In modern industrial systems, circuit board layout has become an integral part of the design itself. Design engineers therefore need to understand the mechanisms that affect the performance of high-speed signal-chain designs. In high-speed analog signal-chain design, PCB layout and routing involve many choices. Some choices matter more than others, and some depend on the application. The final answer varies, but in every case the designer should aim to eliminate errors in best practices rather than focus excessively on every layout detail. The guidance here is intended to help with the next high-speed design project.
Highlights:
- The exposed pad is both an electrical ground connection and a primary thermal path, so its solder interface must be uniform, well supported by vias, and properly filled before assembly.
- Decoupling should be selected by capacitor frequency response and PDS impedance, not by scattering many capacitor values across the board; a closely spaced power and ground pair also provides useful intrinsic high-frequency layer capacitance.
- Layer-to-layer coupling and unnecessary ground splits can degrade sensitive ADC performance, so circuit partitioning and controlled return paths deserve more attention than automatic ground separation.
Exposed Pad
The exposed pad, sometimes called EPAD and often referred to as Pin 0, is easy to overlook, yet it is critical for getting the full performance of a signal chain and for adequate heat removal from the device. The exposed pad is the pad beneath most modern devices. It is an important connection because all internal grounds of the chip connect to the center point under the device. Many converters and amplifiers no longer have separate ground pins for this reason.
The key is to attach this pad securely to the PCB by soldering so that a reliable electrical and thermal connection is formed. If the connection is weak, the result can be unpredictable; in practical terms, the design may fail to perform as intended.
Creating the Best Connection
Three steps help achieve the best electrical and thermal connection through the exposed pad. First, where possible, replicate the exposed pad on each PCB layer. The purpose is to form a dense thermal connection to all grounds and ground planes so heat can spread quickly. This step is relevant for high-power devices and for applications with a high channel count. Electrically, it also provides a good equipotential connection for all ground planes. The exposed pad can even be replicated on the bottom layer, where it can serve as a thermal ground point for decoupling and as a mounting location for a bottom-side heat sink (see Figure 1).

Figure 1 | Example of exposed pad layout
Second, divide the exposed pad into multiple identical sections in a checkerboard pattern. Use a silkscreen crosshatch grid over the opened exposed pad, or use solder mask. This step ensures a robust connection between the device and the PCB. During reflow assembly, it is not possible to control exactly how solder paste flows and finally connects the device to the PCB. A connection may exist but be unevenly distributed. It may consist of only one small connection, or worse, a connection at a corner. Dividing the exposed pad into smaller areas helps ensure that each area has a connection point, producing a more reliable and uniform exposed-pad connection (see Figures 2 and 3).

Figure 2 | Example of improper EPAD layout
Third, make sure that each section has vias connecting it to ground. Each area is usually large enough to place multiple vias. Before assembly, it is very important to fill each via with PCB solder paste or epoxy. This prevents exposed-pad solder paste from flowing back into the via voids and interfering with a proper connection.

Figure 3 | Example of a better EPAD layout
Decoupling and Layer Capacitance
Engineers sometimes lose sight of the purpose of decoupling and simply scatter many capacitors of different sizes across the board to connect a lower-impedance supply to ground. The question remains: how many capacitors are needed? Much of the related literature states that many capacitors of different sizes must be used to reduce the impedance of the power delivery system (PDS), but that is not entirely correct. Instead, it is enough to choose capacitors of the right size and the right type to reduce PDS impedance.
For example, consider designing a 10mΩ reference layer. The red curve represents a design that uses many capacitors of different values on the board, such as 0.001μF, 0.01μF, 0.1μF, and others. This of course can reduce impedance over the 500MHz frequency range. Now look at the green curve. The same design uses only 0.1μF and 10μF capacitors. This demonstrates that if the correct capacitors are used, so many capacitors are not required. It also helps save space and bill-of-materials (BOM) cost.
Note that not all capacitors are equivalent. Even from the same supplier, process, size, and style can differ. If the correct capacitors are not used, whether many capacitors or several different types, the result can work against the PDS. The result may be an inductive loop. Capacitors placed improperly, or capacitors using different processes and types and therefore responding differently to frequencies within the system, may resonate with each other (see Figure 4).

Figure 4 | Resonant capacitor
It is important to understand the frequency response of the capacitor types used in the system. Selecting capacitors arbitrarily can waste the effort spent designing a low-impedance PDS.
High-Frequency Layer Capacitance for the PDS
A compliant PDS design requires a variety of capacitors. Typical capacitor values used on a PCB can reduce impedance only from DC or near-DC frequencies to about the 500MHz range. Above 500MHz, capacitance depends on the internal capacitance formed by the PCB. Note that closely stacked power and ground planes help.
The PCB stackup should be designed to support substantial layer capacitance. For example, a six-layer stackup may include a top signal layer, a first ground layer, a first power layer, a second power layer, a second ground layer, and a bottom signal layer. The first ground layer and the first power layer are placed close to each other in the stackup, with a spacing of 2 to 4 mil between them, forming an intrinsic high-frequency layer capacitance. The great advantage of this capacitance is that it is free; it only needs to be noted in the PCB fabrication notes. If the power plane must be split and multiple VDD rails exist on the same layer, use the largest power plane possible. Do not leave voids, and pay attention to sensitive circuits. This maximizes the capacitance of that VDD layer.
If the design allows additional layers, for example changing from six layers to eight layers, place two additional ground layers between the first and second power layers. With the same core spacing of 2 to 3 mil, the intrinsic capacitance of the stackup then doubles (see Figure 5). This structure is easier to design than adding more discrete high-frequency capacitors to maintain low impedance at high frequency.

Figure 5 | Example of high-frequency layer capacitor
The task of the PDS is to minimize the voltage ripple produced in response to supply-current demand. This point is important but often overlooked. All circuits require current; some require large amounts, and some require current to be delivered at a fast rate. Adequate decoupling, low-impedance power and ground planes, and a good PCB stackup help minimize the voltage ripple caused by circuit current demand. For example, depending on the decoupling strategy used, if the system design has a switching current of 1A and the PDS impedance is 10mΩ, the maximum voltage ripple is 10mV. The calculation is simple: V=IR.
With a good PCB stackup, the high-frequency range can be covered, while conventional decoupling at the power-plane entry point and around high-power or inrush-current devices covers the low-frequency range (<500MHz). This ensures that PDS impedance is lowest across the entire frequency range. There is no need to place capacitors everywhere; placing a capacitor directly at every IC would violate many manufacturing rules. If such a severe measure is required, another problem exists in the circuit.
Layer Coupling
Some layouts inevitably have overlapping circuit layers. In some cases, a sensitive analog layer, such as a power, ground, or signal layer, may have a high-noise digital layer below it.

Figure 6 | Example of cross-coupled layer
This is often ignored because the high-noise layer is on another layer, below the sensitive analog layer. However, a simple experiment can prove that this is not the case. Consider one layer and inject a signal into either layer. Then connect the other layer, the adjacent layer, to a spectrum analyzer. The amount of signal coupled into the adjacent layer is shown in Figure 7. Even with 40 mil spacing, the structure is still capacitive in a sense, so it still couples signals into the adjacent layer at certain frequencies.

Figure 7 | Measured results for the cross-coupled layer
Figure 7 shows such an example. For instance, assume that a high-noise digital layer on one plane has a high-speed switching 1V signal. This means that another layer will see 1mV of coupling, or about 60dB isolation. For a 12-bit ADC with a 2-Vp-p full-scale swing, this is 2LSB of coupling. For a particular system this may not be a problem, but note that if the system sensitivity is improved by two bits, from 12-bit to 14-bit, the sensitivity to this coupling increases only four times, that is, 8LSB.
Ignoring this type of cross-layer coupling can cause a system to fail or can weaken the design. It is important to recognize that coupling between two layers can exceed expectations. Pay attention to this when noise spurs are found coupling within the target spectrum. Sometimes the layout dictates that an unintended signal or layer should cross-couple into a different layer. This is also worth attention when debugging a sensitive system. The problem may be on the layer below.
Split Grounding
One of the most common questions from analog signal-chain designers is whether the ground plane should be split into AGND and DGND planes when an ADC is used. The simple answer is: it depends. The detailed answer is: usually do not split. Why not? Because in most cases, blindly splitting the ground plane only increases the inductance of the return path, and the harm outweighs the benefit.
From the formula V=L (di/dt), it can be seen that voltage noise increases as inductance increases. As inductance increases, the PDS impedance that designers work to suppress also increases. As the demand for higher ADC sampling rates continues to grow, the ways to reduce switching current (di/dt) are limited. Therefore, unless a split ground plane is required, keep these ground connections intact.
The key is to partition the circuits properly so that splitting the ground plane is unnecessary. Note that if the layout allows circuits to remain in their own areas, there is no need to split the ground plane. Such partitioning can provide a star ground, which confines return currents to specific circuit sections.
For example, a split ground plane is needed when size constraints prevent the board from achieving good layout partitioning. This may occur when traditional design requirements or dimensions require a dirty bus power supply or high-noise digital circuits to be placed in certain areas. In such cases, splitting the ground plane is critical to achieving good performance. However, for the overall design to be effective, these ground planes must be connected together somewhere on the board through a bridge or connection point. The connection points should therefore be distributed evenly across the split ground planes.
In the end, there is often one connection point on the PCB that is the best location for return current to pass without degrading performance or forcing return current to couple into sensitive circuits. If this connection point is at, near, or under the converter, no split ground is needed.
Conclusion
With so many possible optimum choices, layout considerations can be confusing. Techniques and principles have long formed part of a company's design culture. Engineers tend to draw on experience from earlier designs, while time-to-market pressure makes designers reluctant to change or try new technologies. They remain constrained by risk trade-offs until a major system-level problem appears.
At the evaluation-board, module, and system levels, a simple single-ground scheme is best. Good circuit partitioning is essential, and it also affects layer assignment and adjacent-layer layout. If a sensitive layer sits above a high-noise digital layer, be aware that cross-coupling may occur. Assembly is also important. Manufacturing notes provided to the PCB fabricator or assembly house should be used to full advantage to ensure a reliable connection between the IC exposed pad and the PCB.
Poor assembly often leads to suboptimal system performance. Decoupling near power-plane entry points and near the VDD pins of converters or ICs is always beneficial. However, to increase the inherent high-frequency decoupling capacitance, use tightly stacked power and ground planes with spacing of 4 mil or less. This approach adds no extra cost and requires only a few minutes to update the PCB manufacturing notes.
When designing layouts for high-speed, high-resolution converters, it is difficult to address every specific characteristic. Each application is unique. The key points described in this article should help design engineers better understand future system designs.
Related Reading:
Printed Circuit History and PCB Classification Guide
Grounding Principles, Star Ground, and Ground Planes in PCB Design
Mixed-Signal IC Grounding and Decoupling: AGND, DGND, and Clock Jitter
High-Speed ADC PCB Layout Rules: Grounding, Power, E-Pad
Non-Isolated Switching Power Supply PCB Layout: Hot Loops and Shielding