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

    Perfect Styling for Your Organization with Altium 365

    Davide Bortolami
    |  July 6, 2020
    Perfect Styling for Your Organization with Altium 365

    We all had a moment when piles of annotated schematics were growing on our desk, and we started losing track of what was what. What revision is this? Did my colleague check it? Is this IC the new one, or the one that used to go up in flames every full moon?

    In this article, I want to show you how to make a stunning personalized schematic template for your business that is ready for the Altium 365 and the 21st century. We’re going to integrate the template with all fields and features needed to keep track of our projects in the cloud, and then I will show how to deploy it across your organization using Concord Pro on Altium 365.

    Over the years I took inspiration from software development, governmental accessibility guidelines, and architectural drawings, to create a series of tips and tricks to craft easily readable schematics and title blocks which I hope will help you on your journey through the flood-lands of paper piles on your desk.

    The perfect schematic template

    Many aspects must be considered in crafting the perfect template, and I want to be honest with you, not every approach is going to work equally well.

    The right template should be readable by a broad age group and render well not only on your computer screen but also on paper and old LCD monitors.

    More importantly, care must be taken, so the template displays all information needed to pinpoint your design both outside and inside your organization.

    We should ask ourselves the following question: If our schematics were to be lost in the most unlikely of circumstances, is there enough information for it to be returned? If it were found again after two years, would we be able to pinpoint precisely where and when in the development process it originated?

    Hierarchical naming convention

    Altium is probably the software with the more extensive support for hierarchical projects, and while you can sometimes get lost in the schematics if you implement the structure in a rush, it is a feature which like no others, allows big projects to be kept well-organized.

    A hierarchical structure is one in which schematic sheets are placed one within the other through the use of device sheet objects.

    Altium does not (by default) display this structure on the schematic sheets, and while it’s easy to descend into the sub-circuits by reading the schematic filename from the Device Sheet, it can be a little confusing to crawl back up from the sub-circuit to the high-level schematics.

    One tip I can wholeheartedly recommend is following a similar naming structure to computer directories for your documents.

    For example, if we have a schematic for a digital audio equalizer main-board, we may want to divide it into subcircuits as follows:

    • MAIN: High-level system view
    • MAIN / POWER: power supply
    • MAIN / AUDIO: high-level audio processing view
    • MAIN / AUDIO / ADC: Analog to Digital converter stage
    • MAIN / AUDIO / DSP: Digital Sound Processor stage
    • MAIN / AUDIO / DAC: Digital to Analog Processor stage

    The hierarchical name constitutes our “Title” parameter, separated from “DocumentName”, which is generated automatically by Altium and resembles something like “audio_dac.SchDoc”.

    Example of hierarchical naming structure
    Example of hierarchical naming structure

    Support even the longest paths

    Windows paths, the full address of your files like “/Users/oscar.wilde/Documents/Project/AudioAmplifier2000/main_board.SchDoc” can reach up to 260 characters in length. It’s important to plan and allow enough space. Supporting the whole path instead of just the filename allows you to reduce error and can help you to pinpoint the computer that created the schematic file print through the username.

    The path parameter is called “DocumentFullPathAndName”.

    This path may be too long
    This path may be too long… nevertheless, there is enough space for it

    Use a monospaced font

    Using a mono font may look a little bit weird—almost retro. Mono fonts resemble a typewriter, as the same amount of space separates each character. This is different from most variable-width fonts for which an “I” uses less space than a “K”.

    Using a monospaced font allows you to compare paths and Git MD5 hashes on printed paper more quickly and makes the text size more predictable.

    In our example template, we’ll use courier new as it looks good and is available by default on Windows computers. More modern monospace sans-serif fonts like Source Code Pro can be downloaded and installed, but I would not recommend it unless you have a system in place to deploy them automatically on all computers.

    Example of Git MD5 hashes in a monospaced and variable-width font
    Example of Git MD5 hashes in a monospaced and variable-width font

    Choosing the size of the title block

    In Europe, the two most popular paper sizes are A4 and A3, roughly equivalent to the A and B in widespread use in the United States. Many templates for technical drawings that can be found online, especially those based on earlier Altium templates, have title blocks of about 1/3 the page width.

    I have found it’s neither practical nor elegant to attempt cramming too much into a title block. As any typographer can attest, fonts require whitespace around them to be intelligible.

    The readability of fonts depends on the surrounding whitespace
    The readability of fonts depends on the surrounding whitespace

    I recommend using the shorter side of an A4 (A type in the US) sheet as a reference. It enables to create schematics in both portrait and landscape and looks clean and proportional in all most common paper sizes

    The short side of an A4 sheet as a reference width
    The short side of an A4 sheet as a reference width

    Always Include the Engineer Name and the Company Address

    I have seen many commercial enterprise projects in which some critical information was missing from the title blocks. The most common one is the name of the engineer responsible for the drawing. Some companies decide to omit the names out of secrecy, but I think it’s fundamental to keep track of the individual responsible for a circuit, as well as to provide proof of merit for the designer.

    Writing out the designer name can also help to avoid unnecessary “finger-pointing”: if there is an issue with the design, it’s the responsibility of the person indicated by the designer name to fix it. This simple tip can help many team managers keep their sanity.

    Clearly displayed engineer’s name
    Clearly displayed engineer’s name

    Another piece of of-missing critical information is the complete name and address of your company. Many companies only write their name and logo, but think about this: How many companies with the same name as yours exist?

    Mine is called Fermium, and just in the UK, several limited companies with the same or similar name have been registered in the past years. Similarly, there are many companies called Altium, some of which could be Altium subsidiaries or associates, but undoubtedly not all of them.

    Office addresses tend to change less frequently than website domains and telephone numbers, and leave a more extensive paper trail. Who is to say your design won’t have a comeback in 10 years after you’ve changed jobs and the company has been acquired a couple of times?

    Similarly, I recommend adding a company logo to make your design easily identifiable. If you are a freelancer, crafting a logo communicates professionality and reliability.

    Pro tip: You can hold ctrl while dragging a schematic object to temporarily switch to the smaller grid for tasks such as aligning images.

    Altium has several parameters for address and engineer name, such as:

    • Address1 through Address4 for a standard international multiline address
    • ApprovedBy
    • Author
    • CheckedBy
    • CompanyName
    • DrawnBy
    • Engineer
    • Organization

    You can choose which one to adopt depending on the needs of your organization. More documentation can be found here.

    Track the variants

    Murphy’s law: Every potentiometer will rotate in the wrong direction. I fall prey to her more times than not, and for this reason, I always add four 0-ohm resistors around any potentiometers to switch the direction at the assembly stage.

    Resistor network to invert the direction of rotation of a potentiometer
    Resistor network to invert the direction of rotation of a potentiometer

    Similarly, I’m often not sure if my circuit will work with the internal 100/200K ohm pull-ups of the microcontroller, or if it’s going to require an external 10/47K ohm resistor and thus always leave an unpopulated one.

    In a past company I worked for, we used to keep track of these “hypothetical” components by having resistors with part numbers such as “RES_DO_NOT_PLACE”, which were a source of confusion and frustration for our EMS suppliers.

    A much cleaner way is to use variants: place all the components you need to place, then create a variant called “MAIN” with the default configuration. Update the OutJob, so only that variant is exported. You will be able to keep track of the unpopulated components in your Schematic and DraftsMan document with maximum clarity and minimal errors.

    The variant can be displayed in the title block through the parameter “VariantName”.

    More documentation can be found here.

    Keep the text readable at the proper page size

    Academic research in the topic of user interface design has long concluded that it’s good practice to keep the font size around 10 or 12 points, where 12 is readable by the most age groups, and that the bare minimum is around 6 points.

    In our template, we’ll choose only font sizes in that range. By adopting a font size of 12, our A3 schematics are still readable when printed half-size to A4.

    “Confidential” on every page

    Most NDAs (Non-Disclosure Agreements) restrict the concept of confidential information to documents explicitly marked as such.

    Your schematics probably contain some of the most important trade secrets of your business. You should mark them with a big juicy “Confidential” stamp.

    Schematic clearly marked as confidential
    Schematic clearly marked as confidential

    Create and distribute a schematic template with Altium 365

    I have gone ahead and created a title block that matched all the criteria as mentioned earlier.

    The completed schematic title block
    The completed schematic title block

    We can then create a new Schematic template inside of the explorer panel, open it for edit, and copy-paste our title block into it.

    Creating a new schematic template in the cloud
    Creating a new schematic template in the cloud

    The size of the schematic page can be changed in the properties panel when no component or schematic object is selected.

    Changing the page size
    Changing the page size

    Once completed, the Schematic template can be uploaded to Concord Pro on Altium 365 by using “Save to server” or the ctrl+alt+s shortcut.

    Save to server command
    Save to server command

    Create and distribute a unified color palette

    I’m going to sound like an interior designer for a while—maybe it’s my Italian blood. Choose your colors wisely.

    If you’re lucky enough to still wander in the first middle-half of your life, you may be tempted to use a reduced-contrast palette in your drawings, such as blue and light blue. Resist the urge: your older colleagues may already have a decreased contrast sensitivity.

    Your schematics should not encode information in color, and should be printable in monochrome.

    I have personally switched away from the blue/yellow/red/green/black palette of Altium to an almost blue-only or a black-only, with only NetTies and Text Strings having different colours. If you want to choose more than one colour, I recommend choosing red and blue.

    The human eye, for the majority of people, has three different colour-sensitive cones. In the following chart, depicting the sensitivity of the human-eye cones over the visible light spectrum, green and red overlap a lot, which partially explains why red-green is the most common form of colour-blindess.

    Normalized human eye cone response, courtesy of Wikimedia
    Normalized human eye cone response, courtesy of Wikimedia

    Red and blue, on the other hand, are much apart on the spectrum, and are thus considered easily distinguishable by most colourblind folks.

    Some EDA suites lock their styling to aid sales, as it helps to create a coherent brand, but Altium poses no such limit.

    In this example, I’ve created an all-blue style by changing the default schematic objects in the preferences.

    Examples of blue-red schematic objects
    Examples of blue-red schematic objects

    I’ve then created a preference folder in Concord Pro and used “Send to server” under “save” in the preferences.

    Saving and releasing preferences in the cloud
    Saving and releasing preferences in the cloud

    When the preferences are released to the server, you can choose to apply them automatically to every engineer workstation and lock them, apply them when Altium is first installed, or do not apply them at all, leaving every engineer free to pull them as they please.

    More information can be found at the relevant documentation page.

    Distributing a pre-configured project template

    Some of the custom parameters we have adopted in the schematic template—for example, ProjectTitle—should be added at the project-level in every PrjPcb, so they are easier to remember and edit.

    Luckily, just as Altium allows us to use templating for Schematic or PCBs, we can do the same for the project file.

    We should start by creating a new project template from the Explorer panel taking care of selecting “Open for editing after creation”.

    Managed projects folder in Altium Concord Pro on Altium 365
    Managed projects folder in Altium Concord Pro on Altium 365

    We can then edit the parameters in the project settings and add our own.

    Editing the project parameters
    Editing the project parameters

    The project can be edited and sent to the server by using “Save to server” or the ctrl+alt+s shortcut.

    Releasing to the cloud


    Through Altium’s advanced templating capabilities and Concord Pro on Altium 365, we can create and distribute schematic templates, project templates, and settings to our entire organization.

    Adopting a template that references all required information can ease our job as engineers, and shine a bright light on us as freelancers when showing schematics to customers.

    Choosing a different color palette for our schematic objects can make them more intelligible to older and colorblind colleagues.

    Completed schematic with a red-blue palette and custom title block
    Completed schematic with a red-blue palette and custom title block

    You can download a copy of the template we have just created in this GitHub repository: Fermium/AltiumTemplates.

    Whatever template design or colors you choose to make your design shine, if your company has more than one person in it, Altium 365 and Concord Pro can help you distribute and manage coherent templates and settings for every engineer.

    About Author

    About Author

    David Bortolami is electronic engineer with a broad knowledge in PCB and circuit design. Currently, he is the head of Fermium, a small British enterprise that manufactures some of the world's most advanced scientific instruments for teaching and research.

    "Every product can be made twice as good at half the cost; it's a matter of diving deeply into why it should exist - then taking the rest out."

    As an Entrepreneur, David has experience with all the hurdles of manufacturing, integrated electronic-mechanical product design, meeting EMC & Regulatory requirements. In the past, he ran one of the biggest Italian Fablab/Hackerspace and Coworkings and was in charge of PCB Engineering for companies specialised in EMI-heavy industries such as electronic inverters.

    most recent articles

    Back to Home