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

    Managing Net Connection Order from Schematic to Layout

    Altium Designer
    |  December 20, 2018

    Screenshot of AD18 schematic, rules, and 3D layout in net connection order

    When I first started designing printed circuit boards, it was a very unorganized process. We would create the schematics in our department, and then the system administrators would work their voodoo and transfer all that data from us into the layout department. The layout guys were an even bigger mystery, working all hours of the night and day on these complex Unix machines that supported their CAD layout tools. We would communicate our design intent through documents and spreadsheets followed by meetings and even time spent working with them, and yet somehow it still would get messed up.

    The design tools we use now are much better at managing the net connection order between the schematic and the layout. Altium Designer® gives us several tools that we can use to verify our schematic and even alter the net rules for layout. This has been very helpful in the communication between engineering and layout and has been a big factor in reducing the errors that used to plague us before. Here are some of the features that we are now using in Altium that have helped us.

    Setting up the Error Reporting

    Altium gives you a couple of different tools to work with so that you can control the checking of your schematic before you even go into layout with the design. These tools are found in the project options. You can either go to the Project pull-down menu and select “Project Options,” or right-click in a schematic sheet and select it there. As you can see below, the project options menu has many tabs across it. The first tab is the error reporting tab and it allows you to set up how different aspects of your design are going to be reported. Since we are focusing here on managing net connection orders, we’ve scrolled down to the “Violations Associated with Nets” section.

    Screenshot of AD18 project options menu in net connection order

    The Project Options menu in Altium

    You can set up how Altium will report these different conditions to you by clicking on the colored icons in the “Report Mode” column on the right. The different options available to you are as follows:

    • Green:        No Report
    • Yellow:        Warning
    • Orange:    Error
    • Red:        Fatal Error

    When you click on the colored icon, a drop-down menu will appear where you can select one of four different options as shown below.

    Screenshot of AD18 project options error reporting mode in net connection order

    Setting the error reporting mode in Altium ’s project options

    Altium will run all of the checks that you see in the error reporting tab when you compile the schematic. To compile your schematic, go to the “Project” pulldown menu and select “Compile PCB Project.” If your design doesn’t have any errors in it, your schematic design session will not return any messages.

    In order to show you what an error looks like, we have removed a portion of the net that connects R1 to Q1 in the picture below and run the compiler. As you can see below, Altium has reported back to us that net “NetC1_1” only has one pin on it. Once I reconnected that net, the compiler ran without any reported errors as it should.

    Screenshot of AD18 compiler report in net connection order

    The compiler report showing the missing net error

    Working with the Connection Matrix

    We’ve got the error reporting set up, and that’s good, but we’re not done with the project options yet so don’t close that menu. The next tab is the “Connection Matrix” which will give you control over how to report your connectivity rules between component pins and net objects such as ports. By clicking on the tab you will see the connection matrix displayed as shown below.

    Screenshot of AD18 connection matrix in net connection order

    The project options Connection Matrix menu in Altium

    As with the error reporting tab the connection matrix tab allows you to set up your reporting for “No Report,” “Warning,” “Error,” and “Fatal Error.” Here though you will repeatedly click on the colored icon to change the reporting. As you can see in the picture below, we’ve clicked on the icon where both the passive pins meet to change it to a red fatal error.

    Screenshot of AD18 connection matrix error setting in net connection order

    Setting an error level in the Connection Matrix menu

    Now when we compile our schematic we can see that the passive pins are now reporting an error. Throughout this schematic where there are passive pins connected to each other, Altium displays an error. Not only does the report window show the errors, but by setting up the Compiler options in the Preferences menu we can also highlight each error with a squiggly line on the schematic sheet.

    Screenshot of AD18 net error in net connection order

    Passive pins connected together reported as an error

    There may be times that you want to allow certain errors to go through, and Altium gives you an option for that as well. By using a command to ignore the electrical rule check (ERC), Altium will not flag that specific object as an error. The feature that you will use for this is in the “Place” pulldown menu, and it is the “Directives > Generic No ERC” command.

    To make this work, engage the command and then place the directive symbol that is now on your cursor on the object that you want the compiler to ignore. In this case, we’ve placed the symbol over the lower pin of R1. Now, as you can see below, when we run the compiler the lower pin does not show as an error as it did before.

    Screenshot of AD18 net error with directive in net connection order

    Passive pins connected together reported as an error with a directive exception

    Another portion of the project options menu that will be useful to you is the “Class Generation” tab. Here you can set up Altium to automatically generate net classes for specific parameters as it is being compiled for layout. This is another way that you can help manage the net connections from the schematic.

    Using Directives to Help Your Net Connection Order

    Another useful use of the directives is to alter the design rules as needed from the schematic. The design rules are usually set up in the PCB document by going to the “Design” pulldown menu in layout and selecting “Rules”. Here you can add new rules and modify existing ones. You also have the option of using the Rules Wizard which is in the same Design pulldown menu. With both the schematic and layout available to you in Altium , jumping into the layout makes working with these rules and easy thing to do. But by using the directives, you can work with the rules from the schematic without ever going into the layout.

    As we saw with the “Generic No ERC” directive, go to the “Place” pulldown menu in the schematic and select “Directives > Parameter Set”. With the parameter symbol floating on your cursor, hover over a net and click the mouse button to place it down as shown below. With the goal here of better managing your net connection orders, this will demonstrate to you how to control your PCB layout net rules from the schematic.

    Screenshot of AD18 parameter set directive in net connection order

    Setting a Parameter Directive on a net in Altium

    With the parameter set placed on a net, double-click it to bring up its properties. In the property panel you can see different settings for the parameter set including a rules menu which is currently blank. By clicking on the “Add” button you will bring up the “Choose Design Rule Type” menu as shown below.

    Screenshot of AD18 parameter set chose rule in net connection order

    Choosing a net rule for the parameter directive to use

    For our purposes, we will choose the “Routing > Width Constraint” rule by clicking on it and then clicking OK. This will bring up a menu that will allow you to edit the maximum & minimum width rules for the PCB rules from the schematic. Just as you would when working with these rules over on the PCB layout side of Altium , you will make the same changes here. You can alter the minimum, preferred, and maximum widths, and you can set these widths for specific layers in the design.

    Screenshot of AD18 parameter set width rule in net connection order

    Setting the width rule for the parameter directive

    Looking for software that can manage any layer, produce the PCB design file you need, have easily manipulatable shapes, polygons, and has every step of the design process like a footprint, board design, and schematic view? Altium ensures that all of this is developed thoroughly within an easy-to-learn user interface. No more searching for the right control panel, no more concern over how to connect your design through various PCB footprint edits.

    These are just a few of the features that we have found in Altium that have helped us to manage our net connection order. There are plenty of others in this powerful schematic capture tool, and they have all helped us to improve our communication between the schematic and the layout. Altium Designer is a great set of PCB design software, and has made a real difference in our ability to get our designs done faster and with greater accuracy.

    Would you like to find out more about how Altium can help you with your schematic creation? Talk to an expert at Altium.

    About Author

    About Author

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

    most recent articles

    Back to Home