Thanks for your interest in our webinar on EMI reduction with special Q&A by @karen.burnham!
Missed the webinar? Click the link below to access the recording and slides.
| Question | Answer |
|---|---|
| Is there not a risk of getting decoupling resonance problems if different types and different value capacitors are used? | Yes, there is definitely a risk of getting decoupling resonance problems when using different values and types of capacitors. The solution is that, even if you have to use different values and types of capacitors, you need to look at the response and then decide whether you want that capacitor or that combination of capacitors. The tool used for PDN analysis should help address this quite effectively. You can visualize the graph first and see whether the response is passing the target line or not. Based on the result, you can choose a different capacitor or remove a capacitor from the combination. |
| Is it necessary to maintain 3W spacing between high-speed traces? | It depends on the specific design and the importance of the signals. Maintaining 3W spacing is definitely a good rule of thumb for high-speed traces, but it is not a requirement that applies to every situation. There will be cases where the 3W rule is less critical and traces can be placed closer together without causing significant issues. However, it is generally advisable to maintain 3W spacing wherever practical, and I would be hesitant to reduce the spacing significantly below 3W, especially for critical high-speed signals. |
| What are the EMC tests that PCB designer can generally do on their boards? | There is no single test that you can perform on a prototype PCB that will guarantee its performance in all major EMC chamber tests, whether for consumer electronics, military, or aerospace applications. However, there are two simple tests that can provide a good level of confidence. Use a near-field probe: Scan the PCB with a near-field probe to identify particular frequencies or areas of the board that are radiating significantly more energy than expected. While near-field probe measurements cannot be directly compared with regulatory EMC limits because the test methods are different, they can help identify potential problem areas on the board. Use an RF current probe: For lower-frequency EMC concerns, particularly those involving emissions through cables, use a clamp-on RF current probe around all the conductors going into a single connector. This can provide a good indication of where potential EMC problems may exist. These tests do not directly replicate regulatory EMC tests, but they can help PCB designers identify potential issues early and improve confidence before formal EMC testing. |
| Is it good to always have a chassis ground? | It depends on the type of system and the chassis available. Having a chassis ground is a luxury because many consumer electronics and medical devices use plastic enclosures for cost, aesthetics, or safety reasons. In such cases, there is no conductive chassis to connect to, and it is still possible to design a perfectly good electronic system without a chassis ground. If the system does have a conductive chassis, determining the best way to use it is not always straightforward. In many cases, it makes sense to have a chassis reference, particularly near I/O ports where power and signals enter the system. However, a PCB does not necessarily need to be connected to the chassis for the chassis to provide effective shielding. The need for a chassis ground depends on the type of enclosure, the system design, and the specific EMC objectives. So, “always” is a strong term here. There are very few absolutes in PCB and EMC design, and the use of a chassis ground should be evaluated based on the specific application. |
| How significantly does the choice of PCB material affect EMI performance, and how should the material be selected based on the project’s electrical and EMC requirements? | The impact of PCB material on EMI performance depends largely on the frequency range and the design requirements. For typical EMC issues, roughly from 150 kHz to 6 GHz, particularly when dealing with interference that extends beyond an individual board, the effect of PCB material is generally negligible. In most cases, PCB material is rarely the source of a specific EMC problem during troubleshooting. However, when dealing with much higher-speed designs and signal integrity concerns, PCB material becomes significantly more important. It can have a moderate to significant impact on EMI performance because it directly affects signal integrity, transmission-line impedance, impedance stability, and high-frequency losses. PCB materials have different dielectric constants, loss tangents, and copper foil roughness, all of which influence signal loss. At high frequencies, this signal loss can become a dominant factor in controlling or containing direct emissions. Therefore, the PCB material should be selected based on the project’s signal integrity, operating frequency, transmission-line, and high-frequency loss requirements, rather than treating material selection as a primary factor for typical lower-frequency EMC problems. |
| Should you split digital and analog ground? | No. Splitting digital and analog ground is a recommendation that has been around for a long time, but it is very rarely necessary in modern PCB designs. When high-speed signals have a continuous ground plane adjacent to them, their return currents tend to stay closely coupled to the signal traces rather than spreading randomly across the board. Therefore, if the board is laid out so that high-speed signals consistently have a continuous return path directly beneath them, there is usually no need to split the digital and analog ground planes. In fact, seeing a split ground plane can be a red flag for potential EMC problems, because it can disrupt the return-current path and force currents to take longer paths. There are cases where separating digital and analog grounds may be necessary, but those situations require careful consideration and mitigation of the EMC risks introduced by the split. Ground planes should not be split simply because an application note recommends it; the decision should be based on the specific circuit and EMC requirements. |
| What do you think about mechanical shielding like metal can? Is that effective? | Absolutely. Mechanical shielding, such as a metal can, can be highly effective when properly implemented. However, proper implementation is critical to achieving good shielding performance. Simply placing a metal can over a circuit without providing solid connections around its perimeter will significantly reduce its effectiveness. PCB-level shielding has many of the same considerations as shielding with a larger metal enclosure. For example, any apertures or openings in the shield can affect its performance, particularly if their dimensions are significant relative to the wavelengths of the frequencies of concern. These openings can become potential paths for electromagnetic radiation. The shield must also be properly bonded. When using a metal can for PCB-level shielding, consider in advance where and how the can will make electrical contact. Ideally, it should have a continuous, low-impedance connection to an adjacent ground plane, potentially around the entire perimeter (360°). Therefore, metal-can shielding can provide excellent EMI performance, but its effectiveness depends on proper bonding, perimeter connections, and careful control of apertures and openings. |
| I have a system consisting of 10 cards connected in series. Due to its architecture, each card receives power and ground, which it then passes to the next, and so on. In addition, the system has chassis ground available to all cards. What considerations should I have regarding the ground and chassis ground? How should I connect both grounds? | This is highly dependent on the specific system architecture, industry, and grounding requirements, so it is difficult to give a single recommendation that applies to every 10-card system. For an aerospace application, for example, it may be desirable for each individual card to have a connection to chassis ground. That connection might be made through a capacitor or a very high resistance, depending on the grounding architecture and requirements. Aerospace systems have additional considerations, such as charge buildup and grounding paths, that need to be addressed. In other applications, particularly power electronics, you may want significantly more isolation between the circuit ground and chassis ground. Therefore, the appropriate connection between the two grounds depends on the industry and the specific system requirements. For aerospace applications, NASA Handbook 4001 is publicly available and provides useful guidance on different grounding architectures and their considerations. Ultimately, for a system with multiple interconnected cards, the appropriate grounding strategy should be determined by reviewing the complete electrical schematics, grounding architecture, and mechanical packaging. Without that information, it would be difficult to provide a specific recommendation for how the circuit ground and chassis ground should be connected. |
| How can radiation or EMC issues be eliminated in MHz switching Buck Converters that some requirements require compact spaces for indicators? | For MHz switching buck converters, layout is one of the most important factors in controlling radiation and EMC issues, especially when the available board space is limited. Pay particular attention to the return-current paths. Make sure the return currents do not have to change through a large number of layers or take long, indirect routes across the board. Instead, keep the return paths as short, direct, and tightly coupled as possible. Controlling these current loops and return paths effectively can significantly reduce EMC problems without requiring a large amount of additional board area for filtering components. |
| How does reinforced insulation affect PCB layout and EMC/EMI performance in an isolated power or high-voltage design; What PCB minimum creepage, clearance need for To Pass EMI and EMC testing since PCB board have very dense placement? | Creepage and clearance should be considered separately from EMI and EMC requirements. For a PCB with high-power or high-voltage circuitry, the first step should be to determine all required creepage and clearance distances based on the applicable safety and functional requirements. Once these requirements are established, the EMI/EMC mitigation strategy should be designed around them. Creepage and clearance are primarily related to safety and functional isolation, so EMI/EMC measures should not compromise the required isolation. After determining the required creepage and clearance, focus on the PCB stackup and layout. Make sure that traces do not unintentionally cross plane splits or violate the intended isolation boundaries. Any isolation required by the design should remain properly maintained throughout the PCB layout. Finally, pay close attention to return-current paths. Keeping return currents controlled and ensuring they do not cross isolation boundaries or take unintended paths is critical for good EMI/EMC performance. This aspect is often not emphasized enough during schematic design, but it can have a significant impact on the final PCB’s EMC behavior. |
| How to route ESD noise out of the MCU Sections if some GPIO having Metal Keys? | If the GPIOs are connected to metal keys and are therefore exposed to potential ESD events, the first approach would be to provide dedicated ESD protection rather than trying to route the ESD noise through the MCU section. A common solution is to place TVS (transient voltage suppression) diodes or a similar ESD protection circuit on the exposed GPIO lines. These devices help divert transient ESD energy away from the MCU and protect the sensitive circuitry. Therefore, for GPIOs connected to metal keys, TVS diodes or other suitable ESD protection devices would be the first choice for addressing this type of ESD risk. |
| Which is better for ground connections that components having on top layer and adjacent layer is ground layer then via to each ground pad of components or use polygon and multiple striching vias? | The preferred approach is to place the components on the top layer with a solid, adjacent ground plane, rather than relying primarily on polygons, islands, or similar structures. Ideally, Layer 2 should be as solid a ground plane as possible, with multiple stitching vias connecting the component ground pads to this plane. This provides a continuous and low-impedance return path. Using polygons and islands can work, particularly when the layout has been specifically designed to minimize the risks they introduce. However, these structures can create potential problems with return-current paths and should therefore be used with caution. Whenever possible, prioritize a solid ground plane on an adjacent layer. The same principle applies to the bottom side of the board. For example, on a six-layer PCB, it is desirable to have another solid ground plane, such as Layer 5, to provide a continuous return path. |
| Can EMC/EMI rules be added to PCB design rules in CAD tools? | Yes. Most high-end PCB CAD and layout tools provide design rule checkers (DRCs) specifically for EMI/EMC considerations. These tools allow designers to customize the EMI/EMC rules and use them as design constraints during PCB layout. However, there is a potential drawback: on a complex board, the EMC/EMI checker may flag a very large number of issues, sometimes hundreds or even thousands—which can become overwhelming. Therefore, the rules need to be configured carefully so that the checks focus on the most relevant EMC risks. In general, most advanced PCB layout tools allow you to customize the EMI/EMC rules used as design constraints, although the exact capabilities vary between CAD platforms. |
| Are grounding pads around the perimeter of the board touching the chassis useful or useless when having a metal chassis? Or would just a copper trace around the edge of the board touching the metal be enough? | Yes, intentional grounding pads around the perimeter of the PCB are useful and preferred when the board is mounted in a metal chassis. In theory, a copper trace running around the edge of the PCB and making contact with the metal chassis could provide a grounding connection. However, in practice, it is not something I would rely on because the effectiveness of that connection can vary depending on the mechanical contact and implementation. I would much rather use intentional grounding pads around the board perimeter to establish a reliable and deliberate connection between the PCB and the metal chassis. |