Now we arrive at my favorite part of circuit board design, layout. This is where we will translate the design represented in our schematic to a set of plans that will be used to fabricate the actual circuit board. When we’re done we will have a file that we can send to a board manufacturer like OSHPark to be manufactured.

When you switch to the Board window, you will see all of the footprints that you placed as you added the design blocks to the schematic as well as a bunch of lines between the different pins. These lines are referred to as airwires and will be present on the Unrouted layer (20) between the two closest pieces of the board that represent either end of the net. In this case, because we haven’t defined any traces yet, the airwires will span the whole distance between each pair of pins.

Our next steps will be to first define the general shape of our board by modifying the Dimension layer (layer 20), then we will position the headers on the board and finally we will use the route tool to lay down the copper traces that will make the connections that our nets represent.

Layers

It's worth taking a moment here to talk about how layers are used in Eagle. Eagle organizes information about a board's layout into a vast array of layers, most of which we don't need to concern ourselves with just yet. The free version of Eagle comes with two routing layers, Top(1) and Bottom(16) that represent the design of most of the copper connections and footprints for components on the respective sides of the finished PCB. A large amount of our layout work will be done on these layers using the routing tools.

The Pads(17) and Vias(18) layers both represent the locations of plated through holes on the board that make an electrical connection between layers. The main difference between the two is that the Pads layer is generally used to connect the pins of a through hole component such as our headers both mechanically and electrically to the board.  Vias are essentially pads that are only used to electrically (and sometimes thermally!) connect layers of the board. Since they aren't meant to have anything physically passing through them they are normally smaller than pads so that they don't use more space on the board than needed. 

Finally we will be using the tPlace(21) and bPlace(22) to add stuff to the silkscreen design that will be printed on the top and bottom of the board respectively. At a minimum you should use this layer to label things on the board like pins or perhaps orientation information.

There are many more layers, some of which you will use in the future and some that you may never use. OSH Park has an excellent guide covering the commonly used layers in Eagle.