Now that we have a completed schematic we need to fill in some extra information to enable us to build a PCB. Each of the symbols that we have placed need to be associated with a Footprint. Footprints describe how a component will attach to a PCB. It defines how many pads there are, where they are and how they map to the component pins.
To set the footprint for a symbol, hover over it and press E to bring up the symbol properties.
Start by doing this with the SAMD10 MCU symbol:
If you look at the Footprint field, you can see that it is already populated with a footprint. In this case, it's using the Package_SO:SOIC-14_3.9x8.7mm_P1.27mm footprint. Some symbols in the library already have a suitable footprint associated to them, so we can leave this one alone.
Let's look at the bypass capacitor symbol C1 next. Bring the mouse over it and press E:
Notice that the Footprint field is blank. Let's assign one.
Select the Footprint field by clicking on it in the list. On the right-hand side of the window click the Browse Footprints button to bring up the footprint browser:
Footprints are organised into categories, although these don't really match up with the symbol library categories.
For this project we're going to use Surface Mounted components, in 0805 size so let's browse to the Capacitor_SMD category and find the Capacitor_SMD:C_0805_2012Metric_Pad1.15x1.40mm_HandSolder footprint. Double-click it to select it and set it as the footprint for this symbol.
We need to set the footprints for each symbol (excluding the power net symbols - +3V3, GND and +BATT). To speed things up a little, we can copy and paste the field value between similar components. This schematic has 3 capacitors which will all have the same footprint. Select the text in the field and copy it, then you can press E over the other two capacitors and paste the value in.
Do the reset pull-up resistor next. Hover over the symbol and press E, use the symbol browser to find an 0805 SMD resistor footprint:
Next up is the LED:
Then the programming connector - we'll use a Through-hole footprint for this one so we can solder header pins in:
Similarly, the GPIO connectors will be through-hole. Don't forget that there's 2 of those too!
Last is the button. I have about a million 6mm through-hole tactile switches, they're really common. I'm going to use the footprint for that switch:
With footprints all assigned to the symbols, the last step in designing our schematic is to generate a Net list. The net list describes how all of the components connect together and is used by the PCB design software to keep track of everything.
Choose Generate Netlist File... from the Tools menu:
Default settings are all fine, click the Generate Netlist button to create it. You'll be asked to save a file. Save it in the same folder with the rest of your project.
And that's it, we're finally ready to start designing the PCB.