Eight Common Problems in EMC and Signal Integrity

Leidy J. Márquez M. ---> CAF ---> Fuente: http://www.ce-mag.com/archive/06/07/kimmel.htm

William D. Kimmel and Daryl D. Gerke

Although EMC and SI share some board-design similarities, each has factors that must be considered. Here's what to look for.
Although there are differences in emphasis between electromagnetic compatibility (EMC) and signal integrity (SI), there are major similarities in design at the circuit board level. A few years ago, the IEEE EMC Society added a committee on SI, recognizing the commonality of these two issues. We like to say that a board that is well designed for SI will go a long way toward being a good performer for EMC. But there are differences, as well. This article compares the two disciplines, examining their differences and similarities. It also reviews some of the common stumbling blocks.
EMC and SI Compared
It is important to start with a definition of EMC: the successful operation of equipment in its intended electromagnetic environment. Basically, this means the equipment works when exposed to the expected interference environment and does not emit energy that degrades the function of nearby equipment. Thus, EMC is concerned about emissions from your equipment impairing the operation of nearby equipment and about external interference impairing the operation of your equipment. In the European Union, this is known as immunity, and to other disciplines, notably the military, it is known as susceptibility. These requirements are defined in various specifications and may be invoked as a law or as a contractual requirement.
But the interference problem goes inside the equipment as well, and these are not covered by any specification. Internal devices fight with other internal devices, creating an internal compatibility problem. A noisy power supply or large motor can interfere with internal electronics. The discipline that covers such issues is known as self-compatibility.
At an even more local level, the circuit board, power circuits interfere with digital and analog circuits, while digital circuits interfere with analog and other digital circuits. This closes in on the subject of SI, and this article concentrates on electromagnetic interference (EMI) and SI at the circuit board level.
The term signal integrity was originally coined to address problems with high-speed digital electronics. Increasing speeds demanded path considerations, including impedance control and crosstalk. Smaller geometries and lowered supply voltages reduced noise margins. Hence, signal integrity became a buzzword. But analog electronics have advanced, too, and these devices now have greater sensitivities than in the past. It is appropriate, therefore, to define SI in terms of all signal issues, whether digital or analog.
EMC and SI Issues
Allowed Levels. Integrated-circuit (IC) vendor application notes specify decoupling capacitors to minimize Vcc droop and to control EMI. But the needs are significantly different. Vcc droop applies to the primary operating frequency of the chip, whereas EMI problems dominate at clock harmonics, typically to the 10th harmonic. Further, the allowed voltage for emissions is in the microvolt level, whereas Vcc can tolerate millivolts—about three orders of magnitude difference. So, decoupling that is adequate for SI may be woefully inadequate for emissions.
Similarly, adjacent-line crosstalk allowances are much lower for emissions than they are for SI. Even with continued reduction of supply voltages, a reading in the tens of millivolts is still tolerable for signal integrity, whereas a designer is limited to tens of microvolts for emissions for critical lines, notably those lines that leave the circuit board.
Emphasis. High-speed digital problems concentrate on the data bus and, of course, the clock if it is distributed around the circuit board. For this article, the emphasis is on keeping the signal intact. The principal problems are impedance control in the signal path, terminations in the signal path, and crosstalk from adjacent traces.
Low-level analog devices mostly draw signals (microvolt to millivolt levels) from off the board. Here, the emphasis will be in keeping digital and power currents from generating these voltages on analog ground.
Common EMI and SI Problems
With a basic understanding of how EMI and signal integrity relate, it is possible to examine some common problems encountered on the circuit board. Whole books have been written on the subject, and there are lots of subtleties involved, especially regarding emissions. Most problems, however, are the result of overlooking some fundamental issues. The following discussion outlines eight of the most common EMI and SI problems and how to avoid them.
Ground Impedance. At the circuit board level, most problems involve ground impedance. And even if ground impedance is not at the root of the problem, it will need to be brought under control before the problem can be solved.

Figure 1. Noisy and sensitive circuits sharing ground.

Figure 1 shows a typical SI problem, that of shared ground impedance. It is also known as common impedance coupling. In this example, the ground path is shared by two circuits, the noise source and the receptor, perhaps a low-level analog circuit. The voltage drop across the ground path looks like a signal to the receptor circuit. How much noise can be tolerated is dependent on the application, but if the receptor is a sensitive analog circuit, the allowed voltage may be quite low.
The mathematics of this problem is simple: E = IR (Ohm's law). The sensitivity of the recipient circuit will be dependent on the application, but the low millivolt range is common, and the low microvolt range is not uncommon. The solution is simple: either reduce the resistance to near zero or reduce the current to near zero.
To reduce the resistance to near zero, use a ground plane. At computer frequencies, the impedance of even a short trace is perhaps three orders of magnitude higher than that of a ground plane. Therefore, while the impedance of a short trace at 100 MHz may be 10 Ω or more, the impedance of a plane will be 10 mΩ. So, 1 A of current will bounce the signal ground trace about 10 V, which is clearly unacceptable in any digital signal case, but the same current will bounce the ground plane only 10 mV, a level that will almost always be acceptable.
To reduce the current to near zero is not so easy. The current in the power path usually can't be reduced. Presumably, high current exists for a reason other than to just dissipate power. Rather, the alternative involves steering the currents along separate paths. This technique enables the current to avoid sharing return paths.
Control Path Impedance. Controlling impedance is especially difficult with SI in high-speed circuits, where an impedance discontinuity causes a signal reflection. Impedance control is becoming increasingly important in high-speed circuit design, especially in telecom and computer applications.

Figure 2. The return path is discontinuous at vias.

There have been many articles describing impedance discontinuities, including corners, branches, and stubs, in the signal path. But it is important to remember that the signal path is only half the path. The return path is the other half. There are more ways to create a return-path discontinuity than there are in the signal path. Figure 2 shows the most common case, where the signal path passes through a via to another routing layer. The return-path impedance may be well controlled when the trace is immediately above a plane, whether a ground plane or a voltage plane. A discontinuity will appear every time reference planes are switched. In the figure, the reference plane switches from ground plane to voltage plane and back to ground plane. There is a discontinuity whenever the signal trace crosses a slot in the plane, whether the slot is a break in voltage planes or simply a gap where some copper has been borrowed. There is also a discontinuity at both the driver and receiver ends, because the signal current goes out the signal line and back through either the voltage pin or ground pin.
The discontinuity also creates an emission problem. A signal crossing a slot energizes the slot, launching an electromagnetic wave, and increases the voltage drop across the plane, creating a common-mode voltage.
The fix is to avoid switching reference planes if at all possible and to unconditionally avoid crossing a slot with a high-speed signal line. If it is necessary to switch planes, place a decoupling capacitor alongside the via.
Terminate High-Speed Lines. This completes the impedance-controlled path. This is the textbook case of signal reflections, but there are several aspects that need to be addressed in addition to the basic characteristic impedance control situation.
Impedance termination techniques include the textbook termination at the load, ac termination, series termination, and several nonlinear load terminations. All of these prevent or at least minimize reflections, but the series impedance termination is the only technique that puts the termination at the source, rather than at the load. Therefore, it is the only termination that inherently restricts the high frequency from leaving the driver. Series termination (also known as source termination or back termination) has some downsides, including a slower switching time. However, if it can be used, it will be quieter than the load terminations. Although primarily an SI issue, it also results in reduced trace radiation.
Slow the Edge Rates for Critical Signals. The general rule for both SI and EMI is to use no signal faster than needed for the desired function. Any high-frequency components not needed for the function only produce excess energy that can do nothing but interfere with neighboring signals. Excess energy means increased crosstalk to other adjacent signals and degraded signal quality. And, if the affected signal leaves the board, this excess results in unwanted energy piggybacking onto the signal lines.

Figure 3. RC filter can slow edge rate.

The best place to slow the edge rate is to place a filter immediately at the driver, such as a series R and shunt C (see Figure 3). Usually, the signal on the circuit board can tolerate the dc drop. Use as large a series resistance as possible. If the signal requires impedance termination, it will require series resistance of about 30 Ω. Some chips are available with built-in 25-Ω resistors, which are suitable for this problem. A shunt capacitor is usually not necessary, because the stray capacitance on the line and load completes the filter.

Figure 4. Power to the board must be filtered for both input and output lines.

Filter Lines Entering or Leaving the Board. The most vulnerable lines on a circuit board are those that enter or leave the board. Once on the board, signals are fairly well protected, especially on multilayer boards. Both input lines and output lines are vulnerable for emissions and immunity, but output lines are more prone to creating emission problems, and input lines cause more immunity problems. Figure 4 shows an example for both cases. Power to the board must also be filtered.
It is particularly important to use high-frequency filtering for low-frequency analog input circuits. Even though the nominal bandwidth of the amplifier may be in the kilohertz range, the input can be overloaded with sufficiently strong interference levels. An amplifier that is looking for an input signal of 10 mV will respond to a high-frequency input of 10 V. Basically, the amplifier is driven beyond its nominal range, and rectification occurs.
Keep Digital and Switching Power Currents from Circulating in Analog Ground. This problem goes hand in hand with the ground impedance issue mentioned above. Currents traveling on ground modulate signals.

Figure 5. Split ground planes for functional areas.

Split planes serve one purpose: to contain adverse currents within selected boundaries. At low frequencies, currents spread out over the available ground or power plane, limited by the plane boundaries. Segmenting the planes prevents high currents from power circuits from traveling through more-sensitive circuit areas. Similarly, digital currents can be prevented from circulating through sensitive analog areas. The purpose is to keep high currents from modulating the ground voltage. The most common method of doing so is shown in Figure 5.
There is nothing gained from splitting the planes to separate high-speed digital currents. The basic laws of physics dictate that the signal current loop will be the lowest-energy path. Given the chance, the return current would stay immediately beneath the signal path. Therefore, segmentation is not necessary, nor is it particularly desirable.

Figure 6. Ideal LC filter (a) and a real-world LC filter (b) with parasitic capacitance and inductance.

Ensure that Filters and Decoupling Work at the Frequency Range of Interest. EMC demands for decoupling are much higher than SI. There are two kinds of components: those described in textbooks and those that engineers install on circuit boards. All components have built-in parasitic elements. The dominant ones are the series inductance in capacitors and shunt capacitance in inductors. Figure 6 shows an ideal LC filter and a real LC filter.
Both elements have a resonant frequency, above which the components cease to function as desired. The resonant frequencies are much lower than most people would guess, and the components almost assuredly are past resonance in the frequency range of interest. A surface-mount-technology capacitor, as mounted, will have 2 nH of series inductance, at best. A 0.01-µF capacitor will then resonate at about 35 MHz, becoming an inductor above that. This is a very low useful frequency for decoupling considering the clock frequencies in modern microprocessors, not to mention the harmonic frequencies that go 10 times higher. Even most industrial controls are typically using 20-MHz clocks.
So to decouple, select capacitors with low equivalent series inductance (ESL), mount for minimum series inductance and use plenty of capacitors. Even if the board is running past resonance, additional capacitors will still reduce the impedance at high frequencies.
Watch for Coupling to Adjacent Elements. The most obvious case is coupling to adjacent signal traces, or crosstalk. But there are a plethora of other coupling paths contributing to emissions. These include stand-up elements such as headers and connectors, power-filter capacitors, heat sinks, adjacent circuit boards, and cables. Although onboard coupling can occur between traces and chips, and between capacitors and resistors, those components are low enough that they do not result in strong coupling. Most coupling at computer speeds is capacitive. Switching power supplies and regulators run at lower frequencies and higher currents, which can cause substantial magnetic field coupling.
Conclusion
SI and EMC design issues overlap, but the emphasis and allowed levels differ significantly. In most cases, the needs of EMC are much more demanding. On the other hand, some key SI issues are not a problem for EMC.
Many common EMC and SI problems, some of which are quite subtle, arise from not addressing the basic issues. Although following these basic considerations won't guarantee success, it will avoid major disasters, and, fixing the problem will be relatively easy.