ECE101 – Basic Electrical and Computer Engineering

Seven Segment LED – Schematic

With the most basic pieces of the software covered, you should feel comfortable with the idea of doing a simple project. I’ll only be using parts from the libraries supplied with EAGLE in order to keep the focus on the schematic and board themselves, though we will cover creating custom parts and libraries in the near future.

In this example, we’ll be designing a seven segment led display controlled by four DIP switches. While this isn’t something that you would likely ever need to build, it is a useful exercise to learn the basic features of the software. Below are the icons and descriptions for the tools that will be used in this example.

Toolbar Buttons

Add – adds components to the schematic

Autoroute – attempts to route all incomplete connections (airwires) on the board

Board (Schematic) – switches from the schematic to the board (and vice versa)

Copy – copies components (and applicable values) already placed on the schematic

DRC – performs a design rule check on your board (I’ll cover this with creating gerber files)

ERC – performs an electrical rule check (more on this later)

Errors – lists the errors found by the DRC and ERC

Group – allows multiple components to be selected

Invoke – allows adding normally implicit pins to the schematic

Mirror – flips components

Move – moves components

Net – creates an electrical connection between two pins on the schematic

Ratsnest – cleans up the airwires showing connections that still need to be made on the board

Ripup – removes already routed traces from the board

Rotate – rotates components

Route – routes traces on the board (only used on airwires)

Value – changes the value of a component (such as a resistor)

Wire – routes traces on the board without being restricted to airwires

Once you know the project requirements, you should figure out what parts you need to fulfill those requirements. For this project, we’ll use the following parts:

Qty	Description	Part	Purpose
1	Common Cathode 7 Segment LED Display	7SEG-CK
1	BCD to Seven Segment Decoder	4511D
1	4x DIP Switch	SW_DIP-4	to set the LED value
1	BNC Connector	B35N57	to power the board
7	0603 Resistors	R-US_R0603	current limiting resistors

As stated earlier, all of the parts I’ll be using can be found in the libraries included with EAGLE. To start, right click on the eagle folder on the EAGLE Control Panel and select New Project. Name your project, right click on its red folder icon, and select New -> Schematic. On the left toolbar, click on the Add button. When the Add dialog appears, type “*7*segment*” in the search box and press Enter. EAGLE’s search function can be finicky, so I tend to be pretty liberal in my use of asterisks. Towards the bottom of the list of parts, there should be one called 7SEG-CK (any common cathode seven segment LED will work). Select it, press OK and click to place it on the schematic. Repeat this process for the other parts, searching for the part number listed in the table above. In the end, you should have a schematic that looks something like the image below.

If you didn’t place 7 resistors, you can click the copy button on the left toolbar, click on the resistor you did place, then place the new one just like you would have if you had selected it from the Add dialog.  For this design, the output side of the DIP switches (marked with “On”) needs to be connected to the inputs of the 4511D (IA, IB, IC, ID).  LT and BI on the are connected to VDD, while LE is connected to GND.  The outputs (A-G) are connecteed through the resistors to the corresponding pins on the Seven Segment LED.  The cathodes and decimal point of the LED are connected to ground, while the inputs of the DIP switches and the center pin of the BNC are connected to VDD.

In order to make connecting the pins easier, I suggest rearranging the parts so that the signals flow from left to right.  This is also good practice as it makes it easier for someone (including yourself) to read your schematics in the future.  To move the parts, left click on the move button then click on the center of the part, move it where you want it, and left click to place it.  To move a group of parts (such as the resistors), click the group button and click and drag around the parts you want to select them.  To move them, click the move button, but instead of left clicking, right click the group, select move group, then place the group where you want it by left clicking.  You can see mine in the previous picture.

While it isn’t technically necessary, you’ll want to add supply schematics (VDD and GND) to the schematic.  Look for them in the supply and supply2 libraries.  For now, don’t worry about the name of the supply, just pick a positive supply and a ground.  Connect the pins as described above by first clicking on the net button, clicking on a pin, then clicking on the pin you want to connect the first pin to.  For example, after selecting the net tool, click on LE, then click on your ground symbol.  If done correctly, the net should terminate on the second pin.  Otherwise, you will continue seeing it as you move your mouse.  If you want to change the bend of your net, simply right click before you click on the second pin.  You’ll see the net change.  If you look on the top toolbar, you’ll see EAGLE cycling through the diffferent bends.  Finish connecting the pins and your schematic will look similar to the one below.

Now that the schematic is done, you need to check for errors by clicking the ERC button.  When I click on it, I have errors. While it looks like everything is connected, there are some implicit pins that will cause errors.  These pins aren’t normally shown on the block diagram.  In this case, the power and ground pins for the 4511D are hidden.  If you selected VDD and VSS for your power and ground supplies, you won’t see this error because the power and ground pins of the 4511D are implicitly connected to VDD and VSS.  If you need to show these implicit pins, click the invoke button and click on the 4511D.  EAGLE will show a dialog box with any available schematic symbols.  Select the row with P for the gate value, click OK, and place the power pins on the schematic.  Connect VDD to your positive supply and VSS to your ground supply and your schematic should look similar to mine.

This is already a very wordy post.  If anyone could suggest some cheap (read free) desktop video recording software that can record at a decent frame rate, please email me or post your suggestion in the comments.  In the next post I’ll cover turning this schematic into a board.  If you want to get ahead, just click the Board/Schematic icon and start playing around with the board.