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 Impedance Calculation With Altium Designer 20

    |  February 25, 2020


    Today’s PCBs contain many transmission lines. Combine this with increased clock frequencies and data rates and the result is a critical challenge to high-speed design. Neglecting these dynamics can undermine product development by compromising performance, power consumption, EMC/EMI compliance, and more - leading to delayed design cycles and opening gaps that can be exploited by your competition.


    Hone your high-speed design skills by joining us as we discuss the typical transmission lines encountered in today’s designs, the PCB variables that affect impedance, as well as how to create, calculate, and design transmission lines in Altium Designer. Learn how to maximize the built-in SIMBEOR® engine by Simberian to craft impedance profiles and manage transmission lines in your designs.

    Impedance profiles


    We're going to start by talking about current electronics development trends. Introducing a simple concept of the Trace Transmission Line Model and how impedance on these transmission lines are either intentionally or inadvertently manifested on printed circuit boards. We're going to follow that with a discussion on a very important topic called Return Current. Then we're going to review the PCB design, some of the key PCB design rules, and how they influence impedance.

    Current Electronics Development Trends

    Everyone knows that everything's going faster every year and we're expected to do it in a quicker amount of time, using a smaller footprint, and lower power consumption. A great example is Ethernet data rates that have been increasing dramatically, all the way up to 100 gigabits and beyond these days. At the same time, we see an increase in clock rates. These increases result in reduced edges of the signal and quicker rise and fall times.


    Data transfer rate for the Ethernet port depending on the year


    Transmission Line Model

    A transmission line is really a direct return system of the conductors that are generally placed together to form a single electromagnetic field. Examples of transmission lines are the cable you use for satellite or terrestrial base cable TV. Anytime you have a conductor, you're going to have some resistance (R) , as well as, some inductance (L) in that conductor because it's metal. If we look at this drawing here representing the spacing between the signal line and the return path or return line we're going to have some separation there. That's going to also create capacitance (C) determined by transmission line and the materials. And then finally, we've got this G which is conductance representing the sort of the leakage or the wasted energy, if you will, that results due to the particular characteristics of the dielectric material. These are the main factors that influence transmission line performance.


    R, L, C, G – 

    Primary Electrical Parameters of the Transmission Line

    R - active line losses

    L - inductance, determined by line configuration and materials

    C - capacitance, determined by the line and materials

    G – conductance, influenced by leakage in the dielectric material

    Transmission line impedance

    When we talk about transmission line impedance in a circuit board, we often see microstrip setups with the conductor on the top separated by dielectric and a return plane on the bottom. One of the fundamentals about impedance, especially when we're talking about sending a signal down a path and then waiting for the return, is that the signal source impedance should equal the receivers impedance. The standing wave ratio ideally wants all of that signal that you're transmitting down that line to be received. 

    Impedance - secondary electrical parameter of the transmission line:


    When you have an impedance mismatch, you get reflections leading to solar scope images. We have the signal as we really expect it down at the receiver on the left, and we have the signal as we actually encounter it. You can see some of the original signal in that image on the right, but there's a lot of reflections that occur because of the mismatch of signal impedance not meeting the specifications of the transmission line and receiver. 


    Just in general, your impedance equals this equation


    One thing we want to look at here, you can see real quick that if your capacitance is going up that value is going to get smaller. Your impedance is going to get smaller.


    The ideal PCB transmission line and pins is between 40 and 120 Ohms. The thing to remember is because we are using a consistent cross section, or so called Homogeneous transmission line, that this important ratio is constant throughout the line and we only need to be worried about the impedance and not the length of the line.


    Here's an example of routing guidelines. I remember when I used to look at routing guidelines. A lot of times it was just the footprint layout, maybe some exit strategies. Well now, in this day and age, we all have to worry about differential impedance, single ended impedance spacing between differential pairs, and high speed periodic signals.


    Important ratio: L*C = constant across the length of the line!

    inductance * capacitance = constant


    What we have on the left here is his original USB 480 megabit and we have the current version I believe that's the current version USB 3.0 at 5 gigabits and we see that there are differences and these are part of the design guidelines now to take into account these types of parameters so that we can design our circuits.

    Transmission lines on PCB

    Let's talk a little bit more of about the types of transmission lines we see on today's printed circuit boards:


    Homogeneous transmission lines have a cross-section of the transmission line, as well as the medium, in which it is constant along its entire length.


    Coplanar is when the signal and the return path is on the same layer

    you have a dielectric underneath. The circular nature of magnetic fields is influenced by the dielectric and also the dielectric constant of air.


    We have a similar situation with a microstrip line. That's where the conductor is on the outside layer and the return path is a ground plane. 


    You can actually submerge that micro strip equally embedded into that dielectric and get improved performance with an embedded microstrip line. We see that on the the third image from the top.


    Symmetrical stripline is where you have the conductor perfectly centered in that dielectric and surrounded by two ground planes. This is an excellent excellent transmission line, albeit they're hard to fabricate because you really want them to be exactly equidistant.


    Asymmetrical stripline has one side of the dielectric that is larger than the other one. So again, I mentioned it earlier, but again, it's an important concept we want to use these homogeneous transmission lines where the cross section is identical across the length.


    Now, we mentioned here a balanced transmission line is where you have a straight and a return conductor with the same length. They have the same shape and cross section. An example of that is a differential pair. And of course we run into both of these implemented on PCBs.

    Return current

    Let's talk about return current! We have two setups here at 1kHz and 10 MHz.


    Let’s start at the return current representation at 1 kHz. The current searches searches for the path of least impedance. In the case of 1 kHz, the long wavelengths result in a path of a straight line due to capacitive reactance.

    When we go to higher frequencies as seen in the 10 MHz signal, the path hugs closer to that signal path also due to the capacitive reactance. As a component of impedance, when we look at their relationship we can see right away that as that frequency increases the capacitive component dominates and these types of designs in most cases is going to result in a lower impedance. That's why, as the frequency goes higher, we're going to see that return signal which is really an electromagnetic field hug very, very close to that conductor.


    Now let's look at the differences between homogeneous and heterogeneous transmission lines.

    Discontinuities in the reference layer are not advisable!


    As mentioned previously, a homogeneous transmission line has an identical cross section throughout signal and medium (usually dielectric).


    Then we have a heterogeneous transmission line with a slot or an area of the plane, not through the whole layer stack, but just one plane the return plane. In this case, there is an opening with no copper. 


    We see on the homogeneous transmission line, that the return current flows as we would expect close to the conductor. However, on the heterogeneous transmission line the slot causes the signal to take a circuitous route in order to get back to that source and this creates all kinds of issues. For instance, that return route might go over some other signal conductors and that generates crosstalk. You can also get reflections in here and that generates issues, trying to get your product or board to pass EMI testing.It is highly recommended to avoid any types of slots or any other discontinuities in the return path. That's a simple mistake that I know I've made in the past, which really has caused some odd behavior.


    PCB Design Influences on Impedance

    Next let's talk about typical design rules and how they influence Impedance.


    We will discuss four parameters Conductor Width, Thickness of the Dielectric, Dielectric Constant, and Thickness of Copper


    Conductor Width - increases have high dependency in decreasing impedance.

    Thickness of the Dielectric - increases that's going to generally increases impedance. 

    Dielectric Constant - average dependency as its impact is not as great as thickness. As the dielectric constant increases, the impedance decreases slightly.

    Thickness of Copper -  lower dependency on the thickness of the copper as there is inductance in the transmission line, but it's generally not as big of the of the factor as the capacitance. As the copper thickness increases, the impedance decreases slightly.




    Rules of Thumb

    When you have a Microstrip conductor outside layer having a return path of a plane underneath separated by a dielectric if the width of that trace is two times the height of the dielectric for FR4 you can be basically assured that you've got a nice 50 Ohm transmission line. 

    Similarly, if you're using a symmetric stripline approach the height of the dielectric would need to be two times the width of the conductor and for FR4 with a dielectric constant of 4 to 4.6 that would give you 50 Ohms.

    Transmission line with specified impedance in AD 

    We've talked about the background and the theory of transmission lines. Now we're going to talk about how we actually address this in Altium Designer. The Layer Stack Manager (LSM) is your hub for impedance profiles definition. It is very important to have the Properties Panel open when using the LSM as it is used heavily in these operations. After you define your layerstack, you must define your Impedance Profiles in the tab of the LSM. You can think of an impedance profile as a definition for a particular type of transmission line. For example, when we saw the USB specification, we saw there were some defined 95 Ohm differential transmission lines. We can create 95 Ohm impedance profiles to ensure appropriate traces are created for your design.


    In this instance, we have created a single ended signal with a default return path with the default name S50 (single ended signal 50 Ohm). Let’s take a deeper view of the impedance profile definition in a project. When you create your impedance profiles, you highlight the various layers to change layer parameters with the Properties Panel to refine the impedance to ensure alignment with your layerstack. You can then apply these impedance profiles to your project and individual design rules. Before we do that, we want to talk about the types of transmission lines that we currently support in Altium Designer.


    Transmission Line Types in Altium Designer

    Single ended structures have a conductor with a return path. You can have the return path on another layer or on the same layer known as coplanar. Note that even the solder mask is taken into account because it has dielectric properties that can influence signal propagation. We also have coplanar single ended structures where the return path is on the same layer found on either side of the conductor.



    Similarly, we have differential structure and coplanar differential signals.


    Impedance Calculation

    When you highlight your layer in your impedance profile, you immediately see your constituent layers in said profile. In this case, we have one dielectric 1 and 2 with internal ground and power on either side. Impedance on this layer will be automatically calculated with this profile and you will see the cross-section that the system will generate. When you set up an impedance, you're able to define the impedance value and the target tolerance gives you more wiggle room to have trace widths and topology that's going to work best for your design. We see the result in transmission line parameters in the Properties Panel. If we want, we can allow the system to just generate the trace it recommends for the given parameters or we can trace width we want for our layer. For example, define a 0.1 trace width and hit the fx button and it will calculate all parameters.

    Assign Impedance Profile To Nets

    Once you have your impedance profiles complete, you can go into your design rules to assign your impedance profiles to associated nets. 

    What's really nice about using these rules and impedance profiles is that if you decide you need to change the impedance profile, you change it the profile once in the layer stack manager and it echoes to all of the associated rules that reference it. This is incredibly powerful over existing approaches where external calculators are used and individually annotated because you have the ability to update things quickly and uniformly. Best of all the retrace route functionality will update any existing routes to the proper trace thickness for your new impedance profile definition.


    About Author

    most recent articles

    Back to Home