The Path of Least Impedance: How to Use Return Paths for Better PCB Design

High-speed signals don't follow the path of least resistance; they follow the path of least impedance. This article series provides thoughts on PCB design layout for your next project.

Yesterday’s electronics were rather forgiving. Bad schematic design and poor PCB layout would still produce a functional board. Skill can increase over time, but luck will eventually run out. 

When engineers first began working with solid-state electronics, chips operated at higher voltages with slower rise times than microchips made today. But in the push to make PCBs and microchips smaller, we’ve also reduced their operating voltages and subsequently their noise margins. As we continue to push to lower and lower IC operating voltages, engineers need to be increasingly mindful of their choices to ensure that their design works without costly and time-consuming redesign.

So what are some types of noise to look out for, and how do you improve your design to avoid them?

This article is one of several that were inspired by the keynote address, given by Dr. Eric Bogatin at Altium Live 2018.

Deliberately Route Return Paths! Propagation Delay

Electromagnetic fields run along and encircle conductors, and permeate objects in their vicinity. The energy that exists in those fields will be transferred somewhere in your circuit—hopefully in the location that you intend.

Changes in the electromagnetic field propagate at a fast but finite speed, and it takes some time for the changes in the field to reach the far ends of your circuit.

When playing with simple circuits and looking at schematics on a page, many people imagine the changes in the circuit happen immediately: a switch is pressed and a light appears to shine instantly. It is easy to develop a false intuition that the change in switch state immediately changes the light state. 

 

 

The misconception occurs because the changes in state exceed the limits of human perception by many orders of magnitude. When dealing with circuits where the time for the changes to propagate (propagation delay) are comparable to or exceed the time it takes to change state (rise-time/fall-time), you must clarify your thought process to accommodate propagation delay.

Changes in electromagnetic fields will propagate throughout your circuit at a fraction of the speed of light. A change of state (logic low to logic high) on a PCB trace establishes an electric potential along the length that generates electrical current. That electrical current creates an electromagnetic field around the conductor. But since it takes time for changes in electromagnetic fields to propagate, it is possible for two ends of a trace to be in two different states, with a transition point that moves along the length. 

Inductive and capacitive coupling instantly create a return circuit for the current.

This diagram shows two conductive traces on opposite sides of a PCB. When a current starts to flow in the top trace, a return current is immediately established in the bottom trace.

 

If you do not provide an immediate return path near your traces and vias, unwanted currents will form in nearby conductors, especially if you have quick transitions (<1ns).

Best practices dictate the following: Always provide a ground return path in the same layer or an adjacent layer for single-ended signals, differential pairs, and power planes.

Always provide a ground return path in the same layer or an adjacent layer for single-ended signals, differential pairs, and power planes.

 

Ground return via. Image from " by Dr. Howard Johnson from "High-Speed Signal Propagation", Fig. 5.33, p. 353. via Signal Consulting, Inc.

High-Speed Signals and the Path of Least Impedance

High-speed signals don't follow the path of least resistance; they follow the path of least impedance.

When new engineers design PCBs, their tendency is to completely forget about the reactive part of impedance in their circuit return paths and focus strictly on the resistive. When old engineers design PCBs, they tend to do the same things. And who can blame them?  Few have ever had access to an electromagnetic simulator that allows them to visualize the circuit’s behaviors at various frequencies.

When thinking about return paths, remember that the reactive part of impedance becomes increasingly important as the frequency increases, and as rise/fall times decrease.  

At even modest frequencies, the return path of the current will attempt to flow directly underneath the conductor. If you do not provide that path, it will find a less desirable route through and around other parts of your circuit—perhaps creating an antenna along the way.

Return currents seek the path of least impedance. At low frequencies, most of the return current in the ground plane flows directly from load to source. This straight line between load and source represents the path of least resistance and, at low frequencies, the path of least impedance as well. As frequency increases, mutual inductance between the trace and the copper directly beneath the trace creates a low-impedance path that causes return current in the ground plane to follow the trace on the signal layer. 

How to Use Return Paths in PCB Design

On a PCB, route fast changing signals with a return path in their immediate vicinity. Differential traces should come out of the package pins and immediately be brought into close proximity. Clock signals and other fast rise-time/fall-time signals should be surrounded by ground pours and/or have a complete, uninterrupted ground plane beneath them to minimize radiated EMI noise. If your design requires FCC testing, you might even need to route your fast-changing signals between two ground planes and surround them with via-stitching.

The following two images demonstrate PCB layout examples that show two ways to reduce ground noise: 

• Keep differential pairs together through their entire route
• Provide a ground return path either directly beneath or directly adjacent to your signal lines

 

Differential pairs coupled together

 

Place ground return vias near differential pair vias to provide a ground return path for the signals as they propagate from layer to layer.

 

In the example below, the left PCB layout shows several layers of a PCB stackup from above (signal, power, ground, signal) and demonstrates routing over a power plane. Signals that travel over power planes before reaching ground layers will share their electric fields with the power plane, and the noise of the plane can create noise in the signal lines.

The PCB section on the right demonstrates ground pours and stitching around two signal traces. Copper pours around interconnects can become radiating elements if they are not tied to the ground plane below.

Conclusion: Utilize Ground Return Vias and Ground Return Paths 

Careful and deliberate planning of a ground return path will keep unwanted currents from forming in parts of your circuit where they should not be. Provide deliberate ground return vias and ground return paths for all of your signals—especially high-speed switching signals.