Soldering defects are one of the most common causes of PCB assembly failures. Many issues are often attributed to process parameters such as stencil design and reflow profiling. Pad geometry, copper distribution, solder mask definition, and via placement all play a critical role in how solder behaves during assembly.
The infographic above summarizes the most common soldering defects, their primary causes, and design strategies to prevent them.
The following sections elaborate on each defect and explain how design choices can significantly impact PCB soldering.
Tombstoning
It is a defect where one end of a surface-mount component lifts off the pad during reflow, leaving the component standing vertically. Tombstoning is most common with small passive components such as 0402 and 0201 resistors and capacitors.
The root cause is uneven wetting forces, which occur when one pad reaches solder reflow temperature before the other. Unequal pad sizes, asymmetric copper connectivity, and traces routed under only one side of the component all contribute to thermal imbalance.
To prevent tombstoning, match the pad dimensions for both terminals. Balance copper connectivity by maintaining similar trace widths and routing lengths to each pad. Use thermal relief spokes when pads connect to large copper pours or planes to moderate heat flow and ensure both pads reach reflow temperature simultaneously.
Solder bridging
It occurs when solder unintentionally connects adjacent pads, creating electrical shorts. Solder bridging is particularly common in fine-pitch components such as QFNs, BGAs, and high-density SMT packages.
Design-related causes include oversized pads relative to component pitch and insufficient solder mask dams between pads. Inadequate solder mask clearance or poor mask registration can allow solder to spread beyond the intended joint area.
To prevent solder bridges, use IPC-7351–compliant land patterns to define accurate pad geometry, especially for fine-pitch components. Maximize the solder mask dam between adjacent pads, targeting a minimum spacing of 4 - 5 mil as recommended in IPC-SM-782. Also, confirm solder mask registration tolerances with your PCB fabricator to ensure the mask openings stay properly aligned and remain effective even under worst-case manufacturing conditions.
Solder balling
Solder balling refers to the formation of small solder spheres around pads or components after reflow. It is often associated with paste printing or reflow profiling. Several design-related factors can significantly increase its likelihood.
One of the most common causes is via-in-pad outgassing. During reflow, trapped volatiles escape from open vias and eject molten solder onto the board surface. Moisture absorbed by the PCB or solder paste can further exacerbate this issue.
To mitigate solder balling, fill and cap vias placed within component pads using epoxy or resin-filled VIPPO structures. Maintain uniform copper weights across layers to promote even preheating and reduce localized outgassing. For moisture-sensitive designs, specify bake-out requirements in the fabrication notes per IPC/JEDEC J-STD-033 to further lower defect risk. Limit the number of vias in large thermal pads to reduce potential outgassing paths.
Excessive solder
Excessive solder results in overly large fillets, solder pooling, or unintended solder accumulation near joints. This defect may not always cause immediate electrical failure; it can lead to reliability issues such as solder cracking or bridging during thermal cycling.
Oversized pads are a primary contributor, as they inherently hold more solder paste than required. In through-hole designs, large annular rings can act as solder reservoirs during wave or selective soldering.
To control excessive solder, size pads according to IPC-7351C land pattern recommendations to regulate solder volume. For plated through-hole components, limit annular rings to approximately 5 mil to prevent solder buildup. Avoid placing large non-functional pads near solder joints, as they can unintentionally draw excess solder and cause bridging or uneven fillets.
Pad lift/delamination
Pad lift/delamination occurs when copper pads separate from the laminate during rework. This defect can render the PCB unrepairable.
Common causes include poor copper-to-laminate adhesion, contamination during fabrication, and repeated exposure to high rework temperatures.
To prevent pad lift and delamination, specify an appropriate copper thickness for your design. Use 1 oz copper for most standard boards, and consider 0.5 oz copper for fine-pitch HDI designs when approved by the fabricator. Request proper inner-layer oxide treatment in the fabrication notes to improve copper-to-laminate adhesion. For high-reliability designs, use teardrop pad geometries to better distribute mechanical and thermal stress at pad-to-trace transitions.
Insufficient wetting
It occurs when solder fails to fully spread across the pad and component lead. Insufficient wetting often leads to high contact resistance or intermittent failures.
From a design perspective, insufficient wetting is frequently caused by undersized pads, solder mask encroachment onto pad edges, or inadequate thermal relief for pads connected to large copper pours.
To prevent insufficient wetting, extend pads beyond the component lead on all sides. Maintain a minimum solder mask clearance of 1.6 mil to avoid mask overlap that can restrict solder flow.
Most soldering defects can be traced back to predictable, preventable design decisions. By following IPC-recommended land patterns, balancing copper distribution, controlling solder mask geometry, and documenting fabrication requirements clearly, designers can significantly reduce assembly defects before the board ever reaches the production floor.
Designing for solderability is not just an assembly concern; it is a critical aspect of PCB design for manufacturability and long-term reliability.