Three surface details are specified on almost every board and misunderstood on many: the solder mask, the silkscreen legend and the treatment of vias. Each looks cosmetic. Each has a manufacturing limit that can make a board fail.
Solder mask
Solder mask is the polymer coating, green on most boards, that covers the copper except where you want to solder. It does three jobs: it stops solder from flowing where it should not, it protects copper from air and dirt, and it insulates tracks against accidental contact.
It is applied over the whole board, then exposed to light through your mask layer and developed, so that openings appear over pads. Your mask Gerber file shows the openings, not the coating.
- Solder mask: the coating over the board.
- An opening at a pad: the copper is bare, with its surface finish, so that solder can wet it.
- Silkscreen ink, printed on the mask and kept off the pads.
- A track under the mask: protected and insulated.
- Mask between two pads, a bridge. If it is too thin it is lost and solder can join the pads.
Colours
Green is the standard colour and the one every factory supports. Other colours (red, blue, black, white, yellow and others) are common. They are similar in purpose, but a factory may support them with different limits:
- Some colours may have a different minimum mask bridge or a longer lead time.
- Dark and matt masks make tracks hard to see, which makes visual inspection and rework harder.
Ask which colours are supported for the features you use; the standard colour is the safe choice for a dense board.
Mask openings and bridges
The opening around a pad is called the mask expansion or clearance. Two kinds of pad are described:
- Non-solder-mask-defined (NSMD). The mask opening is larger than the copper pad, so the pad edge is exposed. Preferred for most parts.
- Solder-mask-defined (SMD). The mask overlaps the copper edge and defines the pad. Sometimes used under BGAs to limit pad size.
Between two pads there is a strip of mask: the mask bridge (also called web or dam). It keeps solder from joining neighbouring pads. If the bridge is thinner than the process can print, it peels away or is left out, and bridges of solder then form during assembly. This happens on fine-pitch parts. Common practice is that a bridge of about 0.1 mm is possible in many factories' standard processes, and below that it fails or needs special processing; check the number for your factory. The remedy is a smaller pad opening, or no mask between pads and a design that tolerates it.
Mask on pads, and misalignment
The mask is registered to the copper with a small tolerance. If your mask opening only just clears a pad, a small shift covers part of it. Allow a margin. Do not let mask cover a pad that needs solder.
Silkscreen (legend)
The silkscreen is the printed text and symbols on the board, usually white on green, applied by inkjet or screen printing. It carries reference designators, polarity marks, pin 1 marks, logos and version numbers. For assembly and rework, it is often the only guide a person has.
Rules that avoid problems:
- Keep it off pads. Ink on a pad blocks solder. Factories usually remove legend from pads, which can erase part of your text or polarity mark.
- Make lines and text thick and tall enough. A line width of about 0.15 mm and a text height of about 0.8 mm to 1 mm are commonly legible; smaller text blurs. Check your factory's minimum.
- Do not put important marks under parts. Mark pin 1 and polarity where they can be seen after the part is placed.
- Use the same side as the part, except where you must not.
- Do not rely on tiny text for safety information. Use larger text, or a label.
Vias and what to do with their mask openings
A via is a plated hole that joins layers. By default, vias are covered or not depending on the mask file: an opening in the mask over the via leaves it open (an "untented" via), while a mask layer without an opening covers it. The question is what happens to the hole itself. The standard IPC-4761 describes seven treatments, from I to VII. In simple terms:
| Treatment | What it means | Typical reason |
|---|---|---|
| Tented (type I) | Mask covers the via from one or both sides, without filling the hole | The usual, cheap treatment; covers the via and insulates it |
| Tented and covered (II) | A second layer of mask covers the tent | Extra protection |
| Plugged (III) | The hole is filled partly with ink or resin from one side | Keeps solder or flux out of the hole |
| Plugged and covered (IV) | Plugged, then covered with mask | The same, with a covered surface |
| Filled (V) | The hole is filled completely with resin or paste | Needed before a via is placed in a pad |
| Filled and covered (VI) | Filled, then covered with mask | A closed, flat via surface |
| Filled and capped (VII) | Filled, then plated flat over the top | Via-in-pad: a flat copper surface that can be soldered |
The distinction between plugged and filled is by how complete the fill is. Factories may support some types and not others.
- Tented: mask covers the via, the hole stays empty.
- Untented: the mask is open around the via.
- Plugged: resin in the hole, mask over it.
- Filled and capped: resin all through the hole, copper plated flat over both ends. The mask opens at this pad.
Why this matters
- A via in a pad. If a via sits in a solder pad and is open, the solder runs down the hole during reflow and the joint is starved. That calls for a filled and capped via, which costs more. If you can move the via beside the pad, do.
- Vias under BGAs. On the side where the BGA sits, open vias near pads can carry solder away. Tenting or plugging them is a common choice.
- Test points. A via used as a test point should be open on that side.
Tented vias and the mask file
A tented via needs the mask layer to be closed over it on the side being tented. If the via has an opening in the mask file, it will not be tented, whatever the order form says. Many tools offer a setting to tent vias. Check the mask file in a viewer.
How this shows up when you order here
Several of the 25 checks look at these details: they find solder mask between pads too thin to hold, and silkscreen on pads or too thin to print, and they report vias inside pads as a feature found in the files, which then must be matched by an ordered via treatment. The check shows the places and the measured value against the limit. The colours and via treatments available are on the capabilities page. The check cannot judge whether your legend is useful, only whether it can be printed. See also Design for manufacture: the mistakes we see.