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
  • 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

    How to Simplify Your Circuit Replication with Multi-Channel Design

    David Cousineau
    |  March 27, 2017

    Circuit replication, especially in flat designs, presents several unique challenges that occur when you copy PCB layout designs. You can't simply copy and paste footprints around your PCB layout and expect all of your design data to remain synchronized without errors. What about reverse engineering? Similarly, when you need to reuse circuit blocks in a schematic, taking the copy and paste approach simply takes too long and can make your schematics very disorganized.

    When you take a multi-channel design approach to circuit replication and design reuse, you can successfully overcome the challenges associated with flat designs. Multi-channel design also works within hierarchical schematics in Altium Designer®, giving you an easy tool for circuit replication and design reuse. In this article, I'll present a simple example that illustrate the power of multi-channel design for quickly replicating circuit blocks in a schematic and in the printed circuit board layout.

    The Advantages of Multi-Channel Design

    Altium Designer offers many methods for multi-channel design (i.e. repeating circuitry within a single design). No matter how you choose to do multi-channel design, the main advantage is the ease of circuit replication and design reuse. Once you have an existing schematic, you can copy board blocks into new sheets, or you can place symbols that represent other schematics. This makes replication of circuit blocks easy as any change to the underlying circuit only needs to be made once.

    There are many users, however, who have not worked with hierarchical designs and feel more comfortable using a flat design methodology. Some projects might be too simple to warrant setting an entire design as hierarchical. Whatever the case, there are a number of legitimate occasions where a Project is set up as flat, but circuit replication is necessary within a single schematic and as part of a hierarchy to enable circuit replication and design reuse. How can this be done?

    Whether you're using a flat design with multiple sheets or creating a design hierarchy, you’ll find that Altium Designer will automate most of the circuit replication work for you. Once you've finished your schematics and are working on your layout, there is one bit of manual intervention required by the user during the process to ensure easy replication and synchronization between the PCB layout design and schematics.

    Step 1 - Schematic Design and Circuit Replication

    Let’s walk through an example to see how this works. We’ll start by creating a power regulator section on the first schematic sheet for a new project. This sheet is named “Channel_1.SchDoc”, as shown below. In our example, Channel_1 can be reused multiple times in a different schematic, i.e., it can be used as a child schematic as part of design reuse in a schematic hierarchy. This would be done by placing a Sheet Symbol in the parent-level schematic, as is normally done in hierarchical design. If you want to maintain a flat project, you can also perform design reuse by copying these circuit blocks across a project.

    Channel 1 Schematic before replication
    The Channel_1 schematic will be used for circuit replication

    Ports have been placed in the above schematic to show where connections will be made within the design hierarchy or as part of a flat project. This schematic can also be used in a flat project, where the schematic is just replicated multiple times in multiple sheets. A second, blank schematic sheet (“Channel_2.SchDoc”) can be added to the Project; we want to copy the circuitry in Channel_1 to our new schematic sheet Channel_2.

    Once you create the first circuit in Channel_1 with its own reference designators, you want to ensure the reference designators will reset to unassigned values when they are copied and pasted to Channel_2. This will prevent duplicated designator conflicts when repeating circuit blocks. The ports “V_IN” and “V_OUT” have been made unique in Channel_1, as has the “Channel_1” text identifier.

    Go to the Tools menu while and select Preferences. Expand the Schematic group and select the Graphical Editing section. In the Options area, make sure the “Reset Designators on Paste” option is enabled.

    Next we’ll group-select the components in Channel_1, copy and paste them into Channel_2, and then make any edits necessary to Channel_2 to ensure proper connectivity with the rest of the schematic design. Once you paste the circuit blocks into Channel_2, be sure to rename the input and output ports in the Channel_2 schematic, as well as any net names that might have been duplicated during circuit replication (see CS and CS2 in our schematics as an example).

    We can now add whatever additional sheets are necessary for the design. However, it is important that no further additions or changes be made to any of the repeated schematic sheets. Doing so may cause the Copy Room Formats feature to fail later on. For this project, a third sheet (“Connector.SchDoc”) will be added to include a connector with the design. Since the reference designators on Channel_2 have all been reset, we can run Tools > Annotation > Annotate Schematics Quietly to set the new reference designators in Channel_2.

    Another important note has to do with multi-part components. An example, the TL074ACD op-amp, which includes 4 symbols. After running reference designator annotation, make sure any unused portions of multi-part components are not mistakenly added to another schematic. There needs to be consistency between each physical so that the routing can match.

    Step 2 - Setup for Circuit Board Project Options

    The next step is to set the Project Options to automate Component Class and Room generation. To do this, we’ll go to Project > Project Options and switch to the Class Generation tab.

    We need to ensure that the checkboxes for Component Classes and Generate Rooms are enabled for all multi-channel sheets. Any other sheets are optional. To finish up, we’ll close the Project Options dialog and save all schematic documents, as well as the Project file.

    Step 3 - Schematic Capture and PCB Layout

    The final step is to create and save a new PcbDoc file, then use Design > Import Changes… to populate the circuit board. Ensure that the ECO includes the creation of the Component Classes and Rooms. If not, recheck the Project Options setup in the previous step. The PCB schematic will then be populated with the Rooms once the components are imported into the blank PCB.

    An example is shown below, where a new layout has been imported from 3 different schematic sheets. With the rooms creation option, the components are automatically grouped into rooms and the layout settings can be replicated between different rooms. 

    The image below shows a completed layout inside and Room and its routing in the circuit board area. The Room outline can be resized if necessary. Take a look at the Altium Designer documentation to see how you can copy room formats to other rooms using our PCB design software
    Resetting schematic designation in Preferences
    Reset reference designators when they are pasted in your schematics.

    Check out Altium Designer in action...

    About Author

    About Author

    Dave has been an Applications Engineer for 20 years in the EDA industry. He started in 1995 at a mid-Atlantic reseller that represented PADS Software, ViewLogic, and a host of other EDA tools. He moved on to work directly for PADS Software, and stayed on as they were acquired by Innoveda and then by Mentor Graphics. He and a business partner formed a VAR of their own in 2003 (Atlantic EDA Solutions) to represent Mentor's PADS channel, and later on Cadence's OrCAD and Allegro products. Since 2008, Dave has been working directly for Altium and is based at his home office in New Jersey.

    most recent articles

    Back to Home