Categories

The Role of PCB Stackup in Controlling EMI Radiation and Design Techniques

There are many ways to solve EMI problems. Modern EMI suppression methods include the use of EMI suppression coatings, appropriate EMI suppression components, and EMI simulation design. This article starts from the most fundamental PCB layout and discusses the role of PCB layer stacking in controlling EMI radiation, along with relevant design techniques.
Aug 7th,2026 101 Views

There are many ways to solve EMI problems. Modern EMI suppression methods include the use of EMI suppression coatings, appropriate EMI suppression components, and EMI simulation design. This article starts from the most fundamental PCB layout and discusses the role of PCB layer stacking in controlling EMI radiation, along with relevant design techniques.

Power Buses

Placing decoupling capacitors of appropriate capacitance near the power pins of an IC can make the output voltage transitions faster. However, the problem does not end there. Because capacitors have a limited frequency response, they cannot provide clean harmonic power across the entire frequency band to drive the IC output. In addition, transient voltages formed on the power bus cause voltage drops across the inductance of the decoupling path, and these transients are a major source of common‑mode EMI interference. How should we address these issues?

For the ICs on our board, the power plane surrounding the IC can be regarded as an excellent high‑frequency capacitor. It can collect the energy that leaks from discrete decoupling capacitors and supply high‑frequency energy for clean output. Moreover, a good power plane has low inductance, so the transient signals caused by that inductance are smaller, thus reducing common‑mode EMI.

Of course, the connection from the power plane to the IC power pins must be as short as possible, especially as the rise times of digital signals become increasingly faster. Ideally, it should connect directly to the pad of the IC power pin – though this is a separate topic.

To control common‑mode EMI, the power plane must aid decoupling and have sufficiently low inductance. This requires a well‑designed pairing of power and ground planes. Some may ask: how good is good enough? The answer depends on the separation between planes, the dielectric material, and the operating frequency (i.e., a function of the IC rise time). Typically, with a power‑plane spacing of 6 mils and FR4 dielectric, the equivalent capacitance per square inch is about 75 pF. Clearly, smaller spacing yields larger capacitance.

Devices with rise times between 100 and 300 ps are not yet common, but given the current pace of IC development, a high proportion of devices will fall into this range. For circuits with 100‑300 ps rise times, a 3‑mil spacing will no longer be adequate for most applications. At that point, it will be necessary to use layer spacings below 1 mil and replace FR4 with higher‑permittivity dielectrics. Today, ceramic and ceramic‑filled plastics can meet the design requirements for 100‑300 ps rise‑time circuits.

Although new materials and methods may be adopted in the future, for today's typical 1‑3 ns rise‑time circuits, with 3‑6 mil plane spacing and FR4 dielectric, this is generally sufficient to handle the high‑order harmonics and keep transient signals low enough – in other words, common‑mode EMI can be reduced significantly. The PCB stackup examples in this article assume a spacing of 3‑6 mils.

Electromagnetic Shielding

From a signal routing perspective, a good stackup strategy is to place all signal traces on one or more layers that are immediately adjacent to power or ground planes. For the power supply, a good strategy is to place the power plane adjacent to the ground plane with as small a distance as possible between them. This is what we call the "layering" strategy.

PCB Stackup

What stackup strategy helps with shielding and EMI suppression? The following layer‑stacking schemes assume that power current flows on a single layer, with a single voltage or multiple voltages distributed across different sections of that same layer. The case of multiple power layers will be discussed later.

4‑Layer Boards

Four‑layer board designs have several potential issues. First, the traditional 62‑mil‑thick four‑layer board, even with signal layers on the outside and power/ground on the inside, still has too large a spacing between the power and ground planes.

If cost is the primary concern, the following two alternatives to the traditional 4‑layer design can be considered. Both can improve EMI suppression performance, but they are only suitable when component density is low enough and there is sufficient area around the components to place the required power copper pours.

The first and preferred option is to use the outer layers as ground planes and the two inner layers as signal/power layers. Power on the signal layers is routed with wide traces, which lowers the impedance of the power current path and also lowers the impedance of the signal microstrip paths. From an EMI control perspective, this is the best 4‑layer PCB structure available. The second option places power and ground on the outer layers and signals on the two inner layers. This offers less improvement over the traditional 4‑layer board, and the inter‑layer impedance remains as poor as in the conventional design.

If controlled impedance is required, both stackups require careful routing of traces under the power and ground copper islands. Additionally, the copper islands on the power or ground layers should be interconnected as much as possible to ensure DC and low‑frequency connectivity.

6‑Layer Boards

If the component density on a 4‑layer board is relatively high, a 6‑layer board is preferable. However, some 6‑layer stackups provide poor electromagnetic field shielding and do little to reduce transients on the power bus. Two examples are discussed below.

In the first example, power and ground are placed on layers 2 and 5 respectively. The high impedance of the power copper pour is very unfavourable for controlling common‑mode EMI radiation. However, from an impedance control perspective, this approach is quite correct.

In the second example, power and ground are placed on layers 3 and 4. This solves the power copper impedance problem, but differential‑mode EMI increases because the outer layers (1 and 6) have poor shielding. If the number of signal traces on the outer layers is minimised and their lengths are kept very short (less than 1/20 of the wavelength of the highest signal harmonic), this design can address differential‑mode EMI. Filling unused areas on the outer layers with copper and grounding that copper (at intervals of 1/20 wavelength) provides especially good differential‑mode EMI suppression. As mentioned earlier, the copper fills should be connected to the internal ground layer at multiple points.

A common high‑performance 6‑layer design uses layers 1 and 6 as ground, and layers 3 and 4 for power and ground. With two signal microstrip layers placed between the power and ground planes, EMI suppression is excellent. The drawback is that only two routing layers are available. As noted earlier, if the outer traces are short and unused areas are copper‑filled, a conventional 6‑layer board can achieve the same stacking effect.

Another 6‑layer arrangement is: signal, ground, signal, power, ground, signal. This provides an environment suitable for high‑level signal integrity design. Signal layers are adjacent to ground, and power and ground are paired. The obvious disadvantage is the unbalanced layer stack.

This often causes manufacturing difficulties. The solution is to fill all empty areas on layer 3 with copper. If, after filling, the copper density on layer 3 approximates that of the power or ground layer, the board can be loosely considered as structurally balanced. The filled areas must be connected to power or ground. The via spacing remains 1/20 wavelength – not necessarily required everywhere, but ideally should be followed.

10‑Layer Boards

Because the insulating layers between multiple layers are very thin, 10‑ or 12‑layer boards have very low inter‑layer impedance. As long as the layering and stacking are sound, excellent signal integrity can be expected. Manufacturing a 12‑layer board to a 62‑mil thickness is difficult, and not many fabricators can produce it.

Since signal and return layers are always separated by an insulating layer, allocating the middle six layers for signal routing is not optimal in a 10‑layer design. Moreover, it is important to place signal layers adjacent to return layers. A recommended stackup is: signal, ground, signal, signal, power, ground, signal, signal, ground, signal.

This arrangement provides good paths for signal current and its return current. An appropriate routing strategy is: route layer 1 in the X direction, layer 3 in the Y direction, layer 4 in the X direction, and so on. Intuitively, layers 1 and 3 form a pair, layers 4 and 7 form a pair, and layers 8 and 10 form the last pair. When a signal needs to change routing direction, it should be routed from layer 1 through a via to layer 3 before changing direction. In practice, this may not always be possible, but it should be followed as a design concept.

Similarly, when a signal changes direction, it should go through vias between layers 8 and 10, or from layer 4 to layer 7. This ensures the tightest coupling between the forward and return paths. For example, if a signal is routed on layer 1 and its return is on layer 2 only, then even if the signal is transferred via a via to layer 3, the return path remains on layer 2, thereby maintaining low inductance, high capacitance, and good EMI shielding.

What if the actual routing differs? For instance, if a signal on layer 1 goes through a via to layer 10, the return signal must then find a ground plane on layer 9. The return current must locate the nearest ground via (such as the ground pin of a resistor or capacitor). If there happens to be such a via nearby, that is fortunate. If not, inductance increases, capacitance decreases, and EMI will definitely rise.

When a signal must leave its current pair of routing layers to other layers via vias, a ground via should be placed near that via so that the return signal can properly return to the appropriate ground layer. For the layer‑4 and layer‑7 pair, the signal return will come from the power or ground plane (layer 5 or 6), since the capacitive coupling between power and ground is good, allowing easy signal transfer.

Design with Multiple Power Planes

If two power planes of the same voltage need to deliver large currents, the board should be laid out with two pairs of power and ground planes. In this case, an insulating layer is placed between each power‑ground pair. This yields the desired two power buses with equal impedance, splitting the current equally. If the stacking of the power planes results in unequal impedances, the current distribution becomes uneven, transient voltages become much larger, and EMI increases sharply.

If the board contains multiple different supply voltages, multiple power planes will be required. Remember to create dedicated paired power and ground planes for each different supply voltage. In both cases, when determining the placement of the paired power and ground planes on the board, keep in mind the fabricator's requirements for balanced construction.

Summary

Given that most engineers design conventional printed circuit boards that are 62 mils thick, without blind or buried vias, the discussion in this article on layer stacking is limited to that scope. For boards with significantly different thicknesses, the stackup recommendations given here may not be ideal. In addition, boards with blind or buried vias follow different manufacturing processes, and the stacking methods described here are not applicable.

In PCB design, thickness, via fabrication, and the number of layers are not the critical factors. A good layer stackup is the key to ensuring proper bypassing and decoupling of the power bus, minimising transient voltages on power and ground planes, and shielding the electromagnetic fields of signals and power. Ideally, there should be an insulating layer between the signal routing layer and its return ground layer, and the spacing between paired layers (or multiple pairs) should be as small as possible. Based on these fundamental concepts and principles, it is possible to design boards that consistently meet requirements. With IC rise times already very short and continuing to decrease, the techniques discussed here are essential for solving EMI shielding problems.

About Maxipcb

Maxipcb empowers innovators to turn cutting-edge technologies into reality.We offer one-stop solutions for design, simulation, testing, PCB manufacturing, component procurement and SMT assembly, enabling efficient development, rapid deployment and risk control across the full product lifecycle.
Serving the world in communications, industrial automation, aerospace, automotive, semiconductor and beyond, we build a safer, more connected future together.