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

    Making friends with differential pairs

    Karen Beard
    |  February 21, 2017

    A question arises when working with differential pairs, particularly when you inherit or import designs where the differential pair directives were not added to the schematics. Is it actually necessary to set up the directives in the schematic documents?

    A question arises when working with differential pairs, particularly when you inherit or import designs where the differential pair directives were not added to the schematics. Is it actually necessary to set up the directives in the schematic documents?

    In order to use the schematic Differential Pair directives in Altium Designer®, a specific naming convention must be used. The negative and positive signals of the pair must follow the conventions signalname_N and signalname_P respectively, and each signal must have a Differential Pair directive attached. If the differential net names were denoted in another way, such as with a + and - or _H or _L, you would need to rename the nets with the _N and _P suffixes in order for Altium to be able to utilize the schematic directives.

    However, there is a method which can be employed in the PCB Editor to create differential pairs based on a more configurable naming convention. All that’s required is that the differential signals have Net Labels on the schematic that in some way consistently define the positive and negative nets of the pair. Even if you have followed the _P, _N conventions on the schematic, the following method allows you to create the differential pairs within the PCB Editor without having to first place Differential Pair directives in the schematic.

    In order to create the differential pairs from named signals on the PCB, make sure all net data is loaded into the PCB through the execution of the ECO. Either use Design » Update PCB from Schematics, or from the PCB Design » Import Changes from <projectname>.PrjPcb. Execute the changes from the ECO and the nets will be loaded into the PCB.

    In the PCB Editor make sure the PCB panel is visible by going to View » Workspace Panels » PCB » PCB. Place the panel in Differential Pairs Editor mode, by selecting Differential Pairs Editor from the drop-down list at the top of the panel.

    The three main list regions of the panel will change to reflect, in order from the top: differential pair classes, individual member differential pairs within a class and the constituent nets (negative and positive) that form a differential pair.

    Differential pair objects can be created from the nets in your design using the Create Differential Pairs From Nets dialog. This dialog is accessed by clicking on the Create From Nets button, beneath theNets region of the PCB panel.

    The efficiency of this automated method greatly depends on the naming convention that is used for the specific nets that are to be routed as differential pairs. The filters at the top of the dialog enable you to quickly target these nets in terms of the net class to which they belong and the particular differentiating factor that has been used to distinguish the positive and negative nets in an intended pairing. You can also define a prefix to be added to the differential pair objects created and also determine in which differential pair class they are to be added.

    The image shows an example of differential pair objects created from design nets. In this case I’ve based my search on the _P and _N suffixes.

    For each potential differential pair object found in the design, the dialog lists its constituent positive and negative nets. You can exclude nets from which you don’t want to create differential pairs by clearing the associated Create checkbox. When all options are set as required, click the Execute button - the differential pair objects will be created and the PCB panel will update accordingly.

    Filtering will be applied to show the created pairs in the workspace.

    The differential pairs now exist as defined objects in the PCB and they are listed in the PCB panel under the Differential Pairs section.

    By clicking on a pair within the PCB panel, the third region will be populated with the nets of the pairs.

    Remember to press Clear (at the bottom right corner of the workspace) to refresh the view and get ready to start a command.

    Differential pairs are routed as a pair. That is, you route both nets of the pair simultaneously. To route a differential pair, select Interactive Differential Pair Routing from the Place menu. You will be prompted to select one of the nets in the pair. Click on either to start routing.

    As you route the differential pair the standard conflict resolutions modes are available, including Walkaround, Push, Hug and Push, and Ignore obstacles. Use SHIFT + R to cycle through the modes. Use the * key on the numeric keypad to switch layers, and the *5 shortcut to cycle possible via patterns. Press the Shift+F1 shortcuts to display all of the available shortcuts.

    About Author

    About Author


    most recent articles

    Back to Home