Technical Guidance: Character Design Specifications
8 min
- 1. Character Size Parameters:
- 2. Character-to-Solder-Pad Distance:
- 3. Treatment of Characters on Copper Surface:
- 4. Treatment of Characters on Substrate:
- 5. Special Character Design Instructions:
- Additional Design Recommendations
- FAQ: PCB Character Design Specifications
- Conclusion
To facilitate component assembly, future maintenance, and traceability of PCB manufacturing information (such as manufacturer, production date, batch number, etc.), various character markings are typically silk-screened onto the PCB. These include component designators, polarity marks, test point labels, company logos, and production traceability information.
Traditional PCB character silk-screening uses the screen printing process, hence the term “silk-screen characters.” High-definition characters and high-precision characters options are also available. Customers can select them according to requirements when placing an order. These processes differ in resolution, clarity, and applicable scenarios. It is recommended to choose reasonably based on board density and the importance of the characters.
1. Character Size Parameters:
The stroke width and height of characters should maintain an appropriate proportion, with sufficient gaps between characters to ensure clarity. It is recommended to use solid linear strokes rather than hollow outlined fonts, as this results in more uniform ink distribution and higher clarity in the final product.
❶ Standard Font: Character stroke width ≥ 0.15 mm, character height ≥ 1 mm (high-precision characters supports a minimum character stroke width of 0.1 mm and a minimum character height of 0.8 mm).
❷ High-Precision Characters: Support minimum stroke width of 0.1 mm and minimum character height of 0.8 mm.
❸ Hollow Font: Character stroke width ≥ 0.2 mm, character height ≥ 1.5 mm.
Recommended Production Standards vs Absolute Minimum Limits (based on current manufacturing capabilities):
| Parameter | Absolute Minimum Limit | Recommended Production Standard | Remarks |
|---|---|---|---|
| Character Height (H) | 0.8 mm (32 mil) | ≥ 1.0 mm (40 mil) | Recommended for good readability |
| Line Width (W) | 0.15 mm (6 mil) | ≥ 0.2 mm (8 mil) | More stable with standard process |
| Width:Height Ratio | Approx. 1:5 ~ 1:6 | 1:6 | Avoids character distortion |
| Hollow Font Internal Gap | > 0.2 mm | > 0.25 mm | Prevents insufficient ink fill |
| Character Gap | > 0.15 mm | ≥ 0.2 mm | Improves overall visual clarity |
Note
If the design dimensions fall below the above parameters, the engineering team will not arbitrarily adjust the character height in the files, but may appropriately widen the strokes to meet process capabilities. The manufacturer assumes no responsibility for blurry or unclear characters caused by designs exceeding production limits. Lines that are too thin are usually automatically widened to the minimum acceptable value.
2. Character-to-Solder-Pad Distance:
Characters should not overlap solder pads. Characters should be at least 0.15mm away from solder pads, with a gap of more than 0.15mm between character lines.
Note
If the clearance is insufficient, characters covering pads or positioned too closely will be automatically removed during engineering review to prevent solder bridging, shorts, or poor soldering during SMT assembly. It is recommended to set the minimum clearance between pads and silkscreen to ≥ 0.25 mm for optimal yield and assembly reliability.
3. Treatment of Characters on Copper Surface:
Characters located on exposed copper areas (including tinned or gold-plated regions) will be directly removed, as silkscreen ink in these areas can cause soldering issues or affect electrical contact.
4. Treatment of Characters on Substrate:
Characters on substrates with no copper (whether with or without ink), will be retained entirely. These areas have minimal impact on character adhesion and clarity.
5. Special Character Design Instructions:
To avoid interfering with component assembly, characters overlapping pads or copper areas should follow the default rule of prioritizing exposed copper/pad areas (i.e., removing characters from copper). If there are specific functional requirements, they must be clearly noted in the order remarks, and the final confirmed production files shall prevail.
Example: Please specify in remarks “allow characters XXX to overlap with the solder pad.”
Once again, without specific instructions when placing the order, characters overlapping with solder pads or copper areas within 0.15mm will be removed.
Attention to these details is crucial, so make sure to communicate these requirements to your PCB design team. Don't simply provide files without conveying this information. The image below is an example of the default process where CAM engineering directly removes the corresponding characters in the window area.
Image shows the comparison between the original draft and the production draft.
Additional Design Recommendations
- Prioritize vector fonts or standard silkscreen fonts built into PCB design software; avoid overly complex decorative fonts.
- For high-density boards, perform DFM checks early in conjunction with layout, and use Gerber viewers to verify clearances between silkscreen, pads, traces, and solder mask.
- Silkscreen ink is a non-conductive special epoxy resin and will not affect the electrical performance of the circuit. Common colors are white (default) and black (optional). Ensure sufficient contrast with the solder mask color for readability.
- Modern manufacturing processes can significantly improve character precision, but strict adherence to the above size and spacing rules is still required for optimal results.
- It is recommended to incorporate silkscreen layer Design Rule Checks (DRC) during the schematic and PCB design phase and reserve sufficient space for important markings.
FAQ: PCB Character Design Specifications
Q: What are the minimum character size requirements for standard silkscreen?
For standard fonts, the character stroke width must be at least 0.15 mm and the character height at least 1.0 mm. High-precision characters support smaller sizes: minimum 0.1 mm stroke width and 0.8 mm height. Hollow fonts require larger sizes — minimum 0.2 mm stroke width and 1.5 mm height. It is strongly recommended to use the higher “Recommended Production Standards” values for best readability and yield.
Q: Why do characters sometimes disappear after production, and how can I prevent this?
Characters that overlap solder pads or exposed copper areas, or are closer than 0.15 mm, are automatically removed during engineering review to prevent soldering defects. To prevent unwanted removal, maintain at least 0.15 mm clearance (preferably ≥ 0.25 mm) and add clear remarks in your order if you need specific characters to overlap pads.
Q: What is the difference between the Absolute Minimum Limits and Recommended Production Standards in the table?
Absolute Minimum Limits are the smallest sizes the factory can technically produce. Recommended Production Standards are safer values that provide better readability, higher yield, and fewer issues. Using the recommended values significantly reduces the risk of blurry or incomplete characters.
Q: Can I place characters directly on exposed copper or solder pads?
By default, characters on exposed copper (including tinned or gold-plated areas) will be removed. Characters on bare substrate areas (no copper) are fully retained. If you have special requirements to keep characters on pads, you must explicitly note this in the order remarks (e.g., “Allow characters R101, C202 to slightly overlap corresponding pads”) and confirm the production preview.
Q: What design practices are recommended to achieve the best silkscreen quality?
Use solid linear strokes instead of outlined fonts, maintain proper gaps between characters, choose high-contrast colors (white is default), and perform DFM checks using Gerber viewers. Avoid complex decorative fonts and reserve sufficient space for important markings. Incorporating silkscreen DRC rules early in the design phase is highly recommended.
Q: What should I do if I have special character requirements that may conflict with the standard rules?
Clearly specify your requirements in the order remarks and carefully review the production files (gerber preview) before confirming the order. Examples include allowing overlap with specific pads or retaining certain test point markings. Without explicit instructions, the factory will follow the standard removal rules to ensure manufacturability and assembly quality.
Conclusion
Adhering to the PCB Character Design Specifications is fundamental to achieving high-quality production, smooth assembly, and reliable long-term maintenance of printed circuit boards. By properly controlling character sizes, maintaining adequate clearances, correctly handling interactions with solder pads and copper areas, and making full use of order remarks and production file confirmation, designers can significantly reduce engineering changes, improve first-pass yield, and provide clear and durable identification throughout the product lifecycle.
It is highly recommended that all PCB designers incorporate silkscreen character design rules into their DFM review process from the layout stage. Using the Recommended Production Standards rather than merely meeting the Absolute Minimum Limits will deliver superior visual quality and manufacturing yield. Ultimately, excellent design practices not only reduce production costs but also enhance the professional image and user experience of the final product.
Keep Learning
Smart PCB Array Design for Higher Yield and Lower Production Costs
Key Takeaways Smart PCB array design is a critical strategy for achieving higher manufacturing yield and significantly lower production costs. By optimizing panelization with proper board spacing, V-scoring, tab routing, and mouse bites, designers can dramatically improve material utilization by 20-30%, enhance production throughput, and simplify handling and depaneling while minimizing mechanical stress and defects. Effective use of fiducials and careful component clearance further ensures high-quali......
Why Accurate NPTH Design Matters for Reliable PCB Manufacturing
Key Takeaways NPTH are mechanical holes (no copper plating) used for mounting, alignment, and tooling. Poor NPTH design often causes PCB cracks during assembly or screw tightening. Follow key rules: ±0.08 mm tolerance, ≥0.5 mm diameter, 0.2–0.3 mm copper clearance. Keep adequate material around edge holes and clearly mark NPTH in fabrication files. Proper NPTH design + DFM checks ensure reliability from prototype to mass production. Ever get a slight crack in a finished PCB when putting it into an enc......
Gerber of PCB: A Comprehensive Guide
Introduction: Printed Circuit Boards (PCBs) are the backbone of modern electronics, serving as the platform on which components are mounted and interconnected. One of the most critical elements in PCB design and manufacturing is the Gerber file. Gerber files are the standard format used to communicate the design of a PCB to the manufacturer. These files provide precise information about the PCB layers, component placement, copper traces, and more. Understanding Gerber files is essential for anyone inv......
Electronic Board Manufacturing: Efficient Strategy and Quality Control Processes
Electronic board manufacturing is a critical process in the electronics industry, and the quality of the boards produced can significantly impact the performance and reliability of the final product. Therefore, it is essential to follow efficient strategies and quality control processes throughout the manufacturing process to ensure the highest quality of the boards. In this article, we will explore the various steps involved in electronic board manufacturing, including materials selection, design and......
Best Practices for Successful Electronic Manufacturing
Key Takeaways Mastering best practices in electronic manufacturing — from optimized PCB design and DFM to rigorous testing, verification, and high-quality production — is essential for achieving reliable, cost-effective, and timely electronic products. By following proven methodologies, leveraging advanced tools like EasyEDA, and partnering with a trusted manufacturer such as JLCPCB, designers and engineers can significantly reduce errors, accelerate time-to-market, and ensure superior performance acr......
How Laser-Made PCBs Are Used in Rapid Prototyping
Key Takeaways Speed & Precision: Digital lasers enable 24-hour quick-turn HDI and FPC prototyping without mechanical tooling. LDI Patterning: Replaces physical photo-films to deliver precise circuit traces down to 2/2 mil. HDI Microvias: UV/CO2 lasers drill 0.075–0.15 mm blind vias (1:1 aspect ratio) for 1+N+1 to 3+N+3 stackups. Laser Profiling & Stencils: Achieves ±0.05 mm FPC cut accuracy and ±0.003 mm LPKF stencil aperture precision. Laser DFM: Maintain ≥ 0.30 mm copper clearance on FPCs and ≥ 0.07......