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

    Creating a Ground Plane for Your PCB Design

    Altium Designer
    |  August 10, 2018
    Creating a Ground Plane for Your PCB Design

    It used to be that printed circuit boards seemed to have the same basic layer configuration, or at least that’s the way I tend to remember it. This meant that they were usually six layer multi-layer boards, with a ground plane and a VCC plane. The old CAD systems didn’t really have the ability to do much with power planes except to designate layers as a bottom layer or the like. The most you would see in them would be some “X’s” where there was supposed to be a connection for a thru-hole pin or via that connected to that plane. 

    Thankfully this all changed long ago. Now instead of being driven by the limitations of those older CAD systems, you can drive the design tools to create the plane layers the way you want them to be. You have the choice of creating a ground plane that is either a positive copper fill, or a negative plane depending on what your needs are. Any CAD system can do this, but some are better at it than others. Take Altium Designer for example. This PCB design system does a great job of enabling you to create the planes that you need. Let me show you how.

    Creating Ground Plane | PCB Design | Info graphic

    Make Sure that Your Schematic Nets are Correct

    Before you create your ground or voltage planes in layout, you will want to make sure that your schematic is set up correctly. This means that you have assigned the right net names so that all of your power and reference planes can be created correctly in layout. In Altium Designer’s schematic editor you can either assign a net name to a net, as pictured below, or attach a power port to the net as you see on the right side.

    Screenshot of Altium Designer schematic nets in creating a ground plane

    Naming Schematic Nets in Altium Designer

    The advantage of the power port is that it will connect across all sheets of your schematic without having to attach an offsheet connector to a named net. Once your nets are correctly named, you are ready to synchronize your schematic and layout to begin working with your power and ground planes. 

    Using an Internal Plane in Creating a Ground Plane

    In Altium Designer, you can create your planes either as a negative (Internal) plane or as a positive plane (Polygon Pour). First we will look at the process of creating a negative or “Internal” plane. 

    The first thing to do when creating an internal plane is to add a design layer specifically for the plane. In the picture below, you can see in that two layers have been added as internal planes in the layer stack manager, which is found in the “Design” pulldown menu. They have been named “GND” and “PWR” respectively and occupy layers two and three. These two internal plane layers also have a “Pullback” value assigned to them which will keep their edges 20 mils away from the edge of the board.

    Screenshot of Altium Designer layer stack manager in creating a ground plane

    Creating Internal Plane layers using Altium Designer’s Layer Stack Manager

    The next thing to do is to assign the correct size for the thermal relief pads and clearances that you want on your plane layers. To do this we will open up the design rules in Altium Designer which is also found in the “Design” pulldown menu. As you can see in the picture below, you have the ability to specify the expansion, air-gap, and conductor width of a thermal relief pad. You can also specify the type of connection you want. In the example below you can see how the pad connection is set for a thermal relief while the via connection is set as a direct (solid) connection to the plane.

    Screenshot of Altium Designer plane connect styles in creating a ground plane

    Setting up thermal relief pads in the design rules of Altium Designer

    The menu above also gives you the ability to set other values for your planes. Note on the left side of the picture that in addition to the plane connection style, there are also categories for plane clearances and polygon connect styles. 

    Once you have set everything up, you are ready to assign the net name to the internal plane layer. On the left side of the picture below, note that the pins and vias do not have any visible connections yet to the power plane. This is because the net name has not been assigned. You can also see on the left side of the connection menu that pops up when you double click on that layer within the layout session. This same menu is used to name both single and split planes.

    Screenshot of Altium Designer assigning net name to internal plane in creating a ground plane

    Assigning the net name to the internal plane layer

    In the drop-down menu on the left side of the picture above we have selected “GND” as the net name that we want for this internal plane. This way it will match the GND net of the pins that you can see in the picture. Once we have made this assignment, the vias are directly connected to the plane and the pins have thermal pad connections as you can see on the right side of the picture. Remember that this is a negative plane, so the metal of the thermal spokes and plane area is represented by the darker color. 

    Keep in mind that if your printed circuit board has an antenna, the antenna ground plane can be a critical aspect of the antenna functionality and is worth learning more about.

    Using a Polygon Pour in Creating a Ground Plane

    Now we’ll create a positive plane, or a “Polygon Pour”. On the left side of the picture below you can see that this signal layer does not have any metal on it yet. To create the polygon pour you can either use the pulldown menu command “Place > Polygon Pour”, or you can click on the polygon icon in the active bar at the top of the session window.

    Screenshot of Altium Designer polygon pour in creating a ground plane

    Creating a Polygon Pour in Altium Designer

    While in the polygon pour mode you will click where you want to place a vertex of the plane that you are creating. If you make a mistake simply use your backspace key to remove the last placed vertex. Once you are finished, right click in the work space to exit the polygon pour mode. As in the right side of the picture above, you will see the plane that you created assumes the color of the layer that you are working on. You will note though that there aren’t any connections yet to the pins and vias. 

    Next, select the plane that you just created and go to the properties panel. As you can see in the picture below, you will have a list of nets to choose from for assigning to this plane. As you can see, we have selected the GND net.

    Screenshot of Altium Designer net name for polygon pour in creating a ground plane

    Assigning the net name to the polygon pour

    In addition to selecting the net, there are other options and values that you can set up in this panel for your plane. As you can see above, there are options for copper islands, arcs and nets as well as setting your plane up as a solid pour or hatched. 

    While the plane is still selected you will next need to re-pour the plane in order to make a connection to the net name that you just assigned to it. To do this, right click on the selected plane in the main session window.

    Screenshot of Altium Designer repour polygon pour in creating a ground plane

    Re-pouring the polygon pour to connect the net

    In the picture above our right mouse click has opened up the “Polygon Actions” menu on our selected plane. To connect the plane to the net we will select “Repour Selected”. 

    At this point the net name is associated with the polygon pour that you created. In the picture below you can see that the metal shown in red is now connected directly to the vias and with thermal relief spokes to the pins. This ground plane in your PCB layout is now complete.

    Screenshot of Altium Designer polygon pour ground plane in creating a ground plane

    A completed polygon pour ground plane in Altium Designer

    There is much more in Altium Designer for the creation of power planes and ground connection capabilities than what we have shown you here. Altium Designer is both powerful and flexible, making it one of the best PCB design software systems available. It will provide you with the tools that you need to expertly handle the design challenges that you are working with today.

    Would you like to find out more about how Altium Designer can help you to create your ground planes on your next PCB design? Talk to an expert at Altium Designer.

    About Author

    About Author

    PCB Design Tools for Electronics Design and DFM. Information for EDA Leaders.

    most recent articles

    Back to Home