Grounding Concepts and Methods for PCB and Backplane Design

Grounding is one of the most effective ways to suppress electromagnetic interference and improve the EMC performance of electronic equipment. Correct grounding increases a product's immunity to electromagnetic disturbance while reducing the EMI it radiates. The principle is simple to state but easy to get wrong in practice, because the "ground" shown on a schematic symbol is not a zero-impedance node, and the way grounds are split and rejoined across a board and a backplane determines whether return current flows where the designer intended. This article explains what grounding means and why it is done, reviews the three basic grounding methods (single-point, multi-point, and floating), examines the ground-loop mechanisms that create interference, and then applies these principles to system, backplane, and board-level grounding, including the rules for splitting and rejoining different ground domains on a PCB.

Highlights:

Single-point grounding suits circuits below about 1 MHz, multi-point grounding suits circuits above 10 MHz, and mixed high/low-frequency designs should use hybrid grounding; in the transition band, keep ground leads shorter than λ/20 to avoid common-impedance coupling.
Multi-point grounding shortens the return path and suppresses high-frequency standing waves, but it can create ground loops that reduce immunity to external fields; loop area and impedance imbalance are the root causes of ground-loop EMI.
On a board, different ground domains should be rejoined through a ferrite bead or a single PCB point, with a 0.1 μF (or 0.01 μF) capacitor at the junction, and split lines at least 100 MIL wide to isolate the primary and secondary sides.

The Meaning of Ground

In electronic equipment, "ground" usually carries two meanings: "earth" (safety ground) and "system reference ground" (signal ground). Grounding means establishing a low-impedance conductive path between the system and some potential reference plane. "Earthing" takes the earth's potential as the reference and the earth as zero potential, connecting the metal enclosure and the circuit reference point of the equipment to earth.

Connecting a ground plane to earth is generally done for the following reasons:

To improve the stability of the equipment's circuit system.
To discharge static electricity.
To provide safety protection for operating personnel.

In switching and access network products, a board's ejector handle is typically connected to protective ground through its locating holes so that static charge can drain away. During an ESD test on the PON16, the DMU's ejector handle was not connected to PGND because a locating hole that should have been metallized was mistakenly designed as a non-metallized hole, so the board's handle never reached protective ground. When electrostatic tests (contact and air discharge) were performed on the rear panel of the chassis (central office or remote end), the board was prone to reset. After the pad design was changed and the handle was connected to PGND, the reset problem disappeared and the ESD test passed. This case highlights the importance of proper grounding and protective connection design in EMC design, particularly for ensuring ESD immunity and preventing unexpected equipment resets.

The Purpose of Grounding

Grounding serves three main purposes:

Safety, i.e., protective grounding.
Providing a stable zero-potential reference for signal voltages (signal ground or system ground).
Shielding grounding.

Basic Grounding Methods

Electronic equipment uses three basic grounding methods: single-point grounding, multi-point grounding, and floating ground.

Single-Point Grounding

In single-point grounding, only one physical point in the entire system is defined as the ground reference, and every other point that needs grounding is connected to that one point.

Single-point grounding is suitable for low-frequency circuits (below 1 MHz). If the system's operating frequency is high enough that the operating wavelength becomes comparable to the length of the ground lead, the single-point approach becomes problematic. When the ground line length approaches a quarter wavelength, it behaves like a short-circuited transmission line: the current and voltage on the ground line take the form of a standing wave, the line turns into a radiating antenna, and it no longer functions as a "ground." To reduce ground impedance and avoid radiation, the ground line length should be less than one-twentieth of a wavelength. Single-point grounding can generally be considered for power supply circuits. For the digital circuits widely used in these products, which contain abundant high-order harmonics, single-point grounding is generally not recommended.

Multi-Point Grounding

Multi-point grounding means that each ground point in the equipment is connected directly to the ground plane nearest to it, keeping the ground lead as short as possible.

The multi-point circuit structure is simple, and high-frequency standing-wave phenomena on the ground line are significantly reduced, making it suitable for high-frequency applications (above 10 MHz). However, multi-point grounding can create many ground loops inside the equipment, lowering the equipment's ability to withstand external electromagnetic fields. When multi-point grounding is used, ground loops deserve particular attention, especially when different modules and equipment are networked together.

Electromagnetic interference caused by ground loops: an ideal ground is a physical entity with zero potential and zero impedance, but a real ground has both resistance and reactance, so a voltage drop appears whenever current flows through it. The ground forms loops with other wiring (signal lines, power lines), and when a time-varying electromagnetic field couples into such a loop, an induced EMF appears in the ground loop and is coupled through it into the load, creating a potential EMI threat. Consider the following figure:

Figure 1 | Figure | Common-ground impedance coupling

Because of distributed capacitance, a loop B–C–D–E–F–A exists between the transmission line and ground. Because of the ground impedance, when the ground current Ig flows through the ground plane, it produces a voltage drop Vi across Zg — that is, a voltage Vi appears between points B and E of the circuit. This voltage Vi is common to both signal lines, driving currents I1 and I2 through them. Since the impedance of the paths taken by I1 and I2 differs, this impedance imbalance produces a differential-mode voltage V0 across the load. This is one source of ground-loop EMI.

When an external electromagnetic field links with the ground loop, it induces a voltage Vi in the loop that satisfies ∮E·dl = ?dΦ/dt, where:

E is the electric field strength,
dl is the differential vector element used in the contour integral around the loop,
Φ is the total magnetic flux through the area enclosed by the loop (the flux of B),
B is the magnetic flux density.

This voltage acts as a potential EMI source for the common-mode currents I1 and I2 that circulate around the two loop areas enclosing the two connecting wires.

Floating Ground

Floating ground means that the equipment's ground system is electrically isolated from earth.

Because of its intrinsic weaknesses, floating ground is not well suited to general large systems and is rarely adopted, so it is not discussed in detail here.

Mixed (Hybrid) Grounding

Combining the methods above yields hybrid grounding, in which different sections of a design use the technique best suited to their frequency range.

General Selection Principles for Grounding Methods

For a given device or system, at the highest frequency of concern (with corresponding wavelength λ), a circuit is treated as high-frequency when its transmission line length L becomes a significant fraction of λ, and as low-frequency otherwise. According to the rule of thumb, circuits below 1 MHz are best served by single-point grounding, while circuits above 10 MHz are better served by multi-point grounding. For frequencies in between, single-point grounding can be used as long as the longest transmission line L is less than λ/20, which avoids common-impedance coupling.

The general selection principles are:

Low-frequency circuits (<1 MHz): single-point grounding is recommended.
High-frequency circuits (>10 MHz): multi-point grounding is recommended.
Mixed high- and low-frequency circuits: hybrid grounding.

The system, backplane, and board grounding methods are described in the sections that follow.

System Grounding Methods

A detailed discussion of system grounding methods is provided in the grounding specification that governs the overall grounding architecture.

Backplane Grounding Methods

For existing products other than switching products, the system operates above 10 MHz and most of the circuitry is digital, containing abundant high-order harmonics. It is therefore recommended that, apart from BGND, all grounds be joined at the backplane — a multi-point connection in which every ground other than BGND (such as GND, PGND, AGND, and DGND) connects directly from each board to the nearest point on the backplane.

Case study: a comparison of multi-point connection versus single-point grounding on a 10G backplane (results pending).

Board Grounding Methods

At the circuit level, it is not appropriate to impose specific grounding requirements. For a given board, the necessary splitting is generally carried out according to the device datasheets. To join different ground types on a board, use a ferrite bead, or make a single-point connection directly on the PCB. For a power rail that is single-point connected without a ferrite bead, place a 0.1 μF (or 0.01 μF) capacitor at the single-point junction for filtering, with one end connected to that power rail and the other to the corresponding ground.

When splitting power and ground, take care to cut off the path by which EMI can leak from the primary side to the secondary side through the reference plane. This is especially important at the splitting of filters, common-mode chokes, ferrite beads, and similar devices.

The figure below shows the ground-splitting diagram for an isolation transformer from Pulse:

Two points about the ground split for this isolation transformer:

Position of the split: at the junction between the primary and secondary sides.
Width of the split line: no less than 100 MIL.

The purpose of this split is to isolate the primary and secondary sides and to control interference from the source end coupling to the secondary side through the reference plane. The ground-splitting diagram recommended by Intel, shown below, makes the same point: the position of the split line matters a great deal. Besides achieving isolation, adjacent-layer routing must be considered so that important signal lines do not cross the split region.

Sample Network Card Layout Layer 2 (Ground Plane)

For most of the ICs in use today, suppliers provide detailed PCB design requirements, including power and ground splitting. Hardware engineers should work with CAD engineers to analyze these requirements carefully and follow the supplier's recommendations wherever the actual situation permits.

Related Reading: