FCC and EMC Compliance Requirements Explained for PCB Design

FCC rules limit the electromagnetic emissions a product may release, while EMC describes a device's ability to work in its environment without causing or suffering interference. Both shape grounding, filtering, shielding, and layout decisions from the first schematic through final compliance testing.

Highlights:

• FCC requirements set emission limits for electronic products placed on the market.
• EMC covers two sides of the same problem: emissions and immunity.
• Compliance is a design outcome, not a final test step.

Safety Compliance: FCC and EMC

Q1: What do FCC and EMC specifically mean?

A1: FCC stands for Federal Communications Commission, the U.S. communications regulator. EMC stands for electromagnetic compatibility. FCC is a standards organization, while EMC is a standard. Standards are issued for specific reasons and are accompanied by corresponding test methods.

Q2: When fabricating a PCB, should ground traces form a closed loop to reduce interference?

A2: In general, the loop area should be reduced to lower interference. When routing ground, do not form a closed loop; a tree-like or branched structure is preferable. The ground area should also be made as large as possible.

Q3: How can crosstalk be avoided in PCB design?

A3: A changing signal, such as a step edge, propagates along a transmission line from A to B and produces a coupled signal on transmission line C-D. Once the transition ends and the signal returns to a stable DC level, the coupled signal no longer exists. Crosstalk therefore occurs only during signal transitions. The faster the signal edge, or the higher the slew rate, the greater the crosstalk.

The coupled electromagnetic field in space can be represented as a collection of many coupling capacitors and coupling inductors. The crosstalk signal produced by coupling capacitance on the victim net can be divided into forward crosstalk and backward crosstalk, denoted Sc; these two components have the same polarity. The crosstalk signal produced by coupling inductance is also divided into forward crosstalk and backward crosstalk, denoted SL; these two components have opposite polarity. The forward and backward crosstalk produced by coupling capacitance and inductance exist simultaneously and are nearly equal in magnitude. On the victim net, the forward crosstalk components have opposite polarity and cancel each other, while the backward crosstalk components have the same polarity and add.

Crosstalk analysis modes usually include default mode, tri-state mode, and worst-case mode. Default mode is similar to actual crosstalk measurement: the aggressor driver is driven by a switching signal, the victim driver is held in its initial state, high or low, and the crosstalk value is calculated. This mode is effective for crosstalk analysis of unidirectional signals. In tri-state mode, the aggressor driver is driven by a switching signal and the victim's tri-state termination is set to high impedance to detect the crosstalk level. This mode is more effective for bidirectional or complex-topology networks. Worst-case analysis holds the victim driver in its initial state and the simulator calculates the sum of crosstalk from all default aggressors to each victim. This mode is generally used only for selected critical nets because there are too many combinations and simulation is slow.

Q4: During EMC testing, clock signal harmonics were found to exceed limits severely. Only decoupling capacitors were connected at the power pins. What aspects of PCB design should be considered to suppress electromagnetic radiation?

A4: The three elements of EMC are the radiation source, the coupling path, and the victim. Coupling paths are divided into radiated propagation through space and conducted propagation through cables. To suppress harmonics, first determine the propagation path. Power decoupling addresses conducted propagation. In addition, necessary matching and shielding are required.

Q5: In PCB design, ground is often divided into protective ground and signal ground, and power ground is divided into digital ground and analog ground. Why are grounds divided?

A5: The main purpose of splitting grounds is EMC: to prevent noise on the digital supply and ground from interfering with other signals, especially analog signals, through conduction. The division between signal ground and protective ground is based on ESD considerations in EMC, similar to the role of lightning rod grounding. No matter how the grounds are divided, there is ultimately only one earth; only the noise discharge paths differ.

Q6: In PCB design, is it necessary to add ground shielding on both sides of a clock trace?

A6: Whether to add shielding ground traces depends on the crosstalk and EMI conditions on the board. If the shielding ground is not handled properly, it may make the situation worse.

Q7: Are near-end crosstalk and far-end crosstalk related to signal frequency and signal rise time? Do they change with these parameters? If so, is there a formula?

A7: The crosstalk caused by the aggressor net on the victim net is related to the signal transition edge; the faster the transition, the greater the crosstalk, as expressed by V = L × di/dt. The effect of crosstalk on the decision of a digital signal on the victim net is related to signal frequency; the higher the frequency, the greater the effect.

Q8: Two stack-up options are being considered. Stack-up 1: Signal → Ground → Signal → Power +1.5 V → Signal → Power +2.5 V → Signal → Power +1.25 V → Power +1.2 V → Signal → Power +3.3 V → Signal → Power +1.8 V → Signal → Ground → Signal. Stack-up 2: Signal → Ground → Signal → Power +1.5 V → Signal → Ground → Signal → Power +1.25 V/+1.8 V → Power +2.5 V/+1.2 V → Signal → Ground → Signal → Power +3.3 V → Signal → Ground → Signal. Which stack-up is preferred? In Stack-up 2, will the two split power layers in the middle affect the adjacent signal layers? These signal layers already have ground planes as return paths.

A8: Both stack-ups have advantages. The first ensures plane integrity. The second increases the number of ground layers, effectively lowering the impedance of the power plane and helping suppress system EMI. Theoretically, power and ground planes are equivalent for AC signals. In practice, the ground plane has better AC impedance, and signals prefer the ground plane as the return path. However, stack thickness affects this. For example, if the dielectric between a signal layer and a power layer is thinner than the dielectric to ground, then in Stack-up 2 a signal crossing a split still has an incomplete return path at the power split.

Q9: When using Protel 99SE to design a PCB with an 89C51 processor, a 12 MHz crystal, a 40 kHz ultrasonic signal, and an 800 Hz audio signal, how should the PCB be designed to provide high immunity to interference? For an 89C51 and similar microcontrollers, how large a signal can affect normal operation? Besides increasing spacing, are there other techniques to improve system immunity?

A9: To provide high immunity, the edge rate of the interfering source signals should be reduced as much as possible. The frequency that can affect the 89C51 depends on the level of the interfering signal and the PCB trace length. In addition to increasing spacing, matching or topology can be used to address reflection and overshoot of the interfering signal, which can also effectively reduce signal interference.

Q10: In PCB routing, do power distribution and routing require the same attention as grounding? What problems occur if they are neglected? Will interference increase?

A10: If power is treated as a plane, it should be handled similarly to a ground plane. To reduce common-mode radiation from the power plane, it is recommended to pull the power plane inward by 20 times the height from the power layer to the ground layer. If power is routed, a tree structure is recommended, and power loops should be avoided. A closed power loop causes relatively large common-mode radiation.

Q11: I built a TFT LCD display. During EMC testing by others, interference signals coupled through space caused the displayed image to shake with a large amplitude. How should this be handled? A burst of interference pulses was applied to several signal lines; I am not sure of the exact test name, but the interference was radiated out through the signal lines.

A11: For a standalone LCD, the burst test in EMC testing is almost impossible to pass, especially when a coupling clamp is used. If the LCD is used in an instrument, the problem is easier to solve: decouple the signal lines, use conductive paste to appropriately reduce the impedance at the LCD inlet, and add a shielding conductive mesh on the screen surface.

Q12: During a recent EMC test, a GSM fixed wireless phone exhibited radiated spurious emissions between 100 MHz and 300 MHz. The company sent me two phones with shielding cases coated with electrostatic paint. The laboratory would not allow replacing the entire phone, so I swapped the case with the ferromagnetic electrostatic paint onto the phone that needed modification for the test. The test result showed that the previous spurious emissions were gone, but a problem appeared at the main frequency. The phone's operating main frequency is 902 MHz, but several frequencies appeared between 905 MHz and 910 MHz. That is the basic situation. During the modification, I only changed the case; the circuit board and other hardware were not modified at all.

A12: Phone types can be understood as wireless handsets, cordless phones, and so on. It is necessary to clarify the phone type, the host operating frequency range, and the type of electrostatic spray material on the case: ferromagnetic or non-ferromagnetic conductive material, as well as its conductivity.

Q13: When using Protel DXP solid copper pour, what are the side effects of selecting "pour over all same net objects"? Will it cause interference signals to run around the whole board and affect performance? I am working on a low-frequency data acquisition card, so this problem may not need to be a concern, but I still want to understand it.

A13: For a mixed analog/digital PCB, it is recommended to separate analog, digital, and ground, then connect them at a single point, for example with a ferrite bead or a 0-ohm resistor. High-speed data lines are best routed with two parallel ground traces to reduce interference. The "pour over all same net objects" option has no effect on signal performance; it mainly affects soldering of some pads because heat dissipation is faster. It should be beneficial for EMI because it increases the contact area between the pad and the copper. Selecting this option has no side effect. Thermal relief pads should be selected instead of solid pads because solid pads dissipate heat quickly and may cause tombstoning during reflow.

Q14: What is a ferrite bead, and what is it used for? What is meant by ferrite bead connection, inductor connection, or 0-ohm resistor connection?

A14: A ferrite bead is used specifically to suppress high-frequency noise and spike interference on signal lines and power lines, and it can also absorb electrostatic discharge pulses. A ferrite bead is used to absorb very-high-frequency signals. RF circuits, PLLs, oscillator circuits, and circuits containing very-high-frequency memory such as DDR SDRAM and RAMBUS all require a ferrite bead at the power input. An inductor is an energy-storage component used in LC oscillator circuits and low-to-medium-frequency filter circuits; its application frequency range rarely exceeds 50 MHz.

The main function of a ferrite bead is to eliminate RF noise present in a transmission-line structure, that is, in the circuit. RF energy is an AC sine-wave component superimposed on a DC transmission level. The DC component is the desired signal, while the RF energy is unwanted electromagnetic interference that propagates along the line and radiates as EMI. To eliminate this unwanted signal energy, a chip ferrite bead acts as a high-frequency resistor, or attenuator: it allows DC signals to pass and filters out AC signals. Typically, high-frequency signals are above 30 MHz; however, low-frequency signals can also be affected by chip ferrite beads.

To select a ferrite bead correctly, the following points must be considered: (1) the frequency range of the unwanted signal; (2) the noise source; (3) the required noise attenuation; (4) the environmental conditions, including temperature, DC voltage, and structural strength; (5) the circuit and load impedance; (6) whether there is space on the PCB for the ferrite bead. The first three items can be judged from the impedance-frequency curves provided by the manufacturer. In the impedance curve, three curves are very important: resistance, inductive reactance, and total impedance. The total impedance is described by Z = √(R2 + (2πfL)2). From this curve, select a ferrite bead that has maximum impedance in the frequency range where noise attenuation is desired and minimum signal attenuation at low frequency and DC. The impedance characteristics of a chip ferrite bead are affected by excessive DC voltage. In addition, if the operating temperature rise is too high or the external magnetic field is too strong, the bead impedance will be adversely affected. The choice between a chip ferrite bead and a chip inductor depends mainly on the application. Resonant circuits require a chip inductor. When unwanted EMI noise must be eliminated, a chip ferrite bead is the best choice.

EMC and Interference Troubleshooting: Practical Design Q&A

Q15: How do you determine the capacitance needed to cancel crosstalk between traces?

A15: Rather than hunting for a capacitor value, the first priority in PCB routing is to avoid excessively long parallel runs, especially for high-speed or high-swing signals. Where parallel routing cannot be avoided, keep sufficient spacing between the aggressor and victim traces, or insert a ground trace as a guard between them. In locations where board volume is tightly constrained and immunity requirements are high, a metal shielding enclosure can be used to provide isolation.

Q16: A prototype works on the bench but is disturbed as soon as it is connected to a vehicle chassis ground. What is the cause?

A16: In this case a small auxiliary battery was paralleled with the vehicle supply, with a diode added to prevent the small battery from being pulled down during freewheeling. The moment the terminal was tied to the vehicle chassis ground, however, interference appeared. This is a classic EMC problem: spark discharge on the vehicle couples into the terminal, either as radiated energy or as conducted noise reaching the equipment through cables. Several causes deserve investigation: 1. Grounding. Examine how ground is routed on the terminal main board and how the copper pour is arranged. 2. Enclosure shielding. A metal housing is preferable; if part of the enclosure is non-metallic, covering it with copper or tin foil is worth trying. 3. Board layout. Keep the power section and the CPU section as separate as possible, route power traces as wide and as short as practical, and follow established routing rules. 4. Layer count. Automotive electronic main boards are generally better with at least four layers; a two-layer board usually provides weaker immunity. 5. Ferrite cores. During testing, clamp a magnetic ring around the power cable to see whether the disturbance falls. Many other measures exist as well, and the right combination depends on the specific installation, but these five areas cover the majority of vehicle-borne interference cases.

Q17: Why are series resistors placed on SCL, SDA and AS lines, and how does the value affect circuit behavior?

A17: The pull-up resistor improves noise immunity; a typical value is derived from Vcc/1mA up to roughly 10K. The series resistor serves as a damping element, usually selected in the range of 33 ohm to 470 ohm. When the pulse frequency on a signal line is high, energy reflects from one end of the line to the other, which can corrupt data and generate EMI. Inserting a series resistor in the middle of the line effectively controls that reflection.

Q18: Radiated emissions at 200MHz exceed the acceptable limit during CE/FCC testing. How should this be fixed, how should ferrite beads be selected, and how should crystal harmonic radiation be suppressed?

A18: Without seeing the product, no exact answer can be given, but a practical troubleshooting sequence can be followed. If the emission is definitely a harmonic, the device that generates it becomes the primary target. A quick experiment is to build a simple shield over that device — a can cut from a beverage container works, provided the shield is properly grounded — and retest. If the emission drops, the source is confirmed and the device should be shielded permanently. If nothing changes, focus on exposed transmission lines. Any line that can be grounded should be grounded; a shielded cable can also be substituted temporarily to see whether the result changes, confirming whether the cable is the radiating path. The final item is shielding of the enclosure itself. This is the most complex and costly option and should only be considered when the earlier measures have failed. After these steps have been tried, the emission level should be reduced.

Q19: A 2KW vacuum cleaner passes functional testing but fails EMC. Can software alone fix it?

A19: The firmware implements soft start and soft speed regulation, so the motor accelerates gradually without abrupt speed changes; it allows the motor speed to be adjusted; and it drives the motor through a triac by chopping the sine wave. The hardware is correspondingly simple, with only a 0.1uF safety capacitor handling EMC. Under those conditions, software algorithms alone can hardly solve the problem; close coordination with the hardware team is required, and most of the effort will have to go into the hardware and the chopping strategy.

Q20: A decoder's DA conversion frequency radiates from the chip through power and ground at 166M, and capacitors on the supply do not remove it. Why?

A20: The board is a two-layer design with a short power loop, and 1 nF, 630 pF and 30 pF capacitors were all tried without success. Three suggestions were offered: Power quality (load capability) may be inadequate. The DA converter should be fed from its own dedicated supply. Check that the output stage is well grounded, and place a ferrite bead in series with the signal output as an experiment. A magnetic bead rated for 100M can be used to suppress the 166M component.

Q21: Multi-channel thermocouple acquisition: supply, front-end and filtering questions

A21: The design uses K-type thermocouples, a charge-pump conversion module, and AD620 plus OP07 devices in a two-stage amplifier chain. Three uncertainties were raised. First, the 12V battery is converted by the charge pump to ±12V, and the resulting ripple is unfavorable for signal acquisition — would a single supply derived directly from the battery be better? Second, should the two thermocouple leads be connected straight into the AD620 inputs as shown in the datasheet examples, and how should the EMI filter section shown there be adapted for thermocouple measurement? Should the cold junction be grounded or tied to a stable voltage? Third, because the measured temperature range extends below zero, the AD620 output must pass through non-inverting and inverting amplification before the A/D input; the plan is to use OP07 devices for two filter stages, the first an infinite-gain filter and the second a filter with 2x non-inverting and 2x inverting gain. If the thermocouple cold junction is grounded — and in many instruments one thermocouple lead is already grounded — and the measurement extends below zero, a bipolar ± supply is the usual and preferable approach. Supply ripple should be low, and the rails need not be symmetrical; a stable LDO can be added afterwards. Low-frequency filtering strongly affects the result, but a single stage should be sufficient. Whether the EMI filter section is needed depends on the application environment. For multi-channel measurement, place the multiplexer ahead of the amplifier to reduce cost; the multiplexer should have differential inputs, and the extension wiring from the thermocouple should itself be thermocouple-grade wire, which is fairly expensive.

Q22: What EMC problems appear most often during certification?

A22: For general electronic products, the three most frequent failures are RE (radiated emissions), CE (conducted emissions) and ESD (electrostatic discharge). Communication products must additionally deal with Surge, meaning lightning-induced impulses. Medical equipment most often fails on ESD, EFT (electrical fast transient immunity), CS (conducted immunity) and RS (radiated immunity). In the dry northern regions of China, ESD requirements for products are particularly demanding; in Sichuan and other thunderstorm-prone areas of the southwest, EFT and lightning surge requirements are correspondingly high.

Q23: How can electromagnetic interference on ICs be eliminated?

A23: The interference that ICs suffer is mainly ESD. Protection has two aspects: ESD and EMI considerations during board layout, and the addition of dedicated protection devices. Two device types are available. The varistor is made of zinc oxide, responds relatively slowly, clamps relatively poorly, and ages with every ESD strike until it eventually fails. The TVS (transient voltage suppressor) is a semiconductor device with fast response and good clamping, and it can be used indefinitely. On cost, the varistor is cheaper than the TVS.

Q24: GPS sensitivity collapses in a handheld/vehicle terminal that also carries MP4, MP3 and FM functions. How is this interference solved?

A24: Such a terminal has an internal GPS antenna, which sits close to the MCU, the SDRAM, the crystal and other components, so electromagnetic interference severely degrades satellite acquisition and can make positioning impossible. Part of the answer lies in circuit design, and much of the problem usually traces back to inadequate protection and shielding. In one case, Bluetooth interference and remote-control interference were both present; the remote-control link was addressed by extending its effective range to 5M, while the Bluetooth issue remained unresolved. Module placement on the PCB is critical. Before layout, plan the floorplan according to current magnitude and the operating frequency of each crystal, and ground each section properly — this addresses interference coupled through shared supply and ground. Measurements show that the physical spacing between the dominant oscillators strongly affects radiation; moving them slightly farther apart produces a clear reduction. If space does not permit, local shielding is warranted, but only within a common PCB ground area. Decouple at the power entry and exit points; ferrite beads with capacitors are a good choice, and Bluetooth and GPS blocks can use printed inductors. The switching frequency of DC/DC converters also matters: harmonics must not coincide with the operating frequencies of other circuits, particularly receiver frequencies. Some DC/DC converters have a fixed frequency, in which case a simple filter is enough. Co-frequency interference is the main reason GPS and remote-control receiver sensitivity drops, and the local oscillator amplitude in the receive chain should be kept as low as practical, otherwise it becomes a continuous interference source. In one design, Bluetooth, the GPS receiver, a second 2.4GHz transceiver and a 433M remote receiver were all integrated in a single enclosure with good results and high GPS sensitivity.

Q25: Conducted emissions from an MCU system exceed the limit by a single point at 24M. Is this conducted or radiated?

A25: The system uses a Motorola MC908JL3 controller, an 8M ceramic resonator, and a power connection made through a cable. During EMI testing the conducted voltage exceeds the limit by 0.8dB at a single point at 24M. Suggested remedies include adding a ferrite ring and Y2 capacitors. The first step, however, is to clarify the measurement: if the EMI test shows 24M over the limit in the radiated measurement it is a radiation problem, and if the exceedance appears during the conducted measurement it is a conduction problem.

Q26: A triac controlling a DC motor disturbs the supply and corrupts zero-crossing detection, causing loss of control or speed drift. What is the fix?

A26: Two mechanisms are usually at work. The motor is a non-resistive load, so phase shift appears in the circuit and the control timing becomes inaccurate; a capacitor can be added to filter this. In addition, when a triac drives a high-power or high-current load, zero-crossing turn-on rather than phase control reduces the EMC impact. Phase-shift speed control is nonetheless a common approach. If the zero-crossing detection hardware is sound, the software handling should be improved: within one mains cycle (50Hz, 20ms) the triac must be turned on twice, and the delay between detecting the zero crossing and issuing the output determines the phase angle.

EMC Design, Shielding, and Grounding: Practical Engineering Questions

Q27: Has anyone completed EMC design for V.35, E1, G.703 (64K), and relay interfaces? Can you offer some guidance? The main standards to pass are GB/T 17626.12 (IEC61000-4-12), electromagnetic compatibility test and measurement techniques, oscillatory wave immunity test; GB/T17626.2 (IEC61000-4-2), electromagnetic compatibility test and measurement techniques, electrostatic discharge immunity test; GB/T 17626.3 (IEC61000-4-3), electromagnetic compatibility test and measurement techniques, radiated RF electromagnetic field immunity test; GB/T 17626.4 (IEC61000-4-4), electromagnetic compatibility test and measurement techniques, electrical fast transient burst immunity test; GB/T 17626.5 (IEC61000-4-5), electromagnetic compatibility test and measurement techniques, surge immunity test; and GB/T 17626.6 (IEC61000-4-6), electromagnetic compatibility test and measurement techniques, immunity to conducted disturbances induced by RF fields.

A27: These standards are basic EMC test standards, and the specific limits still need to be determined according to the product. The interfaces mentioned are communication interfaces and generally have standard circuits. When the schematic filter design and the PCB layout and routing are correct, the tests can usually be passed. In other cases, EMC filtering and transient suppression devices need to be added, and the analysis must be made for the specific interface.

Q28: Routing must not cross the gap between split power planes. Can someone explain this in detail?

A28: If one power plane is split into several different power sections, such as 3.3V and 5V, signal traces should preferably not appear on different power planes at the same time. In other words, routing must not cross the gap between split power planes. Otherwise, unnecessary EMC problems will occur. The same applies to ground: routing must not cross the gap between split ground planes.

Q29: A microcontroller uses a Darlington transistor and an optocoupler to control a 12V relay, and the relay controls the pull-in of an AC contactor. At the instant of pull-in, the microcontroller often resets. A oscilloscope measurement at the reset pin detects a valid reset signal, and a three-pin reset IC is used. The microcontroller is powered from 5V, and 1000uF capacitors are fitted both before and after the 5V regulator. No supply fluctuation is observed with the oscilloscope. If the relay is unloaded, that is, without the AC contactor connected, no reset occurs. How can this be solved?

A29: One solution is to connect an RC snubber across the AC contactor coil, consisting of a resistor in series with a capacitor. The capacitance can be between 0.01uF and 0.47uF, and the voltage rating should preferably be 2 to 3 times the coil rated voltage. Another view is that this is caused by EMC interference generated when the AC contactor operates. The RC snubber is a good solution, and a high-voltage capacitor of 100pF to 47pF can also be considered in parallel with the output contacts of the 12V relay. Adding RC absorption at the AC contactor is effective, but the power circuit should also be checked. See whether the CPU power trace is too long, add decoupling capacitors at the chip power pins, and consider adding an LC filter in the regulator section to absorb as much interference from the supply as possible. A step-by-step check can also be used: first test without the load to see whether the same phenomenon occurs. Disconnect the optocoupler first, then the relay. If reset still occurs without the optocoupler, check whether the hardware output port is shorted to reset. If there is no reset, connect the optocoupler but not the relay. If reset still occurs, possible causes are that the ground trace is too thin, the ground of the reset pin is too close to the optocoupler and far from the supply, or the optocoupler current-limiting resistor is too small, causing the ground potential to rise momentarily. During routing, the CPU should be kept away from high-current devices, and a star single-point ground should be used. If reset still occurs, the cause is electromagnetic interference from the relay coil, contact arcing, or large load changes. Shielding and methods to eliminate contact arcing can be used. In most cases, the power supply has not been handled well, the ground or +5V trace is too long and too thin, or the CPU position is unreasonable.

Q30: Can AC filters and DC filters be used interchangeably? Generally, an AC line filter can be used in a DC application, but a DC line filter absolutely cannot be used in an AC application. Why?

A30: The bypass capacitors used in a DC filter are DC capacitors. Under AC conditions, they may overheat and be damaged. If the DC capacitor has a low voltage rating, it may also break down and fail. Even if neither of these two situations occurs, the common-mode bypass capacitors in a DC filter generally have a large capacitance. When used in an AC application, this causes excessive leakage current and violates safety standard requirements.

Q31: In box-type equipment such as an Ethernet switch or a PC, there is a chassis ground and a circuit working ground. I have found that some equipment connects the two grounds with a capacitor, some with a 0 ohm resistor, and some with a ferrite. Which is correct?

A31: We generally use a 102 high-voltage ceramic capacitor.

Q33: What is meant by "mechanical protection"? Does it mean protection of the enclosure?

A33: Yes. The enclosure should be as tight as possible, use little or no conductive material, and be grounded as much as possible.

Q34: What impact does an all-metal enclosure, such as aluminum or stainless steel, have on ESD protection? How should it be handled?

A34: If the product uses an all-metal enclosure and the grounding is poor, this is of course unfavorable for ESD protection. As long as the grounding is done well, however, there should be no problem. How to ground it depends on the specific equipment. For large equipment, the equipment can be connected directly to earth, and the effect is naturally ideal.

Q35: Why can a spectrum analyzer not observe transient interference such as electrostatic discharge?

A35: A spectrum analyzer is a narrowband swept receiver. At any one moment, it receives only the energy within a certain frequency range. Transient interference such as electrostatic discharge is pulse interference. Its spectrum is very wide, but its duration is very short. Therefore, when the transient interference occurs, the spectrum analyzer observes only a small part of its total energy and cannot reflect the actual interference situation.

Q36: When diagnosing electromagnetic interference problems on site, near-field probes and spectrum analyzers are often needed. How can a simple near-field probe be made from coaxial cable?

A36: Strip the outer layer, that is, the shield, from the coaxial cable to expose the center conductor. Form the center conductor into a small loop with a diameter of 1 to 2 cm and 1 to 3 turns, and solder it to the outer shield.

Q37: Measuring biomagnetic information from the human body is a new medical diagnostic method. This biomagnetic measurement must be carried out in a magnetic shielding room. The room must be able to shield alternating electromagnetic fields from the static magnetic field up to 1GHz. Please propose a design for this shielding room.

A37: First consider the choice of shielding material. Because very low-frequency magnetic fields must be shielded, a high-permeability material such as permalloy should be used. After permalloy is machined, its permeability decreases, so heat treatment is required. Therefore, the shielding room should be made as an assembled structure built from panels. Each panel is machined according to the design in advance, then heat-treated, transported to the site, and installed very carefully. The joints between panels must overlap so that a continuous magnetic path is formed. A shielding room constructed in this way has good shielding effectiveness against low-frequency magnetic fields, but the seams cause high-frequency leakage. To compensate for this shortcoming, an outer second shielding layer made of welded aluminum plate is added outside the permalloy shielding room to shield high-frequency electromagnetic fields.

Q38: When designing a shielded enclosure, what factors should be used to select the shielding material?

A38: From the perspective of electromagnetic shielding, the main consideration is the type of electric field wave to be shielded. For electric field waves, plane waves, or higher-frequency magnetic field waves, ordinary metals can generally meet the requirement. For low-frequency magnetic field waves, a material with higher permeability should be used.

Q39: Besides the shielding material, what else affects the shielding effectiveness of an enclosure?

A39: Two factors affect it. One is conductive discontinuities on the enclosure, such as holes and seams. The other is conductors passing through the shielded enclosure, such as signal cables and power cords.

Q40: What should be noted when shielding a magnetic field radiation source?

A40: The wave impedance of a magnetic field is very low, so the reflection loss is small, and shielding depends mainly on absorption loss. Therefore, a shielding material with higher permeability should be selected. In addition, during mechanical design, the shielding layer should be kept as far as possible from the radiation source to increase reflection loss, and holes and seams should be kept away from the radiation source as much as possible.

Q41: One principle in shielding structure design is to keep cables inside the enclosure away from seams and holes as much as possible. Why?

A41: A magnetic field always exists near a cable, and magnetic fields leak easily through holes, regardless of the magnetic field frequency. Therefore, when a cable is very close to a seam or hole, magnetic field leakage occurs and the overall shielding effectiveness is reduced.

Q42: Why do we often use grounding rather than connection to the power supply to suppress noise signals? Both ground and power are layers in a multilayer PCB. According to the relativity of the voltage zero point, can the power layer also serve as the voltage zero point?

A42: Grounding can also be understood as connection to a reference point. Since it is a reference point, it must be able to perform the reference function. When we regard something as ground, we at least treat it as zero with no impedance, although in practice this depends on the layout. If the power supply output impedance is zero, then the power supply can of course also be used as a reference point and as a bypass path for noise signals. Signal ground has several meanings: absolute earth, relative ground or reference ground, and no ground. Sometimes, to reduce interference, the 0 and 1 states of a signal are deliberately made relative to each other rather than to ground, so the signal 0 state is not taken as ground. CAN signals work in this way. One of the difficulties in hardware design is how to solve the grounding problem well, from an IC chip to a large system. Using the ground clip of an oscilloscope probe on a power supply may burn out the oscilloscope. The ground clip of an oscilloscope probe is connected to the ground of the oscilloscope power cord unless an isolated probe is used. Clipping it to a power supply directly shorts the power supply to ground. Using ground clips of different probes on points at different potentials will also cause a short circuit. A recommended practice is to feed the oscilloscope power through an isolation transformer. Alternatively, as is commonly done, remove the ground pin from the oscilloscope power cord to eliminate the risk. Grounding and isolation are issues that must be watched constantly during design and testing. Although both the power layer and the ground layer are AC voltage zero points, the ground layer is relatively cleaner, so grounding is usually used instead of the power supply.

Q43: A handheld test product can be powered by a battery and can also use an external adapter. The adapter alone with a load passes the radiated emission (RE) test. The handheld product powered by the battery also passes RE, and both have a relatively large margin. However, with the external adapter connected, the emission exceeds the limit considerably around 160 MHz and cannot pass certification. What is the cause? How can the interference source and coupling path be located? Once located, how can it be solved?

A43: There are two possible interference sources: the switching frequency of the adapter, and the crystal oscillator and internal switching power supply frequency of the handheld test product itself. The individual tests do not exceed the limit, so the combination test exceeding the limit indicates that the coupling path is the product power cable. Several methods can be used for location. First, add ferrite rings at both ends of the power output cable, that is, the product power input cable. If the reduction is relatively large near the adapter end, the adapter is the cause; otherwise, the interference source is inside the handheld product. Second, use a spectrum analyzer at the common-mode inductor of the product power input connector to see which side has a larger interference amplitude. If the interference inside the common-mode inductor is larger, the handheld product is the source. Third, if the external adapter is suspected, simply replace it and test. If the frequency point disappears, the adapter is the problem. Location by the above methods showed that the adapter was indeed the problem. Although the switching power supply frequency is only at the kHz level, the interference can often reach tens or hundreds of MHz. In addition, the radiated emission test result of the power adapter varies with different loads.

Crystal Oscillator Emissions and Filtering

Q44: A handheld battery-powered device exceeds radiated-emission limits at 700 MHz. The emission source is traced to a 10 MHz active crystal oscillator and the DSP internal PLL. Adding 10uF and 0.1uF capacitors to the oscillator supply filter reduces the 700 MHz point noticeably but raises the 800 MHz point. Replacing the through-hole crystal with an SMD type to reduce fan-out produces little improvement. What other improvements are possible, and what special requirements apply to the crystal filter circuit?

A1: The emission source may be the 10 MHz crystal itself or a 10 MHz multiple inside the DSP. For high-frequency exceedances at 700 MHz or 800 MHz, address several areas. (1) Crystal treatment: filter the supply, apply RC filtering to the clock trace, or replace the resistor with a ferrite bead. (2) If board traces are the radiating path, filter those traces with ferrite beads and capacitors. (3) Because the exceedance is at high frequency, the PCB may have high ground impedance or a large ground loop; review the PCB layout. (4) For a metal enclosure, check for shielding leakage. (5) If interface cables radiate, filter the cable interfaces, with measures selected for each interface type.

Establishing an EMC Design Process

Q45: EMC is often not discussed during design or is given insufficient attention. EMC problems emerge after tooling is opened or the product is finalized. How can this be solved?

A45: This is common in many companies. The key issue is the lack of a strict EMC design process. Most engineers lack EMC design experience, so EMC principles are not integrated into early product development, and problems are expected. Companies should first develop engineers' EMC design skills and awareness. More importantly, they should establish an EMC design process and platform, including schematic design rules, design checklists, guidance, and monitoring. This makes early EMC design practical and helps ensure the final product meets EMC targets. The issue is systemic and spans structure, power, hardware circuits, PCB, and other areas.