PCB Silkscreen Legend: Rules for Legible Boards

The silkscreen is the last layer added to a board and the first one anybody reads. It carries the reference designators that make assembly possible, the polarity marks that stop a part being fitted backwards, and the board identifier that ties a unit to its test record. It is also the layer most often squeezed at the end of a project.

What the Legend Has to Do

A silkscreen legend has three jobs, and they are worth separating because each one has different constraints.

The first is assembly. An operator or a pick and place programmer needs to know which component goes where, which orientation is correct, and where pin one is. That information has to survive being read through a microscope, at an angle, under a top light, on a board that is the same colour as the ink.

The second is field service. A technician repairing the board needs the same information, usually with a component fitted and a can or a heatsink in the way. Marks hidden under a part are close to useless in service.

The third is traceability. Board part number, revision, date code and often a serial number, a manufacturer mark and a compliance symbol. These are usually required by the customer or by a regulator, they are frequently overlooked until the first audit, and they take up space that has to be reserved early.

Clearance from Copper and Pads

Silk is printed on top of the solder mask, so it sits directly over the board surface, and that position determines the main design rule. Ink must not land on an exposed pad. There are two reasons. Ink on a pad contaminates the surface and can impede wetting, producing a joint that is weak or that fails inspection. Ink can also flake during reflow and leave debris on the assembly.

The usual requirement is a clearance of 0.15 mm to 0.2 mm between any silk feature and any exposed copper, measured from the edge of the ink to the edge of the mask opening. That number is tighter than the board minimum clearance and it is the one that decides whether text will fit. Most layout tools will check it, but only if the silkscreen layer is included in the design rule check rather than treated as decoration.

Printing over covered copper is a different matter. Silk over mask that covers a trace is normal, and it does not affect the circuit. What it does affect is appearance and adhesion: ink over a raised trace edge is thinner and can wear, and on very fine pitch areas the ink may not fill the gap cleanly.

Vias deserve their own note. A tented via with silk over it is generally fine, but an untented via under ink can wick ink into the hole or leave a pinhole. Keep text off via fields unless the vias are fully tented.

Minimum Text Size and Line Width

Silk is a screen printed or inkjet deposited layer, and it has a resolution floor. Features below that floor do not come out as intended: strokes merge, characters fill in and the text becomes a smudge. The practical industry limits are close to the following.

• Character height: 0.8 mm absolute minimum, 1.0 mm a reasonable working minimum, 1.5 mm comfortable for hand assembly.
• Stroke width: 0.15 mm minimum, with 0.15 mm to 0.2 mm the normal range for text at 1 mm height.
• Character spacing: at least one stroke width between characters, and two for small text.
• Clearance to exposed copper: 0.15 mm to 0.2 mm, from the ink edge to the mask opening edge.

Two rules of thumb follow. The stroke width should be roughly one sixth to one eighth of the character height for a stroke font, and the text should never be smaller than the smallest feature the fabricator can print reliably. Asking for 0.5 mm text with a 0.1 mm stroke is asking for characters that disappear in production even if they look perfect on screen.

Filled fonts are a separate case. Vector text rendered as an outline produces thin strokes at the edges of curved characters, and those strokes can fall below the print resolution. Stroke fonts, where every character is a line of constant width, are safer for small silk text and are what most fabricators prefer. Most tools let the silkscreen layer use a dedicated stroke font while the copper layer uses a normal vector font.

Reference Designators and Placement

Designators are the reason the layer exists, and placement is where most boards go wrong.

Keep each designator next to its component, on the same side, and far enough that it is not hidden by the part when it is fitted. A designator under a module, a shield can or a tall capacitor is not a designator. Where space is genuinely tight, moving the text slightly away from the part is almost always better than shrinking it below the readable minimum.

Keep the text orientation consistent. Every designator should read in the same direction on the board, so that a person looking at the assembly reads all of them without rotating the board. Rotating a designator to fit a tight spot, or allowing the tool to auto-rotate text, produces a legend that has to be scanned line by line instead of read.

Trim the designator to what is needed. The full reference prefix consumes width, and where space is tight, shortening the silkscreen to the number while keeping the full reference in the assembly drawing is a common compromise. What must not happen is a designator that collides with its neighbour, because a misread designator is a mis-placed component.

Finally, remember the assembly drawing. A board does not have to carry every piece of information on the silk. On a dense design the sensible approach is to keep orientation and polarity marks on the board and put the rest in the documentation and the pick and place file, because operators work from both.

Polarity, Orientation and Pin One

The marks that prevent assembly errors matter more than any other part of the legend.

Polarised parts need a mark that survives rework and that cannot be confused with the outline. A diode is usually marked with a cathode band, an electrolytic capacitor with a positive or negative side bar, and an IC or a connector with a pin one indicator such as a dot, a corner chamfer or a filled square. Whatever the convention, it must be consistent across the board: a dot that means pin one on one footprint and polarity on another is worse than no mark at all.

The pin one mark should be visible with the part fitted, which means it cannot sit under the body. For a large IC where the corner is covered, the mark belongs outside the courtyard, aligned with the pin one corner.

Connector marking deserves the same care. Pin one, the mating direction, and where relevant the keying, should all be apparent from the silk. A board that needs a cable inserted the right way round but gives no indication of which way that is will eventually be assembled backwards in the field.

Board Identity and Compliance Marks

The marking block is easy to forget and hard to add later, because the space it needs is usually in a corner that has already been assigned to a mounting hole.

A typical marking block carries the board part number, the revision, the date code or a serial number, the customer or manufacturer mark, and any compliance symbols the product requires. A UL recognised assembly, for example, carries a recognised component mark together with the manufacturer identifier, and the file reference has to match what the certification records. Some customers also require a country of origin, a lot code, or a binary date code in a small matrix of dots.

The practical rules are the same as for any other text: readable size, clearance from pads and mounting hardware, and a position that a label or a reader can reach. If the marking is expected to be scanned, the symbol needs quiet space around it and enough contrast, and if it is expected to be read after the board is fitted into a housing, that position has to be checked against the mechanical assembly rather than assumed.

Reserve this area during layout, not during documentation. A 20 mm by 8 mm block in a corner of the board costs almost nothing when the plane is still being drawn and is nearly impossible to find later.

Contrast, Colour and Readability

Silk readability depends on contrast with the mask underneath, and the standard combinations are white ink on green, black on white, and white on matte black. Low contrast combinations, such as dark grey on black or white on a light coloured mask, look fine on a screen and become unreadable under the amber light of a rework station.

Two other factors matter in production. Glossy mask finishes reflect a top light back into the operator eye, which is why matte finishes are preferred for boards that are inspected visually. And ink over a copper edge is thinner than ink over bare laminate, so the same text can appear lighter in places, which is a reason to keep fine text away from trace edges.

DFM Checklist

• Check the silkscreen layer with the same design rule check used for copper, including the clearance to mask openings.
• Keep every text height at or above 0.8 mm, with 1 mm as the working target.
• Use a stroke font for small text and confirm the stroke width meets the fabricator minimum.
• Remove or move silk that overlaps pads, test points, fiducials or tooling holes.
• Keep designators visible with the component fitted, and in a consistent reading direction.
• Mark pin one and polarity on every polarised part, using one convention throughout.
• Reserve space for the part number, revision and date code block before routing is finished.

It is worth confirming these limits with the fabricator rather than assuming a generic figure, because the achievable stroke width depends on the printing method. An inkjet legend holds smaller text than a stretched screen, and a board printed with a coarse screen may need 1.2 mm text to stay legible. For a prototype the legend can often be more generous, since the operator is likely the designer; for a volume build the legend is working documentation for people who have never seen the design, and it should be treated that way.

FAQ

• Does the silkscreen affect the electrical performance? No. It is a printed layer on top of the mask and has no electrical function.
• Can silk be printed on top of a pad? It should not be. Ink on an exposed pad can impede soldering and contaminate the joint.
• What happens if the silk is too small to print? The characters fill in or break up, and the legend becomes unreadable. Most fabricators will flag this during the DFM review rather than print a defect.
• Is the silkscreen the same as the solder mask? No. The mask is the protective coating with openings for pads, and the silk is the printing on top of it.

Summary

The silkscreen is the interface between the design and everyone who handles the board afterwards. That means a clearance rule that keeps ink off exposed copper, a minimum text size the printing process can actually hold, designators placed where they can be read with the parts fitted, and polarity marks that use one convention consistently across the board.

None of this is difficult, but all of it competes for space with routing, and it is therefore the layer that gets sacrificed when a schedule tightens. Reserving the marking block early, checking clearance with the same rigour as copper, and reviewing the legend during the layout review and again at assembly and test keeps a board from being built correctly and labelled badly.