{"id":700,"date":"2017-04-05T08:00:46","date_gmt":"2017-04-05T15:00:46","guid":{"rendered":"http:\/\/www.autodesk.com\/products\/eagle\/blog\/?p=700"},"modified":"2023-09-26T13:30:12","modified_gmt":"2023-09-26T20:30:12","slug":"library-basics-part-2-creating-first-symbol-autodesk-eagle","status":"publish","type":"post","link":"https:\/\/www.autodesk.com\/products\/fusion-360\/blog\/library-basics-part-2-creating-first-symbol-autodesk-eagle\/","title":{"rendered":"Library Basics Part 2: Creating Your First Symbol in Autodesk EAGLE"},"content":{"rendered":"

Library Basics Part 2: Creating Your First Symbol in Autodesk EAGLE<\/span><\/h1>\n

Welcome back to the Library Basics Series, Pirates! In Part 1<\/a> you got your hands dirty creating your very first package in Autodesk EAGLE. Now, it\u2019s time to continue on your journey by learning how to build your first symbol. Regardless of what kind of design you\u2019re creating, it all begins with symbols and schematics. You can think of these symbols as the map to the chest of schematic treasure! Symbols show off all the functionality of your design without having to get into the nitty gritty of physical dimensions and packages.<\/span><\/p>\n

Let\u2019s begin!<\/span><\/p>\n

Prep Step – Remember the Datasheet<\/h2>\n

Before we set sail, you’ll need to gather your datasheet! In our example, we\u2019ll be making a symbol for a MOSFET switch from Texas Instruments. Feel free to follow along with the <\/span>TPS92411 datasheet<\/span><\/a>.<\/span><\/p>\n

Within most quality datasheets you\u2019ll find both a table and drawing that gives a summary of all the pins and their intended functions for a device. This summary is important when it comes to making your symbol, as it tells you exactly what pins you need and what their labels are without having to guess. Lucky for us Texas Instruments makes some impressive datasheets, and if you look on page 3 you\u2019ll see the <\/span>Pin Configuration and Functions <\/b>heading. We\u2019ll be using the SOT23-5 package type, which requires 5 pins, including:<\/span><\/p>\n

    \n
  1. RSET<\/b> – This pin serves as the reset of the device, allowing the switch to open. <\/span><\/li>\n
  2. VS<\/b> – This pin serves as the internal switch and the device\u2019s floating ground. <\/span><\/li>\n
  3. VIN<\/b> – This pin serves as the positive supply for our device. <\/span><\/li>\n
  4. DRAIN<\/b> – As its name suggests, this pin serves as the drain for our device. <\/span><\/li>\n
  5. RSNS<\/b> – This pin senses the VS voltage relative to our system\u2019s ground. <\/span><\/li>\n<\/ol>\n

    This is all the information you need to get started with your symbol.<\/span><\/p>\n

    \"tps92411-datasheet\"

    If only every datasheet was this easy to read! All the pins for our TSP92411 symbol.<\/em><\/p><\/div>\n

    Step 1 – Creating Your First Symbol<\/h2>\n

    If you haven\u2019t already done so, go ahead and open your library from the EAGLE <\/span>Control Panel<\/b>. You can do this by right-clicking on the name of your library and selecting <\/span>Open. <\/b>This will open the <\/span>Library Window<\/b>, which provides a summary of all the devices, packages and symbols in your personal library. To add a new symbol to your library:<\/span><\/p>\n

      \n
    1. Select the <\/span>Symbol \"open-symbol-icon\"\u00a0<\/b>icon at the top of your interface to open the <\/span>Edit Dialog<\/b>. <\/span><\/li>\n
    2. Next, enter a name for your symbol in the <\/span>New: <\/b>field and select <\/span>OK. <\/b>In our example, we\u2019ll give our symbol a name of \u201cTPS94211.\u201d<\/span><\/li>\n
    3. A warning dialog will open, select OK <\/b>to confirm that you want to create the new symbol name.<\/span><\/li>\n<\/ol>\n
      \"new-symbol-name\"

      Adding the name for our first Autodesk EAGLE symbol – TPS92411 from TI.<\/em><\/p><\/div>\n

      Now that you have a new symbol added to your library you\u2019ll be greeted with the <\/span>Symbol Editor<\/b> window.<\/span><\/p>\n

      Step 2 – Adding Pins to Your Symbol<\/h2>\n

      Let\u2019s insert some pins to your symbol. Based on the datasheet, we need 5 pins in total, 3 on the left and 2 on the right. Here\u2019s how to add them:<\/span><\/p>\n

        \n
      1. Select the <\/span>Pin\u00a0\"pin-icon\"\u00a0<\/b>icon on the left-hand side of your interface.<\/span><\/li>\n
      2. Left-click in your <\/span>Symbol Editor <\/b>workspace to place your first pin.<\/span><\/li>\n
      3. Go ahead and repeat this process for the remaining pins on your symbol. To place the 2 pins on the right, <\/span>right-click<\/b> twice to rotate your pin 180\u00b0 and then <\/span>left-click<\/b> to place. <\/span><\/li>\n<\/ol>\n

        We\u2019ve left a gap between ours for easier readability as shown in the image below. But those pin names aren\u2019t right; we will change those now.<\/span><\/p>\n

        \"schematic-pins\"<\/p>\n

        Step 3 – Changing Your Pin Names<\/h2>\n

        You probably noticed that Autodesk EAGLE names all of your pin names by default as you place them. But we need to change these to match what it shows on our datasheet. To do this:<\/span><\/p>\n

          \n
        1. Select the <\/span>Name \"name-icon\"\u00a0<\/b>icon on the left-hand side of your interface.<\/span><\/li>\n
        2. Select the first pin you placed, and the <\/span>Name <\/b>dialog will open. <\/span><\/li>\n
        3. Enter \u201c<\/span>RSET<\/span><\/i>\u201d in the <\/span>New Name:<\/b> field and select <\/span>OK<\/b>. <\/span><\/li>\n<\/ol>\n

          One down, four to go. Change all of your pin names to:<\/p>\n