The silkscreen, or legend, is the layer of printed ink that carries the human-readable information on a printed circuit board: component outlines, reference designators, polarity markings, the board name and revision, warning symbols and company logos. It is non-conductive, it carries no signal, and no board requires one to function.
Designed carelessly, it also causes assembly errors, gets silently deleted by your fabricator, and occupies space you needed for something else. It is worth about an hour of attention.
Why include a silkscreen at all
Plenty of boards ship without one. The reasons to include one are practical rather than aesthetic:
- Assembly, test and debug. Reference designators and component outlines give a direct visual identification of every position on the board. An engineer probing a prototype should not have to open the layout tool to find R47.
- Error prevention. Conventional polarity markings -- a dot or a "1" at pin one, a cathode bar, a plus sign at an electrolytic -- reduce the rate of reversed and misplaced components during hand assembly and rework.
- End-user interaction. Labelling the LEDs, buttons and connectors that somebody outside your team will touch is cheap and saves support calls.
- Identification. Board name, revision, date code and serial number make a returned board traceable.
- Branding. A logo costs nothing to print and makes an assembly look considered.
At Newmatik we also use the silkscreen layer to generate the assembly layouts and instructions our production team works from throughout the assembly process. That is true whether or not the legend is physically printed on the board -- which brings us to the exception.
When to leave it off
High-density boards are the clear case. When component pitch shrinks, there is simply nowhere to put a legible designator that does not overlap a pad, a via or another designator. A legend that overlaps things it should not is worse than no legend, and printing it anyway does not make it readable.
The standard practice here is to keep the silkscreen data in the Gerber layer -- .gto for the top legend, .gbo for the bottom -- and in the assembly
drawing, without printing it. Designators can then be placed inside footprints where a human would never see them, because the pick-and-place machine, the
inspection operator and the rework technician are all reading the documentation, not the board. Some designers print only the marks that genuinely have to be
on the physical board: pin one, polarity, connector labels, warnings, revision.
This is a legitimate and common approach, not a compromise.
How the legend gets printed
The three methods differ in resolution by roughly a factor of two, which is exactly the range where your design rules live.
| Method | Ink | Minimum line width | Accuracy |
|---|---|---|---|
| Manual screen printing | Epoxy | > 0.18 mm (7 mil) | ~0.13 mm (5 mil) registration |
| LPI (liquid photo imaging) | Photosensitive epoxy | ~0.10 mm (4 mil) | High |
| DLP (direct legend printing) | Acrylic | < 0.10 mm | Highest |
Manual screen printing pushes ink through a stencil. It is the legacy method: cheap, coarse, and still perfectly adequate for a board with generous spacing. LPI exposes a photosensitive epoxy through a film negative and develops it, which is far more precise. DLP is essentially an industrial inkjet with an inline UV-LED cure -- no stencil, no film, the highest accuracy and the fastest turnaround, at a higher consumable cost.
There is no single "standard" method today. LPI and DLP dominate modern production, and DLP has become the default at quick-turn prototype houses. Manual screen printing is legacy. If you have fine legend requirements, ask your fabricator which they use rather than assuming.
Design rules
The ink is a non-conductive epoxy, or an acrylic in the case of DLP. The numbers below are typical fabricator minimums; design a notch above them and your legend will survive whichever house builds the board.
| Parameter | Typical minimum | Design target |
|---|---|---|
| Line / stroke width | 0.15 mm | ≥ 0.20 mm |
| Character height | 0.80 mm | ≥ 1.00 mm |
| Clearance to pads and vias | 0.15 mm | ≥ 0.25 mm |
Keep the stroke-to-height ratio at roughly 1:6. A 1.0 mm character with a 0.30 mm stroke fills in and becomes an illegible blob; the same character with a 0.05 mm stroke disappears.
Keep the legend off exposed metal
This rule is usually stated as "do not print silkscreen on traces", and that is not quite right. Legend printed over solder-mask-covered copper -- including traces and planes -- is completely normal and causes no problem at all. The mask is between the ink and the copper.
The rule is to keep the legend off exposed metal:
- SMD and through-hole pads
- Open, untented vias
- Test points and probe pads
- Gold fingers and edge connectors
Silkscreen ink on a pad behaves as an organic contaminant. It blocks solder wetting, prevents the intermetallic from forming properly, and produces cold joints, dewetting or opens. It also interferes with test probes.
Fabricators know this, which produces a second-order effect worth understanding: most will automatically clip legend that falls within roughly 0.15 mm of a pad edge, a rule usually called solder-mask precedence. They will not tell you. If you place a polarity marking too close to a pad, it will simply not be on the board you receive, and you will not find out until an operator places a diode backwards. Give your markings clearance so they survive.
Component and board markings
Reference designators. The class-designation letters -- R for resistor, C for capacitor, U for integrated circuit, D for diode, Q for transistor -- come from IEEE 315 (ANSI Y32.2), and the designation system is defined in ASME Y14.44. IEC 60617 is frequently cited for this and is the wrong reference: it governs graphical symbols, not designator letters, and the IEC letter-code scheme is a different system entirely (IEC 81346).
Place designators so they remain visible after the board is populated. A designator underneath the component it names is only useful to whoever depopulates the board.
Polarity and pin one. Use conventional markings: a dot or the numeral "1" at pin one, a square pad, a bar for the cathode, a plus sign for the anode of a polarised capacitor. Orientation and pin-one conventions are covered by IPC-7351 for land patterns and IEC 61188-7. The point of a convention is that it needs no explanation -- an inventive polarity marking that requires the assembly drawing to decode is not a polarity marking.
Board markings. Company logo, board name, revision and date code aid identification and traceability. Leave space for them before the layout is full.
UL markings. This is where drawings most often go wrong. A bare printed circuit board is a UL Recognized Component, not a UL Listed product. It therefore carries the Recognized Component Mark -- the reversed "RU" symbol -- not the UL-in-a-circle Listing Mark. Alongside it belong the manufacturer's identification, the UL file number (the E-number), and the type designation for the recognised construction.
The flammability class, 94V-0, is a UL 94 material rating. Many fabricators mark it next to the UL mark and the material type is encoded in the type designation, but it is not itself a mandated board legend. Keep it, and the date or batch code, conceptually separate from the UL mark: the batch code is good traceability practice, not part of the certification marking. Our article on UL certification for PCB assembly covers the certification itself.
Reserve legend space for all of this early. Retrofitting a UL mark onto a finished layout is unpleasant.
Colour and cost
White is the default. Black and yellow are common alternatives, and all three offer good contrast against standard solder mask colours, which matters for optical inspection as much as for human readers.
- Adding a silkscreen does not normally cost extra. At prototype fabricators, standard white legend -- often on both sides -- is included in the base price. It is a standard process step.
- Second-side legend is fabricator-dependent. Prototype houses usually include it. Traditional volume fabricators may treat it as a separate line item, because it is a second print and cure operation.
- Non-standard colours cost extra and add lead time. Anything beyond white and black typically carries a surcharge and a few extra days.
Do not choose an exotic colour on a board that will be optically inspected without checking the contrast against your solder mask first.
In summary
The silkscreen is not required to manufacture a board, and a good one still repays its cost many times over. It gives the production line, the test engineer and the field technician unambiguous visual cues, and it prevents the misplaced and reversed components that cause the most tedious and expensive class of assembly error.
Design it to real numbers: 0.20 mm strokes, 1.0 mm characters, 0.25 mm clearance to anything exposed, standard polarity conventions, and space reserved for the UL mark and batch code. If a design cannot accommodate a legible legend, put the data in the Gerber and the assembly drawing and print only what has to be physically on the board. Both are correct answers. Printing an illegible legend is not.
If you would like a layout reviewed before release, our engineering team is happy to look at it.
Sources
- IEEE 315 (ANSI Y32.2) -- Graphic Symbols for Electrical and Electronics Diagrams, Clause 22, Class Designation Letters
- ASME Y14.44 -- Reference Designations for Electrical and Electronics Parts and Equipment
- IPC-7351 -- Generic Requirements for Surface Mount Design and Land Pattern Standard
- IEC 61188-7 -- Printed boards and printed board assemblies -- Design and use
- IPC-SM-840 -- Qualification and Performance of Permanent Solder Mask and Flexible Cover Materials
- UL 796 -- Printed-Wiring Boards; UL 94 -- Tests for Flammability of Plastic Materials