Stock KiCad has Package_TO_SOT_SMD:SOT-23-5. Use a stock footprint when its pads match the land pattern the datasheet recommends; the reviewer checks exactly that.
Open the AP2210 datasheet at page 29, "Suggested Pad Layout", SOT25 (Diodes' name for SOT-23-5):
| symbol | value | meaning |
|---|---|---|
| Z | 3.60 mm | outer edge to outer edge of the two pad rows |
| G | 1.60 mm | gap between the rows |
| X | 0.70 mm | pad width (along the pin pitch) |
| Y | 1.00 mm | pad length (across the package) |
| E1 | 0.95 mm | pin pitch |
| E2 | 1.90 mm | outer pin to outer pin (2 x E1) |
Datasheet page 29, Suggested Pad Layout for SOT-23-5. Z, G, X, Y, E1 and E2 are the table above.
Row centres sit (Z + G) / 2 = 2.60 mm apart, so the pads go at X = -1.30 mm and X = +1.30 mm.
Stock SOT-23-5 uses 1.06 x 0.65 mm pads with rows 2.20 mm apart. Different pattern, so we make one named after the part: SOT-23-5_AP2210K. When the numbers do match stock, put the stock name in the symbol's Footprint field and skip the rest of this document.
From the project manager click Footprint Editor. In the library tree pick UWRL_Regulator (the one with the project icon). File → New Footprint (Ctrl+N) opens an empty footprint called Untitled. File → Footprint Properties…, General tab:
SOT-23-5_AP2210KSOT-23-5 land pattern from the Diodes AP2210 datasheet p.29); Keywords: SOT-23-5 SOT25 AP2210
Footprint Properties. Name, description, keywords and component type live here.
The finished footprint: five pads, fabrication outline, silkscreen, courtyard.
Place → Add Pad, click roughly where the pad goes, then double-click it to open Pad Properties.
Place menu: Add Pad, then Draw Lines and Draw Rectangles for the outline, silkscreen and courtyard.
Pad numbers must equal the symbol's pin numbers; that is the only link between the two. Footprint coordinates have Y pointing down, so a negative Y is above the centre.
| pad | X | Y |
|---|---|---|
| 1 | -1.30 | -0.95 |
| 2 | -1.30 | 0.00 |
| 3 | -1.30 | 0.95 |
| 4 | 1.30 | 0.95 |
| 5 | 1.30 | -0.95 |