Now that we have the design blocks for the Trinket and breakout, we can start assembling the schematic for our board. To start, we need to create a new blank schematic and board file.
With the schematic window open, use the File > New to create a new schematic. If you haven't saved the current schematic you will be given a chance to save. After creating the new schematic, click the SCH/BRD button. You will be prompted to create a board file from the schematic; say yes so that we are able to paste in both the schematic and board parts of the design blocks we created in previous steps. You will be prompted to save the current board if you wish.
Since the board we are creating is, in essence, a set of jumper wires, the schematic will only contain these connections themselves, not the complete circuit with the Trinket and the breakout.
This step is analogous to what you would do when assembling a circuit on a breadboard, using wires to connect signals between different pieces. In this case, however, instead of connecting the components of the circuit with the tracks of a solderless breadboard and jumper wires, we'll be documenting those connections in Eagle with “nets” which are Eagle’s way of representing the connections between the parts of a circuit.
Nets are used to record the “what” of the connection between two parts of a circuit. The “how” is done later when doing the layout in the board file. This separation of concerns is useful because this leaves you the flexibility to make choices about how the connection is made when laying out the board.
First we’ll need to add the headers for the Trinket and INA219 to the main schematic. To do this, select the Add a Design Block tool, expand the Design Blocks node and select the first piece of your circuit. I generally start with the main processor or development board but the order doesn’t matter. Select the design block that you created for the Trinket header and click OK and you will see a copy of the schematic from the Trinket header design block following your cursor.
Choose a section of the schematic to place it in and right click to put it down. Once you do this, your screen will change to the board view to allow you to place the elements from the design block on the board layout. Try to place it in the general area you will want it, but don’t worry about getting it perfect at this step.
Once you have placed the board elements you will be show the Paste from file dialog that looks like this:
This dialog allows you to change the names of the “incoming” design block to avoid using the same name of an net that already exists in the main schematic. In Eagle, two nets are connected if the have the same name, even if there isn’t a visible connection between the two parts of a schematic. The “paste from file” dialog allows you to avoid unintended connections by changing the name of the nets from the design block before they’re added to the schematic. In our case since this is the first piece of the schematic there are no conflicts.
Click OK to finish adding the design block to the schematic.
Repeat this process for the INA219 header design block. When the Paste from file dialog appears the one common net name is GND which is of course the ground connection. For this project and most others if the incoming design block has a GND net it will be OK to leave the name as it is since you generally want your grounds connected. When you use these techniques in your future projects you will have to make that decision based on the needs of your project.
Click OK to finish adding the INA219 header.
Congratulations! You’re not done but you’re closer than when you started! The next step is to create the nets needed to make the connections between the different parts of your circuit. As before, the nets we create here will be virtual representations of the connections of our circuit; you can think of them as equivalent to the jumper wires you used to connect the parts of your circuit on your breadboard.