The worked example is the AP2210K-3.3, a 300 mA low-dropout regulator from Diodes Incorporated, SOT-23-5 package. Open the datasheet now and keep it open: diodes.com/assets/Datasheets/AP2210.pdf. Page 3 has the pin table ("Pin Descriptions", SOT23-5 column):
| pin | name | electrical type in KiCad | why |
|---|---|---|---|
| 1 | VIN | Power input | a supply pin; ERC wants it driven by a power source |
| 2 | GND | Power input | same |
| 3 | EN | Input | a logic input |
| 4 | BYP/ADJ | Passive | bypass capacitor to GND for low noise (10 nF); on the fixed 3.3 V part it only ever sees a capacitor |
| 5 | VOUT | Power output | the regulator drives this net; ERC flags two outputs fighting |
Datasheet page 3, Pin Descriptions. Use the SOT23-5 column; the SOT23-3 numbering is a different package.
Order code: MPN AP2210K-3.3TRG1 (the TRG1 is the reel), LCSC C176959.
<aside> 💡 House style, every symbol Supplies at the top, GND at the bottom. Inputs on the left, outputs on the right. Group pins by function, not by pin number. Pin names and numbers exactly as the datasheet. Pins on the 50 mil (1.27 mm) grid. No project-specific text in the symbol: the symbol is the chip, the board is the context.
</aside>
From the project manager click Symbol Editor. In the library tree on the left, the project's libraries show a small project icon; the stock libraries do not. Find UWRL_Regulator and click it. Only ever edit UWRL_* libraries. Stock libraries are overwritten by the next KiCad update.
The Symbol Editor with the tree filtered to UWRL_Regulator, showing the finished symbol this document builds. The blue labels are the pin electrical types.
File → New Symbol…. Fill in:
AP2210K-3.3U (ICs are U; connectors J, resistors R, capacitors C, inductors L, diodes D, transistors Q, crystals Y, switches SW)
New Symbol. Name and reference designator are the two fields that matter.
Click OK. An empty canvas opens with the reference and value text placed.
Place → Add Rectangle (or the rectangle tool on the right toolbar). Click two opposite corners, about 15 mm wide by 10 mm tall, centred on the origin. Keep the grid at 50 mil (1.27 mm); the grid selector is in the top toolbar. Set the fill to "Fill with body background color" (double-click the rectangle to edit it) so the body reads as a chip.