Select the Route tool and select 10 from the width dropdown in the route tool's menu bar. This will set the width of the traces you will create to 10 mils since you set the grid to use mils. 10 mils is a good default width; it's more than enough to carry the current that this project will be dealing with while still being small enough to not take up more board space than necessary. Additionally because the INA219 breakout is open source, we can see that it uses 10 mil traces for the VCC, GND, SCL, and SDA signals.
Like other things in Eagle, there isn't a required starting place for routing, so for the sake of this guide I'm going to start with the I2C connections, followed by the VCC connection. We're going to keep GND for last for a reason that will be apparent when we get to it.
With the Route tool still selected, verify that the Top layer (1) is selected and click on the SCL pin of the INA219 breakout to start a trace. Move your cursor towards the SCL pin on the Trinket's header, clicking along the way to lay down trace segments. Finally click on the Trinket's SCL pin. When you are done there should no longer be an airwire for the SCL net.
Continue using the Route tool to connect the SCL and VCC pins
It's inevitable that you will either make a mistake or just decide that you don't like the way a trace trace looks. When you want to remove a trace you can either use EDIT>UNDO menu item if you just routed it, but if you added it a while ago you can use the RIPUP tool to remove it.
Select the Ripup tool and click on the trace segments that you want to delete. Easy peasy.
You can use the Delete tool to remove traces however if you accidentally click on the airwire left after removing a trace, you'll get this somewhat confusing error:
This is Eagle complaining because it thinks you are trying to delete the airwire which is a functional part of the schematic. Eagle is saying it can't "backannotate" which is what it calls keeping the Schematic and Board in sync. In this case it is refusing to apply this "deletion" to the schematic because it would totally change the circuit.
One technique that is useful to learn is creating ground planes. You may have noticed when looking at some boards that they have large areas of copper filling most, or all, of the otherwise empty space around the components and the traces. These areas of copper, called ground planes, are often used to simplify making ground connections that the circuit requires. There are several other reasons why using ground planes makes sense on boards more complex than we're making, however again the reasons behind that are outside the scope of this guide. The Wikipedia page on the topic does a good job of explaining how and why they're used. This board is simple enough that a ground plane really isn't needed however learning the technique now to apply to more complex boards in the future will make routing a lot easier.
To create a ground plane we'll first use the Polygon tool to create a polygon slightly larger than the outline of our board.
Select the Polygon tool and click around the perimeter of the board to create a polygon, ending the polygon by returning to the beginning of the outline and clicking on the start.
Once you complete the polygon, you will be prompted to name the signal that the polygon will belong to. Enter GND so that the polygon becomes part of the GND net.
Once you specify the signal that the polygon is part of, click the Ratsnest button to fill the area outlined by the polygon with the GND signal. Since this creates a contiguous path between the two GND pads, this will complete that connection, removing the final airwire.
If you add new traces after creating the ground plane you will need to use the RATSNEST tool to generate a new ground plane that accounts for the new traces.
Sometimes when routing a board you will find that there is no easy way to find a route for a trace because it would have to go get to the other side of a trace and there is no quick way to go around it. This is where vias and double sided boards are useful. On a single sided board, you would use a jumper to cross another trace, however since our board has two sides, we can use a via to continue the trace on the other side of the board, avoiding the trace in the way.
This is entirely unnecessary for this board however I will give you an example of how to use both sides of a board by re-routing the SCL connection using vias to switch sides.
Starting with the SCL trace ripped up, again verify that the Top layer(1) is selected and click on the SCL pin of the INA219 breakout header. Start clicking to lay a path and when you want to switch sides, with the route tool still active select the Bottom layer (16). Once you do this, the trace will continue to follow your cursor however there will be a via at the tip of your cursor. The next time you click you will place a via and the traces will continue on the bottom layer. Route as you wish and then select the top layer again and repeat the process to continue on the top layer.
Because the pads for the headers are like large vias connecting both sides of the board, once you've switched to the bottom layer, you can in fact just complete the rest of the trace on the bottom of the board (if you're paying attention, you'll notice that you could also just have the whole trace on the bottom).