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

    Enhancing Your Design Efficiency with Project Templates

    February 10, 2017

    Download the PDF to keep learning offline


    New Altium Designer users may not fully understand the benefits of organizing schematic sheets into a hierarchical top-down or bottom-up perspective. As a result, users often proceed with simple (flat) schematic designs without giving a second thought to project organization. In this paper, we’ll take a comprehensive look at the sheet symbols and how they’re used to synchronize the parts of a larger design.


    In Altium Designer, starting a hierarchical design requires the creation of sheet symbols. A schematic sheet symbol is an electrical primitive, used to represent a sub or child sheet in a hierarchical schematic organization or hierarchy org chart. Sheet symbols also include sheet entries, which provide a work breakdown structure with net connection between parent and child schematic sheets, similar to the way that ports provide nodes between schematics in a flat-sheet schematic design diagram. The sheet symbols can be used to organize multiple schematics on a large design and provides users with the overall flexibility to view net connections across their entire project.

    In the image below, the sheet symbol is defined by a designator. This can be used to set the category of the design, with its respective file name linked to a particular schematic sheet. When defining the entries in the sheet symbol, the sheet entry names are then linked to the same name in their sub sheets.

    Figure 1 - Generic Sheet Symbol with Sheet Entry

    Figure 1 - Generic Sheet Symbol with Sheet Entry

    To create a sheet symbol in Altium Designer, simply go to Place -> Sheet Symbol in the schematic editor. Once you’ve done that, you can add a sheet entry by going to Place -> Sheet Entry and placing it in the sheet symbol onto the schematic.

    The sheet symbol’s properties in Altium Designer can define a designator to be labeled for your viewing purposes, as well as a filename, which is crucial for linking. Once the filename is defined, the sheet entry can then be added and edited. Its name must match to either an existing port or power port in the sub-sheet level.

    Figure 2 - Sheet Symbol Properties

    Figure 2 - Sheet Symbol Properties

    Figure 3 - Sheet Entry Properties

    Figure 3 - Sheet Entry Properties

    Easy to Navigate Through the Schematic Design:

    In a hierarchical structure design composed of multiple PCB sheet symbols, each with its own respective entry, it’s very easy to navigate to a particular sheet of the project by using Ctrl + double clicking on a sheet entry. This will focus on a particular net-named port on its respective sheet, and allows users to view its connection through a hierarchy perspective.

    Figure 4 - Top Level Sheet of Hierarchical Design

    Figure 4 - Top Level Sheet of Hierarchical Design

    Top-Down Schematic Design Approach:

    A top-down design approach is essentially described as a work breakdown structure decision-making process, stepwise design, or a decomposed design. This means taking the overview of the design, which is usually described in the top sheet level, and breaking it down into subcategories that describes each one in depth.

    Figure 5 - Navigating the Hierarchy

    Figure 5 - Navigating the Hierarchy

    The commands below are the first steps to start the hierarchy of a top-down design approach. These functions can be found Altium Designer under the Design selection.

    - Create Printed Circuit Board sheet from the symbol

    - Create VHDL file from the symbol

    - Create Verilog file from the symbol

    All four of these hierarchy structure functions are performed under the software’s schematic editor. When using the “create sheet from symbol” function, it essentially creates a sub-sheet from the top level and includes matching ports in it.

    Figure 6 - Altium Designer’s schematic editor

    Figure 6 - Altium Designer’s schematic editor

    Bottom-Up Schematic Design Approach:

    The bottom-up design approach is the opposite from a top-down approach, but still is a hierarchy based process. In bottom-down, you’re essentially inspecting a flat design of sub-sheets and using them to create a top level that combines all of that information together into a single category. As an end result in Altium Designer, the structural view remains the same.

    Figure 7 - Hierarchical Net Connectivity Scope Example

    Figure 7 - Hierarchical Net Connectivity Scope Example


    There are five different structured Printed Circuit Board methods of defining net connectivity: hierarchical, ports global, net labels global, net labels and port global, and off-sheet connectors. Which one you use is dependent on the structure of your multi-sheet designs. For a hierarchical design, the connection between the parent sheet and the sub-sheets is defined using named sheet entries in a top level sheet, which matches respectively to the named ports in the sub-sheets through component net labels.

    Setting the Net Scope in Altium Designer:

    When creating a hierarchical design process in Altium Designer, users are required to define the scope before proceeding. Otherwise, they would encounter unusual compiling errors, of which the most common is duplicate net names. The scope can be defined by going to Project -> Project Options -> Options -> Net Identifier Scope.

    Figure 8 - How to Define Hierarchical Net Identifier Scope

    Figure 8 - How to Define Hierarchical Net Identifier Scope


    In a structured multi-sheet design, it may be difficult to view connectivity and show the project viewer the overall work breakdown structure. That’s why it’s extremely beneficial to use sheet entries to define a hierarchical structure. This will allow project users to save time and eliminate the headaches associated with multi-sheet design as they proceed to schematic design review prior to production.


    most recent articles

    Back to Home