Successful BGA routing depends less on pushing density limits and more on making fabrication-aware decisions early in the layout process.

For a long time, I have wanted to provide engineers with straightforward, specific guidance when starting a ball grid array (BGA) layout to complement the overall guidelines from many PCB fabricators. BGA routing often appears straightforward during layout, but many of the real challenges emerge later during fabrication, assembly, testing or field use. A design may pass CAD checks but still cause avoidable manufacturing problems if routing decisions are made without considering how the board would be built. For engineers new to BGAs, the objective should not be to maximize density or use advanced techniques prematurely. The goal is to apply disciplined design choices that are manufacturable, reliable and scalable.

The first factor to evaluate is the package pitch. Pitch determines how easily signals can escape the device and what routing strategies are realistic. At 1.0mm pitch, routing is relatively simple, with ample channel space and conventional fan-out methods working well. At 0.8mm, designs remain manageable but require more intentional planning. By 0.65mm, routing density increases enough that a clear breakout strategy is needed. At around 0.5mm pitch, high-density interconnect (HDI) techniques such as microvias, blind/buried mechanical vias and sequential lamination often become necessary to use innerlayers to relieve surface congestion. At 0.4mm pitch, HDI is typically unavoidable, and forcing conventional methods usually creates downstream manufacturing issues. Once a 0.35mm pitch is reached, engineers will need HDI and most certainly every layer interconnect (ELIC) buildups.

A common mistake is designing for the tightest trace and space capabilities available rather than the most robust. Although some suppliers can process ultra-fine geometries, manufacturability and yield often improve significantly when designs remain at 3mil trace and 3mil spacing or larger. Conservative geometries provide process margin, improve portability between fabricators, and reduce cost and yield risk. Tighter features should be reserved for designs that truly require them.

Another common mistake is simply reducing the diameter of the through-holes to permit space to reroute the breakout. To maintain manufacturability, I recommend a minimum 6mil finished hole size/8mil drilled hole. This will permit the widest global manufacturing capability.

Escaping signals from the BGA marks the beginning of routing complexity. Larger-pitch packages are commonly handled with dogbone fanouts, in which vias are placed just outside the pads, and traces are routed outward. As pitch decreases, via-in-pad structures become more practical because they permit signals to transition directly into internal layers and free surface routing space. Routing traces between pads becomes increasingly limited as the pitch shrinks. In many successful designs, a hybrid approach is used: dogbone fanout where possible and via-in-pad where necessary.

Approach via-in-pad solutions carefully. While attractive in layout, they shift complexity to fabrication because vias must be filled, planarized and plated reliably. Combining via-in-pad structures with aggressive trace and space dimensions compounds manufacturing risk and increases cost. When via-in-pad is used, the cap process adds an additional plating step, which generally requires a larger than 3/3 trace and gap. A good rule of thumb is to plan for a 3.5/3.5 trace and gap when working with via-in-pad. If spacing cannot permit this, then use caution and communicate directly with your PCB fabricator. For 0.5mm and especially 0.4mm pitch devices, via-in-pad may be necessary, but it should be used strategically.

When HDI enters the design, it should be part of the original plan rather than a late-stage correction. Microvias are commonly used to route signals from outer rows into innerlayers, preventing outer layers from becoming congested. More complex designs may require sequential buildup structures to maintain route ability. If HDI is added after routing difficulties arise, the result is often inefficient in-layer usage, compromised stackups and unnecessary complexity.

It is also important not to focus solely on fanout at the expense of signal integrity. Signals still require continuous reference planes, controlled impedance and clean return current paths. Every layer of transition introduces the need to consider returning to the current continuity. A clean breakout under the BGA provides little benefit if the signal path becomes electrically discontinuous deeper in the stackup.

Finally, passing design rule checks does not guarantee manufacturability. Designers should evaluate whether vias are right for board thickness, whether stacked microvias are truly needed, and whether pad-to-via relationships can be drilled and plated consistently. Early collaboration with the fabricator is especially valuable for designs at 0.5mm pitch and below.

Successful BGA routing is not about using the most advanced techniques available. It is about selecting the simplest structure that meets the electrical and mechanical requirements, then increasing complexity only when the design demands it. Conservative, fabrication-aware decisions made early in layout often prevent the most expensive problems later in production.

Jeffrey Beauchamp is director of technology & engineering at NCAB Group USA (ncabgroup.com); This email address is being protected from spambots. You need JavaScript enabled to view it.. He started his career in the PCB industry in 2003 at P.D. Circuits, now part of NCAB Group, and works with PCB customers to provide optimal solutions. His column runs quarterly.