Tutorial 3: Self-Defined Libraries

(Selected materials from autodesk.com)

In Autodesk EAGLE, all of the parts that you place on your designs are stored in libraries. These provide an easy way to keep parts organized based on their category. For example, you might have a library for a general category like capacitors. Or specific communities like Sparkfun have their own dedicated libraries that contain a variety of parts for specific projects. Libraries and the parts within are connected in a simple hierarchy in Autodesk EAGLE. This makes it easy to understand how everything’s connected. Here’s how it’s organized:

-Libraries.
All of your parts will be stored in your personal library folder in Autodesk EAGLE. Each part will contain a device, symbol, and package.

-Devices.
Within every library, you’ll have one or multiple devices. These devices include both a schematic symbol and a package in one accessible location.

-Symbols.
Within every device, you’ll have a symbol, which provides a visual representation of a part for use on a schematic.

-Packages.
Within every device, you’ll also have a package, which is the physical representation of a part for use in a PCB layout.

When you put all of these pieces together, you’ll get a tree structure that shows off how libraries in Autodesk EAGLE are organized. Check it out below.



Creating Your Library

Now that you understand how libraries work in Autodesk EAGLE, it’s time to make your own! You can skip this step if you already have your personal library folder, otherwise:

-Open Autodesk EAGLE, and you’ll be greeted with the Control Panel.

-Next, select File New Library to open your Library Window.

-Before creating any new parts, you need to save your library by selecting File Save (or Cmd + S on Mac and Ctrl + S on Windows)

-Now that your library is saved, you just need to activate it. Go back to your Control Panel, right-click your new library, and select Use. You’ll know if your library is ready to go if it has a green dot next to it in your Control Panel.



The .lbr file will be the library file that contains Devices. Every device is a combination of a 'symbol' and a 'package'. A symbol can have many packages (layouts) since the same symbol can be used to represent many types of layouts like SMT or DIP. However, every package usually only has one symbol to represent it in the schematic. Keep in mind that, the schematic is just a symbol to represent the role of an electrical component in a circuit, it does not have to changed all the time unless necessary.

You can put your .lbr file  (includes devices, symbols, and packages) into different folders. You can even have subfolders for these folders to host your .lbr files.

I created a folder called YL in the 'Libraries' menu. After I had my library window pops up, I saved it to my 'YL' folder, and I named it as 'crazyCar.lbr'.


Library Basics Part 1: Creating Your First Package

Packages serve a super important purpose when used on your PCB layout, offering a set of pads that provide both electrical connectivity and a way to solder parts onto your board. As you can imagine, making sure these pads are placed exactly where they need to be is a necessary challenge; otherwise, you’ll get a board back from manufacturing that doesn’t work! Check out the image below of the package you’ll be creating today. Here are all of the elements that you will start to work with:



1. Pads. The pads are the red rectangles on this part and are numbered according to your datasheet. When placed on a PCB, each of these pads will be connected to a trace and provide electrical connectivity for a part.

2. Package Dimension. The package dimension is the rectangular gray outline that you see connecting all of the pads. This outline represents the actual physical dimensions of your part can help during your PCB layout process to see if you’re placing components too close together.

3. Silkscreen Outline. The silkscreen outline is the rectangular yellow lines lying over the gray package dimension lines. While this piece is optional, it helps to provide a visual indicator for your manufacturer when they are assembling parts on your bare board.

4. Name and Value. These text elements are placeholders and will come in handy during your PCB layout stage. As the text suggests, Name will be used to identify the unique name of your part when you place it on your PCB layout, and Value can be utilized for things like labeling the resistance of a resistor, capacitance of a capacitor, etc…

Step 1 – Creating Your New Package

Alright, time to get rolling with the tutorial part of this guide. The very first step you need to complete is creating a new package in your library. Here’s how: Open Autodesk EAGLE, and you’ll be greeted with the Control Panel. Select the Arrow icon to expand the main Libraries and lbr folders, then right-click your personal library and select Open. This will open your Library Window. From here, choose the Package package-icon icon to open the Edit Dialog. Next, enter a name for your package in the New field and select OK. If you’re following our example, then enter “MC14049UB_DIP.” Select Yes to confirm you want to create the new package.

Let's start with the 'package'. Double click the crazyCar.lbr in the control panel to open the library window. Single left click the 'package' button, copy and paste the name '
MC14049UB_DIP' in the Edit window.



Great, so with that complete you now have your first very package added to your personal library and a blank Package Editor should be open as shown below.



Step 2 – Changing Your Grid Size

Now’s the time to tweak some basic grid settings before you start placing any pads. Changing the grid size will allow you to quickly and precisely place pads according to your datasheet measurements.

-Select the Grid grid-icon icon in the top-left corner of your interface.

-In the Grid dialog, change your Display from Off to On if it isn’t already enabled.

-Next, change your Size: from inch to mm, and enter “0.5” as the value, use '0.05' for Alt. 

-Select OK to save your grid settings.



The 'Alt' function is really nice. If you setup the main grid to be 0.5 mm, sometimes it is anoying since you cannot make small movements with the components. The Alt grid is the secondary grid which only start working when you press the 'Alt' key on the keyboard when you are moving the components.

After confirming your settings, you might notice that you can’t see your grid in the package editor. It’s not gone! You just need to zoom in a bit with the Zoom in zoom-in-icon icon until it becomes visible again.

Step 3 – Deciphering Your Datasheet

Alright, time for some datasheet detective work. Open your MC14049UB_D.PDF datasheet and head on down to the Land Pattern Data section on page 25. This page will give you all the information you need to precisely place your pads. Here’s what you need:

Through-holes: The unit of the value beside the Dimension/Scale bar is mm (mili meter). Check the unit and scale of the grid on the left top part of the window (0.05 mm here). The green ring sybmol highlighted on the left is the through-hole. The current diameter of the through-hole is 1.05 mm.





Looking at our datasheet in page 5. Refer to the dimension entry 'D'. The width of the pin is 0.53 mm, but we usually set the diameter of the hole to be 1 mm in this case to make sure the pin can be inserted into the hole. Right click the center of the through-hole, select 'properties', set the coordinate of the ring to be '0, 0', and the drill to be 1 mm, the diameter to be 2 mm.



Now, we need 2x8 of these through-holes for the 16 pins of the chip. The distance between each two pins on the same side is the dimension of 'G' (2.54 mm, let's use 2.6 mm). The distance of the two pins across the chip is the dimension of 'L' (7.74 mm, let's use 7.8 mm).

 

Copy the first ring and paste it beside it. Right click the second ring and set the coordinate at 2.6, 0, so the distance is set to 2.6 mm.



Repeat this until you have 16 evenly distributed rings (through-holes).

This will tell the PCB manufacturer to drill 16 holes using your defined layout onto the PCB board.

Step 4 – Adding Your Origin Point

You’ll need to add an origin point to Pad 1 so that your manufacturer knows the correct way to orient your part during assembly. Here’s how to do this:
-Select the circle icon on the left-hand side of your interface.
-Select the width: dropdown at the top of your interface and select 0.
-Select the layer dropdown at the top of your interface and select layer 21 tPlace.
-Left-click in the bottom-left corner of Pad 1 and drag your cursor to the right to adjust the size of your circle.
-Left-click again to confirm the size of your circle and place it.

The size of your origin point is totally up to you. All that’s important is that it’s on Pin 1 so your manufacturer knows how to orient your part. If you need to move your origin point, use the Move move-icon tool.

Step 5 – Adding Your Package Dimension

You now need to add a package dimension, which will help you to see if your parts are placed too close together on your PCB layout. This process again requires some brief datasheet detective work. The dimensions are 'A' and 'B', which is about 19.6 mm, and 6.9 mm.

   

-Select the Line wire-icon icon on the left-hand side of your interface.
-Select the Layer dropdown at the top of your interface and choose layer 51 tDocu.

The final result looks like this:


Step 6 – Adding Your Silkscreen Outline

Now you just need to add a silkscreen outline, which is a helpful way to tell your manufacturer where your part will be placed. Here’s how to do it: Select the wire-icon on the left-hand side of your interface. Select the Layer dropdown at the top of your interface and choose layer 21 tPlace. You now need to draw silkscreen wires on top of your package dimensions.

The silkscreen and the dimension layer have the same color. To make sure your silker screen layer is done, go to 'View - Layer Settings', to uncheck the 'eye' in front of 'tDocu' to make the 'tDocu' layer invisible. If you are still able to see the rectangular shape like I have below, you know that the silker screen layer is ok.


Step 7 – Adding Your Name and Value Placeholders

Alright, time to finish this up! The last thing you need to add is both a name and value placeholder to your package. This will allow EAGLE to create a unique identifier for each and every part on your PCB layout, making it easy to reference specific parts if you need to make changes down the road. Let’s do it:

-Select the Text text-icon icon on the left-hand side of your interface.
-In the Text Dialog, enter “>NAME” in the Enter text: field and select OK.
-Next, select the Layers dropdown at the top of your interface and choose layer 25 tNames.

You’ll know that you put your >NAME text on the right layer if it displays in a gray colored font. Go ahead and repeat the steps above, this substituting >NAME for >VALUE on layer 27 tValues and place it on the bottom of your package. Here’s how your completed package should look:



At last, you’re done! This is how your completed package should look with its new name and value placeholders.

Library Basics Part 2: Creating Your First Symbol

Now, it’s time to continue on your journey by learning how to build your first symbol. Regardless of what kind of design you’re 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.

Find the Pin configuration of the chip from the datasheet:


Step 1 – Creating Your First Symbol

If you haven’t already done so, go ahead and open your library from the EAGLE Control Panel. You can do this by right-clicking on the name of your library and selecting Open. This will open the Library Window, which provides a summary of all the devices, packages and symbols in your personal library. To add a new symbol to your library:
-Select the Symbol open-symbol-icon icon at the top of your interface to open the Edit Dialog.
-Next, enter a name for your symbol in the New: field and select OK. In our example, we’ll give our symbol a name of “
MC14049UB_DIP
-A warning dialog will open, select OK to confirm that you want to create the new symbol name.



Close the Package edit window, and reopen the library edit window from the control panel as above. Click the 'Symbol' button in the menu.

We name the symbol '
MC14049UB' instead of 'MC14049UB_DIP' here as the package since the same sybmol may have different packages. If the other package is an SMT layout, then you may want to name it as 'MC14049UB_SMT'. But they both can share the same symbol, which is 'MC14049UB'.


Zoom out the window, you can see the origin cross:


Step 2 – Adding Pins to Your Symbol

Let’s insert some pins to your symbol.
-Select the Pin pin-icon icon on the left-hand side of your interface.
-Left-click in your Symbol Editor workspace to place your first pin.
-Go ahead and repeat this process for the remaining pins on your symbol. To place the 2 pins on the right, right-click twice to rotate your pin 180 and then left-click to place.

We’ve left a gap between ours for easier readability as shown in the image below. But those pin names aren’t right; we will change those now.



Try the best to make the origin cross in the middle of your symbol. I circled the origin in the snipshot above.

Step 3 – Changing Your Pin Names

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:
-Select the Name name-icon icon on the left-hand side of your interface.
-Select the first pin you placed, and the Name dialog will open.
-Enter “VDD” in the New Name: field and select OK.

 
   

Please note that, NC1 and NC2 are both the NC pin on the chip. This pin will not be used, or 'No Connection'. Eagle does not allwo you to have two pins using the same name. This is why I name them diffrently.

Step 4 – Adding Your Symbol Outline

To complete the visual of your symbol, you’ll now need to add an outline to group all of your pins together. Here’s how to accomplish this:
-Select the Line wire-icon icon on the left-hand side of your interface.
-Next, left-click on a starting point to begin drawing your outline.
-Continue to drag and left-click as needed to complete each side of your outline to draw a full box.



Use the 'T' button to add Text '>Name' and 'Value' to the sybmol.



Library Basics Part 3: Creating Your First Device in Autodesk EAGLE

In this guide, we’ll be pulling together everything you learned about creating a package in Library Basics Part 1 and creating a symbol in Library Basics Part 2. Now, it’s time to create your very own device. You’ll be able to do the PCB design with a brand new part.

Step 1 – Creating Your New Device

Creating a new device follows a familiar set of steps that you should be used to by now after creating a package and symbol. Close the Symbol edit window, enter the library windwo again from the control panel.


Click the 'Device' button, name it as '
MC14049UB_DIP'.



Step 2 – Adding Your Symbol and Package

Add the symbol:


Adding Your Package:
Select the New button on the bottom-right corner of your Device Editor.


Select OK, and your package will automatically be placed on the right panel of your Device Editor.



Looks exciting!! Now, let's connect the symbol to the physical layout (package). After click 'Connect', the window as follows will pop up to let you match the corresponding pins in the symbol and in the layout. Pin 1 is VDD, so I select these two in the two windows, and then click connect.





Add some descriptions. We did not make the description very professional since our project is simple.


Don't forget to save it before you close it:



Also, don't forget to have Turn ON your library:



Now, you can directly use your parts in both the Schematic view and the Layout View to complete your circuit.

Use the same mathod to design the library (Device, Symbol, and Package) for the Motor Driver L293D.

The schematic of the Obstacle Avoider is:


All the other components are 'Two Terminal' components, which are easy. You can build the libraries for them as well. Or probably just make one package, and call it 'Two_Termi', and then design different symbols to connect them to this package to make different devices.