Solder mask expansion requirement!

I often come across suggestions for 2-4 mils of solder mask expansion, but I’m curious about the rationale behind it. Why is this expansion necessary?

Hardware engineers design towards ideal materal and process conditions but PCB fabrication is not a perfect process. Allowances need to be built into the design to allow for small variances that are bound to occur. This applies to more than solder mask but in the case of solder mask, the expansion amount allows for slight misalignment during application with the intent that solder mask is not applied where it is not wanted (typically on solderable pad surfaces or holes that need to stay open).

The amount of mask expansion is usually detemined by component lead pitch in relation to PCB fabricator’s capabilities. I consider 3 mil (per side) expansion to be typical industry capability and many fab shops can also provide 2 mil (or less) expansion (sometimes at extra cost) which are typically preferred for 0.5mm or smaller lead pitch packages.

1 Like

This ensures the pad is completely exposed allowing the solder to make contact with both the top and sides of the copper feature –creates a stronger three sided joint. Also helps contain the solder so bridging and shorts are prevented.

1 Like

Theoretically, if the solder mask expansion were set to zero and everything aligned perfectly, the board could function correctly. However, in practice, perfect alignment is rare. Variations like solder mask shrinkage and movement during fabrication can cause misalignment. If the solder mask expansion is insufficient, these misalignments can result in partial or complete overlap of the solder mask with SMT pads and through-hole pads. If the solder mask completely covers most or all of the pad, it can lead to complete disconnection of the SMT component from that pad, causing the board to fail the end-of-line go-nogo test.
Many designers adhere to IPC’s fillet recommendations when designing pad footprints. If the solder mask partially covers these pads, the resulting solder fillet may be smaller than expected. A small fillet compromises the mechanical attachment of the SMT or through-hole part. Over time and through vibration cycles, solder may crack, leading to complete disconnection of the part from the pad or hole, which can lead to noticeable issues for the customer. This scenario is far more problematic than a board failing an end-of-line go-nogo test.

1 Like

Various factors contribute to errors in the plotting and placement of different layers and holes in a PCB. The capabilities and yield of the board house are crucial considerations, and they typically provide guidance on the allowances needed. For instance, minimum annular ring is specified when drilled holes are significantly off-center, potentially leading to issues with plating to the pads. Solder mask clearance ensures that even in worst-case scenarios of mask placement offset, the pad remains uncovered.

In simple prototype scenarios, default numbers may suffice, and any clearance violations can be accepted by the board house. However, for high-cost boards or large production runs, precise clearance numbers tailored to the board house’s capabilities are advisable. It’s worth noting that board houses may offer different classes with varying tolerances, accompanied by different pricing structures. Unless extremely tight registrations are essential for your product, opting for the most lenient clearance numbers that meet your budget constraints is prudent.

1 Like

Solder mask layers are typically designed slightly oversized to accommodate potential mask shrinkage, movement during fabrication, and minor inaccuracies. It’s crucial, especially for designs involving QFN or LGA packages and components with fine pitches, to ensure that the solder mask does not overlap with the SMD pads. In such cases, if the solder mask covers the pads, even slight registration issues could significantly reduce the solderable area of these small pads, causing potential assembly challenges.

1 Like