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

Downloads

Download the latest in PCB design and EDA software

  • PCB DESIGN SOFTWARE
  • Altium Designer

    Complete Environment for Schematic + Layout

  • CircuitStudio

    Entry Level, Professional PCB Design Tool

  • CircuitMaker

    Community Based PCB Design Tool

  • NEXUS

    Agile PCB Design For Teams

  • CLOUD PLATFORM
  • Altium 365

    Connecting PCB Design to the Manufacturing Floor

  • COMPONENT MANAGEMENT
  • Altium Concord Pro

    Complete Solution for Library Management

  • Octopart

    Extensive, Easy-to-Use Component Database

  • PRODUCT EXTENSIONS
  • PDN Analyzer

    Natural and Effortless Power Distribution Network Analysis

  • See All Extensions
  • EMBEDDED
  • TASKING

    World-Renowned Technology for Embedded Systems Development

  • TRAININGS
  • Live Courses

    Learn best practices with instructional training available worldwide

  • On-Demand Courses

    Gain comprehensive knowledge without leaving your home or office

  • ONLINE VIEWER
  • 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

    ALTIUMLIVE

    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

    Downloads

    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

    Creative use of flexible tools

    Colby Siemer
    |  April 12, 2016

    A question came up on the forums today asking how to make a design rule in Altium Designer® to check for silkscreen clearance to the board outline. Knowing that there is no direct method to achieve this, I had to get creative.

    A question came up on the forums today asking how to make a design rule in Altium to check for silkscreen clearance to the board outline.  Knowing that there is no direct method to achieve this, I had to take step back and ask myself if I had the tools required to make this happen, even if there is not a direct feature to support it. 

    This is something that is commonly done, and I imagine many of us have our "bag of tricks" or creative ways of using existing tools to accomplish things that were not likely envisioned when the tool was created.   

    One of the things I have always loved about Altium is that it’s so flexible, and the tools it provides can be used in creative ways to accomplish far more than their intended purpose.  The solution to the problem mentioned here is one example of that. 

    As an Application Engineer working for Altium over the years, I’ve always been thrilled when I see that a feature or tool that I’ve requested added to the software. But even more impressive is that our R&D guys always seem to implement in a way that does not limit it to the function I requested it for. It always gets the job done, but it remains flexible and open to creative ‘manipulation’. 

    Some call it ‘thinking outside the box’, but in this context I like to think of it more as understanding what is actually in your box, and then using it creatively to accomplish a given task in an innovative way. 

    So here’s my solution to the problem of making a rule for silkscreen vs board outline (if your interested you’ll find the original post here).

    1) Use the Design-->Board Shape-->Create Primitives from Board Shape tool

       - Set it to use Route Tool Outline

       - Set it to place on Top Overlay

       - Give it small width you are not likely to use for anything else(I used 0.5mil)

    2) Run this tool a second time if you also want to check the bottom overlay, and simply change it so it adds to the Bottom Overlay instead of the Top, keep everything else the same.

    3) We now have an outline surrounding our board shape for both Top and Bottom Overlays, using widths of 0.5mils, so using the Filter panel, lets find and select all of our 0.5mil items (these should be the only items this thin)

      - Create the filter (Width = AsMils(0.5))

    4) With them all selected, use the Inspector panel to set the Keepout property to TRUE.  This will allow us to use them in this way, but will prevent them from appearing in the Gerber.

    Finally, create a new higher priority design rule for Silk to Silk clearance.

      - First Object = All

      - Second Object = (Width = AsMils(0.5))

      - Set appropriate clearance

    With this new rule in place, and the keepouts set on the silkscreen layers, this will notify you if you place any text too close to this area.  And will not effect your Gerber output since we set the keepout property for these items.

    Even though this is just one example of how this flexibility can be employed, I hope it helps you stop and think about the tools at hand, and sparks some creative thought of your own on how these flexible tools can be employed.

    About Author

    About Author

    Altium expert and seasoned support and services professional with a knack for rapidly learning and distilling abstract technical concepts. Proven troubleshooter and problem solver, with a generous ability to share knowledge and success.

    most recent articles

    Back to Home