What Is PCB Silkscreen? Markings, Colors, and Design Rules Explained

A bare PCB can be electrically correct and fully manufacturable while still being difficult to assemble, inspect, test, repair, or identify. Without visible component references, polarity symbols, connector labels, test-point names, revision numbers, and compliance markings, technicians must work from drawings or guess what each feature means.

The visible identification layer commonly called PCB silkscreen solves this problem. It provides permanent markings on the outer surfaces of the board so that assemblers, inspectors, service technicians, and end users can understand the hardware without tracing every net or opening the design files.

Although the industry still uses the word “silkscreen,” many modern PCB legends are produced by photoimageable or digital printing processes rather than a traditional mesh screen. The design function remains the same: create readable, durable markings without interfering with pads, soldering, component placement, fiducials, holes, or board separation. This guide explains what belongs on the legend layer, common colors and processes, practical design rules, and how Linked Electronics Co., Limited reviews silkscreen data before fabrication.

What Is PCB Silkscreen?

PCB silkscreen is the printed legend or marking layer applied to the outer surface of a printed circuit board. It normally sits over the cured solder mask and identifies components, connectors, test points, polarity, board orientation, revision status, manufacturing information, and other features needed during assembly or service.

Most rigid PCBs use a top legend, and many also use a bottom legend. The markings do not form part of the electrical circuit. They are visual information only, but they can still affect manufacturability if they overlap solderable surfaces, fiducials, component pads, routed edges, or other controlled features.

The legend artwork is normally delivered as its own fabrication layer in the Gerber or IPC-2581 data package. Typical layer names include:

• Top Silkscreen
• Bottom Silkscreen
• Top Legend
• Bottom Legend
• Top Overlay
• Bottom Overlay

Different CAD systems use different names, but the manufacturing purpose is the same.

Why Is It Still Called Silkscreen?

Traditional PCB legends were printed by forcing ink through a patterned mesh screen onto the board surface. The process is similar in principle to screen printing used for signs, textiles, and product labels. Historically, silk mesh was used, which produced the term “silkscreen.” Modern industrial screens normally use synthetic mesh, but the old name remains.

PCB manufacturers now use several legend-printing technologies. A board marketed as having “silkscreen” may therefore use screen-printed, photoimageable, or digitally printed marking ink.

How PCB Silkscreen Is Applied

Traditional Screen Printing

A patterned mesh screen is aligned over the PCB, and a squeegee pushes legend ink through the open areas of the mesh. The ink is then cured according to the material process.

Screen printing is established, economical, and suitable for standard text and outlines. Its resolution is limited by the mesh, ink viscosity, stencil quality, registration, and surface topography. Very small text and narrow strokes may close, spread, or become incomplete.

Photoimageable Legend

A photoimageable marking material is applied over the board, exposed through artwork, developed, and cured. This method can provide finer registration and more consistent small features than conventional screen printing.

It is useful where dense components leave limited space for reference designators, although the fabricator’s minimum line width and character size must still be followed.

Digital Inkjet Legend Printing

Digital legend printers deposit ink directly from the fabrication data without producing a physical screen. This improves flexibility for prototypes, frequent revisions, serialised markings, and designs with dense or detailed artwork.

Digital printing can provide good registration and avoids screen-tooling preparation, but capability depends on the printer, ink system, board surface, selected color, curing process, and required production volume.

What Information Should Be Included?

Component Reference Designators

Reference designators connect the physical PCB to the schematic, BOM, assembly drawing, test procedure, and repair documentation. Typical examples include:

• R1, R2, R3 for resistors
• C1, C2, C3 for capacitors
• U1, U2 for integrated circuits
• D1 for a diode or LED
• Q1 for a transistor
• J1 or CN1 for a connector
• TP1 for a test point
• F1 for a fuse

Place each designator close enough to its component to avoid ambiguity, but not inside the solderable pad area or under a component body when it must remain visible after assembly.

Component Outlines

A component outline helps assemblers confirm component location and approximate orientation. The outline should represent the physical body rather than the full component courtyard.

The assembly courtyard is a placement-clearance rule and is normally maintained in the CAD documentation rather than printed as a complete legend box. Printing every courtyard boundary can overcrowd the board and make the legend harder to interpret. See the component courtyard clearance guide for placement-spacing rules.

Polarity and Pin-One Markings

Polarity symbols are among the most important legend features. They help prevent reversed installation of:

• Diodes and LEDs
• Electrolytic and tantalum capacitors
• Integrated circuits
• Transistors
• Connectors
• Batteries
• Fuses and protection devices with defined orientation

Use an unambiguous symbol and apply it consistently. For an IC, mark pin one with a dot, triangle, chamfer indicator, or another clearly documented symbol. For a diode, ensure the legend agrees with both the footprint orientation and the component manufacturer’s cathode marking.

Critical polarity should not rely on silkscreen alone. Where practical, support it with an asymmetric footprint, copper feature, solder-mask opening, mechanical keying, or assembly drawing. Legend ink can be clipped, hidden by the installed component, or removed during CAM cleanup if it overlaps an exposed pad.

Connector and Interface Labels

Labels such as POWER, INPUT, OUTPUT, GND, TX, RX, CAN, USB, MOTOR, SENSOR, and programming-header pin names reduce wiring errors during integration and service.

Pin labels should be placed so that technicians can read them after the connector is installed. Do not place all connector information directly underneath the connector body.

Test-Point Identification

Test-point names help production technicians, debug engineers, and service teams locate power rails and signals. Useful labels include:

• 3V3
• 5V
• 12V
• GND
• RESET
• SWDIO
• SWCLK
• TX
• RX

The test pad must remain free of legend ink. Place the label beside the test point rather than over it.

Board Name, Part Number, and Revision

A board should normally include enough information to identify:

• Product or PCB name
• Customer part number
• PCB revision
• Assembly revision where different
• Manufacturing date or date-code area where required

Revision identification is especially important when several board versions look physically similar but have different firmware, component values, routing, or safety approvals.

Compliance and Manufacturing Marks

Depending on the product and contractual requirements, the PCB may include:

• Lead-free or other material-identification marks
• Halogen-free identification
• UL-related manufacturer identification
• RoHS-related wording
• ESD or high-voltage warnings
• Customer logos
• Traceability codes

Do not add certification logos or compliance claims unless the product and manufacturing process are authorised to use them. A silkscreen symbol does not create regulatory compliance.

PCB Silkscreen Colors

White is the most common PCB legend color because it provides strong contrast on green, red, blue, purple, and black solder masks. Black is often selected for white or light-colored solder masks. Yellow and other colors may also be available, depending on the fabricator and marking process.

Color selection should prioritise contrast and readability rather than appearance alone. A visually attractive combination that becomes unreadable under factory lighting or after component installation provides little practical value.

PCB Silkscreen Design Rules

The dimensions below are practical DFM starting points rather than universal IPC limits. Actual minimum capability depends on the legend process, ink, color, solder-mask surface, board finish, equipment, and manufacturer. Confirm the final values with the selected fabricator.

Use Simple, Open Fonts

Use a simple sans-serif font with consistent stroke width. Avoid decorative fonts, very narrow characters, outlines without fill, or fonts with small internal gaps.

Letters such as A, B, R, 6, 8, and 9 contain enclosed or closely spaced areas that can fill with ink when the text is too small. A clear engineering font is more reliable than a visually complex corporate font.

Use Vector Text Where Possible

Vector-based text generally produces cleaner manufacturing data than low-resolution raster artwork. Before generating Gerbers, ensure the chosen CAD font is embedded, converted correctly, or otherwise preserved in the final output.

Always inspect the final Gerber files. A font that looks correct inside the CAD program can change during plot generation if the font is missing or substituted.

Maintain Clearance from Exposed Copper

Legend ink must not cover component pads, edge contacts, test pads, thermal pads, exposed copper, or other solderable surfaces. Ink on a pad can interfere with solder wetting, probe contact, connector mating, or wire bonding.

Many PCB CAM systems automatically clip silkscreen away from solder-mask openings. This protects the pads but can remove part of a designator or polarity symbol. A marking that depends on the fabricator’s clipping operation may become unreadable.

Do Not Print Over Fiducials

Fiducials need clean visual contrast between exposed metal and the surrounding solder-mask clearance. Legend text, outlines, copper fill, or other graphics inside the optical clearance area can reduce recognition reliability.

Keep the complete fiducial area clear, not only the exposed centre. See the fiducial mark placement guide for local, global, and panel-fiducial rules.

Keep Text Away from Board Edges and V-Scores

Text and logos placed too close to the finished outline may be partially removed during routing. Markings across V-score lines, mouse-bite tabs, or routed breakaway regions may crack, disappear, or become unreadable after depanelisation.

Apply clearance to the final finished edge, not only to the panel outline.

Avoid Placing Essential Text Under Components

Text under components can be useful during bare-board inspection, but it disappears after assembly. Do not place information needed during test, servicing, or field installation underneath a component body.

For dense boards, prioritise visible markings in this order:

1. Polarity and pin-one indicators
2. Connector and interface labels
3. Test-point labels
4. Board part number and revision
5. Component reference designators
6. Optional outlines and descriptive text

Verify Bottom-Side Text Orientation

Bottom-side silkscreen is intended to be readable when viewing the physical PCB from the bottom. CAD tools and Gerber viewers may display the layer from different viewpoints, which can create confusion about mirroring.

Generate the bottom legend using the normal CAD-output procedure, then inspect the final manufacturing data in a Gerber viewer from the physical bottom view. Do not manually mirror the entire layer without confirming how the CAD and CAM tools interpret it.

Reference Designator Placement Rules

Keep the Designator Associated with One Component

Do not place a reference designator midway between two similar components. During inspection or repair, the operator must be able to determine immediately which component the text identifies.

Use Consistent Orientation

Where space permits, orient most text in one or two reading directions, commonly left-to-right and bottom-to-top. Random text rotation slows inspection and makes dense boards harder to understand.

Do Not Obscure the Component Outline

Place the designator outside the main component body outline where possible. On dense designs, a shortened or repositioned outline is preferable to overlapping text.

Keep the Assembly Drawing as the Master Reference

Silkscreen cannot always display every reference designator on a dense HDI or BGA board. The assembly drawing and centroid data remain the complete manufacturing references. The visible legend should support assembly and service rather than attempting to reproduce every CAD layer.

Polarity-Mark Design Rules

Integrated Circuits

Use a clear pin-one dot, triangle, line, or corner mark. The symbol must agree with the CAD footprint, assembly drawing, pick-and-place orientation, and component package marking.

Diodes and LEDs

Use a documented cathode or anode indicator and apply the same convention throughout the product. The legend should not create ambiguity between the package mark and the schematic symbol.

Polarised Capacitors

Electrolytic and tantalum capacitors use different package-marking conventions. Confirm whether the visible package stripe identifies the negative or positive terminal for the selected component family, and ensure the PCB marking matches the actual part.

Connectors

Mark pin one and any keyed or high-voltage position clearly. Where wiring errors could damage equipment, add signal names or polarity symbols near the accessible connector side.

Silkscreen and Solder Mask Are Different Layers

Solder mask is a protective polymer coating that covers copper, limits solder bridging, and defines exposed solderable areas. Silkscreen is printed identification placed over the finished board surface.

The two layers have different functions:

The selected surface finish also applies to exposed copper independently of the silkscreen. See the PCB surface-finish guide for ENIG, HASL, OSP, immersion silver, and immersion tin.

Logos, Barcodes, and QR Codes

Company Logos

A logo should use simplified vector artwork with strokes and spacing above the fabricator’s minimum capability. Very fine trademark details may merge or disappear.

Confirm that the logo is legally authorised for use and that its size does not interfere with designators, pads, fiducials, isolation areas, or test access.

Barcodes and Data Matrix Codes

Machine-readable codes require stricter control than ordinary text. Module size, contrast, quiet zone, surface flatness, printing resolution, and scanner capability all affect readability.

For production traceability, laser marking, dedicated labels, or controlled digital printing may be more reliable than ordinary screen printing. Validate the complete marking and scanning process before volume production.

Serial Numbers

Traditional screen printing is best for fixed artwork. Variable serial numbers normally require digital inkjet printing, laser marking, labels, or another traceability process. Specify the format, location, contrast, code size, and data source during quotation.

Common PCB Silkscreen Mistakes

Text Over Pads

This is the most common legend error. CAM clipping may remove the overlap, but it may also cut off part of the component name or polarity mark. Correct the design rather than depending on automatic clipping.

Text That Is Too Small

Very small text may appear correct in the CAD view but become filled, broken, or unreadable after printing. Use the manufacturer’s preferred character and stroke dimensions.

Incorrect Diode or Capacitor Polarity

A wrong polarity symbol is more dangerous than no symbol because operators trust the board marking. Check the footprint, BOM, datasheet, assembly drawing, and pick-and-place orientation together.

Reference Designators Hidden by Components

Designators placed directly under parts provide no value during inspection or repair. Move the most important references outside the component body.

Silkscreen Inside a Fiducial Clearance

Ink near the fiducial can reduce optical contrast and cause alignment failures. Keep the entire fiducial clearance zone free of legend artwork.

Markings Across V-Scores or Routing Tabs

Text crossing a depanelisation feature becomes incomplete after separation and may make two different boards appear to carry the same partial marking.

Unverified Bottom-Side Mirroring

Incorrectly generated bottom text can arrive mirrored on the physical board. Always inspect the final fabrication output from the correct viewing direction.

Too Much Information

A crowded legend is not automatically a better legend. Excessive outlines, comments, and repeated values can hide the markings that actually matter. Prioritise polarity, interfaces, test access, revision control, and service information.

PCB Silkscreen DFM Checklist

• Confirm the top and bottom legend files are included.
• Verify the final Gerber orientation in a viewer.
• Use approximately 1.0 mm or larger text where space permits.
• Use approximately 0.15 mm or wider strokes where possible.
• Keep all legend ink away from exposed pads and contacts.
• Keep the complete fiducial area clear.
• Keep markings away from routed edges, V-scores, and breakaway tabs.
• Check that component designators identify only one component.
• Verify every polarity and pin-one symbol against the assembly data.
• Keep essential service information visible after assembly.
• Confirm the legend color provides sufficient solder-mask contrast.
• Confirm special logos, serial numbers, or machine-readable codes with the fabricator.
• Remove obsolete text from previous PCB revisions.
• Check that no compliance mark is used without authorisation.

How Linked Electronics Co., Limited Reviews Silkscreen Data

During fabrication engineering review, Linked Electronics Co., Limited checks the top and bottom legend data against the solder-mask, copper, drill, profile, and assembly-related layers.

The review includes:

• Legend overlap with solder-mask openings
• Text and line dimensions below practical production capability
• Markings too close to routed edges or V-scores
• Legend artwork inside fiducial clearance zones
• Text covering test pads or exposed contacts
• Bottom-layer orientation
• Potentially unreadable logos or machine codes
• Silkscreen color and solder-mask contrast

Manufacturing CAM may clip unavoidable legend-to-pad interference, but clipping should not be used to repair important design information silently. If a polarity symbol, reference designator, compliance mark, or essential label would become incomplete, the issue should be clarified before production.

For assembled projects, Linked Electronics Co., Limited also reviews the legend together with the BOM, centroid data, component footprints, and assembly drawings. The complete PCBA manufacturing process guide explains how DFM review, solder paste printing, component placement, reflow, AOI, X-ray inspection, and functional testing fit together.

Conclusion

PCB silkscreen is the visible identification system of a printed circuit board. It connects the physical hardware to the schematic, BOM, assembly drawing, test plan, repair procedure, and product documentation.

A useful legend includes readable reference designators, polarity marks, connector labels, test-point names, board identity, revision information, and only the compliance marks that are actually authorised. It must remain clear of exposed pads, fiducials, holes, board edges, V-scores, and other manufacturing features.

The best design does not attempt to print every available CAD detail. It prioritises the information required to assemble, inspect, test, service, and identify the board. Linked Electronics Co., Limited can review the final legend data together with the Gerber files and assembly documentation before PCB or PCBA production begins.

Frequently Asked Questions

What is PCB silkscreen used for?

PCB silkscreen identifies components, polarity, connectors, test points, board orientation, revision status, warning information, manufacturing data, and other features needed during assembly, inspection, testing, installation, and repair.

Is PCB silkscreen always printed through a silk screen?

No. Silkscreen is the traditional industry name for the PCB legend layer. Modern manufacturers may use mesh screen printing, photoimageable legend material, or digital inkjet printing, depending on resolution, volume, color, equipment, and production requirements.

What is the standard PCB silkscreen color?

White is the most common legend color because it provides strong contrast on green and most other dark solder masks. Black is commonly used on white or light-colored solder masks. Other colors may be available but should be confirmed with the fabricator.

What is a good minimum PCB silkscreen text size?

A character height of approximately 1.0 mm with a 0.15 mm stroke is a practical preferred starting point. Approximately 0.8 mm text may be possible with a capable process, but smaller characters have a greater risk of filling, breaking, or becoming unreadable. The fabricator’s confirmed capability controls the final design.

Can silkscreen be printed over a solder pad?

No. Legend ink should remain clear of exposed solder pads, test pads, edge contacts, thermal pads, and other solderable surfaces. PCB CAM systems often clip legend ink away from mask openings, but that clipping can remove part of a designator or polarity symbol.

Should component reference designators remain visible after assembly?

Important designators should remain visible wherever practical, especially for connectors, fuses, test points, adjustable components, polarised parts, and serviceable devices. On very dense boards, the assembly drawing remains the complete reference, but essential service information should not be hidden under components.

Can PCB silkscreen be used for serial numbers or QR codes?

Fixed artwork can be printed as part of the normal legend, but variable serial numbers require digital printing, laser marking, labels, or another controlled traceability method. Machine-readable codes must be validated for module size, contrast, quiet zone, surface condition, and scanner performance.

What files should I send Linked Electronics Co., Limited for silkscreen review?

Send the complete Gerber or IPC-2581 data, drill files, board profile, stack-up, BOM, centroid file, assembly drawing, required legend color, and any logo, compliance, serialisation, or traceability requirements. Linked Electronics Co., Limited will review legend clearances and manufacturability before production.

← Back to Blog