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

    Calculating Series Termination Resistance Values in Altium Designer

    Zachariah Peterson
    |  May 5, 2019

    Components and an integrated circuit on a green PCB

    You might need to determine the right series termination resistance value for this type of circuit

    With transmission lines, some things never seem to be simple. Determining the termination technique and the values of components in a termination network shouldn’t be a difficult task. Most PCB design programs force you to look online for calculators, or you’ll have to run the calculations by hand. Instead, your design software should make it easy to test a range of component values in your termination network.

    Some components, traces, differential pairs, and interconnects that route through vias should be impedance matched in order to prevent transmission line effects from arising in high speed or high frequency circuits. While you can get away with small impedance mismatches, some signal drivers will have an impedance that does not match the standard 50 Ohm value typically used with signal traces. One should note that some routing and computer architecture standards (i.e., PCIe Gen 2 and Gen 3) also use a different value for differential pair impedance.

    Whenever the propagation delay along a trace becomes longer than one quarter of the signal rise time, your trace will start to exhibit transmission line effects. For analog signals, transmission line effects start to appear when the propagation delay is longer than about 10% of the oscillation period. In these cases, you will need to terminate your traces to suppress transmission line behavior and prevent signal reflection. Thankfully, Altium Designer® includes signal integrity tools that allow you to examine potential signal integrity problems and experiment with possible termination networks. These tools are accessible within the unified design interface, and you won’t have to access an external program or buy a new extension.

    Which Termination Network Should I Use?

    There are several answers to this question as there are several possible networks. The correct answer really depends on whether you will need to increase or decrease the impedance of your transmission line. In addition, different components may need more than a simple resistive network or an RC network. For example, an antenna will need to use an LC network, and the exact placement of the inductor and capacitor (either in series or as a shunt element) depends on how you need to shift the impedance in order to match the resonance frequency.

    If the impedance of your signal driver is smaller than your trace impedance, you can place a series resistor at the output of your driver, allowing you to easily compensate the impedance of the trace and match it to the impedance of your trace. If your driver has high output impedance, you can use a parallel resistor to ground to compensate the impedance mismatch. More complicated networks like an RC network provide other benefits.

    Determining Series Termination Resistance

    We’ll take a look at determining how a series termination resistor can compensate impedance mismatch in a single-ended trace and in a differential pair. Here, you’ll want to set up a board with a pair of single-ended traces between a driver and a load, as well as a differential pair between a driver and a load. You’ll need to assign net names to each trace in your schematic. Don’t forget to add “_P” and “_N” to the net name for the differential pair and assign a differential pair directive in your schematic.

    The signal integrity tool for designing a termination network functions by iterating through a range of component values. Your job is to choose some maximum and minimum values for your components in this network. Once you run the simulator, you’ll see a graph that shows how each component value in the network affects your signal. This allows you to visually determine the best component values to use in your termination network.

    Once you capture your schematic and layout your board, you’re ready to determine the appropriate termination resistor for your traces. Once you have your board prepared, you can access the signal integrity tool in Altium Designer from the Tools -> Signal Integrity… menu.

    Accessing the signal integrity tool in Altium Designer

    Accessing the Signal Integrity tool in Altium Designer

    Once you’ve opened up the signal integrity tool, you should see the Signal Integrity dialog shown in the image below. Here, you’ll need to select which signal nets you want to examine. You can double click the signal nets you want to examine, and these will be added to the table on the right side of the dialog.

    The Signal Integrity tool in Altium Designer

    Choosing nets and termination networks for your signal integrity simulation

    You’ll also see a list of termination networks. In the example that follows, we’re going to examine two single-ended traces (NC1 and NC2). Note that you can change the number of sweeps, as well as the parameters in the termination network. You could also examine one of the differential pairs (i.e., NC3_P and NC3_N) using the same steps presented here.

    We’ll look at a series termination network, as well as the “Parallel Res to VCC & GND” termination network. Note that you can choose the maximum and minimum values for your sweep, as well as your VCC voltage.

    Setting up your matching network in Altium Designer

    Here, you can modify the values of the termination resistors in your matching network

    Now that you have set up the simulation, click the “Reflection Waveforms…” button to start the simulation. Altium Designer will iterate through the various resistor values and generate a series of graphs. The results for nets NC1 and NC2 are shown in the figure below.


    Signal integrity results showing signal reflection in Altium Designer

    Signal reflection results for various matching networks

    From the results above, we can see that the series matching resistor (top two graphs) and the combination of resistors to VCC and ground are actually not the best choices for this board. Both results help reduce ringing somewhat, but we also need to compensate for the slow rise time. Therefore, we should try a different network and repeat the process.

    Here, we can go back and choose the “Parallel Res & Cap to GND” network and check to see how this network affects the signals in nets NC1 and NC2. The results for this network are shown below. To see the values for each component in the network, just click on one of the labels in the legend on the right side of the graph. In this board, it turns out that the optimum trace network uses a 56.67 Ohm resistor and an 83.33 pF capacitor (the red signal in the bottom graph).

    Signal integrity results reflection in Altium Designer

    Signal reflection results for the resistor/capacitor network

    To examine a differential pair, you can go back to the Signal Integrity dialog and add both ends of the differential pair to the simulation. You can then check termination using the same steps as you would for a single-ended trace. You can also try working with other matching networks to see which produces the best results.

    Going Further With Impedance Control Routing

    Without a doubt, your best bet is to use impedance controlled routing so that you can ensure your traces will have consistent impedance values throughout your board. Ideally, this will help avoid the need to apply a termination network to every single trace in your board, saving you a significant amount of design time.

    Determining the right termination network to use in your PCB is much easier when you work with a PCB design package that includes power design and simulation tools. With Altium Designer, you’ll have full control over your layer arrangement and design, and your simulation tools will take data directly from your layout. These tools are directly adaptable to rigid-flex and multi-board systems.

    Download a free trial of Altium Designer to see how the powerful signal integrity tools can help you. You’ll have access to the best design features the industry demands in a single program. Talk to an Altium expert today to learn more.

    About Author

    About Author

    Zachariah Peterson has an extensive technical background in academia and industry. Prior to working in the PCB industry, he taught at Portland State University. He conducted his Physics M.S. research on chemisorptive gas sensors and his Applied Physics Ph.D. research on random laser theory and stability.His background in scientific research spans topics in nanoparticle lasers, electronic and optoelectronic semiconductor devices, environmental systems, and financial analytics. His work has been published in several peer-reviewed journals and conference proceedings, and he has written hundreds of technical blogs on PCB design for a number of companies. Zachariah works with other companies in the PCB industry providing design and research services. He is a member of IEEE Photonics Society and the American Physical Society.

    most recent articles

    Back to Home