At higher frequencies signal loss and noise is reduced when ground-return vias are placed close to the signal vias.

There is often a lively discussion when it comes to the importance of “ground” or ground-return vias for high-speed signals that travel from layer to layer in a PCB. Many claim that there are many ground vias that stitch together the various ground layers, so there is little concern about their exact location. Others will insist that the ground-return vias are important to both EMI/EMC and SI performance for high-speed signals. The real truth lies somewhere in the middle. It depends on the data rate of the signals, and the amount of signal loss and/or noise generated between the planes.

The basic issue is that when a signal travels from one reference plane to another, it may travel through a pair or more of board layers. The return current must also travel from one plane to another. If a nearby metal conductor (ground-return via) is provided, the current will spread out between the planes, using the natural displacement current of the capacitance between the planes. The distance the current will spread is determined by the board’s operating frequency, its dielectric thickness, and the amount of inductance associate with the return current path.

Current will always take the path of least impedance. This means the distance the current will spread depends on the impedance caused by the loop inductance of the path created by the signal via and the current return path. This spreading distance becomes very small at high frequencies (> 1 GHz) and any benefit from a ground-return via will only be realized if the ground return via is close to the original signal via.

Single Plane Pair Transition

We can start by examining the signal loss seen by a high speed signal traveling through a single plane pair, changing reference planes from one plane to the other. Figure 1 shows several configurations for the planes and potential ground-return vias. Figure 1a shows a signal via and a ground-return via connected to both ground planes. Figure 1b shows the configuration if one plane is ground and another plane is a power (or other) layer. Only one plane is connected to the potential return via in this configuration. Figure 1c shows the configuration when the potential return via is not connected to either plane, or if a second signal via is nearby the original signal via.

First, if we examine the loss for the signal, using S21 as a transfer function of signal “in” versus signal “out”, and we move a ground-return via (Figure 1a) to various distances from the signal via, we can see the impact in Figure 2. Frequencies below approximately 1 GHz are not impacted by the location of the ground-return via. However, higher frequencies have significant impact on the amount of loss to the signal. If we are using a 2 Gb/s signal, the first harmonic is at 1 GHz, the third harmonic at 3 GHz, etc. Figure 2 shows that the first and third harmonics are not greatly impacted by this return via. However, if a 6 Gb/s signal is used, the first and third harmonics are at 3 GHz and 9 GHz, respectively. Placing a ground-return via only 50 mils from the signal via can improve the 3rd harmonic by more than 1 dB, which can be very significant, especially for long trace lengths where losses, including dielectric loss, can have a major impact to the signal quality.

Figure 3 shows the impact of removing the ground-return via while keeping the return via configurations in Figures 1b and 1c. There is no discernable difference between these return vias and having no ground-return via. Clearly, other signal vias and power vias cannot be assumed to provide a return current path for the original signal via.

Multiple Plane Transitions

Now, lets consider a PCB where there are multiple layers – for example, a backplane PCB. We can perform the simulation again for any number of plane pair transitions. Figure 4 shows the signal loss as additional plane pair transitions are added. Three planes mean a 2-plane pair transition, and so on. As additional planes are added, the signal loss increases, especially at high frequencies.

When a ground-return via is placed in close proximity to the signal via, the loss can be improved, even for a greater number of plane-pair transitions. Figure 5 shows the impact of a ground-return via when the transition is all the way through a many layered PCB with no via stub. When a large via stub is present, and the signal simply transitions from one layer to the next, the results in Figure 6 show that a ground-return via can again help reduce signal loss.

EMI Effects

Another way for via transitions to impact EMI is for noise signals to be launched between planes and coupled onto other vias or connector pins some distance away. Again, the location of a ground-return via can significantly improve (reduce) the amount of this noise launched between planes. Figure 7 shows that the impact is greatest between 1 to 10 GHz, and above about 10 GHz the difference was minimal. Using the previous example, at 3 GHz, a ground-return via placed 50 mils from the signal via would reduce the noise injected between the planes by 6 to 7 dB, easily making a pass/fail difference in some systems.

Summary

The question of whether a ground return via needs to be placed close to a signal via can be resolved only when the frequencies of interest are known. At lower frequencies, these ground-return vias are not critical, and normal ground-to-ground stitching can be used to provide a suitable return path. However, at higher frequencies, the amount of loss to the intentional signal’s harmonics and the amount of noise injected between the planes (and potentially escaping the system metal enclosure) can be significantly reduced when a ground-return via is placed close to the original signal vias. Return vias that are not connected to both planes will not provide the needed improvement. PCD&F

References

1. Xin Chang, Bruce Archambeault, Matteo Cocchini, Francesco De Paulis, Vysakh Sivarajan, Yaojiang Zhang, Jun Fan, Samuel Connor, Antonio Orlandi, and Jim Drewniak. "Return via Connections for Extending Signal Link Path Bandwidth of Via Transitions,” accepted for publication in EMC Europe Symposium, September 2008.

Dr. Bruce Archambeault is an IBM Distinguished Engineer and IEEE Fellow; This email address is being protected from spambots. You need JavaScript enabled to view it..