Cadsoft’s Eagle is a useful tool that can be used to make schematics and board layouts. This tutorial will cover making a schematic using the pre-defined library parts, and then turning that schematic into a board layout.
To begin with, let’s make a very simple schematic. First, from the Eagle Control Panel, go to file -> new -> schematic. You will be greeted with a screen that looks something like this:
Next, click on the “add” button on the left hand side of the screen. You will be greeted with a large list of libraries. Each library contains many different parts that you can use in your schematics and boards. Eagle comes supplied with many libraries containing many different parts, but it is also handy to know how to add your own parts to the libraries so this will be covered later. For now, click the plus next to the “rcl” library. This library contains basic discrete components – resistors, capacitors, and inductors, in many different packages. Next, let’s add a resistor. Start by clicking on the plus next to “R-US_”. You will see many different resistors listed. As you highlight each resistor, it’s schematic symbol and board footprint will be shown in the right hand corner of your screen:
Select the part called “R-US_0411/12”. This part is a good fit for the quarter watt resistors that are used in many ECE lab classes. Click on OK. Now, you should be carrying around a resistor symbol. Click somewhere, and that symbol will be dropped on the schematic. Drop two more, anywhere you please. Next, click on the add component button again, go back to the the RCL library, and add a C-US025-025x050 from the C-US section to the schematic. Next, let’s search for a component. Click on the add component button, type in *555*, and hit enter. This just did a search for any part that has “555” in its name. You will see this screen:
Add the LM555N from the *555 section of the linear library to your schematic. Next, go back to the add component screen. You’ll notice that your screen still has the last search shown. Clear where it says “*555*” and hit enter, and you should be back to your normal add component screen. Before we start connecting things, add one each of the “+5V” and the “GND” components from the supply 1 library to your schematic, then add a “PINHD-1X2” part from the pinhead library, and then add a “LED5MM” from the LED section of the LED library. Your schematic should look something like this:
Now let’s move things around. Click on the move tool . Now, click on a part, and then move your cursor. The part should follow your cursor around. If you right click, the part will 90 degrees. Now click somewhere else, and the part should be dropped in that place. Move the parts around so that they are in about the same places as shown below. Note that you will need some more copies of the +5V and GND parts. To get these, use the copy tool and click on the part you want duplicated, and you’ll be able to drop another of that part on your schematic.
Now it’s time to connect the parts. Click on the net tool . You can connect two pins of a component by clicking on one lead and then clicking on the other lead. For example, click on the pin sticking out of the top of the GND symbol that is located below and to the left of the LM555N part. You should now have a wire sticking out if it following your cursor around. Click on the pin sticking out of the bottom left corner of the LM555N to connect the two. Connect the rest of the components as shown below. Note that you can route nets by clicking in intermediate places between the two parts that you are connecting. You can also change their shape by right clicking. This will cycle through the various shapes of nets.
Now that the schematic is done, it’s time to make a board. Click on the board button . You will be brought to a screen that looks something like this:
You can see all the parts that we dropped into the schematic in the corner of the screen, and a blank PCB in the middle outlined in white. Just like before, move all the parts onto the PCB. Normally choosing the best place for parts is an iterative process and can take quite a while. However for this tutorial, just place them as shown below:
By now you probably have noticed the lines coming off of many of the pins of the components. The lines are showing connections that exist in the schematic that don't yet exist in the layout. They are only there for your reference and are not part of the layout itself. Let's get rid of those lines! Click on the Route tool: . You'll see a tool bar show up in the top of your screen. Select "16 Bottom" from the leftmost drop down box and put in a width of .032. This means that you will be drawing traces on the bottom of the board that are .032 inches wide. The reason for starting out on the bottom is that if you have this board made at the ECE Electronics shop - it will be much, much easier to solder if all your traces are on the bottom. Now click on the bottom-most pin of the LED. You should now have a blue outlined trace following your cursor. You can change the various possible shapes of the trace by right clicking. You can see your choice of shapes displayed in the Route tool bar next to the layer drop down box. I recommend using the second and fourth of these as PCBs are typically only designed with 45 and 90 degree angled traces. Click on left pin of R2 - and you can now see your trace drawn in. Now connect the rest of the traces, making sure none overlap. One possible connection scheme for them is shown below:
And with that - you have a final board layout! You can follow the instructions on the ECE electronics shop website to make the appropriate files to give to them so that they can mill out your board.