When creating and connecting nets in a schematic, I like to start with power connections but you can really start anywhere. Additionally there are several ways that you can create nets between two pins or components.
Since the GND net is already connected from when we added the two design blocks to the schematic, start to use the first approach of connecting nets to make the 3.3v power connection between the headers for the Trinket and the INA219. We are going to use the Net tool to draw the connection between the two net stubs on each of the headers.
To start, select the Move tool and click on the VCC symbol attached to the VCC net for the INA219 header and stretch out the net a bit to give yourself more room to draw the net. Then do the same for the 3.3V net for the Trinket (which may be hard to see).
Now that we have a bit more room to work with, select the Net tool and first click on the green VCC net extending from pin 1 of the INA219 header. Then click to lay down net pieces towards the 3.3v net extending from pin 1 of the JP2 header for the Trinket. Finally click on the 3.3V net to join the two nets into one. Eagle will present you with a Connect Net Segments? window and will ask you to choose the new name for the combined net. Choose 3.3V and click OK to join the two nets.
For the remaining nets, we'll use the fact that Eagle considers two nets as the same if they have the same name. Using this technique allows to to keep your schematic tidy by not requiring nets to cross the whole schematic to be connected. It's up to you to decide which approach makes your schematic easier to understand.
Select the Name tool and click on the D2_A1_PA09_SCL_MISO net connected to pin 2 of the Trinket's JP2 header. Eagle will show a Name dialog that allows you to change the name of the given schematic element, in this case a net. As the name suggests the D2_A1_PA09_SCL_MISO net represents a connection to the Trinket's SCL pin which is what we want to connect to the net of the same name for the INA219 breakout. Change the name to SCL and click OK. Eagle will verify that you want to connect the two nets. Click Yes to change the name and make the connection.
Repeat the process, renaming the D0_A4_PA08_SDA net to SDA to make the final connection. The remaining nets do not need to be connected for this project so you can leave them as they are.
Once you have connected nets between all of the pieces of your circuit that need to be connected, I suggest clicking on each of the nets with the Show tool to highlight all the connected parts of the net to verify the connections.
Congratulations! You’re not done but you have a functional circuit schematic. For this project the schematic is a means by which to create a circuit board however schematics are valuable on their own as documentation of how a circuit is constructed. Schematics are the circuit, the arrangement of information that creates a thing where one did not previously exist.