Skip to main content
Sierra Circuits
Best-in-Class PCB Fabrication, Assembly, & Components.
Industry Leading PCB Designer's Tools.

Speak to an Account Manager Telephone +1 (800) 763-7503

Quote Now
Controlled ImpedanceSignal Integrity

What is a PCB Transmission Line?

A PCB transmission line is a type of interconnection used for moving signals from their transmitters to their receivers on a printed circuit board. A PCB transmission line is composed of two conductors: a signal trace and a return path which is usually a ground plane. The volume between the two conductors is made up of the PCB dielectric material.


Author headshot: Atar Mittal

By Atar Mittal

February 3, 2020  |  7 Comments

coplanar-transmisison-line-structure.jpg

A PCB transmission line is a type of interconnection used for moving signals from the transmitters to the receivers on a circuit board. It is composed of two conductors: a signal trace and a return path which is usually a ground plane. The volume between the two conductors is made up of the dielectric material.

The alternating current that runs on a transmission line usually has a high frequency to manifest its wave propagation nature. The key aspect of the wave propagation of the electrical signals over a transmission line is that the line has an impedance at every point along its length. Also, if the line geometry is the same along the length, the line impedance is uniform. We call this line a controlled impedance trace. Non-uniform impedance causes signal reflections and distortion. It means that at high frequencies, transmission lines need to have a controlled impedance to predict the behavior of the signals.

To learn more about controlled impedance, see why controlled impedance really matters?

It is crucial to pay attention to the transmission line effects in order to avoid signal reflections, crosstalk, electromagnetic noise, and other issues which could severely impact the signal quality and cause errors.

 

PCB Transmission Line eBook - Cover Image

PCB Transmission Line eBook

5 Chapters - 20 Pages - 25 Minute Read
What's Inside:
  • What is a PCB transmission line
  • Signal speed and propagation delay
  • Critical length, controlled impedance and rise/fall time
  • Analyzing a PCB transmission line

What are the types of transmission lines?

There are usually two basic types of signal transmission lines in PCBs: microstrips and striplines. There is a third type – coplanar without a reference plane but it is not widely used.

A microstrip transmission line is composed of a single uniform trace located on the outer layer of a board and parallel to a conducting ground plane. This plane provides the return path for the signal. The trace and the ground plane are separated by a certain height of PCB dielectric as shown in the image below.

microstrip-pcb-transmission-line.jpg
Microstrip PCB transmission line

A stripline is composed of a uniform trace located on the inner layer of a circuit board. The trace is separated on each side by a parallel dielectric layer and then a conducting plane. So it has two return paths – reference plane 1 and reference plane 2.

stripline-pcb-transmission-line.jpg
Stripline PCB transmission line

In addition to conventional microstrips and striplines described above, a coplanar waveguide structure has the signal trace and the return path conductor on the same layer of the board. The signal trace is at the center surrounded by two adjacent outer ground planes. This structure is called “coplanar” because these three flat structures are on the same plane. The dielectric is located underneath. Both microstrips and striplines may have a coplanar structure. Below is a coplane microstrip waveguide with a ground plane:

coplanar-transmission-line-structure.jpg
Coplanar transmisison line structure

Example of a coaxial cable (which is not a PCB transmission line)

A coaxial line has a circular shape and is not a circuit board transmission line. This circular cable is composed of a central wire conductor and an outer conductor for the return path. The space between the two conductors is filled with a dielectric material. The outer conductor wire completely surrounds the signal wire. Coaxial lines are mostly used as cables for high-frequency applications, such as television, etc. These cables must have a uniform geometry of conductors and the properties of the dielectric material must be uniform throughout the cable length.

structure-of-coaxial-cable.jpg
Structure of coaxial cable

It is essential to keep in mind that a PCB transmission line is composed of not only the signal trace but also the return path, which is usually an adjoining ground plane or a coplanar conductor, or a combination of both.

When is an interconnection considered a transmission line?

The set of electrical conductors used for transmitting a signal between source and destination is called a transmission line. If it is not possible to ignore the time it takes for the signal to travel from the source to the destination, as compared to the time period of one-fourth of the wavelength of the higher frequency component in the signal.

Two very important properties of a transmission line are its characteristic impedance and its propagation delay per unit length. If the impedance is not controlled along its entire length, or the line is not terminated by the right value of impedance, signal reflections, crosstalk, electromagnetic noise, etc. will occur. This degrades the signal quality and affects the signal integrity of the circuit board.

When the signal frequencies (in case of analog signals) or the data transfer rates (in case of digital signals) are low (less than 50 MHz or 20 Mbps), the time taken by a signal to travel from its source to its destination would be very small (< 10%) compared to the time period of one-fourth of a wavelength or the fastest rise time of a digital pulse signal. In this case, it is possible to approximate the interconnect by assuming that the signal at the destination follows the signal at its source at the same time. In such a low-speed scenario, the PCB signal can be analyzed by conventional network analysis techniques and we can ignore any signal propagation time or transmission line reflections, etc.

However, when dealing with signals at higher frequencies or higher data transfer rates, the signal propagation time between the source and the destination cannot be ignored in comparison to the time period of one-fourth of a wavelength or the fastest pulse rise time. Therefore, it is not possible to analyze the behavior of such high-speed signals using ordinary network analysis techniques. The interconnects need to be considered as transmission lines and analyzed accordingly.

Impedance Calculator by Sierra Circuits

How to predict the signal behavior on microstrip and stripline?

At high frequencies, transmission lines need to have a controlled impedance to predict the behavior of the signals and avoid signal integrity issues.

This is the reason why you need to know at which speed signals propagate on transmission lines and the time they take to do so. We will give you a few equations to calculate the signal speed and the propagation delay for both stripline and microstrip structures.

What is signal speed?

Let’s first discuss the speeds at which signals propagate on a PCB interconnect.

Electromagnetic signals travel in vacuum or air at the same speed as of light, which is:

Speed-of-light.jpg
The equation for the speed of light

A signal travels on a transmission line at a slower speed, affected by the dielectric constant (Er) of the dielectric material. The relations for calculating the signal speed on a PCB are given below:

equations-for-signal-speeds-in-microstrip-stripline-structures.jpg
Equations for signal speeds in microstrip and stripline structures

Where:
Vc is the velocity of light in vacuum or air
Er is the dielectric constant
Ereff is the effective dielectric constant for microstrips; its value lies between 1 and Er, and is approximately given by:

effective-dielectric-constant.jpg
Effective dielectric constant

Thus, the speed of signals is less than that of air. If Er ≈ 4 (like for FR4 material types), then the speed of signals on a stripline is half that in air, i.e. it is about 6 in/ns.

Henceforth, we can use Vp to denote the speed of signals on a PCB.

 

High-Speed PCB Design Guide - Cover Image

High-Speed PCB Design Guide

8 Chapters - 115 Pages - 150 Minute Read
What's Inside:
  • Explanations of signal integrity issues
  • Understanding transmission lines and controlled impedance
  • Selection process of high-speed PCB materials
  • High-speed layout guidelines

 

 

What is propagation delay?

The propagation delay is the time taken by a signal to propagate over a unit length of the transmission line:

propagation-delay.jpg
The equation for propagation delay

 

Where:
V is the signal speed in the transmission line

In vacuum or air, it equals 85 picoseconds/inch (ps/in).

On transmission lines, the propagation delay is given by:

propagation-delay-in-microstrip-and-stripline.jpg
Propagation delay in microstrip and stripline structures

 

What materials are used in PCB transmission lines?

The most used materials are Isola 370HR, Isola I-Speed, Isola I-Meta, Isola Astra MT77, Tachyon 100G, Rogers 3003, and the Rogers 4000 series.

The signal speeds and propagation delays for a few board materials are given in the table below:

Signal-speed-propagation-delay-table.jpg
Signal speed propagation delay table

 

Teledyne Lecroy by Sierra Circuits banner

What are the transmission line effects?

Let’s discuss critical length, controlled impedance, and rise/fall time.

As mentioned above, for high-speed or high-frequency signals, we need to consider the transmission line effects. We can use a few thumb rules:

In the case of high-frequency analog signals, let the maximum frequency content in the signal

Equation

 

 

How to define the critical length?

wavelength-calculation-of-high-frequency-signals.jpg
Wavelength calculation of high-frequency signals

For analog signals, the critical length lc is defined as one-fourth of the wavelength of the highest signal frequency contained in the signal.

critical-length-for-analog-signals.jpg
Critical length for analog signals

 

In the case of digital signals, the fastest rise/fall time of a signal pulse is the most important parameter. It defines the transition time from one logic level to another logic level. Basically, the transition time of the data bit. For digital signals, the critical length lc is defined as the line length over which the signal propagation time is half of the fastest rise/fall time of the signal pulses.

If tr = fastest rise/fall time of the digital signal, the time of the propagation of the signal over the length lc is tpd (propagation delay).

critical-length-for-digital-signals.jpg
Critical length for digital signal

 

This definition implies that the signal should be able to travel from the source over a length lc of the line. This signal should return over the same length back to the source point in a total time equal to the rise/fall time tr.

Equations 2a and 2b are related if we consider the highest frequency content in a digital signal rise/fall time.

The highest frequency content in a digital signal of rise/fall time tr is given by (as per Fourier Analysis):

 

critical-length-calculations.jpg
Critical length calculations

Which is the same as equation 2a.

What is a shortline?

If the line length Equation there is a shortline and it is not necessary to consider its transmission line effects, nor to design it as a controlled impedance line.

But if the line length Equation it then becomes necessary to consider the transmission line effects and to design such lines as controlled impedance lines.

Example:

If the fastest signal rise/fall time is: tr = 1ns, then, assuming the FR4 material with a dielectric constant Er = 4, Equation and the critical length Equation Therefore, signal traces longer than 3/1.5 = 2 inches need to be designed as controlled impedance lines. Note here that tr of 1ns corresponds to a maximal signal frequency: Equation

How to estimate the rise/fall time from data transfer rate (DTR) or clock frequency?

The data transfer rate is measured in bits per second (bps or bits/sec or b/s) and the clock frequency (Fclock) in Hz.

DTR is usually ≥ 2 Fclock. Henceforth, it will be safe to use the following rule:

Equation

If we don’t know the signal rise/fall time, we can use the following rule:

Equation

Example:

For Fclock = 1GHz or DTR = Gbps, and for a PCB material with Er = 4, we get:

Equation

How to obtain the 3 dB bandwidth?

For a signal with rise/fall time tr, the 3 dB bandwidth is given by the following rule:

Equation

Therefore, for a clock of frequency Fclock, we get:

Equation

How to analyze a PCB transmission line?

High-speed signals generate electromagnetic fields around them during their travel along a transmission line. Their behavior is best analyzed using Maxwell’s electromagnetic equations and the theory of electromagnetic wave propagation. In this method, we have to deal with electric and magnetic fields instead of the usual voltages and currents. The voltage between the signal line and its return path will generate an electric field and a current in the conductors. This in turn will create a magnetic field around them. Thus, voltage, current, electric and magnetic fields all travel as waves along the transmission line.

There exists a close analogy between the electromagnetic waves propagation and the propagation of voltages and currents along a transmission line. As it is easier to think in terms of familiar voltages and currents rather than electric and magnetic fields, we should use the voltage/current analysis of the transmission line in the following treatment.

What are the transmission line parameters?

A transmission line is a large number of infinitesimal length segments. Each segment can be analyzed by network theory concepts at a particular point in space and time, ignoring the travel time in the infinitesimal segment as its length is extremely small.

In this analysis technique, we will be dealing with quantities like voltages and currents, and transmission line parameters like resistance, inductance, capacitance, and conductance. We will model an infinitesimal segment of a transmission line in terms of the following parameters:

R = the resistance per unit length (or p.u.l.) (R in Ohms p.u.l.)
L = the inductance p.u.l. (L in Henrys p.u.l.)
C = the capacitance p.u.l. (C in Farads p.u.l.)
G = the conductance p.u.l. (G in Mhos p.u.l.)

We can denote the length of the infinitesimal transmission line by Δx.

Then we can picture this transmission line segment as follows:

Transmission-line-segment.jpg
Transmisison line segment

Where:
V(x,t) = signal voltage at location x at time t
I(x,t) = signal current at location x at time t

Let’s do the analysis of this circuit in the frequency domain. Here, we assume that the signals vary with time sinusoidally with an angular frequency ω, so that the time-varying part of V(x,t) and I(x,t) can be shown by the factor Equation and we now have:

analysis-of-a-circuit-frequency-domain.jpg
Analysis of a circuit in the frequency domain

 

Using Kirchhoff’s laws on the above segment, we obtain the following relations:

application-of-kirchoffs-law-in-circuit-analysis.jpg
Application of Kirchoff’s-law in circuit analysis

 

And from these, by differentiation, we get:

 

differenciation.jpg
Differentiation in circuit analysis

A solution to this equation is:

solved-equation.jpg
Solved equation

And from Equation 2,

Equation

α has units of p.u.l.

If we multiply Equation 4a by Equation to reincorporate the time variations of the sinusoidal voltages and currents, we will see that now the equations represent voltage and current signal waves traveling in the positive x-direction over the transmission line:

voltage-and-current-signal-waves-traveling-in-the-positive-x-direction.jpg
Voltage and current signal waves traveling in the positive x-direction

If you would like to learn anything specific about PCB transmission line analysis, please let us know in the comment section.

 

 

Controlled Impedance Design Guide - Cover Image

Controlled Impedance Design Guide

6 Chapters - 56 Pages - 60 Minute Read
What's Inside:
  • Understanding why controlled impedance is necessary
  • Stack-up design guidelines
  • How to design for impedance
  • Common mistakes to avoid
Subscribe
Notify of
guest
7 Comments
Oldest
Newest Most Voted
Inline Feedbacks
View all comments
Share this article
Zero Defects guaranteed on all PCB fabrication

Reduce Re-Spins with our Zero Defect Guarantee.

Our platform sources the whole package, creating a thread from design to delivery. Fabricating PCBs. Procuring parts. Assembling your boards.

Once you upload your BOM, Our best-in-class software automatically checks for errors and cleans your file for you. After you place an order, your dedicated CAM engineer will run a full DFM and DFA check to ensure your prototype achieves Zero Defect every time—all at no additional cost to you.

Get to market faster and spend less time troubleshooting.

Start Quote

Talk to a Sierra Circuits PCB Expert today

24 hours a day, 7 days a week.

Call us: +1 (800) 763-7503
Email us: through our Customer Care form