Skip to main content

Minimum Solder Mask Dams in SMD Components

PCB soldering

Solder mask is important for more than just protecting your PCB, it is one of the factors that can ensure accurate assembly of a PCBA. Solder mask sizes and settings are two of those things we often set to some default values in design rules inside PCB design software applications. Because of this, the solder mask is sometimes not seen for its value in assembly. In reality, the solder mask starts to become an important assembly and layout tool once SMD pad and lead pitches become small.

When lead pitches are small, assembly concerns start to dominate and the solder mask needs to be sized carefully. In particular, the solder mask dam could be too small in cases with small lead pitch, particularly when solder mask expansion is applied around a pad by default in a PCB layout. This article will look at ways to overcome the problem of small solder mask dams in a PCB such that assembly can be assured.

Solder Mask and Lead/Pad Pitch

In surface mount devices, pad pitch refers to the distance between neighboring SMD pads on a PCB, and lead pitch is the distance between neighboring leads. SMD component packages might have extended leads, leadless packaging with bottom-side pads, gullwing leads, or they may be packaged as a ball grid array (BGA). In any case, there will generally be some specified distance between the pads based on the component package.

Due to tiny package sizes used in SMD components, a process is needed to develop component footprints and land patterns to ensure accurate assembly. Machines used in modern surface assembly are entirely automated, but the land pattern and surrounding features in the PCB (solder mask, silkscreen, dam placement, etc.) can still cause solder defects during placement and soldering of components during PCB assembly.

Package type

Minimum lead pitch


Multiple lead pitches, as low as 0.4 mm


Smallest ball pitch is less than 0.5 mm


1.27 mm


1.27 mm


Multiple lead pitches, as low as 0.4 mm

The list above is short, but it covers a huge range of components that appear in standard packaging. Two related parameters that determine the required processing capabilities in assembly are the pad/opening sizes required in a bare PCB. Each of the packages listed above needs a particular footprint, which includes a definition for a solder mask opening around the pad. Based on the lead pitch, which solder mask opening size should be used in a component footprint?

Solder Mask Opening Size

The solder mask is simply an area around an SMD pad in the PCB layout where solder mask is not present. Solder mask is always applied to professionally built PCBs, with the primary goal of protecting conductors and preventing solder bridges across component leads.

When creating footprints and setting the design rules in a PCB layout, the solder mask opening will need to be set to satisfy two goals:

  • To provide a dam between component leads that prevents reflow
  • To ensure there is enough copper even if some misregistration occurs
  • To define the size of the solderable area in non-solder mask defined pads

By default, a PCB CAD application will typically apply a solder mask opening that is 3-4 mils larger than the SMD pad. An example for an SOIC package is shown below.

Solder mask opening

The solder mask outline is generally larger than the SMD pad on most components, and it can be set to a default value in your PCB footprints.

This is fine for larger lead/pad pitch values, such as the SOIC or SOP packages listed above. When the spacing between pads gets too small, the solder mask opening needs to be smaller. This is because the leads force the landing pads to be closer together, so the solder mask dam between pads becomes smaller as well.

This brings up another question, particularly for designers searching for an assembly house that can scale up to volume production with high yield: what is the minimum solder mask opening size for SMD components? Lead pitches are specified in component packaging standards, but this will drive the land pattern in the PCB layout. A designer needs to know how much copper to expose for soldering as lead pitches approach their minimum values, and how small the solder mask dam can be between pads.

What Should Be the Minimum Solder Mask Opening?

The typical minimum dam size that can be accurately fabricated by a manufacturer is 4 to 5 mils. For a particular lead pitch, the minimum allowable solder mask dam between SMD component leads (or maximum aperture in the solder mask) is constrained by two factors:

  • The mechanical strength of cured solder mask films
  • The fabrication house capabilities

The fabrication house capabilities are further broken into a misregistration limit in the layer buildup, and the photoimaging limit during solder mask exposure. Usually, bare PCB manufacturers cannot ensure the retention of solder mask dams between pins when the pad size to pitch ratio decreases. Solder may flow easily across the surface of a PCB and connect neighboring pins if there is no solder dam. Short circuits can occur if the PCB is not designed properly for confined places, requiring the PCBA to be reworked by the assembler.

Large solder mask expansions can be applied without ever worrying about exceeding the capacity of the solder dam if the lead pitch is sufficiently large. It is also possible to go below the minimum solder mask dam size when the lead pitch is very narrow or when components are packed closely together. If that's the case, you'll have to make a call on whether you'd rather have some solder dam present at all times or prefer to compensate for misregistration.

Can You Always Have a Solder Mask Dam?

In an ideal world, solder would stay confined exactly on the pad where it was applied, and solder mask dams would not be needed. However, the world is not perfect, and we need solder mask dams to some extent.

The solder mask area that fills the gap between two SMD pads is most often called a solder mask dam. It acts as a buffer that helps confine solder on the pads where they are applied, thereby protecting neighboring leads on SMD components from being accidentally shorted. Solder mask dams between SMD pads are essential for fine-pitch ICs and should be included whenever practical. The issue involved here is in sizing the appropriate solder mask dam while ensuring there is enough exposed copper in SMD pads.

When there is insufficient room between pads, you have two choices:

  • Eliminate the solder mask dam entirely by removing solder mask between component pads
  • Set solder mask opening to zero (matches the pad size) or to a negative value (covers some copper on the pad)
  • Set a minimum solder mask dam between SMD pads of 1 mil to ensure there is always some dam

Depending on the expansion value applied on an SMD pad, the resulting dam thickness could be less than 4 mils. There is then a danger that the leftover solder mask will detach from the PCB and will break off from the solder mask film. These bits of solder mask that flake off the PCB are known as “slivers”, and they leave a possible path for bridging between two SMD pads.

How to Handle BGAs

BGA packages are typically used to securely mount large processors, including microprocessors for computers or networking equipment, as well as application processors and high pin count ASICs. The holes or aperture in the solder mask covering the BGA pads could be placed as solder mask-defined pads at small pitch, or as non-solder mask defined pads when the pitch is large enough to allow dog bone fanout.

1.0 mm pitch BGA

This 1.0 mm pitch BGA can work with non-solder mask defined pads, where the copper pad is totally exposed to soldering.

For a BGA, as the pitch gets smaller, you may need to switch to solder mask defined pads to ensure there is always a large enough dam and opening in the solder mask to place and mount components. This means expand the size of the pad, and reduce the size of the solder mask opening, while keeping the total exposed copper area constant.

Wrapping Up: What’s the Process?

To wrap up, it’s important to note that a footprint check process is needed in the PCB layout. You can still use your standard set of footprints, but the solder mask dam rule settings needed for different components can be targeted, or the rule can be modified in components individually as needed. We would suggest a process as follows:

  1. Set a default design rule for minimum solder mask dams of 1-2 mils to account for misregistration
  2. When the rule is violated on fine pitch components, reduce the solder mask opening size to 0 mil
  3. If the dam is still too small, apply negative opening size only up to the limit of the lead size

This will ensure you always have an exposed pad that matches the lead size, but in #3 you are vulnerable to misregistration and insufficient solder. Make sure you understand the risks of negative solder mask opening before setting this in your PCB layout.

The CAD features in OrCAD from Cadence are designed to give you full control over all the features in your PCB layout. OrCAD is the industry’s best PCB design and analysis software with utilities covering schematic capture, PCB layout and routing, and manufacturing. OrCAD users can access a complete set of schematic capture features, mixed-signal simulations in PSpice, and powerful CAD features, and much more.

Subscribe to our newsletter for the latest updates. If you’re looking to learn more about how Cadence has the solution for you, talk to our team of experts.