Open the board project and start the Schematic Editor.
Press A (Place → Add Symbol), type AP2210 and pick UWRL_Regulator:AP2210K-3.3. Click to place it. The footprint and the datasheet came with it: the symbol carries both fields.
The symbol on the sheet, straight from the library.
Wire it as the datasheet's typical application shows: VIN from the input rail with a 1 uF ceramic to GND next to the pin, VOUT to the 3.3 V rail with another 1 uF, EN tied to VIN (always on) or to a control signal, GND to ground. BYP/ADJ takes an optional 10 nF capacitor to GND for lower noise; leave it open otherwise.
Select the symbol and press D (or right-click, Show Datasheet) to open the PDF from the symbol's Datasheet field.
Tools → Annotate Schematic… gives U? a number.
Annotate Schematic with the defaults. U? becomes U1.
Inspect → Electrical Rules Checker must be clean on a finished sheet. The pin electrical types you set in document 3 are what ERC uses: an unconnected Power input, or two Power output pins on one net, shows up here and nowhere else.
ERC before wiring: every pin is listed, which is the pin types doing their job. Wire the part and run it again; the list must be empty before you commit.
Tools → Update PCB from Schematic… (F8), then Update PCB. The PCB Editor opens with the SOT-23-5_AP2210K footprint attached to the cursor; click to drop it.
Update PCB from Schematic: U1 arrives with the UWRL_Regulator:SOT-23-5_AP2210K footprint and the symbol's fields.
The footprint on the board: pads, courtyard, reference and value.
View → 3D Viewer (Alt+3) shows the STEP body on the pads.
The 3D viewer. No board outline yet, hence the warning; the part itself is right.