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

    Design Rules to Fanout a Large BGA

    Altium Designer
    |  January 11, 2019

    Screenshot of 3D fanout routing in fanout a large BGA

    I have known people during my career who insisted on hand-routing every PCB design that they worked on. They would say that their manual routing performed better, looked better, and was just better in general. I’m not going to argue one way or the other on that, but I will say that there is one thing that can not be argued with; all of that manual routing took them a much longer time to complete then if they had used automated routers. With today’s higher density routing being packed into reduced design schedules, PCB layout engineers need help in speeding up the routing process.

    Fortunately, CAD tools like Altium Designer® have the automated trace routing features that PCB designers need today to stay ahead of their schedules. One such feature is the ability to set up the design rules to fanout a large BGA. Altium Designer provides a lot of options in the design rules so that you can get great results from the fanout utility. Take a look here at how these tools can help you save time on your routing by automatically fanning out a BGA.

     

    Get Your Design Set Up for Fanning Out the BGA

    Fanning out a BGA will often require adjustments to your design rules for smaller trace widths and spacing as well as vias. Altium Designer provides for this by giving you the ability to set up “rooms”. These rooms will allow you to apply different design rules to that specific area of routing, which in many cases is exactly what you need for your BGA fan out.

    Screenshot of the BGA to be routed in fanout a large BGA

    Here’s the BGA that we will create the fanout routing for.

    In the picture above you can see the BGA that we will be working with. You will want to make sure that your design has enough layers to accommodate the fan out traces, and in this design, we have plenty to work with. The larger the BGA, the more layers it will take for the fan out utility to do its job, although for demonstration purposes we are using a smaller BGA.

    To create a room for the BGA specific design rules, you will go to the “Designs > Rooms” menu selection. There are many ways to create rooms, and in our case, we have pre-selected the BGA part on our board, and then selected “Create Rectangle Room from selected components” from the menu. This will create a room perfectly around our selected BGA as you can see in the picture below.

     Screenshot of AD19 rooms menu in fanout a large BGA

    The Rooms menu in Altium Designer 19

     

    Set Up the Design Rules to Fanout a Large BGA

    Once the room has been created, it is time to start working with the design rules. Open up the design rules by going to the “Design > Rules” menu selection. On the left side of the PCB Rules and Constraints Editor menu, go down to the “Placement” rules and click on the arrow to open up these rules. In the “Room Definition” category you will see the new rule for the room that you just created; it will have the name of “RoomDefinition”.

    Screenshot of AD19 room rules in fanout a large BGA

    Setting the design rules for the BGA room

    In the picture above you can see the rules for the room definition category, and the changes we made to the rule. You will need to change the rule name to something more descriptive, and in our case, we have chosen “BGA_Fanout”. Make sure that the settings for object matching are set the way the picture shows, and apply these rules to save them.

    Next, you will need to create a special clearance setting for the BGA_Fanout room. To do this you will remain in the design rules menu, and go up to the top of the menu on the left side to the “Electrical > Clearance” category. Right click on this category and create a new rule giving it the name of “Clearance_BGA_Fanout” in its dialog box. You will also want to adjust the clearances to a value of 0.1 MM as shown in the picture below.

    Screenshot of AD19 clearance rules in fanout a large BGA

    Setting a clearance rule for the BGA room

    To associate this clearance rule with the room that we’ve created around the BGA, we will specify a custom query as our object match. To do this click on the drop-down button under “Where The First Object Matches”, and select “Custom Query.”  In the text box that pops up, start typing the word “WithinRoom.” Before you finish you will see an option for “WithinRoom” pop up. Select this option and immediately another option for the room that you want to select will pop up, which in our case is the room “BGA_Fanout”. Once you select the room that you want the new rule dialog will be complete as shown in the picture above, and you can click on “Apply” to save it.

    Next, we will need a new rule for a smaller trace width in the BGA_Fanout room. Create a new routing width rule and name it “Width_BGA_Fanout.” Follow the same procedures to set up its object matching and specify a routing width of 0.1 MM for all widths as shown in the picture below. When you are finished, click “Apply” again to save this rule.

    Screenshot of AD19 width rules in fanout a large BGA

    Setting a width rule for the BGA room

    We will also need a new via for the BGA fan out. Create a new “Routing Via Style” rule with a diameter of .4MM and a hole size of .2MM. As with the clearance and width rules, you will follow the same procedure to associate this rule with the “BGA_Fanout” room as shown below.

    Screenshot of AD19 via rules in fanout a large BGA

    Setting a via rule for the BGA room

    The last design rule that we will want to work with is the Fanout Control rule. This rule includes different rules for fanning out different component styles such as SOIC’s, LCC’s, and BGA’s. In our case, we will want to verify the settings in the BGA fanout rule specifically.

    As you can see in the picture below, this rule already has a custom query set up to match a BGA object. Check that the “Fanout Style” is set to “BGA.” There are other settings in there such as “Auto” and “Inline Rows,” but for our purposes we want it to use the BGA style. The other rules should be set up as shown. Once you have verified that this and the rest of the rules are all set up correctly, you can click “OK” to close the PCB Rules and Constraints Editor.

    Screenshot of AD19 fanout rules in fanout a large BGA 

    Setting the fanout control rules in Altium Designer 19

     

    Once Your Rules Are Ready, Push the Button

    It’s time to press the button and route this fan out. There are different ways to accomplish this, and in our case, we will use the “Route” menu. Select “Fanout > Component” from the route pulldown menu, and the “Fanout Options” sub-menu will pop up. Enable the “Fanout Pads Without Nets” and “Include escape routes after fanout completion” options as shown below, and click OK.

    Screenshot of AD19 fanout options in fanout a large BGA

    The fanout options

    You will now have a green arrow pop up on your cursor to select the BGA for fanning out. When you click on the BGA, Altium Designer may pop up a “Component Selection” sub-menu. In that case, enter the reference designator of the BGA and click OK. Give it a few moments, and the fanout routing will be done. Results will obviously vary depending on what BGA is being routed, how many layers you are working with, and the connectivity, but here is a picture of what our fan out looked like.

    Screenshot of final fanout routing in fanout a large BGA

    The BGA after fanning out the traces and vias in Altium Designer 19

    To get the job done on time or even ahead of schedule, PCB designers need all the help that they can get. Thankfully Altium Designer is PCB Design Software that is full of helpful tools and utilities like the fan out router. These powerful features can make the difference when you are up against a deadline.

    Would you like to find out more about how Altium can help you with your next PCB layout’s fanout routing and other time-saving enhancements? 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