater).

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

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

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

    • Silkscreen line width should nominally be 0.12mm

    • 0.1mm is allowed for high density designs

    • 0.15mm is allowed for low density designs

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

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

Back