8.1 Silkscreen Design Considerations
 General Requirements
- The width of the silkscreen line should be greater than 5mil. Designers must ensure that the silkscreen
character’s height is large enough to be read by the naked eye (recommended h 50mil).
- Recommended spacing between silkscreen objects is h 8mil.
- The silkscreen must not overlap with solder pads or Fiducials. The minimum spacing between both is
- White should be the default silkscreen ink color. Special requirements should be specified in the
PCB’s drill hole layer
- For high-density PCB design, the contents of the silkscreen can be chosen according to specific
requirements. Any silkscreen text should follow the convention of left to right, top to bottom.
8.2 Silkscreen Contents
 The contents of the silkscreen can include PCB name, version, component serial number, polarity and
direction label, barcode box, mounting hole location code, component footprint, board direction of travel
indicator, anti-static label, heatsink label, etc.
 PCB board name and version:
Board name and version should be placed on the top side of the PCB. The font should be chosen such that it can be easily read. The top and bottom sides of the PCB should also be marked with ‘T’ and ‘B’ (or similar).
 Barcode (optional):
The barcode should be orientated horizontally or vertically on the PCB, refrain from orientating the
barcode at any other angle.
The recommended position of the bar code on a typical board is shown in the figure below; the
position on non-standard boards can use this for reference.
Figure 52: Barcode recommended positioning.
 Component silk screen:
- Component labels, mounting holes and positioning holes must be indicated on the silkscreen clearly
and should be located by the relevant features.
- Silkscreen characters, polarity and direction labels must not be covered by components.
- For components installed horizontally (such as lying electrolytic capacitors), the silkscreen should
include the component outline on the corresponding position.
 Mounting holes, pilot hole:
It is recommended that the locations of the mounting holes and pilot holes on the PCB be labelled as “M
**” and “P **,” respectively.
 Direction of travel:
For the PCBs that are required to be fed into equipment, such as wave soldering equipment, in a specific
orientation, the direction of travel should be indicated on the board. This is also suitable for PCBs with solder
thieves and teardrop solder pads.
For power PCBs that require a heatsink, if the projected area of the heatsink is larger than the component,
the actual size must be indicated on the silkscreen.
 Anti-Static Label:
The anti-static silk screen should preferentially be placed on the top side of the PCB.
1. Brief Introduction
2. Seeed Fusion PCB Specification
3. Panelization and Bridge Design
4. Component Layout Considerations
5. PCB Hole design
6. Solder Mask Design
7. Copper Trace Design
9. PCB Lamination Structure
10. PCB Dimensions Specification
11. Fiducial Mark Design
12. Surface Treatment
13. Files for Manufacture Requirements