Downloading, Installing and Starting Eagle

Eagle is an electronics layout and design software that is very comprehensive as well as free (with minor restrictions). It is produced by CadSoft and is available for download at www.cadsoft.de . Just look for the freeware download version on the site for the latest release.

The only limitations to the freeware version are the board size, the number of signal layers, and the number of schematic sheets. The maximum board size in the freeware version is 100mm X 80mm, or about 4” X 3.2”. The freeware version only allows the creation of two signal layers, the top and the bottom and it can create only one schematic sheet per project. For most projects, those restrictions are well within the requirements of the inventor. Also, before you can use the software to produce a product for sale, you must purchase the license for the lite version. The cost is minimal at $49. If you require additional signal layers, board size, or schematic sheets, the software has two upgrade versions available for $199 and $399. You can check their site for the features offered with each upgraded version.

Choose your correct language and operating system for the software download. My language is English and I am using Windows XP ^TM . The download I chose was labeled eagle-win-eng-4.15.exe. The file name will change as new revisions are released, but you get the idea.

When it is installed, launch Eagle and a registration screen will appear. Unless you have purchased a license, click the 'Run as Freeware' button.

Figure 14.1

The next screen that appears will be the main control panel. Start by clicking File, New, then Project.

Figure 14.2

A new subdirectory named New_Project_1 will be created and highlighted. You can rename the project to whatever you wish. I will name mine Atmegaproject1. When you have decided on a name or are satisfied with the default name, right click on the project, go to 'New' and click on 'Schematic.'

Figure 14.3

Creating a Schematic

The schematic editor window will open. The default name of the schematic is 'untitled.sch' and is stored under the project folder you just created. I will start by doing a 'Save As' and naming the schematic file Atmegaproject1.sch.

Figure 14.4

Let's start by inserting our main component on the schematic, the Atmega16. Click on Library then Use.

Figure 14.5

A window opens displaying all of the library files currently available to the editor. For the Atmega chip, we will select the atmel.lbr by double clicking the file. The window will immediately close and you will again see the schematic page. Selecting a library file loads all of the devices within the file for you to use while reducing the number of components to sort through by not loading any of the library files you do not select. Sometimes you may have to look through several files before determining where the components you want are located.

When the file is loaded, click the add button.

Figure 14.6

A list of the loaded parts is displayed. Click the plus symbol next to atmel and go down to the Atmega161. Click the plus sign next to the Atmega 161 and choose th TQFP Atmega161A option. While we are using the Atmega16, not the 161, the pin layout is the same for the TQFP design as far as the pins we will be using.

Figure 14.7

Click OK and the screen will disappear and you will be moving a schematic representation of the microcontroller around the schematic page. Wherever you click, a microcontroller will be pasted. If you click too many times, just delete the extra components by selecting the delete icon and clicking on the undesired components.

Figure 14.8

Perform the same operation to add the four switches. The switch I used is located in 'switch-misc', DT, DT6. The placement on the schematic is at your discretion. The schematic does not need to look like the final board. In fact, laying out your components in a logical order in the schematic drawing will help you follow your circuit.

Figure 14.9

Now add the LEDs, resistors, capacitors, and the voltage regulator. Also, you will need to add holes to solder the positive and negative inputs to the board. The component locations in the libraries are listed below.

LED 'led', 'LED', 'LEDCHIPLED_1206'

Resistors 'rcl', 'R-US_', 'R-US_R0805

Capacitors 'rcl', 'C-US_', 'C-USC0805'

Voltage Regulator 'linear', '78*', '7805DT'

Hole connectors 'solpad', 'LSP10'

You should have all of the necessary components on the board at this time.

Figure 14.10

Controlling Components

Rename the components using the Name tool button and the component values, such as the resistor's values, using the Value tool button.

Figure 14.11

You can rotate the components and arrange them in a logical fashion using the Rotate tool button and the Move tool button. This is how my arrangement looks.

Figure 14.12

The component names and values are listed in the following table.

Component	Name	Value
S1	NO CHANGE	NO CHANGE
S2	NO CHANGE	NO CHANGE
S3	NO CHANGE	NO CHANGE
S4	NO CHANGE	NO CHANGE
R1	NO CHANGE	1.5K
R2	NO CHANGE	1.5K
R3	NO CHANGE	1.5K
R4	NO CHANGE	1.5K
R5	NO CHANGE	360
R6	NO CHANGE	360
LED1	NO CHANGE	NO CHANGE
LED2	NO CHANGE	NO CHANGE
U1	NO CHANGE	ATMEGA16
U2	NO CHANGE	NO CHANGE
C1	NO CHANGE	0.01
C2	NO CHANGE	0.01
THROUGH HOLE CONN1	POS	NO CHANGE
THROUGH HOLE CONN2	NEG	NO CHANGE

Figure 14.13

Circuit Traces

We will use the Wire tool button to connect the components. There is also a bus function for adding a bus line, but it is unnecessary for this project as it is simple enough to interconnect without using a bus.

Click the Wire tool button and start by connecting POS to C1, then C1 to pin 1 of U2. After the trace is complete, press the ESC key to start a new trace.

Figure 14.14

Connect the next traces as follows.

U2 pin 2, C2

C2, Atmega16 pin VCC

NEG, C1

C1, U2 pin 3

U2 pin 3, C2

C2, Atmega16 pin GND

Here is what the circuit should look like at this point.

Figure 14.15

Connect the switches to the Atmega with the following trace orders.

Atmega16 pin 42, R1

R1, S1 pin 3

Atmega16 pin 43, R2

R2, S2 pin 3

Atmega16 pin 44, R3

R3, S3 pin 3

Atmega16 pin 1, R4

R4, S4 pin 3

Figure 14.16

Connect the LED's and then the switches to ground and LED's to positive voltage.

Atmega16 pin 40, R5

R5, LED1

Atmega16 pin 41, R6

R6, LED2

S1 pin 1, NEG

S2 pin 1, NEG trace

S3 pin 1, NEG trace

S4 pin 1, NEG trace

LED1, C2 pos term

LED2, C2 pos term trace

After making the connections and terminating some of the traces to other traces (to keep from having to make several traces to the same location of GND and VCC) you need to add a junction to each location the traces were connected by clicking the Junction tool button and adding a junction on top of the connecting point of each of the junctions as shown in figure 14.17.

Figure 14.17

Make sure you save your work regularly in case you lose power or your system locks up. In the next section we will cover creating the circuit board layout.