ECE101 – Basic Electrical and Computer Engineering

Seven Segment LED – Board

In this post, I’ll cover doing the board layout for the seven segment led. For reference, I’ve included the same toolbar buttons in this post as I did last time. Some of them don’t apply to laying out a board, but since they’re the basic tools you’ll use, it’s a good refresher.

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

Name – changes the name of a component, net, or trace

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

Polygon – used to create ground (and power) planes on boards

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

Board Layout

With the schematic open from last time, click on the Board button. EAGLE will ask you if you want to create the board from the schematic. Click yes and EAGLE will place all the parts from your schematic in a new board file. The screen should look something like the picture below.

The white box to the right of the parts is the largest board that can be made with the freeware version of EAGLE. Start by moving all of your parts inside the square. After some initial planning, I moved my parts around as shown below.

On most boards, it is good practice to use one side of the board as a ground plane. You can still route other traces on that side of the board and it ensures that your grounds are all well-connected. You can think of it as a very wide trace going to all of your grounds. To do this, press the Polygon button, make sure the bottom layer is selected on the top toolbar (it should read “16 Bottom”, not “1 Top”) and create a box around your board. Click the Name button and rename the polygon to the name of your ground supply (GND in my case). This will make the bottom layer of your board a ground plane. Any signals you route on the bottom layer will be isolated from the ground plane, but too many traces can isolate areas of the bottom layer so that they are no longer part of the ground plane. Click ratsnest and you should see the grounds of your through-hole component connected to the ground plane that now fills the bottom layer. In the picture below, you’ll see the ground connections of the BNC connector as crosses through the hole. This cross forms a thermal break. Rather than not routing the board at all around that drill hole, some of the copper is removed so that it can be easily soldered. Otherwise, you would be trying to heat the entire ground plane when you tried to solder the connector to the board.

All that remains is to route the traces between components. This process is similar to creating a net on the schematic. Select the Route tool, click where you want to start and EAGLE will select the airwire of the trace you are trying to route to show you where you need to end. Click along the way to set the path it will follow, right-clicking to change the bend, and finally, click the end of the trace to finish it. If EAGLE isn’t sure which trace you are trying to route, it will highlight the airwire of the trace it thinks you want to route. If it selects the correct airwire, left click again to begin routing. If it selects the wrong one, right click to cycle through the other nearby airwires and left click when the correct one is selected. I started by routing the power traces and the dip switch outputs to the inputs of the decoder. I also connected the decoder grounds to the ground plane. To do this, you can start routing the trace as you normally would, bring it out from the pad and click to anchor the trace, then switch the trace layer to Bottom, and double click. This will automatically create a via and will connect your trace to the ground plane. Then I figured out where the resistors needed to go for easy routing between the decoder and the LED. You can see my placement in the picture below.

You can also see that my traces aren’t all the same size. Particularly, I made my power (VDD) traces wider. This reduces resistance and, consequently, the voltage dropped between the BNC connector input and the power pins of the decoder and the inputs of the DIP switches. The trace width can be changed on the top toolbar while the Route tool is being used. It can also be changed after routing the traces using the Change tool (the wrench on the toolbar, not shown in my list), selecting Width, then selecting the width you want to change traces to, and lastly clicking the traces that you want to change to your selected width.

I could route the traces from the decoder through the resistors to the LED pins using both sides of the boards, but here we’ll use the space between the resistor pads to keep all traces on the top layer. To do this and not have DRC errors, you’ll need to change the width of traces going between the pads. In the picture below, you’ll see what I mean (and the completed board).

Now that we have the basics out of the way, my next few posts will be shorter, less wordy, and more useful for those with prior experience. As always, feel free to ask questions or correct any of my mistakes. If you’re confused, I recommend checking out the video.