Coupons
Help
  • FAQ
    browse most common questions
  • Live Chat
    talk with our online service
  • Email
    contact your dedicated sales:

High-Speed ADC PCB Layout Rules: Grounding, Power, E-Pad

Author : Alex Chen | PCB Design & High-Speed Engineering Specialist

November 16, 2026


High-speed analog-to-digital converters rarely deliver their datasheet performance on a board that ignores the physical rules surrounding them. The silicon is characterized with clean supplies, quiet grounds, and undisturbed references; the PCB is where those conditions either exist or do not. This article works through the layout and routing practices that matter most when a high-speed converter sits at the center of the design: how to handle the analog and digital ground planes, how to build power planes that actually carry current, how to design the power delivery system and its decoupling, how to attach the exposed pad so that it works both electrically and thermally, and how to keep one PCB layer from coupling noise into another.

Each topic is treated as an engineering problem with a cause and a consequence, not as a checklist item. Where a rule has an exception, the exception and the conditions that create it are described. The intent is that a designer facing a converter with a particular sample rate, resolution, supply arrangement, and mechanical envelope can judge which practices apply, and why.

Highlights:

  • Splitting the analog and digital ground planes usually increases the inductance of the return current and therefore increases noise; in most designs the planes should be tied together, with the connection point placed near or beneath the converter.
  • A power plane placed 2 to 3 mil from its adjacent ground plane provides intrinsic layer capacitance at no cost, and a spread of decoupling values from 0.001μF to 100μF keeps the power delivery system impedance low across the frequency range.
  • An exposed pad only does its job when it is replicated on the available layers, divided into a checkerboard of smaller areas, and via-stitched and filled before reflow.

Should the AGND and DGND Planes Be Separated?

Meeting the datasheet specification with a high-speed converter depends on observing a small number of guiding principles. The first question designers usually raise is also the most persistent one: should the AGND and DGND ground planes be separated? The short answer is that it depends. The detailed answer is that in most cases they should not be.

Separating the ground planes generally does nothing but increase the inductance of the return current path, and that does more harm than good. The relationship is visible directly in V = L (di/dt): as inductance rises, the voltage noise rises with it. The same relationship applies in the other direction as well. As the switching current grows, which is exactly what happens when the converter's sampling rate is increased, the voltage noise grows too. For both reasons, the ground planes should be connected together.

There is a legitimate exception. In some applications, traditional design requirements dictate that a noisy bus supply or digital circuitry be confined to particular regions of the board, and dimensional constraints may simultaneously prevent a clean layout partition from being achieved. In that situation, splitting the ground planes is the key to good performance. Even then, the split is only viable if the planes are joined somewhere on the board through a bridge or a set of connection points, and those connection points should be distributed evenly across the separated planes. In practice, one of those points usually turns out to be the best location for the return current to cross without degrading performance, and that point is typically near or directly beneath the converter.

AGND vs DGND Planes

Building the Power Planes

When the power planes are defined, use all of the copper that those layers can offer. Wherever possible, do not share routing on a power plane. Additional traces and vias cut the plane into small fragments and quickly degrade it. The resulting sparse plane squeezes the current paths into the precise places that need them most, namely the supply pins of the converter. Forcing current through the narrow gaps between vias and traces raises resistance and produces a slight voltage drop at those supply pins.

The placement of the power planes matters just as much as their construction. A high-noise digital power plane should never be stacked directly on top of an analog power plane. Although the two occupy different layers, they can still couple to one another. To keep the risk of degraded system performance as low as possible, these types of planes should be separated in the stackup rather than stacked on each other.

Power Delivery System Design and Decoupling

The design of the printed circuit board's power delivery system (PDS) is often overlooked, yet it is critical for both system-level analog and digital designers. The objective of PDS design is to minimize the voltage ripple that appears in response to the current demanded by the supply. Every circuit needs current; some circuits need a great deal of it, and some need it delivered very quickly. A well-decoupled, low-impedance power or ground plane combined with a sound PCB stackup is what keeps the voltage ripple generated by those current demands to a minimum. As an illustration, if the design draws a switching current of 1A and the PDS impedance is 10mΩ, the maximum voltage ripple is 10mV.

Power Delivery System Design and Decoupling

Stackup for Intrinsic Layer Capacitance

The first step is to design a PCB stackup that supports substantial layer capacitance. A six-layer stackup, for example, might consist of 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 specified to sit close to each other in the stackup, with a separation of 2 to 3 mil, which forms an intrinsic 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 planes must be split because several VDD rails share the same layer, use the largest plane area that the layout allows. Do not leave voids in the plane, and keep sensitive circuits in mind while doing so. Maximizing the continuous copper maximizes the capacitance of that VDD layer. If the design permits additional layers, as when moving from six layers to eight, the two extra ground layers should be placed between the first and second power layers. With the same 2 to 3 mil core spacing, the intrinsic capacitance of the stackup is then doubled.

Decoupling Capacitor Placement

For an ideal PCB stackup, decoupling capacitors should be used both at the entry point of the power planes and around the device under test. This ensures that the PDS impedance stays low across the entire frequency range. Using several capacitors ranging from 0.001μF to 100μF helps to cover that range. It is not necessary to place capacitors everywhere. Pressing capacitors directly against the DUT would break every manufacturing rule there is. If such a drastic measure seems necessary, it is a sign that the circuit has some other problem.

The Exposed Pad (E-Pad)

The exposed pad, sometimes called pin 0, is the pad beneath most modern high-speed ICs. It is an important connection: all of the chip's internal grounds are brought to a central point under the die through it. Because the exposed pad exists, many converters and amplifiers can be built without dedicated ground pins. The critical requirement is that soldering this pad to the PCB produces a stable and reliable electrical connection as well as a thermal connection. If it does not, the system can be seriously degraded.

Three Steps to a Reliable E-Pad Connection

Optimal electrical and thermal connection of the exposed pad can be achieved in three steps.

  1. Wherever possible, replicate the exposed pad on each PCB layer. This provides a thick thermal path for all of the grounds, so heat spreads and escapes quickly, which is especially important for high-power devices. Electrically, it gives all of the ground planes a good equipotential connection. When the pad is replicated on the bottom layer, that copper can serve as the decoupling ground point and as the place where a heatsink is mounted.
  2. Divide the exposed pad into a number of identical sections. A checkerboard pattern is best, and it can be produced with a silkscreen crosshatch or with the solder mask. During reflow assembly there is no way to control how the solder paste flows to form the connection between the device and the PCB, so connections may exist without being evenly distributed, or worse, they may be small and confined to the corners. Splitting the pad into smaller sections gives every area its own connection point, which ensures a reliable and uniform bond between the device and the board.
  3. Ensure that every section has vias connecting it to ground. Each region is usually large enough to hold several vias. Before assembly, each via must be filled with solder paste or epoxy. This step is very important: it prevents the solder paste on the exposed pad from reflowing down into the via voids, which would reduce the chance of a correct connection.

Layer-to-Layer Crosstalk Cannot Be Ignored

In PCB design, the layout and routing of high-speed converters will inevitably place one circuit layer in overlap with another. In some cases a sensitive analog layer, whether power, ground, or signal, may sit directly above a high-noise digital layer. Most designers assume this is unimportant because the layers are physically separate. Is that assumption correct? A simple test answers the question.

Choose one of two adjacent layers and inject a signal into it. Then connect the other layer to a spectrum analyzer. A considerable amount of the signal will be seen coupling into the adjacent layer. Even with a spacing of 40 mil, adjacent layers still form a capacitance in a certain sense, so at some frequencies the signal couples from one layer into the other.

Consider a quantitative example. Suppose the high-noise digital section on one layer carries a 1V signal with high-speed switching. With 60dB of layer-to-layer isolation, the non-driven layer will see a 1mV signal coupled from the driven layer. For a 12-bit analog-to-digital converter with a 2Vp-p full-scale swing, that represents 2LSB of coupling. Whether this matters depends on the particular system, but note what happens as resolution increases: moving from 12 bits to 14 bits raises the sensitivity by a factor of four, so the resulting error grows to 8LSB.

Ignoring cross-plane and cross-layer coupling may not cause a system design to fail outright, and it may not visibly weaken the design, but the designer must remain alert to it, because coupling between two layers can be greater than expected. When noise spurs are found coupling inside the target spectrum, this is worth keeping in mind. Layout and routing can sometimes route an unintended signal, or couple one layer into a different layer. When debugging a sensitive system, remember that the problem may lie on the layer underneath.

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 and Routing Best Practices

Non-Isolated Switching Power Supply PCB Layout: Hot Loops and Shielding

Alex Chen | PCB Design & High-Speed Engineering Specialist Alex Chen | PCB Design & High-Speed Engineering Specialist

Alex Chen is a senior PCB design engineer with extensive experience in high-speed and high-density circuit design. He specializes in signal integrity, impedance control, and multilayer PCB layout optimization. At AIVON, he reviews and refines content related to PCB design principles, EDA tools, and advanced layout techniques. His expertise helps engineers avoid common design pitfalls and improve performance, reliability, and manufacturability in complex PCB projects.

Related Tags


2026 AIVON.COM All Rights Reserved
Intellectual Property Rights | Terms of Service | Privacy Policy | Refund Policy