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

Grounding Principles, Star Ground, and Ground Planes in PCB Design

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

November 16, 2026


Grounding is one of the most troublesome aspects of system design. Its concept is relatively simple, but its implementation is complex. There is no concise, step-by-step method that guarantees good results, and handling certain details incorrectly can create difficult problems. For linear systems, ground is the reference point for signals. In single-supply systems, however, ground also serves as the return path for supply current. An inappropriate grounding strategy can seriously degrade the performance of high-precision linear systems.

For all analog design, grounding cannot be ignored. In PCB-based circuits, proper grounding is equally important. Fortunately, some high-quality grounding principles, particularly the use of ground planes, are intrinsic to the PCB environment. Because this is one of the significant advantages of PCB-based analog design, it receives particular attention here. A ground plane is valuable because it provides a low-impedance return path and a well-defined reference, but it must be used with the same care as any other grounding structure.

Other aspects of grounding must also be managed, including control of stray ground and signal-return voltages that can degrade performance. These voltages may result from external signal coupling, common currents, or simply excessive IR drop in ground conductors. Proper routing, conductor sizing, differential signal handling, and ground isolation techniques allow such parasitic voltages to be controlled.

An important topic is grounding techniques for mixed analog/digital signal environments. In fact, high-quality grounding can and inevitably does affect the entire layout discipline of mixed-signal PCB design. Current signal-processing systems generally require mixed-signal devices such as analog-to-digital converters (ADCs), digital-to-analog converters (DACs), and fast digital signal processors (DSPs). Because analog signals with wide dynamic range must be processed, high-performance ADCs and DACs are necessary. In a harsh digital environment, maintaining wide dynamic range and low noise is closely related to the use of good high-speed circuit design techniques, including proper signal routing, decoupling, and grounding.

In the past, "high-precision, low-speed" circuits were generally considered different from so-called "high-speed" circuits. For ADCs and DACs, the sampling or update frequency is generally used as the speed criterion. However, the following two examples show that in practice most signal-processing ICs today are truly "high speed" and must be treated as such to maintain high performance. This applies to DSPs, ADCs, and DACs alike.

All sampling ADCs suitable for signal-processing applications, meaning ADCs with built-in sample-and-hold circuits, operate from high-speed clocks with fast rise and fall times, typically several nanoseconds. Even when throughput appears low, they must be treated as high-speed devices. For example, a medium-speed 12-bit successive-approximation (SAR) ADC may use a 10 MHz internal clock while its sampling rate is only 500 kSPS.

Sigma-delta ADCs have a high oversampling ratio and therefore also require a high-speed clock. Even high-resolution "low-frequency" industrial measurement ADCs, such as the AD77xx series, with throughput rates from 10 Hz to 7.5 kHz, operate from a 5 MHz or higher clock and provide resolution up to 24 bits.

Further complicating the issue, mixed-signal ICs have both analog and digital ports, so the use of appropriate grounding techniques becomes more intricate. In addition, some mixed-signal ICs have relatively low digital currents, while others have high digital currents. In many cases, these two types of ICs require different treatment to achieve optimum grounding.

Digital and analog design engineers tend to examine mixed-signal devices from different perspectives. This article explains general grounding principles applicable to most mixed-signal devices without requiring detailed knowledge of the internal circuitry.

From the above, it is clear that there is no quick manual for grounding. It is not possible to provide a list of techniques that guarantees successful grounding. We can only say that ignoring certain things may cause problems. A method that works in one frequency range may not work in another. There are also conflicting requirements. The key to handling grounding is to understand how current flows.

Highlights:

  • Ground is both the signal reference and, in single-supply systems, the power return; poor grounding can severely degrade high-precision analog performance.
  • Sampling ADCs and DACs must be treated as high-speed devices even at low throughput because their internal clocks and sampling edges are fast; proper decoupling, routing, and ground isolation are essential.
  • Separate analog and digital grounds should be joined at one carefully selected star point, while converter AGND and DGND pins are typically tied together at the package and returned to system analog ground.

 

Good Grounding Guidelines

The theoretical basis of "star" grounding is that there is always one point in the circuit that serves as the reference for all voltages, called the "star ground" point. A useful analogy is a set of conductors radiating from a common ground point, like a star. The star point does not necessarily look like a star. It may be a point on a ground plane, but a key characteristic of a star ground system is that all voltages are measured with respect to a specific point on the ground network, not with respect to an undefined "ground" wherever the probe is placed.

Although theoretically very sound, the star grounding principle is difficult to implement in practice. For example, if a system is designed with star grounding and all signal paths are drawn to minimize interference between signals and to avoid the influence of high-impedance signal or ground paths, implementation problems follow. When power supplies are added to the schematic, the supplies introduce undesirable ground paths, or the supply current flowing into existing ground paths is large and/or noisy, thereby disrupting signal transmission.

Providing separate supplies for different parts of the circuit, and therefore separate ground returns, usually avoids this problem. For example, in mixed-signal applications, the analog and digital supplies are usually separated.

 

Star Grounding

Digital circuits are, in fact, noisy. Saturating logic such as TTL and CMOS briefly draws large currents from the supply during switching. However, because the immunity of logic stages can be hundreds of millivolts or more, the requirement for supply decoupling is often not stringent. In contrast, analog circuits are very susceptible to noise, including noise on the supply and ground rails. Therefore, to prevent digital noise from affecting analog performance, analog and digital circuits should be separated. This separation involves separating the ground returns and the supply rails, which can be troublesome in mixed-signal systems.

However, if a high-precision mixed-signal system is to achieve its full performance, it must have separate analog and digital grounds and separate supplies. This is critical. In fact, although some analog circuits operate from a +5 V single supply, this does not mean that the circuit can share the same noisy +5 V supply with a microprocessor, dynamic RAM, fan, or other high-current device. The analog portion must use such a supply to operate at maximum performance, not merely to remain operational. This difference necessarily requires close attention to the supply rail and ground interface.

Note that the analog ground and digital ground in the system must be connected at one point so that all signals reference the same potential. This star point, also called the analog/digital common point, must be carefully selected to ensure that digital currents do not flow into the ground of the analog portion of the system. It is usually convenient to establish the common point at the power supply.

 

Separate Analog and Digital Grounds

Many ADCs and DACs have separate "analog ground" (AGND) and "digital ground" (DGND) pins. On device data sheets, users are often advised to connect these pins together at the device package. This appears to conflict with the recommendation to connect analog and digital grounds at the power supply. If the system contains multiple converters, it also appears to conflict with the recommendation to connect analog and digital grounds at a single point.

In fact, there is no conflict. The "analog ground" and "digital ground" labels on these pins refer to the internal portion of the converter to which the pins connect, not to the system ground to which the pins must be connected. For an ADC, the two pins usually should be connected together and then connected to the system analog ground. Because the analog portion of the converter cannot tolerate the voltage drop that occurs when digital current flows through the bond wire to the chip, the two cannot be connected inside the IC package. They can, however, be connected externally.

Such a pin connection reduces the converter's digital noise immunity to some extent, by an amount equal to the common-mode noise between the system digital ground and the system analog ground. However, because digital noise immunity is often in the hundreds or thousands of millivolts, this is generally unlikely to be a problem.

The analog ground (AGND) and digital ground (DGND) pins of the data converter should be returned to the system analog ground.

Analog noise immunity is reduced only by the external digital current from the converter itself flowing into the analog ground. These currents should be kept small, which can be achieved by ensuring that the converter output is not heavily loaded. A good way to accomplish this is to use a low-input-current buffer at the ADC output, such as a CMOS buffer-register IC.

If the converter's logic supply is isolated with a small resistor and decoupled to analog ground with a 0.1 μF (100 nF) capacitor, all fast-edge digital currents from the converter will flow back to ground through that capacitor and will not appear in the external ground circuit. If a low-impedance analog ground is maintained and analog performance can be adequately ensured, the additional noise generated by external digital ground currents is essentially not a problem.

Grounding in PCB Design: Ground Planes, Return Currents, and Practical Layout

Ground Planes

The use of ground planes is closely related to the star grounding system discussed above. To implement a ground plane, one side of a double-sided PCB, or one layer of a multilayer PCB, is made from continuous copper and used as ground. The underlying principle is that a large amount of metal provides the lowest possible resistance. Because a large flat conductor is used, it also provides the lowest possible inductance. As a result, it offers the best conductive performance, including minimizing stray ground potential differences between conductive planes.

Note that the ground plane concept can also be extended to voltage planes. A voltage plane provides advantages similar to a ground plane, namely an extremely low impedance conductor, but it is used for only one or more system supply voltages. Therefore, a system may have multiple voltage planes as well as ground planes.

Although ground planes can solve many ground impedance problems, they are not a cure-all. Even a continuous copper foil has residual resistance and inductance; in certain cases, these are enough to prevent the circuit from working properly. Designers should take care not to inject very high currents into the ground plane, because this can produce voltage drops that interfere with sensitive circuits.

Maintaining a low-impedance, large-area ground plane is important for all analog circuits today. The PCB ground plane serves not only as a low-impedance return path for decoupling high-frequency currents that originate from fast digital logic, but also minimizes EMI/RFI radiation. Because of the shielding effect of the ground plane, the circuit is also less affected by external EMI/RFI.

Ground planes also allow the use of transmission line techniques, such as microstrip or stripline, to carry high-speed digital or analog signals. These techniques require controlled impedance.

Because a "bus wire" has impedance at the equivalent frequencies of most logic transitions, using it as a "ground" is completely unacceptable. For example, No. 22 standard wire has an inductance of about 20 nH/in. A transient current with a slew rate of 10 mA/ns generated by a logic signal, flowing through 1 inch of this wire, creates an unwanted 200 mV drop.

For a signal with a 2 V peak-to-peak range, this drop translates to about 200 mV, or 10% error, roughly "3.5-digit accuracy." Even in all-digital circuits, this error substantially reduces logic noise margin.

The inductance and resistance of the ground return conductor are shared by the analog and digital circuits, causing mutual interaction and ultimately producing error. One possible solution is to route the digital return current path directly to GND REF, as shown in the bottom diagram. This illustrates the basic concept of a "star" or single-point grounding system. True single-point grounding is difficult to implement in systems containing multiple high-frequency return paths. Because the physical length of each return current conductor introduces parasitic resistance and inductance, achieving low-impedance high-frequency grounding is difficult. In practice, the current loop must consist of a large ground plane to achieve low impedance at high frequencies. Without a low-impedance ground plane, it is almost impossible to avoid the shared impedance described above, especially at high frequencies.

All IC ground pins should be soldered directly to a low-impedance ground plane to minimize series inductance and resistance. For high-speed devices, conventional IC sockets are not recommended. Even "small-size" sockets can introduce unwanted shared paths through extra inductance and capacitance, degrading device performance. If a socket must be used with a DIP package, for example during prototyping, individual "pin sockets" or "cage sockets" are acceptable. These pin sockets are available in capped and uncapped versions. Because they use spring-loaded gold contacts, they ensure a good electrical and mechanical connection to the IC pins. However, repeated insertion and removal may reduce their performance.

Low-inductance, surface-mount ceramic capacitors should be used to decouple power pins directly to the ground plane. If through-hole ceramic capacitors must be used, their lead length should be less than 1 mm. Ceramic capacitors should be placed as close as possible to the IC power pins. Ferrite beads may also be required for noise filtering.

Does this mean that more "ground" is always better? Ground planes can solve many ground impedance problems, but not all of them. Even a continuous copper foil has residual resistance and inductance; in certain situations, these are enough to prevent the circuit from operating properly. 

Splitting the ground plane can redirect current flow, thereby improving accuracy.

Because of practical mechanical design, the power input connector is at one end of the board, while the power output section that must be near the heat sink is at the other end. The board has a 100 mm wide ground plane, and it also carries a power amplifier with a current of 15 A. If the ground plane is 0.038 mm thick, a 15 A current flowing through it produces a voltage drop of 68 μV/mm. For any precision analog circuit that shares this PCB and is referenced to ground, this voltage drop can cause serious problems. The ground plane can be split so that the large current does not flow into the precision circuit area, forcing it to flow around the split. This prevents the grounding problem, which does exist in this case, although the voltage gradient in the portion of the ground plane through which the current flows will increase.

In a system with multiple ground planes, be sure to avoid overlapping ground planes, especially analog and digital planes. This issue causes capacitive coupling from one layer, possibly digital ground, to another. Remember that a capacitor is formed by two conductors, the two ground planes, separated by an insulator, the PCB material.

Related Reading:

Printed Circuit History and PCB Classification Guide

Mixed-Signal IC Grounding and Decoupling: AGND, DGND, and Clock Jitter

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

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