Passing EMI Compliance Testing the First Time—Part 5: Advanced Consideration for Precision Analog, Shielding, and Thermal Management

×

Figure 1

   

要約

This five-part series presents an electromagnetic (EM) field-oriented perspective on PCB design intended to help engineers pass electromagnetic interference (EMI) compliance testing. The same techniques used to reduce EMI also mitigate interference, suggesting a universal PCB layout philosophy. Parts 1 and 2 established the foundational physics and illustrated through practical examples how decisions such as signal layer transitions, shared ground planes, and imperfect transmission lines become sources of radiation. Parts 3 and 4 extended those principles into a practical layout workflow: schematic-to-placement strategy, grounding architecture, power system routing, and stack-up selection. This final article addresses the specialized layout requirements that arise in the most demanding designs. Every design, regardless of signal type, must manage heat—not only to protect components but also to prevent thermoelectrically generated offsets from corrupting sensitive measurements. Together, these considerations complete the picture of what it takes to plan and execute a board layout that passes EMI compliance the first time.

Introduction

Electromagnetic interference (EMI) compliance is too often treated as a final hurdle, rather than a design goal; something to address after the schematic is complete, the board is laid out, and the prototype is already in hand. The premise of this series is that compliance need not be a surprise: a board designed with electromagnetic fields in mind from the very first schematic review can be built to pass the first time. Parts 1 and 2 made the case at the physics level, showing that radiation and interference are not random or mysterious but are predictable consequences of unconfined fields—and that the same layout discipline that suppresses emissions also improves a board’s immunity to external fields. Parts 3 and 4 translated those principles into a step-by-step foundational layout workflow: organizing the schematic, placing parts with layout intent in mind, selecting the right grounding architecture, routing the power system first, and choosing a layer count and stack-up that provides field containment for every signal. With that framework in place, this final article turns to the specialized considerations that separate a good layout from a great one. The topics covered here—precision analog, shielding and guarding, and thermal management—apply to any design that pushes the boundaries of performance, connects to the outside world, or operates in a demanding environment. These are the details that determine whether a design that looks correct on paper actually performs correctly on the bench.

Precision/High-Accuracy Analog

Concerning precision or high-accuracy analog and overlooking a fully differential signal chain for now (which is almost cheating), the fidelity of the ground is an important consideration to achieve analog precision. Low-frequency currents will follow the path of least energy taken from the source so any current-consuming circuit using ground as the return will contribute to a ground gradient (and noise) at low frequencies. As an example, consider a 1oz copper plane at 0.5mΩ/square: 100mA of return current on a square of PCB will develop a voltage drop of 0.5mΩ × 0.1A or 50µV. This is a large offset for a precision measurement. The location of the components really makes a difference concerning this problem. There are many ways to reduce the impact of this error ranging from parts placement to running return current in a negative supply rather than ground, replacing the ground plane (for the signal tracks) with a ground tree, slotting planes to direct the ground current, or using board-level differential signaling.

Shielding, Guarding, and Static

This is a topic that applies to any PCB that is handheld or has a cable connection to the outside world. It covers how to connect one grounding system to another over a distance. It is this space or distance that provides additional methods of coupling that make moving signals over a distance difficult. The issue is illustrated in Figure 1.

A second ground system removed with distance will probably not be at the same potential as the ground system of the PCB. There is more than one reason for this.

Lightning

Imagine two system grounds connected and separated by a distance. Now consider each of these grounds has a connection (either direct or capacitive) to earth. Finally, consider the earth as the final conductor completing the loop (see Figure 1). It is this large, closed loop that can develop a voltage, by Faraday’s law, from nearby lightning strikes that can induce a voltage in this ground loop.

Ground Currents from Equipment

All equipment with imperfect layouts can couple current to chassis ground. The return current path for this coupled current can cause voltage drops in grounds separated by a distance. This is the second cause of the ground loop current.

Common-Mode Current

In isolated systems, related to the equipment current above, currents coupled across isolation barriers can cause voltage drops in grounds separated by a distance. This is the third cause for the ground loop current.

Shielding is the solution to all these problems. Figure 1 outlines a properly shielded connection between two ground systems. The solution does not eliminate the current flow between the ground systems; however, it directs the current through a path that does not affect the analog function or measurement.

Guarding is a topic that is closely related to shielding. The purpose of a guard is to prevent AC or DC coupling to a sensitive PCB track or a specific cable conductor. To accomplish this, surround the sensitive conductor with a second conductor driven by a buffered copy of the measured voltage at the guarded net. Without a voltage difference between this conductor and the outside world, there can be no coupled current.

The Movement of Heat in the PCB

This article cannot be complete without covering how the movement of heat can affect analog performance. There is more to this topic than just keeping the parts and the board at a reasonable temperature.

To risk stating the obvious, every design needs a way to remove heat. Even the lowest power designs will die a heat death without the movement of heat energy out of the design. Luckily, all those low-impedance power and ground planes were needed to mitigate interference (with all that thermally conductive copper). All that copper can be used to spread the thermal energy over the entire board so that it can be radiated. Using copper in this way will also reduce thermal gradients across the board, mitigating a bigger problem for precision analog: thermoelectrically generated offsets. Note that in analog, especially for sensitive silicon and precision resistors, it can be necessary to pour planes just to remove heat energy directly from signal lines. This always needs to be done in a way that does not compromise the fidelity of the signal/return transmission line. It is also wise to consider how the operating environment or product use might affect these temperatures—a very wide temperature range may need to be considered (concerning the product’s operating temperature specifications) depending on the use case.

Temperature gradients are the next concern since they can affect the precision analog by directly generating voltages due to the thermoelectric effect. Any dissimilar metal junction can generate a thermal voltage due to the Seebeck and Thompson effects (essentially a thermocouple). The Seebeck and Thompson effects generate voltages in the length of conductors when each end of the conductor is at different temperatures. Since different metals move heat at different rates, each conductor type will generate a different voltage. This can happen on a PCB since the conductors within components, solder, connector pins, and PCB traces are all made from different metals. These errors will occur if the circuit is sensitive to microvolts. To eliminate this, either reduce these point sources of heat or design the heat energy movement in a way that does not compromise the sensitive analog signal path. This is accomplished with slots and copper planes to channel and direct heat energy. The planes guide the energy safely away and the slots exclude the movement of heat energy.

Conclusion

Beginning the layout for a large, complex board can be overwhelming. It helps to break the task into manageable actions—beginning in the schematic by grouping circuit groups in a way that is layout friendly and carrying those notes and groupings into placement and routing. These five parts form a unified, field-oriented methodology for PCB design. Parts 1 and 2 established the physics foundation: that mitigating EMI is fundamentally about controlling and confining electric and magnetic fields, and that the same practices that reduce radiated emissions also improve susceptibility and reduce interference. The series then moves from schematic to placement and grounding architecture in Part 3, through power routing and stack-up selection in Part 4, to the precision analog, shielding, and thermal considerations addressed here—providing a complete checklist for tackling even the most demanding PCB designs. Working through each of these steps in order ensures a placement and stack-up that will help complete the board right the first time, with confidence that it will pass EMI compliance.

References

Feynman, Richard P., Robert B. Leighton, and Matthew Sands. The Feynman Lectures on Physics, Vol. 2: The New Millennium Edition: Mainly Electromagnetism and Matter. Basic Books, 2011.

Johnson, Howard W. and Martin Graham. High-Speed Digital Design: A Handbook of Black Magic. PTR Prentice Hall, April 1993.

Morrison, Ralph. Fast Circuit Boards: Energy Management. John Wiley & Sons Publications, January 2018.

著者について