Written by: Anton Tishchenko
February 23, 2026
The failure rate of electromagnetic compatibility (EMC) testing across the electronics industry is a major problem. This problem persists in 2026, despite the widespread availability of information and knowledge. Its root causes are complex and often related to the internal project management processes of the company, rather than the lack of basic RF technical knowledge by the PCB design engineer. In this blog post, I am also going to assume that the reader is familiar with that. However, what else can we do as engineers to ensure the successful first-pass EMC testing for the product within our organisation? Let’s dive in.
Step 1. Gathering EMC-specific requirements
While this step typically falls under the systems engineering discipline in larger organisations, it is unreasonable to assume that the systems engineer or project manager working on the project has expert knowledge of EMC standards and test methods. It is ultimately the responsibility of the electronics/RF engineer to ask questions like:
● What is the operational environment going to be like for the product that I am working on?
● In which region is this product going to be placed on the market?
● What EMC/Radio standards apply to this environment and this region?
● Which tests and test levels are specified by these standards?
● What is the pass/fail criteria for these tests?
Unfortunately, this simple step is often missed during project planning, leading to inadequate product specifications and failed EMC tests. For example, a product designed for a vehicular operational environment would typically face more stringent immunity requirements for transient supply voltages than a product designed for consumer electronics / domestic environment. A PCB designer working on that product should know that, in order to select appropriately rated components, such as transient voltage suppression (TVS) diodes. Having a crystal-clear specification for EMC testing is critical for the first-pass EMC design, and if the product that you are working on does not have one, then it is your responsibility to make one. A simple Excel sheet or a page on Confluence works well in my experience.
Step 2. Deal with radiated emissions at the source
From Maxwell’s equations, we know that a time-varying current produces magnetic fields perpendicular to the direction of the current’s trajectory. In simple words, any current that is not a true direct current (DC) will produce radiated emissions. Any digital signal with rise-and-fall times is an example of a signal that varies in current and voltage over time. Identification of these noisy sources is a critical part of the design for low radiated emissions. It is the current variation that causes emissions, not the voltage. This is why this emission is the strongest at the source of the rise-fall transition, i.e. the switching transistor. Learning how to treat PCB-level emissions at the source is another key to a low radiated emissions profile and a successful EMC first pass, and there are certain must-do’s that apply to every PCB:
1. Master the energy flow, ensuring that every fast-speed switching transistor has a reservoir of charge timely available for its use. A simple example of this is a power supply pin of an MCU. During the transition, the pin can be expected to draw current at a fast speed. To satisfy this current demand, a charge supply is required. While the board itself may be modeled to have inductive and capacitive charges, it can only satisfy very small currents. So, typically, an additional decoupling capacitor is required. The placement of this capacitor is critical for the chip's EMI performance, because if a capacitor cannot satisfy the current draw, it will be drawn from elsewhere, creating large current loops and potentially interfering with other circuits. The typical rule that I follow is to have 1 decoupling capacitor for each power supply pin, valued between 1-100nF, depending on clock speed. Then, also place this capacitor no more than 2mm away from the pin, including the z-dimension, which is the board’s thickness if the capacitor has to be placed on the other side of the board. Remember that this capacitor is also a part of the current loop, so the placement of the 0V side of the capacitor is equally important. Do not point the capacitor away from the MCU, because this increases the current loop size. Instead, point it towards the 0V pins of the MCU, which are typically located at its center, or place it parallel to the IC.
2. Make sure the return path is as short as possible by providing tight control over the board layer stack. Fast-switching components and traces should have current return planes below or above them, no more than 0.1mm away. This is done to ensure that the radiated energy can be steered to propagate in the dielectric space between the coupling plane and the source as efficiently as possible. Notice that I wrote return planes and not ground planes. There is a difference. A power plane can also act as a return plane, even though this is less desirable, due to its susceptibility to inductive coupling. The rule of thumb is that a return plane should exceed the current source by at least 50mm in every direction to be effective. You can find out more about my PCB layer stack preferences in this video - How to Pass Radiated EMC. 3 Mistakes to Avoid.
3. Avoid crosstalk and interference from high-speed switching elements to other parts of the circuitry. This is where things can be tricky, because inductive coupling can easily propagate via grounds. Physical separation works best to prevent this. For example, if a switch-mode AC-DC supply is used, the best practice is to place it on a separate board, with its own shielding. Read more about the nested shielding approach here. Avoid sharing its 0V return paths with other circuitry. A classic example is an analogue temperature sensor that you may want to place on a heatsink for this AC-DC supply. Terminating the 0V pin of the sensor on the same ground that is used by the AC-DC supply itself often leads to the instability of the temperature reading. The best practice is to physically route the 0V return track of the sensor all the way back to the MCU and to terminate it there. Remember, if the circuit that you are dealing with is not high-speed switching, i.e., analogue sensors or audio, then there’s little benefit in treating it as such. Different rules apply to low-speed (<20kHz) switching circuits, and very often, ground splitting or star-grounds are acceptable, ensuring a sufficient current-carrying capacity, i.e., in your house wiring.
4. Match impedances between current sources and current sinks. A typical mismatch in impedance value results in losses and oscillations within the medium, which can easily create emissions of their own. A perfect impedance match, on the other hand, ensures a lossless transfer of energy from the current source to the current sink. This considers both the differential impedance (USB, HDMI, PCIe, Ethernet, DDRx clock), as well as the single-ended impedance (DDRx banks, audio clocks, etc.). There are specific values to target, such as 50- ohm SE impedance or 90-ohm Diff impedance, which should be added to your design rule check. The impedance is matched via an adjustment of trace width and the distance to the nearest return plane, so a PCB layer stack must be precise for the calculation to be accurate. A very common mistake is that the design has been made with one PCB layer stack, but it has been changed during the production process by the fabrication house. Make sure that this isn’t the case for you by communicating your impedance requirements clearly to the fabrication house.
Step 3. Design for immunity
Like it or not, the propagation of radio frequency energy is reciprocal, which means that whatever RF energy comes out can also come back in via the same path. The immunity to radio frequency interference is often overlooked during PCB design stages, although the remedy is very similar to the radiated emission treatment. This typically involves the nested shielding approach, mentioned in the previous section. An additional shield around critical fast-switching parts of the circuitry is not only helpful to contain emissions, but it also protects the circuitry from external influence or events. While the exact level of protection should be determined during the requirements specification stage, which will influence the shielding strategy, for example, the automotive EMC test level is 10 times higher than the radio EMC! However, for a successful first-pass EMC experience, at least one shield is a must. If you are developing a product that is going to be placed in a metal enclosure, that is frequently sufficient on its own, by following a simple rule that different parts of the metallic enclosure should make frequent contact with each other, i.e., through a conductive EMI gasket, multiple soldering points, or multiple conductive screw terminals. Also, avoid non-conductive surface finishing on the inside of the enclosure , such as painting or anodizing. Often, these have to be scraped off during EMC testing, but the issue can be easily prevented by masking contact areas during surface finishing. The continuity of the enclosure is easy enough to check prior to the EMC test house visit with a simple multimeter, so don’t skip that.
However, if you’re not dealing with a continuous metallic enclosure in your product, then things get a little bit tricky, and the localized shielding around critical components is a must-do. These include power supplies, MCU’s, memory IC’s, Bluetooth/Wi-Fi modules, to name a few, just not the antennas . It might sound obvious, but avoid placing shielding materials close to antennas, maintaining at least one full wavelength (λ) between the antenna and the shield in a 3D space. If this rule cannot be followed, ensure that the antenna gets re-simulated with the shielding material in its proximity to estimate the impact on its performance.
Finally, do not forget about conductive sources of interference, which typically propagate via inputs and outputs of the device, including its AC/DC power supplies, its USB/HDMI ports, and other connections with the outside world. The treatment of AC power supplies is a specialist topic, including additional components such as EMI filters and varistors. You can learn more about this topic in this video - How to Pass Conducted EMC and Immunity - 5 Tricks.However, other I/O’s can be easily protected with the simple addition of electrostatic discharge (ESD) protective elements, such as transient voltage suppression (TVS) diodes. There are different types, which are typically categorized in terms of a) protective voltage, b) unidirectional (DC signals) or bi-directional (AC signals), and c) capacitance of the TVS diode. For high-speed signals and audio, select the TVS with capacitance as low as possible to minimize its effects. Sometimes, TVS diodes should be added in other areas too, where contact with a human hand is likely, such as a volume control knob. Remember, it’s easier to remove a diode from a PCB than to add it to it, so try to develop a habit of ‘sprinkling’ the PCB with TVS diodes, even if most of them are labeled as do not fit (DNF).
Step 4. Go to the EMC test house and be prepared
Even after following the best design practices, the unexpected can be expected to happen. So, make sure that you are well prepared for that. You should own an EMC first-aid kit, full of TVS diodes, common-mode filters, ferrite beads, and wires of various gauge sizes. Then, bring it to the test house, just in case. A last-minute fix can easily make a difference between a wasted booking and a first-pass test report (even if it details the fix that you made!). Having said that, the fix must be repeatable in production. So, make sure that your EMC first-aid kit is frequently maintained and does not include obsolete parts. Also, do not try fixes that take more than 15 minutes to implement, i.e., re-wiring an entire board-to-board cable. Where possible, bring multiple variants of cables from different vendors, such as USB or HDMI, so that they can be swapped during testing. High-speed cables must have 360-degree termination on connectors and a sufficient thickness of the shielding material, which is often overlooked during cable production. This aspect is also discussed in this video - How to Pass Radiated EMC. 3 Mistakes to Avoid.
About the author
Anton Tishchenko received the B.Sc. degree in sound engineering from Wrexham University in 2015, and the M.Sc.(Distinction with Hons.) degree in electronic engineering from the University of Surrey in 2021, where he is currently pursuing a PhD degree within the 5G and 6G Innovation Centres, Institute for Communication Systems, focusing on reconfigurable metamaterials and metasurfaces for the next generation of wireless communication networks. Before his academic work, he established himself as an electronic/RF design specialist, developing hardware for the professional audio, telecommunications, and intelligent transportation industries. As a part of his Principal Electronic Design Engineer role at Cubic Transportation Systems Ltd, he has led several multi-disciplinary engineering teams throughout his career, on Transport for London (TfL), Network Rail, and MTA projects. He hosts an RF-dedicated YouTube channel, “Dr EMC”.
- February 23, 2026
- 6:09 pm