PCB Silkscreen Design Tips: Text Size and Component Labels

PCB Silkscreen Design Tips: Text Size and Component Labels

The silkscreen layer — also called the legend or nomenclature layer — is the printed text and symbols on a PCB that help assemblers, technicians, and engineers identify components, polarity markers, test points, and version information. A well-designed silkscreen dramatically reduces assembly errors and makes debugging far easier. A poor silkscreen leads to expensive rework and confused technicians.

This guide covers silkscreen design best practices, minimum text sizes, component reference designation placement, and common mistakes to avoid when designing PCBs in KiCad or EasyEDA.

What Is PCB Silkscreen?

Silkscreen is ink printed onto the solder mask surface of a PCB. Traditional PCB manufacturing uses a silk-screening process (hence the name), though modern fabs use inkjet printing or photolithography for finer resolution. The silkscreen layer appears in your CAD tool as F.SilkS (front silkscreen) and B.SilkS (back silkscreen) in KiCad, or TopSilkLayer/BottomSilkLayer in EasyEDA.

What goes on the silkscreen:

• Component reference designators (R1, C5, U3, etc.)
• Component values (optional, increasingly common with SMD passives)
• Polarity markers (+ for capacitors, K/A for diodes, pin 1 dots for ICs)
• Connector pinouts and labels
• Test point labels (TP1, TP_VCC, etc.)
• Board name, revision, and date
• Manufacturer part numbers or barcodes
• Warning symbols (high voltage, ESD sensitive)
• Assembly notes and jumper settings

Minimum Text Size Guidelines

Silkscreen resolution is limited by the fabrication process. Most standard PCB fabs (including JLCPCB and PCBWay) have minimum silkscreen feature sizes. Going below these minimums results in text that is blurry, illegible, or simply not printed.

Rule of thumb: Never go below 1mm text height for component references. At 0.8mm, text is legible under good lighting but becomes difficult on assembled boards with components partially obscuring the labels. At 1mm height with 0.2mm stroke width, text remains readable even on densely populated boards.

Text Size vs. Component Pitch

• 0402 SMD passives: Use 0.5mm text with 0.1mm stroke if reference must be near the pad. Place reference away from the component if possible.
• 0603, 0805 passives: Use 0.8-1.0mm text, 0.15-0.2mm stroke
• SOT-23, SOT-223: Use 0.8mm text, keep reference outside the courtyard
• QFP, QFN, BGA: Use 1.0mm text for reference, place away from pads. Add pin 1 marker prominently.
• Through-hole components: Use 1.0-1.5mm text. More space available.

Component Reference Placement Rules

The Golden Rule: Outside the Courtyard

Always place component reference designators outside the component courtyard (the bounding box defining the keepout zone). References that overlap pads or courtyard areas cause DRC violations and may be clipped by the fab (some fabs auto-remove silkscreen over pads to prevent solder bridging issues).

Placement Best Practices

• Consistent orientation: Choose either horizontal-only text or a two-orientation approach (horizontal + rotated 90 degrees). Avoid arbitrary rotations that require the reader to physically rotate the board.
• Near but not on the component: Place references within 3-5mm of the component they label. On dense boards, a clearly numbered silkscreen with a separate component legend sheet is acceptable.
• Avoid solder paste areas: References must never print on exposed pads. Most EDA tools enforce this, but verify with DRC.
• Legible direction: Standard practice is to read the board from bottom-left (0 degrees or 90 degrees rotations only). Avoid 180-degree-rotated text that reads upside down.
• Group related components: For connector pinouts, number pins sequentially near the connector body.

Minimum Spacing from Pads

The silkscreen must clear exposed copper pads by at least 0.15mm (0.25mm recommended). During wave soldering or hand soldering, solder can wick along silkscreen ink residue if it touches a pad. Most EDA tools have DRC rules for this — enable and run them before fabrication.

Polarity and Orientation Markers

Incorrect component polarity is one of the most common assembly errors. Clear polarity marking prevents costly rework.

Capacitors

• Electrolytic and tantalum: Mark the positive (+) terminal with a + symbol on the silkscreen. Some footprints use a filled arc on the positive side.
• KiCad standard footprints include a + marker by default for polarized capacitors — keep it visible.

Diodes and LEDs

• Mark anode (A) and cathode (K) or use the triangle-and-bar diode symbol in silkscreen
• For LEDs, add a small arrow indicating light emission direction
• Schottky and Zener diodes: same K/A marking approach

ICs and QFP/QFN Packages

• Mark pin 1 with a dot, triangle, or beveled corner in the silkscreen
• For QFP packages, add a dot at pin 1 corner that is clearly visible before and after soldering
• For BGA, add a cross-hair or dot at the A1 corner ball location

Connectors

• Label pin 1 explicitly (“1” or arrow)
• For power connectors, add +/- labels near the pins
• For JST connectors, specify the series and pitch: “JST PH 2.0mm” in small text near the connector

Transistors and MOSFETs

• Label G (Gate), D (Drain), S (Source) for MOSFETs in TO-220 or D2PAK packages
• For BJTs: B (Base), C (Collector), E (Emitter)

Special Markings and Labels

Test Points

Label every test point with a function: TP_VCC, TP_GND, TP_SDA, TP_TX rather than generic TP1, TP2. This saves significant time during bring-up and debugging. Use consistent naming conventions across board revisions.

Board Identification

Every professional PCB should include:

• Board name or project code
• Hardware revision (v1.0, rev B)
• Date code (YYYY-MM or YYWW for week code)
• Manufacturer’s identifier (optional but useful)

Suggested placement: bottom silkscreen near the edge, or in a dedicated info box near a corner.

Fiducial Markers

Fiducials are small copper circles (typically 1mm diameter with 2mm clearance from other copper) used by pick-and-place machines for alignment. They appear on the copper layer, not silkscreen, but silkscreen may include “FID” labels nearby. For boards with fine-pitch SMD components (0.5mm pitch QFP, 0402 passives), add at least 3 global fiducials on the PCB.

High-Voltage Warning

For boards operating above 50V AC or 75V DC (IEC 60950 limits), add the standard high-voltage warning symbol (lightning bolt in triangle) near the hazardous area. This is a safety compliance requirement for CE, BIS, and UL marked products.

KiCad Silkscreen Tips

• DRC silkscreen checks: Enable “Silkscreen over pads” and “Silkscreen inside courtyard” checks in PCB Setup > Design Rules. These catch overlapping references before fabrication.
• Reference size defaults: In footprint properties, set text height to 1.0mm and stroke to 0.15mm as your project default. Create a custom fp-lib entry for frequently used footprints.
• Edit all silkscreen at once: Use Edit > Find to select all references of a given type, then bulk-resize using the properties dialog.
• Silkscreen to copper clearance: In KiCad 7+, set DRC rule: (constraint courtyard_clearance (min 0.25mm)) for silkscreen elements.
• Hide values on dense boards: For 0402 resistors, it is acceptable to hide the Value field (keep Reference visible). Paste value visible = false in footprint properties.
• Use correct layer: Graphics on F.SilkS appear on the front. Do not accidentally place silkscreen on F.Cu or F.Fab — the fab will not print it.

EasyEDA Silkscreen Tips

• Silkscreen is on the TopSilkLayer and BottomSilkLayer
• Minimum text size: set font width and height to 0.8mm minimum, stroke 0.15mm
• EasyEDA DRC: run DRC before export to catch silkscreen-over-pad violations
• JLCPCB export: when using EasyEDA with JLCPCB one-click fab, the Gerber export automatically includes silkscreen layers. Verify in Gerber viewer before ordering.
• Component reference auto-placement: EasyEDA’s “Auto Layout” feature places references outside pads but may create inconsistent orientations. Review manually.

Fabrication Rules for Silkscreen

Different fabrication processes have different silkscreen capabilities:

JLCPCB and PCBWay use inkjet printing for silkscreen. Their minimum line width is 0.15mm, but 0.2mm produces more consistent results. Text smaller than 0.8mm height will be illegible or not printed at all.

Silkscreen Colors Available

Standard colors at major fabs:

• White: Standard, highest contrast on green/red/blue solder mask
• Black: Standard on white, yellow, or matte gray solder mask
• Yellow: Available at PCBWay, good contrast on black solder mask

Silkscreen Design Checklist

• All component references placed outside courtyard
• Text height minimum 1.0mm, stroke minimum 0.15mm
• Silkscreen clears all exposed pads by at least 0.15mm
• Silkscreen clears board edge by at least 0.3mm
• All polarized components marked (electrolytic caps, diodes, LEDs)
• All IC pin 1 locations clearly marked
• All connector pin 1 and polarity labeled
• All test points labeled with functional names
• Board name, revision, and date present
• High-voltage warnings present where applicable
• Fiducial markers present for boards with fine-pitch SMD
• DRC run and silkscreen violations resolved
• Gerber silkscreen layers reviewed in viewer before ordering

Frequently Asked Questions