Solder mask bridges: what they are and why they matter

The mask layer describes openings, not ink

Solder mask covers and protects most finished copper. In Gerber data, F.Mask and B.Mask normally describe the places where mask must be removed: pads, exposed test points, and deliberately untented vias. This negative convention causes a common mistake—adding a shape to a mask layer exposes more copper; it does not paint extra mask.

A solder mask bridge, also called a dam, web, or segment, is the strip of mask left between two adjacent openings. On a fine-pitch IC, a surviving web separates neighbouring pads. It can reduce solder bridging during paste print and reflow, protect copper between pads, and make rework cleaner.

It is not the same as copper clearance. Two pads can meet the electrical copper-spacing rule while their enlarged mask openings overlap and remove the web.

Calculate the drawn web from the openings

Suppose adjacent copper pads have an edge-to-edge gap of 0.20 mm. If each pad uses a positive 0.05 mm solder-mask expansion, each opening extends 0.05 mm into the gap:

drawn mask web = copper pad gap - 2 × mask expansion
drawn mask web = 0.20 mm - 2 × 0.05 mm = 0.10 mm

That 0.10 mm is only the nominal data. The mask process has registration and imaging tolerances. A fab may require a larger pad-to-pad gap to guarantee a smaller finished web, or it may remove webs below its process threshold rather than print fragile slivers.

Negative expansion shrinks an opening and can create more web, but it also risks mask encroaching onto the solderable pad when registration shifts. Do not shrink openings simply to make the preview look separated without checking the fab’s minimum mask-to-copper opening and registration rules.

Published limits vary by process and colour

There is no universal web width. Eurocircuits publishes a 0.075 mm minimum mask segment for several direct-imaged colours, along with separate opening, overlap, and pad-to-pad design values. Its white photo-imageable process uses larger numbers.

PCBWay’s solder-mask guidance says its required spacing between IC pads depends on mask colour and copper weight; its cited standard values are larger for non-green colours. These pages describe different equipment and rule definitions, so the figures should not be compared without reading the accompanying conditions.

Check the current capability for the exact service, colour, copper weight, and feature location. Green is often the most capable or forgiving low-cost option because it is the baseline process, but the order’s published matrix is the authority.

Configure mask behaviour in KiCad

KiCad can apply solder-mask clearance globally and override it in a footprint or individual pad. In PCB Editor, review the board’s solder mask/paste settings, then inspect footprint and pad properties for local values. The most specific applicable setting wins.

Positive mask clearance expands the opening beyond copper. KiCad’s minimum mask web setting can merge nearby apertures when the segment would be too narrow, representing the decision that no reliable dam should be drawn there. This is often preferable to sending an impossible sliver and leaving CAM to alter it silently.

For a standard library footprint, compare its mask behaviour with the exact manufacturer’s land pattern and chosen fab. For a custom fine-pitch footprint, inspect every side of the package. Thermal pads, via-in-pad structures, and irregular pads may need local settings rather than one global expansion.

Do not use mask settings to repair a wrong copper land pattern. Pad size and spacing must first satisfy component, assembly, and electrical requirements.

Understand KiCad’s DRC message

KiCad can report Solder mask aperture bridges items with different nets. It means one continuous mask opening exposes copper belonging to more than one net. That can be intentional on a package whose pitch is too fine for a manufacturable web, but it deserves assembly review because solder can move across the shared exposed region.

Select the marker and identify the involved pads. Then decide:

1. Is the footprint correct for the exact package?
2. Did excessive mask expansion merge openings unnecessarily?
3. Can the selected fab reliably produce a web at this pad spacing?
4. If not, is a shared opening expected for this package and paste process?

Exclude the DRC marker only after those questions have documented answers. The broader DRC violations guide explains why exclusions should remain reviewable.

Fine pitch sometimes works better without a dam

For very fine-pitch QFP, QFN, LGA, or similar parts, there may be too little room for a useful mask web. Combining apertures across a row of pads can be a normal manufacturing choice. Solder-bridge control then relies more heavily on correct copper lands, stencil aperture design, paste volume, placement, and reflow profile.

Do not demand a 0.03 mm mask sliver because it appears in CAD. A web below process capability may break away, misregister over a pad, or be removed during CAM anyway. Use an intentionally merged opening that both designer and assembler expect.

Conversely, do not merge all openings globally to silence one package. Coarser-pitch pads benefit from individual apertures and the protection between them. Apply the exception at the footprint or pad level.

Vias and test points are mask decisions too

A tented via has no mask opening on the covered side. KiCad 9 supports board-level and per-via tenting control for top and bottom independently. Tenting is not the same as filling or plugging; ordinary mask can span a small opening but does not create a structurally filled via.

Keep intentional test points exposed and large enough for the probe. If a via near a surface-mount pad is left open, it can wick solder depending on its position and process. Via-in-pad generally needs a specified filling and capping process, not just a mask tweak.

Inspect mask Gerbers before release

Open F.Mask and B.Mask in a Gerber viewer with their copper layers. Verify:

• every solderable pad has the intended opening;
• fine-pitch rows use deliberate separate or merged apertures;
• mask does not expose neighbouring traces;
• tented and exposed vias match the order;
• mask openings do not cross the board edge unexpectedly;
• both sides are present when required.

Then inspect the fabricator’s preview, which may show CAM normalization. If thin webs disappear, compare the result with the capability and assembly plan before approving. Include this review in the pre-order DFM checklist, alongside copper rules from the trace and clearance guide. A mask bridge is useful only when it is wide enough to survive the actual process.