PCB Routing Tips: Navigating Your Way Through BGA Fanout Options

Spanning from standard through-hole builds to HDI, there are only a few BGA fanout routing options available to any designer. PCBs that include BGAs must account for the via size and trace size needed to route into and out of these components, placing important requirements on stackup design and manufacturability. At the higher end of the design spectrum, there are unique fanouts used in HDI which pack even higher numbers of traces into the BGA region.

This article looks at the common BGA fanouts in different BGA pitch ranges. The choice of fanout method has direct consequences for stackup construction, drill selection, and escape routing density. Getting this decision right early in the design process avoids costly respins and manufacturability failures downstream.

The Major BGA Fanouts

There are two primary BGA fanout approaches: dog bone fanout and via-in-pad. Which method applies depends on the via size the design can accommodate and the ball pitch of the BGA package. Coarser pitch packages generally allow dog bone fanout with standard through-hole vias, while finer pitches require via-in-pad solutions with microvias or mechanically drilled blind vias.

Dog Bone Fanout With Through Holes

Dog bone fanout is the standard approach for coarse-pitch BGAs, typically those with ball pitches of 0.8 mm or greater. In this configuration, a short trace routes from the BGA pad outward to a via that sits in the space between adjacent pads, with the pad-trace-via geometry resembling a dog bone. Through-hole vias are the norm in these designs because the ball pitch is wide enough to accommodate the via pad diameter and associated clearances within standard fabrication rules. The traces escape from the BGA field into routing channels on the same layer, then transition to inner layers through the via.

The required drill diameter depends directly on the board stackup thickness. A thicker stackup requires a larger drill to maintain a manufacturable aspect ratio, which is the ratio of board thickness to drilled hole diameter. Most fabricators set a maximum aspect ratio of 8:1 to 10:1 for through-hole vias, beyond which copper plating inside the barrel becomes unreliable. A 1.6 mm board at 10:1 sets a 0.16 mm minimum drill, but accounting for fabrication tolerance and annular ring requirements typically pushes the practical minimum higher. If the ball pitch is wide enough, this is a straightforward constraint to meet. Problems arise when the designer attempts dog bone fanout on a pitch that is too tight to clear the via pad, trace, and adjacent ball pad simultaneously within the design rules. At that point, the design must move to a finer via technology or a via-in-pad approach.

Dog Bone Fanout With Blind Vias

If design clearance constraints are tight and the required drill size will violate aspect ratio limits, it is possible to use mechanically drilled blind vias to fan out a BGA using the standard dog bone pattern. This can be a viable routing strategy when the required drill size becomes too small to accommodate the required clearances in a dog bone fanout pattern. This situation can occur when routing BGA fanouts where vias are required to have large annular rings.

Stackups that incorporate blind or buried vias in sub-laminations are built through sequential lamination, where sub-laminate layers are drilled and plated before the full stackup is completed. Because the blind vias are formed in a separate plating cycle from the through-hole vias, the board requires an additional plating step. This extra cycle adds copper to all plated surfaces, which increases finished copper weight in ways that can tighten trace and space tolerances on fine-pitch layers. It also places additional demands on drill registration and minimum drill size, since the sub-laminate layers are thinner and require tighter process control. Clearance requirements between blind via pads and adjacent features must account for the cumulative tolerances introduced across multiple lamination and plating cycles.

Via-in-Pad Fanout

Via-in-pad fanout is required when BGA pitch becomes too tight to route a trace from the ball pad to an adjacent via. At pitches below roughly 0.65 mm, the space between adjacent pads shrinks to the point where a dog bone escape cannot clear the annular ring of a through-hole via while maintaining the required trace-to-pad clearance. Placing the via directly in the center of the BGA pad eliminates the need for that short escape trace, freeing up space in the fanout region.

Via-in-pad designs can use through-hole vias, mechanically drilled blind vias, or laser-drilled microvias, depending on the pitch and the stackup. Through-hole via-in-pad is feasible for moderate pitches but requires the via to be filled and capped to prevent solder from wicking into the barrel during reflow. Unfilled vias in pad create unreliable solder joints and should not be used in production designs. Laser-drilled microvias are the standard solution for pitches at or below 0.5 mm, particularly in HDI buildup stackups. The aspect ratio for laser-drilled microvias is constrained to 1:1 or lower depending on the buildup dielectric thickness, which means the via depth is limited by the copper-to-copper distance across the buildup layer. A typical buildup dielectric of 75 to 100 microns sets the maximum microvia depth accordingly. When the via-in-pad approach is used with microvias, the via is typically laser drilled after outer layer imaging, then copper filled and plated flush before pad finishing. This produces a flat, solderable pad surface that behaves predictably during reflow.

Middle Ground: Blind Microvias in 0.5 mm Pitch BGA

There is a mid-range pitch value that enables dog bone fanout using blind microvias. This can be done in a 0.5 mm pitch BGA package, which would normally be below the threshold where mechanically drilled vias are no longer practical. An example with a Lattice Semiconductor microprocessor in a PGA package is shown below.

Dog bone fanout with microvias is possible as long as the microvias are sized correctly.

When pitch decreases further to values like 0.35 mm, microvias must be placed in the pad and plated over to allow soldering of the fine-pitch BGA. At this geometry, there is no room for any escape trace between the pad and the via, and the only viable structure is a filled, capped microvia directly under the ball pad.

More Advanced Fanout Routing

There are more advanced fanout routing options for HDI designs which can fit a larger number of vias in tight spaces. These can also provide cleaner routing channels between vias on inner layers, particularly for differential pairs. An example originally shown by Happy Holden is given in the image below.

In this example, two vias in a dog bone fanout are brought close together, nearly to the clearance limit for the copper pads on the vias. As can be seen in the images, this creates a row of vias between the pads and a clear routing channel between the vias on each layer. Stacked blind and buried vias can then continue to reach inner layers. This effectively doubles the number of traces that can fit in the fanout compared to the traditional dog bone fanout.

• Read more about this type of HDI fanout in this article.guidebook

Fanout Selection and Stackup Alignment

The fanout approach and the stackup must be designed together. A via-in-pad design with laser microvias requires an HDI buildup stackup from the start, which affects layer count, lamination sequence, material selection, and fabricator qualification. Define the BGA pitch requirements, via technology, and aspect ratio limits before the stackup is finalized, and confirm that the selected fabricator can meet the drill, plating, and fill requirements for the chosen fanout approach.

Whether you need to build reliable power electronics or advanced digital systems, use Altium’s complete set of PCB design features and world-class CAD tools. Altium provides the world’s premier electronic product development platform, complete with the industry’s best PCB design tools and cross-disciplinary collaboration features for advanced design teams. Contact an expert at Altium today