Library design on EAGLE for beginners
When it comes to schematic and PCB design one corner stone is component library design. All good design starts with a good library. And on today’s blog we are going to share a Library design tip for all newcomer EAGLE users. Because the backbone of any electronic project are its components, the 1st step is always to choose the pertinent components for our desired outcome. One common integrated circuit (IC) in analog design is the OpAmp (Operational amplifier), so today we are going to make a library for a TL082 general purpose OpAmp.
Now that we have chosen the component we’ve come to the time where we need to open our library designer on EAGLE. Simple as clicking file -> new -> library on the control panel interface.
Then the library design user interface (UI) will get displayed for us to start. To start with we must identify the 4 main sections of the UI:
Device: Is the component's final step for its creation. On this column we’ll join both the symbol and the footprint
Footprint: It is the size, shape, and separation of pads where there will be exposed copper for the IC’s terminals to sit on. A footprint can be both through hole (TH) or surface mount (SM) depending on the chosen IC
3D package: An attached model to the IC component that allows the user to export the design as a 3D render
Symbol: A flat 2D representation of the component used in the schematic
Where to start? Although you could start anywhere it is suggested to start by creating the symbol for your component.
The easiest and fastest way to create the symbol is by making a box, or bank, symbol which is composed by a box with all the pins laid out on the sides.
Simple enough but all symbols must contain the following information:
Reference designator (Designador de referencia, >tname on EAGLE)
Pin logic (Lógica de pin)
Pin name (Suggested for box design)
Pin count (Número de pin)
Value (>tvalue on EAGLE)
Graphic representation of the symbol for an inverting Schmitt trigger.
Pin functionality and pin logic are a bit tricky to tackle because it dwells on information regarding the IC’s datasheet. On today’s blog we’re only going to reference Pin functionality. The functionality derives from how a pin interacts when it’s connected to any other component. It could be an input, an output, a power pin, etc. In our case the TL082 has all the 3 functions mentioned before. It has 4 inputs, 2 outputs and 2 power pins that energize the component.
Abstract overview of the pin functionality of the TL082 integrated circuit.
To add a function to a pin we could right click and go to properties and modify the function attribute, but we could also do it by clicking the pin which will open the design manager on the left side. The design manager lays out all the pin’s attributes such as name, function, logic, length. Let’s start with pin 1’s attributes: Pin functions as an output and the pin’s name is OUTA. And repeat the same for the other 7 pins:
Pin 2 (INA-): Input
Pin 3 (INA+): Input
Pin 4 (V-): Power
Pin 5 (INB+): Input
Pin 6 (INB-): Input
Pin 7 (OUTB): Output
Pin 8 (V+): Power
After laying out all our pins we must add the reference designator and value of the IC. Using the text icon of the palette we can create both. In the case of the reference designator, we write down “>tName” and change the layer to tName on the upper right corner. And for value, we write down “>tValue” and change the layer to tValue.
And with that we’ve finished our symbol. Now we follow up with the footprint. Normally we would need to create the footprint’s pad by hand and lay them out as shown on the datasheet but EAGLE has a cheat sheet for newcomers. The tool we’re going to use will take 2 birds with 1 stone. We’ll create the component’s 3D model and the footprint at the same time.
We click on add a 3D model and then choose to create a new 3D package, this will open up a component design interface.
To start we must check on our datasheet the type of component we’re creating, in this case we’re making a SOIC integrated circuit, so we slide down the component creation list and choose SOIC. It is important to note that this list doesn’t include all component types, but it does contain the more common.
From here on it is smooth sailing, using the reference image of the component on the UI we can fill out the sizes checking our datasheet’s reference. NOTE: Always double check you’ve added the correct sizes and you’re filling out the correct space.
Afterward just click finish and like that you have both the footprint and the 3D model. It is important to denote that this tool creates the component’s pads with predefined values. Sometimes you’d need to still tweak the sizes directly on the footprint to comply with your manufacturer’s needs or if you need to comply with an international standard.
Now we are at the end of our journey, the last step is to combine all we have done into one single device. Click on add device and create a new device. Afterwards you’ll be greeted with a UI similar to the symbol creation UI.
Using the add symbol button in the palette add to the device the symbol you created for the library, try to keep in the center. Then add the footprint using the local model button, click and add the model you’ve designed. And lastly, connect each pin of the symbol to its corresponding pad using the Datasheet for reference. Save your library.
And with that you have created your first library!
If you are interested in learning more about electronical design, contact us for more information about our new course!