Tom’s Circuits – How to Save PCB Prototype Build Time for Designs with Vias in BGA Pads

October 2, 2017 , in Blog, Tom's Circuits

Manufacturing speed is critical for rapid prototyping. Did you know that via-in-pad increases board fabrication time? And when designs have both via-in-pad and blind vias, an extra 4 to 5 days can be added to fabrication time. For PCB prototype builds with vias in BGA pads, get a speed benefit by avoiding via-in-pad using BGA dogbones instead.

Via-in-pad Construction

Via-in-pad saves room and improves the performance of a PCB assembly, especially when blind vias are used. To make via-in-pad possible, the board fabrication process includes a step to plate the via holes, fill the plated vias with epoxy, and then cover the whole via with plated copper. These via-in-pad plated-over (VIPPO) steps take extra time. If you are in a hurry for your prototype build, you can skip the via-in-pad design feature to save time.

A typical via-in-pad stack-up uses small vias to route signals from the topside to layer 2, and another single-layer via on the bottom. All other inter-layer connections use a standard through-via. The small vias help with signal and power integrity, due to their short length. For example, a signal from the topside to layer 2 does not have extra length penetrating the board from layer 2 to the bottom side. This extra length forms a “stub” that can cause signal integrity problems in very high speed circuits.

PCB Space Benefits for Via-in-pad

Circuitry is more compact using via-in-pad:

The VIPPO blind via process can use a smaller diameter hole, because the drill depth is smaller. The minimum diameter of machine-drilled or laser-drilled holes increases as the board thickness increases. The thin layer between the topside and the second layer allows the minimum drill size to be used.

The space-saving and performance advantage of via-in-pad construction makes it a popular choice, until the boards need to be built! Costs are higher, and the turnaround time is longer. If through-vias can somehow be used instead, it is worthwhile to save the time and money by using them.

PCB Space Costs for Through-Vias

To connect a part on the topside to an inner layer, a regular via needs extra room for a larger hole. In addition, room is taken up by the hole’s annular ring, plus the minimum distance from pad to via for the solder mask web. The solder mask provides a dam that blocks the solder from flowing from the surface mount pad and down into the via hole during soldering.  In addition to gravity, the surface tension of liquid solder causes the solder to be sucked into the hole during soldering.

A through-via also creates an obstruction through the board’s inner layers, plus it requires yet more room on the backside of the board.

In Ball Grid Array (BGA) layouts, space is at a premium. The routing underneath BGA parts gets dense. As BGA parts continue to shrink, with decreasing pin-pitch and pad size, it is more challenging to find room for through-vias. Part of the problem is with the minimum annular ring size. For IPC Class 2 boards, the annular ring must be 0.004″ larger than the drilled hole. This makes the annular ring 0.008″ larger than the drilled hole. For a 0.006″ hole, the smallest hole that can be mechanically drilled, the minimum pad size is 0.014″.

Via Aspect Ratio

The via aspect ratio is the ratio of the drill depth to the drilled hole size. This limits the application of laser-drilled vias to use only the outer pair of layers.

The limit of the standard drilling process is a 10:1 aspect ratio, and the limit of the advanced drilling process is 20:1. Laser-drilled holes have an aspect ratio limit of 2:1. This limits the application of laser-drilled vias to use only the outer pair of layers.

The Reason for Annular Rings


When using the smallest possible drill and pad, there is a chance that one or more holes will slightly overlap the edge of its pad. This is shown in an exaggerated way in the breakout illustration. Breakout is rare, but when designers push the limits, this can happen to the smallest drills and pads.


When using the smallest possible drill and pad, there is a chance that one or more holes will slightly overlap the edge of its pad. This is shown in an exaggerated way in the breakout illustration. Breakout is rare, but when designers push the limits, this can happen to the smallest drills and pads.


The problem occurs when the breakout is in the same direction as a trace entering the pad. When the hole overlaps the trace, there is a chance of an open circuit or a fragile connection that could crack later. This lowers board yield, increases cost, and lowers reliability.


This problem can be helped by using teardrops. This pad shape extends the size of the pad but only in the direction of the trace. This acts as a larger pad but does not use any additional layout space.

A teardrop pad can help push the process limits for the smallest possible annular ring without increasing cost.

Some CAD tools don’t have the capability to add teardrops. In this case, the board manufacturer might be able to add them to your design.

The result is a BGA layout with dogbone shapes. The amount of copper added to make a teardrop dogbone is small—the drawings above are exaggerated. Teardrops are often barely visible to the naked eye.

When designing prototypes, think about your schedule and the extra 4 or 5 days that via-in-pad and blind vias will add to your fabrication time. Only use them if they are important to your design. In many cases they can be eliminated, especially in early prototypes before feature-creep makes the board more crowded.

Click here to learn more about Tempo Automation or to request a quote.

The latest PCB news delivered to your inbox.

Search Sign In