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

    Changing PCB Reference Planes During Routing in Multilayer Boards

    Zachariah Peterson
    |  May 27, 2019

    Vias for changing layers and PCB reference planes

    Vias with annular rings for reaching an interior PCB layer

    If you’re a new designer and you take a look at some boards in common electronic products, you may not even realize they are multilayer boards unless you know exactly where to look. The fact is that more complex devices simply do not allow every single trace to be placed on a surface layer, thus signals must be routed within an interior layer in order to make the desired connections.

    With complex boards involving multiple signal, power, and ground layers, your routing strategy is critical to ensure signal integrity and tight coupling to a reference plane. If you use the right routing tools and implement the right strategy during design, you won’t need to implement difficult fixes to important signal integrity problems.

    Routing Between Layers in Your Layer Stack

    Ensuring your multilayer PCB works as intended requires designing the right layer stack. Your layer stack will have an important effect on signal integrity, particularly on EMI within your board and its susceptibility to external radiated EMI. This also determines whether the board can pass EMC checks once manufactured.

    Your routing strategy and layer stack will need to complement each other. The right stackup can ensure your routing strategy will eliminate or minimize signal integrity problems. The right place to start is to consider your ground plane arrangement with respect to your signal layers. Each signal layer should be placed directly adjacent to a ground plane. It is important to place a ground layer between a surface signal layer and an interior signal layer as long as traces in the interior signal layer are routed to components on the surface layer. This ensures tight coupling to a PCB reference plane in both layers.

    In the aforementioned arrangement, you can avoid many signal problems if you only route signals through a single ground layer. As the signal vertically traverses the ground layer through a via, it will remain coupled to the ground plane and its return signal will be induced in the ground plane. This ensures tight coupling throughout the route and minimizes the circuit’s loop inductance. This also reduces radiated EMI from traces by ~10 dB.

    The same idea applies to routing through a via across power planes. Although, it is a good idea to place a power plane adjacent to its ground plane. This minimizes loop inductance, thus minimizing susceptibility to EMI and any currents induced in the ground and power planes. This also increases the capacitance between the planes, providing a low impedance return path for any high frequency conducted EMI in your power plane.

    Routing Through Multiple PCB Reference Planes

    The grounding situation becomes more complicated when routing through two or more ground layers in your layer stack. This situation is shown below where a signal routes from an interior layer to a surface layer (shown in the red arrow).

    Here, the signal maintains tight coupling to a ground layer in the interior signal layer and the surface layer. However, during the transition from the interior to the surface, there is a region where the signal is not coupled to anything. You can place a via between the two ground planes to create a return path during the transition (see the blue arrow below).

    Grounded via between two PCB reference planes

    Placing a grounded via between PCB reference planes

    If there is no return path, you suddenly have two problems. First, a return path will form  in the nearest grounded element with the lowest reactance. This is normally a bypass/decoupling capacitor, but it could also be a via that connects to a ground plane. This causes a very large loop inductance in the circuit as the via strongly radiates into the transition region.

    Second, the larger loop area increases susceptibility to external radiated EMI and crosstalk via mutual inductance. If you have a single isolated route between two ground planes, you might not have to worry about EMI or crosstalk problems as long as you are working with low-level signals. If you make several of these transitions in a single area, you may need to place multiple vias between the planes, or improve your stackup and routing strategy.

    Don’t Forget Your Routing Strategy

    If you devise the right routing strategy for each signal net before designing your stackup, you can eliminate the need to route through multiple planes when transitioning between a surface and an interior signal layer. Be careful when using an autorouter; a high-quality autorouter will let you define specific layer transitions as part of your routing strategy, which ideally prevents the need to route through multiple reference planes.

    One area where you will need to consider the relationship between vertical routing and your stackup is when designing a BGA fanout strategy. With low pin count components, where pins are arranged in four rows along the edge of a component (see the image below), a simple dog bone fanout strategy is sufficient and only requires crossing through a single ground layer. When working with higher pin count packages, you may have no choice but to use two or more ground layers for a single signal net. Be sure to consult the manufacturer’s data sheets and keep proper grounding to prevent signal integrity problems.

    HDI routing to a BGA

    Designing multilayer boards and implementing the right strategy ensures your board remains free of signal problems. Altium Designer contains the layer stack design, layout, and simulation features you need to design the best multilayer boards in a single interface.

    Download your free trial of Altium Designer today to learn more about the industry’s best design, simulation, and verification features. 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