A PCB can pass electrical design review and still fail in production.
In many electronics projects, soldering defects are not caused by poor assembly alone. They often start much earlier, inside the footprint, pad size, solder mask opening, or via placement. A few tenths of a millimeter can decide whether a board is easy to assemble or difficult to stabilize in mass production.
BGA packages are sensitive to pad size because the solder joint is formed under the component and cannot be visually inspected like a normal gull-wing lead.
A common design reference is that the BGA pad diameter should be about 70% to 80% of the solder ball diameter. For stronger solder joints, many designs use the higher end of that range.
In one case, a BGA device used solder balls of about 0.25 mm. The recommended PCB pad diameter was around 0.20 mm, but the actual design used smaller pads. This forced the stencil aperture to become smaller as well, reducing solder paste release. During reflow, insufficient solder volume caused hidden BGA open joints.
Design takeaway:
For BGA packages, do not only check the package outline. Confirm solder ball diameter, pad diameter, solder mask strategy, and stencil aperture together.
Via-in-pad is useful in some dense PCB designs, but uncontrolled via-in-pad on SMD pads creates assembly risk.
In one production case, a resistor pad included a via inside the soldering area. During reflow, solder paste could flow through the hole to the opposite side of the PCB. The result was insufficient solder on one electrode of the resistor, creating a weak joint and intermittent open-circuit risk.
For ordinary SMD pads, vias should not be placed inside the soldering area. If a via must be used near a pad, it should be properly filled, capped, or moved away from the wettable surface according to the assembly requirement.
Design takeaway:
Do not treat via-in-pad as a routing shortcut. On small passive components, even a tiny via can change solder volume enough to create poor wetting or tombstoning.
QFN, QFP, SOP, and power packages often use an exposed pad, also called an E-Pad, for grounding and heat dissipation. This pad improves thermal and electrical performance, but it also creates soldering challenges.
In one case, a power IC showed poor soldering on the exposed pad area. Investigation found vias inside the E-Pad region. During reflow, solder paste was pulled downward through the holes, leaving insufficient solder under the component.
For exposed pads, the preferred approach is usually a solid copper thermal pad with controlled solder paste coverage. If thermal vias are required, they should be designed with proper hole size and process treatment. Very large or poorly controlled vias can remove too much solder paste from the joint area.
Design takeaway:
Thermal performance and solderability must be balanced. More vias do not automatically mean a better design.
For standard IC packages, each pin should usually have consistent pad geometry, solder mask opening, and stencil aperture strategy.
In one LGA case, functional testing failed on several boards. Reheating and pressing the IC temporarily removed the failure, which pointed toward a solder joint issue. Further review found that some PCB pads were larger than others, while the stencil apertures were uniform. This meant the same paste volume was printed onto pads with different copper exposure areas. Larger pads formed lower solder joints, increasing the chance of open connections under the package.
The defect rate in this case reached several percent during testing, making it a production-level quality issue rather than a random assembly defect.
Design takeaway:
For bottom-terminated components such as LGA and QFN, visual inspection is limited. Pad consistency is critical because solder joint height cannot be easily verified after assembly.
Solder mask design is often overlooked, but it has a direct effect on solder bridging and solder volume control.
For ordinary SMD pads, the solder mask opening should not be smaller than the copper pad. A typical expansion may be around 0.05 mm to 0.10 mm per side, depending on the process capability and component pitch. However, for fine-pitch ICs and BGA areas, too much expansion can remove solder mask dams and increase short-circuit risk.
In one LGA case, a large combined solder mask opening was used instead of individual openings for each pad. The traces and copper areas between pads became exposed, causing inconsistent wettable areas. After SMT assembly, the component developed hidden soldering defects.
Design takeaway:
For LGA, QFN, fine-pitch ICs, and dense pads, solder mask dams are part of the soldering design—not cosmetic details.
Small components need enough clearance for placement tolerance, solder paste spread, and inspection.
In one PCB layout, adjacent SMT components were placed too close together. Some gaps were only about 0.12 mm. After reflow, nearby pads and components had a high risk of solder bridging or electrical shorting.
As a practical guide, common chip component spacing should be reviewed according to package size and process capability. Fine components such as 0201, 0402, and 0603 require controlled pad dimensions and spacing. Mixed areas around ICs and irregular components should receive extra DFM attention.
Design takeaway:
If the board is dense, do not rely on CAD clearance alone. Assembly clearance and solder behavior must also be checked.
Before sending a PCB to fabrication or assembly, review these items:
PCB pad design is not just a footprint library task. It is a manufacturing decision.
A pad that looks acceptable in CAD may still cause solder starvation, floating, bridging, tombstoning, or hidden open joints in production. The best time to find these risks is before the first build, not after functional testing fails.
At NexPCB, engineering and manufacturing teams review PCB layouts from a DFM perspective before production. This helps hardware teams reduce soldering defects, improve yield, and move from prototype to production with fewer surprises.