Solder Mask Clearance: Rules, Dams and Vias

Solder mask clearance is the gap between a pad and the edge of the mask opening around it, and it is one of the few layout parameters that is decided by the assembly process rather than by the circuit. Get it right and nobody notices. Get it wrong and the board bridges, the mask lifts, or a pad turns out to be a different shape than the component was designed for.

What the Mask Does

Solder mask is the protective coating printed over the finished board. It has four jobs, and each one sets a different requirement on how it is opened around a pad.

It protects the copper and the laminate from contamination, handling damage and moisture. It provides electrical insulation between tracks and between a track and a component body. It acts as a barrier that keeps molten solder on the pad during reflow, which is what stops bridging between adjacent joints. And on a board with a legend, it provides the background that makes the marking readable.

The last two jobs are the ones that interact with pad geometry. A mask opening that is too small leaves mask on the pad and prevents soldering. An opening that is too large removes the barrier between pads and allows solder to flow from one joint to the next, which is a bridge.

Openings, Dams and Registration

Three numbers describe the pattern, and they are worth keeping separate in the design rules.

The opening is the aperture in the mask above a pad. Two conventions are in use. In a non solder mask defined pad the opening is larger than the copper, typically by 0.05 mm to 0.1 mm per side, so the copper pad defines the solderable area. In a solder mask defined pad the opening is smaller than the copper, so the mask overlaps the pad edge and defines where the joint can form.

The dam is the strip of mask that remains between two adjacent openings. It has a minimum width, because a narrow strip of mask between two pads lifts or washes away, taking the insulation with it. Typical minimums are 0.075 mm on a fine pitch board and 0.1 mm on a standard one, and some fabricators can hold less on specific processes.

Registration is how accurately the mask pattern is aligned to the copper. Since the mask is imaged separately from the copper, there is a positional tolerance between them, typically around 0.075 mm to 0.1 mm. That tolerance is what makes the clearance and the dam minimums necessary in the first place: a clearance that just works with perfect alignment will not work when the mask shifts.

The three numbers interact. If the pitch between pads is fixed, a larger opening leaves a narrower dam; a wider dam requires a smaller opening; and a smaller opening encroaches on the pad. On fine pitch parts the available space is often genuinely insufficient and something has to give, which is why the usual answer is a smaller opening on the pad side and a slightly narrower dam, together with a process capable of holding the tighter registration.

SMD and NSMD Pads

The choice between a mask defined pad and a copper defined pad is a real trade, and it depends on the component.

A copper defined, or non solder mask defined, pad gives the largest solderable area and a joint that can wet slightly beyond the copper edge, which produces a visible fillet. The mask opening is larger than the pad, so the solder can spread to the full copper area, and the joint shape is defined by the pad and the paste. This is the usual choice for fine pitch parts, for ball grid arrays and for most passive components, because the extra solderable area helps the joint form.

A mask defined pad has the mask overlapping the copper edge, which anchors the pad and reduces the risk of the pad peeling during thermal or mechanical stress. The trade is a smaller solderable area and a joint with a visible mask step, and the overlap has to be large enough not to be consumed by registration error. This arrangement is often specified on pads that see mechanical load, such as connector lands and test points that are probed repeatedly, and on some components where pad lifting is a known failure mode.

For a ball grid array the choice is usually made in favour of a copper defined pad, because the copper area determines the joint diameter and the mask overlap is small compared to the pad. For a fine pitch device where the dam between openings is already at the process limit, the discussion usually ends with a copper defined pad and a slight reduction in the opening, since there is no room for an overlap.

Vias and Tenting

A via has the same problem as a pad: it has copper at the surface that must either be covered or exposed, and the choice has consequences for assembly.

A fully tented via is covered by mask over the top, with no opening at all. This is the default on most boards, because it protects the via from contamination, keeps solder out of the barrel during reflow, and costs nothing extra. The limitation is that mask over a via can sag into the hole, which is not a problem on a small via but can leave a visible depression or a pinhole on a large one.

A plugged via has the barrel filled with a mask or resin material before the outer layers are coated, giving a flat surface with no risk of solder wicking. It costs more and is used where the via sits under a component pad, or where a flat surface is needed for a thermal interface or a ball grid array escape.

An untented via is left open, which is needed when the via is used as a test point or where a probe must reach it. That is fine electrically, but it means solder can wick into the barrel during reflow, which can starve a nearby joint or leave a solder ball on the surface. Where an untented via must be next to a soldered pad, the layout should keep enough distance that a wick does not affect the joint.

Component Specific Rules

• Fine pitch packages: keep the dam at or above the process minimum, and if the dam cannot be maintained, expect solder bridging between joints.
• QFN and DFN thermal pads: the opening is often divided into a grid of smaller apertures to control paste volume, so the mask pattern has to match the paste pattern.
• Connectors: keep the opening clear of the housing footprint, and check that mask does not sit where the housing presses against the board.
• Test points: they need an opening large enough for the probe to contact the pad without touching mask, but not so large that the probe can wander onto a neighbouring net.
• Castellated and edge features: mask cannot be relied on to protect an exposed edge, so the opening layout has to account for the routing cut.
• Fiducials: must be completely free of mask, with a clear area around them, or the vision system will not find them reliably.

What It Means on the Assembly Line

Mask clearance shows up as specific defects, and each one points back to a layout number.

Bridging between adjacent pads happens when the dam is too narrow or missing, so the mask can no longer stop solder from flowing across. It appears on fine pitch parts first, and it is the most common reason a design is returned for a mask change.

Solder balls are small spheres left on the board, usually after reflow. They come from paste escaping an opening that is too large, from mask slivers that lifted and carried solder, or from an untented via that wicked and expelled solder. They are a cosmetic defect until one lands between two leads.

Tombstoning is a passive component standing on one end. A large opening on one pad and a small one on the other changes the paste volume and the wetting force, and the imbalance is enough to lift a small chip. Symmetry between the two openings is the fix.

Poor wetting occurs when mask encroaches on the pad, either through a deliberately small mask defined opening or through registration drift. The joint forms only on the exposed area, which reduces its cross section and its strength. On a leaded part it may be invisible under the lead.

Pad peeling is the failure that argues in favour of a mask defined pad. Where a pad takes mechanical load, an overlap of mask over the copper edge anchors it and spreads the force, at the cost of a smaller soldering area.

DFM Checklist

• Set the mask opening relative to the pad, and state the convention (mask defined or copper defined) rather than leaving it to the tool default.
• Keep the dam at or above the process minimum for the pitch in use, and confirm that figure with the fabricator.
• Confirm the mask registration tolerance, and make sure the opening still clears the pad at the worst case registration.
• Check symmetry between the openings of a two terminal component.
• Tent every via that does not need to be probed, and plug vias that sit under a pad.
• Keep fiducials and test points free of mask, with adequate clearance.
• Match the mask pattern to the paste pattern on large thermal pads, where the opening is divided into a grid.
• Review the mask layer together with the legend, since both are printed over the same surface and both have clearance rules to copper.

Most of these are checked automatically once the mask layer is included in the design rule check, but the default values in a layout tool are generic and may not match what the supplier can hold. Asking the capabilities question – what dam width and what registration can you hold on this stackup – before the design is released is faster than fixing a bridging problem after the first assembly run.

FAQ

• Should the mask opening be larger or smaller than the pad? Larger for most surface mount pads, so the full copper area is solderable. Smaller where the pad needs mechanical anchoring.
• What is a mask dam? The strip of mask left between two adjacent openings. It stops solder bridging and must stay above the process minimum width.
• Can solder mask be printed over a via? Yes, and it usually is. Full tenting is the default for vias that do not need to be probed.
• Does mask clearance affect the electrical performance? Not directly, since the mask is a dielectric coating. It can affect impedance very slightly when it covers a controlled impedance trace, which is why impedance models include a mask correction.

Summary

Solder mask clearance is a set of three interacting numbers: the opening around the pad, the dam between openings, and the registration tolerance of the printing process. They exist because the mask has to protect the board and simultaneously stop solder from travelling between joints, and on fine pitch parts there is barely enough space to do both.

The convention used on each pad – copper defined or mask defined – should be a decision rather than a default, because it changes the solderable area and the mechanical anchoring of the pad. Vias are the same problem in a different shape, which is why tenting, plugging and open vias all have a place. Getting these right is part of the same review that covers the legend, the layout clearance rules and the assembly process, and confirming them with the fabricator before release removes an entire class of avoidable defects.