Free Trials

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

Altium Online Store

Buy any Altium Products with few clicks or send us your quote to contact our sales


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

    Altium Online Store

    Buy any Altium Products with few clicks or send us your quote to contact our sales


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

    • 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

    PCB Routing Rules for Single-Ended and Differential Signals

    Zachariah Peterson
    |  October 30, 2020
    PCB routing rules for low speed and high speed signals

    Sometimes, the distinction between what qualifies as a “slow” or “fast” signal can seem arbitrary, and it might depend on who you ask. A related topic is whether a PCB trace is considered electrically “short” or “long,” and you might find just as much disagreement on the topic. Whether you need to route slow or fast signals in your PCB, your traces will need to follow some PCB routing rules to ensure your board functions as intended.

    Like many other programs, Altium Designer® helps make this process easy, but Altium Designer goes a bit further and separates PCB routing rules for slow and fast signals into their own categories. Before you start routing signals between components, you’ll need to take a look at your design rules and adjust them to your signalling standards. Here are the important PCB routing rules you need to set before you start routing signals around your PCB.

    PCB Routing Rules for Single-Ended Signals

    Perhaps the most important point to note about PCB routing rules is that routing standards do not necessarily define themselves as “low speed” or “high speed.” This distinction has been largely created and perpetuated by PCB designers, and it largely arose due to signal integrity problems that arise when signal rise times become very fast (less than ~1 ns). As such, it’s more important to understand the constraints in your signaling standards when setting up your design rules, regardless of whether you’re dealing with slow or fast signal speeds.

    The first place to look for the design rules you need is in the documentation for your signaling standards. The documentation for most standards is freely available online. As you create more designs, you’ll become more familiar with these standards and you’ll know which rules to set in your designs. Some of the most common PCB routing rules that apply to many standards for single-ended signals are:

    • Matched lengths. For bus standards or parallel data routing with source-synchronous clocking, you’ll need to enforce length matching for all nets in a group within some tolerance. While routing, this is done by adding length tuning structures to a net. 
    • Via transitions. Some standards recommend limiting the number of via transitions to prevent excess loss, reflections, and other parasitic effects. 
    • Maximum length. The maximum length of a net is sometimes specified for a given loss tangent value to prevent excessive signal attenuation. If you’re using a low-loss laminate, you can extend the length depending on the difference in loss tangent values. 
    • Clearances. Traces need to be kept separated from other objects that aren’t part of the net (pads, components, planes, etc.). This ensures manufacturability, reduces unwanted parasitics, and provides ESD protection in high voltage design.
    • Width and impedance. These two quantities are interrelated and are used for controlled impedance in high speed design. Take a look at this article to see how you can specify impedance and trace width as PCB routing rules. 

    All these design rules and many more can be accessed in the PCB Rules and Constraints Editor in Altium Designer. If you need to assign the same PCB routing rules to a group of nets (very common for groups of single-ended signals), the quickest way is to assign all nets in a group to a Net Class. You can access this feature from the Design → Classes option (see below) in the PCB Editor window. After you’ve assigned nets to classes, can then use the PCB Rules and Constraints Editor to assign design rules to individual nets or to a Net Class.

    Creating a Net Class for PCB routing rules
    Assigning nets to a Net Class allows you to assign PCB routing rules to groups of nets in your design.

    Other PCB routing rules that may not apply to specific signalling standards are used to help ensure you keep your design organized. Two prime examples are routing topology and routing layer restriction. For more advanced designs, such as components with BGA footprint, you can use design rules to configure your fanout strategy. Working with differential pairs requires its own set of design rules, as shown in the next section.

    Differential Pair Routing Rules

    Differential pairs are unique because slow and fast signals can be routed as differential pairs. Regardless of whether the signals are fast or slow, your differential pairs still need to obey some design rules that you would normally enforce for single-ended signals. Four important design rules to consider for differential pairs are:

    • Impedance tolerance. Even if you’re routing at less than the critical length, it’s best to bite the bullet and create an impedance profile for your differential pairs unless your signaling standard says otherwise. Other geometry constraints will depend on the allowed impedance variation along the differential pair. 
    • Maximum uncoupled length. This tells you the longest distance that the two sides of a differential pair can remain uncoupled (i.e., separated by a large distance). This is important as the uncoupled section will look like an impedance discontinuity, so it must be sufficiently short. 
    • Length matching. Remember, a differential signal is read by taking the difference between the two signals, so the two signals need to arrive at the receiver simultaneously. Faster signals require smaller length matching tolerances. 
    • Maximum net length. Just like single-ended signals, differential signaling standards may have a maximum length constraint. Consider CAN bus as an example; even though this is a slow-speed standard, the maximum link length (PCB traces + cable) will depend on the data rate you’ll use in your system. 

    In Altium Designer, you can set up design rules for the first two points above in the Routing → Differential Pairs Routing area of the PCB Rules and Constraints Editor. The other two points can be addressed in the High Speed area. This is shown for the image below:

    PCB routing rules for differential pairs
    Setting up differential pair PCB routing rules.

    If you’re working with high speed differential pairs, any of the other standard high speed design rules discussed above can be applied to differential pairs. Note that the easiest way to do this is to assign the relevant differential pairs to a Differential Pair Net Class, and then select the class that will be governed by each design rule.

    If a design rule is not configured to accept a Differential Pair Net Class in the “Where The Object Matches” drop-down menu, you can create a Custom Query using the query builder. This is shown below for assigning maximum length to a Differential Pair Net Class (found in the High Speed area of the PCB Rules and Constraints Editor).

    PCB routing rules for differential pairs with Query Builder
    Applying differential pair PCB routing rules with the Query Builder.

    Just like with single ended nets, read the documentation on your signaling standard before you start setting PCB routing rules. This is where you’ll find the relevant design rule information for differential signaling standards (usually in the Physical Layer section of the standard). Take a look at this article to see how to create an impedance profile, assign nets to differential pair net classes, and set up some design rules for these classes before you start routing differential pairs.

    We still haven’t looked at signal integrity rules for fast signals, and by now you’ve probably noticed that Altium Designer includes design constraints specifically to address signal integrity problems. You can assign these PCB routing rules with the same process you followed for adding design rules to single-ended nets and differential pairs. These features in Altium Designer give you full control over your design and help you route successfully.

    Altium Designer on Altium 365® delivers an unprecedented amount of integration to the electronics industry until now relegated to the world of software development, allowing designers to work from home and reach unprecedented levels of efficiency.

    We have only scratched the surface of what is possible to do with Altium Designer on Altium 365. You can check the product page for a more in-depth feature description or one of the On-Demand Webinars.

    Altium Designer Free Trial


    About Author

    About Author

    Zachariah Peterson has an extensive technical background in academia and industry. He currently provides research, design, and marketing services to electronics companies. 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 sensing and monitoring systems, and financial analytics. His work has been published in over a dozen peer-reviewed journals and conference proceedings, and he has written hundreds of technical blogs on PCB design for a number of companies. Zachariah currently works with other companies in the electronics industry providing design, research, and marketing services. He is a member of IEEE Photonics Society, IEEE Electronics Packaging Society, and the American Physical Society, and he currently serves on the INCITS Quantum Computing Technical Advisory Committee.

    most recent articles

    Back to Home