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
Typically, a solder mask expansion of 2-4 mils is recommended, but the exact value can vary depending on the manufacturing process and capabilities of the PCB fabricator.
For example, silk screen solder mask application is the most rudimentary method, often requiring larger solder mask expansions to account for alignment inaccuracies. Liquid Photo-Imageable (LPI) solder mask offers a more refined result, while laser direct imaging (LDI) of LPI can achieve the highest precision, potentially allowing for minimal or even zero solder mask expansion.
Additionally, the minimum width of solder mask between pads, known as the solder mask sliver, also depends on the fabrication process and the manufacturer’s tolerances. This is particularly crucial in designs with fine-pitch components, where a narrow solder mask sliver might be needed, or even omitted altogether, depending on the lead pitch and the manufacturer’s capabilities.
When determining pad dimensions relative to IC lead dimensions, it’s best to follow the package manufacturer’s specific guidelines to ensure the appropriate soldermask expansion. Sometimes, these are not included in the main datasheet and require further research in supplementary documents. If no specific guidance is available, you could refer to another manufacturer’s recommendations for a similar package or use a tool like Altium’s IPC footprint wizard, which calculates pad dimensions based on IPC standards and various input parameters.
Always check with your PCB manufacturer for their specific design rules to ensure compliance and avoid potential issues during fabrication.
2 Likes
Pad dimensions refer to the physical size of the pads on the integrated circuit itself, such as the width and length of the pins. For example, a QFN package might have pad dimensions of 0.2mm wide by 0.4mm long
PCB pad dimensions, on the other hand, define the land patterns or footprints on the printed circuit board, which need to be larger than the IC pad dimensions. This ensures that the component pins can be properly soldered onto the board, allowing space for the solder to adhere to both the top and sides of the pads. For the same QFN example, a PCB pad might measure 0.4mm wide by 0.6mm long, but these dimensions should ideally follow IPC standards or the package manufacturer’s recommendations.
The solder mask defines the area where solder should not adhere, so it’s important to leave an expansion zone around the pads to prevent the solder mask from encroaching onto the pad area. This is known as solder mask expansion, typically ranging from 2-4 mils (or more, depending on the manufacturing process). The expansion compensates for alignment variations during fabrication and ensures the solder mask does not interfere with solderability, especially for fine-pitch components like QFN or LGA packages.
Always consult your PCB fabricator’s design guidelines and the IPC standards to ensure correct pad and solder mask dimensions, as these will vary depending on the fabrication technology used, such as LPI or laser direct imaging. Proper soldermask expansion is crucial to maintaining reliable solder joints and ensuring robust mechanical attachment, especially in high-reliability applications.
2 Likes
Solder mask expansion is primarily determined by the accuracy of the alignment between the solder mask and the copper pads during fabrication. This includes compensating for any slight expansion, shrinkage, or misalignment that occurs in the mask during the application process. The key is to ensure that the solder mask doesn’t accidentally cover any part of the pads, which could interfere with soldering. Therefore, the soldermask expansion should be at least as large as the maximum mask misalignment your PCB manufacturer guarantees.
However, there’s a balance to maintain. If you set the solder mask expansion too high, you might lose the solder mask between adjacent pads. Most fabricators will specify a minimum solder mask “web” or “sliver” width between pads, and if the pad spacing is too tight, you could end up with no solder mask between them. For example, if the mask expansion and pad spacing don’t leave enough room for the minimum web (typically around 4 mils), the solder mask between pads may be omitted entirely.
In some cases, especially with fine-pitch components like ICs, missing solder mask between pads may not be a major issue for experienced assemblers who have fine-tuned processes. However, for components like chip resistors or capacitors, where mask between pads is more critical, it’s worth adjusting your pad dimensions and expansion to ensure mask retention. Always consult with your PCB fabricator to confirm their specific tolerances and adjust accordingly to avoid assembly issues.
2 Likes
Thanks everyone!
Solder mask expansion is crucial to prevent solder bridges between closely spaced pads and ensure smooth reflow soldering, commonly used for SMD boards. It also serves other purposes, such as protecting surface traces from shorts and corrosion. Setting the solder mask expansion to zero is risky, as fabrication tolerances could result in the mask partially covering pads, leading to soldering issues. For less dense PCB designs, a safe expansion of around 0.1 mm is typically sufficient. For high-density PCB designs, It is usually use 0.05 mm to avoid clearance problems.
When designing new footprints, It is usualy recommend leaving the solder mask expansion set to Expansion value from rules and applying a general rule across the board. This way, you can easily adjust the mask expansion for all pads if needed during the design process.
2 Likes