Contact Us
  • Home
  • BLOG
  • How Wide Should the Solder Mask Dam Be Between Pads?

How Wide Should the Solder Mask Dam Be Between Pads?

The dam between two pads is 3.5 mil (0.089 mm) on green, blue, red or yellow mask, 5 mil (0.127 mm) on white and black, and 4 mil on the colours in between. On HDI the floor drops to 50 micrometres. What decides whether a board can hold a dam is not the dam number but the gap it has to live in: the dam is the copper gap minus the mask expansion on both sides. At 0.50 mm pitch with 0.30 mm pads the copper gap is 0.20 mm, and with 0.05 mm expansion per side the dam is 0.10 mm. That clears the green floor by 11 micrometres and misses the white floor by 27, which means the mask colour chooses the pitch wall, not the footprint.

Where the dam comes from, and where it goes

A liquid photoimageable mask is printed over the whole panel, dried, exposed through artwork and developed in a 1 percent sodium carbonate spray. The developer removes ink that was not exposed, and it removes it from both faces of the opening at once. A sliver 0.05 mm wide has almost no contact width against the laminate and is undercut from both sides before development is finished, so it either leaves the panel in the developer or stays as a loose tongue that breaks off later in reflow or in cleaning and lands on a pad.

The cured film is only tens of micrometres thick over a trace, so it has no mechanical strength of its own. What holds a dam in place is adhesion to laminate on both sides. Below roughly 0.1 mm that adhesion area is smaller than the tolerance band of the exposure unit, and the dam stops being a feature that can be guaranteed and becomes a feature that happens to survive. That is why our numbers are floor values with the ink colour attached: pigmented ink needs more pigment loading, more pigment means more scatter during exposure, and scatter eats the narrowest features first.

The arithmetic by pitch

Take a mask expansion of 0.05 mm per side, which is the middle of what most footprints use, and subtract twice that from the copper gap.

Pitch Pad Copper gap Dam left What holds
1.27 mm0.60 mm0.67 mm0.57 mmany colour
0.65 mm0.40 mm0.25 mm0.15 mmany colour
0.50 mm0.30 mm0.20 mm0.10 mmgreen, red, blue; not white
0.40 mm0.20 mm0.20 mm0.10 mmgreen only, no margin
0.30 mm0.15 mm0.15 mm0.05 mmnone, single opening

Two conclusions follow. The first is that 0.40 mm pitch is the practical boundary for a green mask with a standard expansion, and it is a boundary without margin: a change from 0.05 to 0.06 mm per side takes the dam to 0.08 mm and under the floor. The second is that a white or matte black board at 0.40 mm pitch cannot hold a dam with that expansion at all, which is why the colour is a process decision on dense boards and not a cosmetic one.

Why a dam that survives fabrication can still fail at reflow

The dam does one job: it keeps molten solder on the pad it was printed on. Solder at 240 degrees wets copper readily and will travel along a copper path if there is one, so the dam has to be continuous, adhered and tall enough to interrupt that path. On a board with 2 oz copper the trace shoulder is a step of about 70 micrometres, the ink thins over the shoulder, and a dam that crosses the step is thinner exactly where the solder arrives first.

The other failure is undercut. A dam etched to 0.09 mm with a 0.02 mm undercut at its base has 0.07 mm of contact on each side and a free top, and the differential expansion between ink and laminate through three reflow passes works that edge until it lifts. Once it lifts, the gap between the pads is open and the next board on the line bridges.

Three ways the dam is lost before the panel

Choosing white or matte black for a dense board. The floor moves from 3.5 to 5 mil and the dam available at 0.40 mm pitch does not move with it. The mask shop will not decline the order; it will remove the dam and produce a single opening, and the bridging appears at the assembly stage where it costs the most.

Leaving a 4 mil expansion in the footprint library. Several CAD defaults still carry 0.1 mm per side. On a 0.40 mm pitch part with a 0.20 mm copper gap, 0.1 mm per side consumes the whole gap: the two openings merge into one, the dam is zero by construction, and no fabrication choice can bring it back. Expansion of 0.05 mm per side is enough for our line and keeps 0.10 mm of dam.

Using a zero expansion to buy a dam. Setting the opening equal to the pad turns every pad into a mask-defined pad, and any registration error then covers part of the copper. A pad that is half covered still passes electrically and fails at assembly, because the paste has nowhere to sit and the joint forms on the mask edge.

What SUPERB PCB holds

Mask colours on the standard line are green, blue, red, yellow, white, black and matte black. Mask opening is 1.5 mil minimum; dam width is 3.5 mil (0.089 mm) on green, 5 mil (0.127 mm) on white and black, 4 mil on the other colours, and 50 micrometres on HDI. ENIG pad to pad spacing is held at 5 mil or more because immersion gold bleeds under the mask edge, and via plugging is held to 10 micrometres of recess so a filled via in a pad is flat enough to print on. The values sit alongside the rest of the tolerance table on the FR-4 process parameters page.

The boundary worth stating: at 0.30 mm pitch the dam is not a process option on any colour, and the choice is a single opening with a stencil that controls paste release, or a via-in-pad layout that moves the connection out of the pad row. SUPERB PCBA prints both, and the decision belongs in the stencil and the land pattern, not in a note asking the mask shop to try harder.

What to send with the order

Smallest pitch and pad width on the board, mask colour, the expansion value in the footprint or a preference for mask-defined versus copper-defined pads, copper weight per layer, whether vias sit inside pads, and whether the assembly is cleaned after reflow. Six items, and the dam question is answered before the panel, where a 0.02 mm change in expansion costs nothing.

Need a quote or a review of your files against these criteria? pcba@superb-tech.com · WhatsApp +86 133 9608 1443