Gnd pins should be assigned the name 'Gnd' (or sometimes VSS, depending on the naming conventions you want to use), and SPI pins should be assigned useful names like MISO, MOSI, SCK, and CS, etc.
Most of the time, the datasheet will contain a schematic symbol we can copy, though, including pin names. The GA1A1S202WP datasheet doesn't contain one, but there are only four pins so it's easy to figure out a basic layout and pin names.
Renaming pins in the symbol editor is the same as renaming pads in the package editor ... you simply select the 'Name' tool from the toolbar (highlighted in yellow below) ...
- Pin 1 = GND
- Pin 2 = GND
- Pin 3 = IO (Analog Output)
- Pin 4 = VCC (the power supply for this device)
This leaves us with the last two pins, both of which are 'Gnd', but it also introduces a problem.
Like pads on your package, pins must all have unique names!
When you have several pins with the same name and functionality (which is often the case with 'Gnd', 'VCC, 'VDD', etc.), we can assign the common name followed by the '@' symbol, and a unique number.
When Eagle renders our symbol on the schematic the @1, @2, etc., part of the name will be hidden, and only the common name preceding the @ will be shown.
Try it out by assign the following names to the last two pins in our symbol: