Estimated reading time: 9 minutes

Designers Notebook: Power and Ground Distribution Basics

The principal objectives to be established during the planning stage are to define the interrelationship between all component elements and confirm that there is sufficient surface area for placement, the space needed to ensure efficient circuit interconnect, and to accommodate adequate power and ground distribution. Although most of the components selected for the electronic product will be surface-mount variations, it is not uncommon to include non-surface-mount devices, which do not have a surface-mount equivalent, such as connectors designed for through-hole termination or large components designed to manage power distribution.

Capacitors are the primary components for managing power and ground. Along with resistors and inductors, capacitors are one of the three basic electrical components that form the foundation of an electrical circuit. The capacitor functions as a storage device, retaining the electrical charge when voltage is applied across it and releasing the charge back into the circuit when needed.

Common capacitor functions include:

• Smoothing: DC signals are moderated using high capacitance to absorb ripple voltage
• Bypassing: Using capacitance in a filtering circuit allows unwanted signals to be directed away to bypass any system-generated frequency noise
• Coupling: Coupling between neighboring circuits can stop DC current and pass AC current.

Capacitor elements are also used to reduce electromagnetic interference (EMI) or other equipment-generated signal noise, to enable a more stable operating system.

Surface Distribution for Power and Ground
For the less complex single and two-sided circuit structures, power and ground can be integrated within signal interconnects. The conductors assigned to distribute power and ground are the first stage of the interconnect planning process, furnishing a significantly wider conductor than the signal-carrying conductors.

If the circuit board designer relies solely on wider circuit traces for power and ground distribution, the different ground connection locations typical of those shown in Figure 1 may cause unequal resistance values and localized voltage drops that can compromise signal integrity.

Before beginning the PCB design, the designer must establish the key operating conditions of the end product. For example, they need to understand the relationship between the thickness of the copper foil and the finished conductor width to comply with the expected current-carrying requirement. During the hole electro-plating process, an additional copper thickness forms onto the base-copper foil surface. Table 1 defines the base-copper foil thickness variations and the minimum post-plating process conductor thickness for IPC-Class 1, 2, and 3 circuit boards.

IPC-2221 Class 3 circuit boards, for example, will be specified for the high-reliability commercial electronic products that must continuously provide the required performance without interruption. During the circuit board fabrication process, this classification of product will undergo a higher-level inspection criterion to ensure that it will provide reliable and dependable service. Another dynamic that affects the current-carrying capability is location of the circuit. The circuit conductors on the outer layer(s) of the circuit board and those laminated within the subsurface layers will have differing proficiencies.

For example, the current carrying capacity of the external layer conductor may require increasing copper thickness from that defined for the internal layer conductor. The circuit board material, number of via holes, and SMT component land patterns within the circuit path can also affect current-carrying capacity. The factors in Table 2 are a conservative guide for estimating conductor width as it relates to copper foil thickness.

Note: For greater detail in determining the current-carrying capacity for printed circuit conductors, refer to IPC-2152. This document is the industry standard for defining the appropriate sizes for both internal and external conductors as a function of the current-carrying capacity required, and calculating the finished copper conductor’s temperature rise potential.

Developing Dedicated Power and Ground Layers
If multilayer circuit board construction is needed, the power and ground distribution will be most efficient if placed on one or more subsurface circuit layers. The power/ground may be furnished as wider conductors routed on the subsurface layer(s), enabling a direct path to the primary voltage management components mounted onto the outer surface through plated vias. Although wide power and ground conductors may be adequate for less demanding applications, dedicating entire layers of the circuit board to accommodate power and ground will significantly benefit product performance.

I recommend establishing copper power and ground layers (or planes) before beginning the circuit routing process for the multilayer circuit board. This may be simply furnishing a large copper area on an internal layer of the circuit board or dedicating entire circuit layers of the board for the power and ground distribution function.

The power plane uniformly distributes voltage to different parts of the board, while the ground plane allows the current to run smoothly, keeping power steady and reducing noise. Unlike thin signal traces that carry one signal at a time, these planes are wide and cover large areas. Think of signal conductors like small roads, and power and ground planes like highways for electrons. 

Having a common ground on the PCB is essential because it ensures that all conductors connected to the ground have the same reference point for measuring voltage. They let current move quickly and cleanly, which is important for modern, high-speed circuit boards. Furthermore, assigning entire layers of the multilayer circuit board to power and ground functions simplifies circuit interconnect for each component and also enhances product performance.

Dedicated Power and Ground Planes
When the power and ground potentials are retained on dedicated circuit layers, they help improve signal integrity by suppressing electromagnetic (EMI) noise and interference. Power and ground can be discrete areas of copper foil or cover the entire surface of the internal layers of the circuit board. How this is achieved will depend on the type of circuit board design system. Most CAD systems can define a power and ground area that appears as a solid graphic representation. When an area of copper is retained on the outer surface of the circuit board, it will likely be positioned to service ground isolation of specific components or a group of related components. For mixed-function applications, the designer may divide the power and ground planes on an inner circuit layer to isolate differing voltage and ground potentials.

Experts in this domain note that frequency signals can radiate EMI if they aren’t routed carefully on the circuit board. Not only can the length and configuration of the conductors be a problem, but conductor and via stubs can also act as an antenna. Another source of EMI is the signal return path, which optimally should be on an adjacent reference plane. If the return path is blocked in any way, the signal will radiate even more noise as it seeks a path back to its source. Two issues that can affect product performance are crosstalk and switching noise:

• Crosstalk (effects of electromagnetic coupling): High-speed transmission lines spaced too close together may inadvertently couple, with one signal overpowering the other, creating crosstalk. This can result in the victim signal mimicking the characteristics of the aggressor signal and not performing its intended task. Not only is this a problem with side-by-side conductors, but also with those routed in parallel on adjacent layers of the board. This type of crosstalk is known as broadside coupling and is why multilayer circuit board designers are advised to alternate the horizontal and vertical routing directions on adjacent layers.
• Switching noise (ground bounce): With several components switching between high and low states on a circuit board, the voltage level may not return all the way to the ground potential (as it should) when it switches to low. If the voltage level of the low state bounces too high, the low signal state may be falsely interpreted as a high state. When this happens simultaneously, it may result in false or double-switching (bounce) and disrupt the operation of the circuit.

Planar Capacitor Design
The general value range for the embedded planar capacitor is contingent on the dielectric material selected for separating the conductive foil layers (Bar Graph 1).

Basic Planar Capacitor
Using the dielectric material sandwiched between opposing copper planes will provide significant capacitance with very low inductance. The dielectric constant of the selected material, material thickness, and the total area determine the resulting level of capacitance.

Distributed Planar Capacitor
Considered the simplest solution and commonly used to replace discrete external power supply decoupling capacitors, the planar capacitors rely on closely spaced power and ground planes that are separated by a thin dielectric layer.

Polyimide (PI) Film Planar Capacitors
Polyimide film dielectrics are typically used to separate the circuit board layers dedicated to the power distribution network. Both the PI area and thickness will determine the planar capacitors’ values. Because the planar capacitance is proportional to the dielectric thickness between the power and ground planes, thin dielectrics are used to increase planar capacitance while reducing planar spreading inductance. The reduction of planar spreading inductance also results in lowering the impedance path while increasing the effectiveness of discrete capacitances.

Divided Planar Capacitors
Grouping components with a localized ground and power plane helps control EMI because the power and ground planes’ geometry is sized and placed. It is not uncommon to require more than a single operating voltage. The segmentation of ground planes associated with specific voltage supply functions and grouping components with a localized ground and power plane helps control EMI because the power and ground plane’s geometry is sized and placed.

Reasons for dividing ground and power planes:

• Separating high and low voltage areas (group devices by voltage required)
• Dividing analog devices from digital devices
• Preventing high-frequency effect on low-frequency circuits
• Segregating one logic family from another 

The designer will develop the power and ground planes for each group so that the planes are the same shape and directly in line with each other, as shown in Figure 2. Avoid routing signal conductors in the narrow gap separating the power or ground planes A and B.

When planning the circuit board design, remember that the major role of power and ground planes is to ensure power is being uniformly distributed to all components on the circuit board’s surface. Instead of routing individual power conductors everywhere, a power plane acts like a solid, wide path that supplies voltage smoothly and consistently, avoiding voltage differentials between widely distributed components. The ground plane keeps signals clean while providing a low-impedance return path for current, essential in high-speed designs. When return currents can flow directly beneath their signal conductors, it minimizes signal distortion and helps improve timing.

Note: Portions of the text, illustrations, and tables included in this column are from my new book, Design Guidelines for Surface Mount & Microelectronic Technology.

This column originally appeared in the October 2025 issue of Design007 Magazine.