Free Trials

Download a free trial to find out which Altium software best suits your needs

How to Buy

Contact your local sales office to get started on improving your design environment


Download the latest in PCB design and EDA software

  • Altium Designer

    Complete Environment for Schematic + Layout

  • CircuitStudio

    Entry Level, Professional PCB Design Tool

  • CircuitMaker

    Community Based PCB Design Tool


    Agile PCB Design For Teams

  • Altium 365

    Connecting PCB Design to the Manufacturing Floor

  • Altium Concord Pro

    Complete Solution for Library Management

  • Octopart

    Extensive, Easy-to-Use Component Database

  • PDN Analyzer

    Natural and Effortless Power Distribution Network Analysis

  • See All Extensions

    World-Renowned Technology for Embedded Systems Development

  • Live Courses

    Learn best practices with instructional training available worldwide

  • On-Demand Courses

    Gain comprehensive knowledge without leaving your home or office

  • Altium 365 Viewer

    View & Share electronic designs in your browser

  • Altium Designer 20

    The most powerful, modern and easy-to-use PCB design tool for professional use


    Annual PCB Design Summit

    • Forum

      Where Altium users and enthusiasts can interact with each other

    • Blog

      Our blog about things that interest us and hopefully you too

    • Ideas

      Submit ideas and vote for new features you want in Altium tools

    • Bug Crunch

      Help make the software better by submitting bugs and voting on what's important

    • Wall

      A stream of events on AltiumLive you follow by participating in or subscribing to

    • Beta Program

      Information about participating in our Beta program and getting early access to Altium tools

    All Resources

    Explore the latest content from blog posts to social media and technical white papers gathered together for your convenience


    Take a look at what download options are available to best suit your needs

    How to Buy

    Contact your local sales office to get started improving your design environment

    • Documentation

      The documentation area is where you can find extensive, versioned information about our software online, for free.

    • Training & Events

      View the schedule and register for training events all around the world and online

    • Design Content

      Browse our vast library of free design content including components, templates and reference designs

    • Webinars

      Attend a live webinar online or get instant access to our on demand series of webinars

    • Support

      Get your questions answered with our variety of direct support and self-service options

    • Technical Papers

      Stay up to date with the latest technology and industry trends with our complete collection of technical white papers.

    • Video Library

      Quick and to-the-point video tutorials to get you started with Altium Designer

    Transmission Line Properties That Affect Impedance—Hidden Features

    Kella Knack
    |  December 29, 2019

    Here and in several other articles published on the Altium Resource section of the company’s website, the topic of transmission line impedance has been addressed from a number of different perspectives. I have addressed transmission line impedance previously in my article, The Evolution Of Simulation Technology and Impedance and, it might seem that we may have exhausted the field of potential information that can be provided on impedance, however, in truth, some features were only addressed in passing. This article will elaborate on those features and their effects along with basic equations that are used in controlling transmission line impedance.

    Sources of Impedance or Mismatch

    As discussed in previous articles, the four main variables that determine the impedance of a transmission line on a surface layer include:

    • Height of the trace above the plane over which it travels.
    • The width of the trace.
    • The thickness of the trace.
    • The insulating material used to support the trace.

    Once the above four variables are known, it is possible to determine which features in a PCB will have a relevant effect on impedance. These features include:

    • Changes in trace width in the same layer. This is generally referred to as trace necking.
      • Trace necking refers to the reduction of the trace width when it approaches a narrower pad such as that found on an SMD (surface mount device) or a through-hole that has a diameter that is less than the width of the trace.
    • Changes in trace thickness.
    • Changes in height above the plane.
    • Stubs along the transmission line.
    • Loads along the transmission line.
    • Connector transitions.
    • Poorly-matched terminations.
    • No terminations.
    • Larger power plane discontinuities.
    • Changes in the relative dielectric constant.

    As noted in previous articles, right-angle bends and vias are not on the above list because neither one of these features is a significant source of impedance mismatch.

    Impedance Equations

    There are a few equations that are helpful in calculating impedance. They are presented below. As noted previously, the impedance of a transmission line is determined by the capacitance and inductance that is distributed along the length of the transmission line. And, the equation used for calculating impedance is repeated here in Equation 1.

    Equation 1. Z₀ = sqrt[ (R₀ + jωL₀) / (G₀ + jωC₀) ]
    Equation 1. The Impedance Equation

    In the above, Z0 is the impedance in ohms; jωL0 is the parasitic inductance in henrys per unit length, jωC0 is the parasitic capacitance in farads per unit length and R0 is skin effect loss (which can be ignored until you get to very high frequencies). G0 is the loss in the dielectric. As noted above, changing either the parasitic inductance or the parasitic capacitance will change the impedance of the transmission line. It’s also been demonstrated that changes in impedance cause signal reflections. For convenience, the reflection equation is repeated in Equation 2.

     Equation 2. % = 100 * (ZI - ZO) / (ZI + ZO)
    Equation 2. The Reflection Equation

    This equation predicts the percentage of the incident EM field that will be reflected back to the source based on the two impedances on each side of a change where Zl is the downstream impedance and Z0 is the upstream impedance. The equation reflects the voltage amplitude of the reflection.

    Based on Equation 1, it is not obvious which variables will have an effect on impedance. Equation 3 is the classic surface microstrip equation. It illustrates the variables in a PCB that determine impedance.

    Equation 3. Z₀ = 79 * ln(5.98 * H / (0.8 * W + T)) / sqrt(er + 1.41)
    Equation 3. The Classic Surface Microstrip Impedance Equation

    This equation is included for illustration purposes only so that the variables can be shown. In a separate article following this one, it will be shown that this equation as well as other equations used to calculate impedance have a limited range over which they are valid. More accurate methods are available and some have been discussed in previous articles. The article following this one will also contain other methods for determining impedance.

    The common characteristics of the features noted above is that they can have a measurable effect on one or both of the variables in Equation 1, parasitic inductance or parasitic capacitance. We can take those features and show the variables that they affect.

    • Change in trace width in the same layer—C0
    • Change in trace thickness—C0
    • Change in trace height above the plane—C0
    • Stubs along the transmission line—C0
    • Loads along the transmission line—C0
    • Connector transitions—C0
    • Large power plane discontinuities—C0
    • Changes in relative dielectric constant—C0
    • Poorly matched terminations
    • No terminations

    As can be seen, with the exception of poorly matched terminations and no terminations, all of the sources of impedance mismatch are caused by something that changed the parasitic capacitance. Within the limits of trace dimensions in PCBs, compared to C0, L0 is relatively constant. This helps when it comes time to design controlled impedance signal paths or troubleshoot impedance problems.

    Once it is understood that virtually all impedance changes along the length of a transmission line are due to changes in parasitic capacitance, it becomes easier to manage those changes and create good impedance control.

    Table 1 shows the relative dielectric constant of the laminate that is commonly known as FR-4. 

    Table 1. Material thickness, construction, resin content, and e_r values at 1MHz and 1GHz for FR-4
    Table 1. Laminate Information for Laminate Commonly Called FR-4

    Not only does the relative dielectric constant change with frequency, it also varies with the amount of glass and resin used to make the laminate. As can be seen, there are four ways to make a 4-mil thick piece of laminate; three ways to make a 5-mil thick piece of laminate and four ways to make a 6-mil thick piece of laminate. Also, note that the ratio of glass to resin is different in each of these formulations as is the relative dielectric constant. If a PCB stackup is designed to use one of these formulations and the fabricator uses one of the others, the impedance will not come out as expected. This is the most common reason that changing fabricators results in PCBs with different characteristics. To avoid this problem, it is necessary to specify, on the fabrication drawing, which laminate formulation is required in each opening in the stackup.


    Understanding the variables and features within a PCB that can affect transmission line impedance makes it easier to design for impedance control right the first time, and easier to troubleshoot any impedance issues that may occur during the design or during the fabrication processes.

    Have more questions? Call an expert at Altium or read on to learn more about incorporating impedance calculations into your design rules with Altium Designer®.


    1. Ritchey, Lee W. and Zasio, John J., “Right The First Time, A Practical Handbook on High-Speed PCB and System Design, Volume 1.”

    About Author

    About Author

    Kella Knack is Vice President of Marketing for Speeding Edge, a company engaged in training, consulting and publishing on high speed design topics such as signal integrity analysis, PCB Design ad EMI control. Previously, she served as a marketing consultant for a broad spectrum of high-tech companies ranging from start-ups to multibillion dollar corporations. She also served as editor for various electronic trade publications covering the PCB, networking and EDA market sectors.

    most recent articles

    Back to Home