0hmX/am3352-zcz-footprint

README.md

# AM3352 ZCZ footprint

Reusable **footprint only** for TI AM3352BZCZ100 / ZCZ0324A (JLCPCB C468247). No board, electrical symbol, signal mapping, or 3D model is included.

## KiCad vs tscircuit verification

![KiCad reference and tscircuit footprint, side by side at the same scale](https://registry-api.tscircuit.com/package_files/download?package_file_id=347dedf8-314a-46b7-ad65-e8012216350a)

Left: native `kicad-cli fp export svg` rendering of the KiCad reference. Right: native `tsci export -f pcb-svg` rendering of this package. Both are shown from the top, at the same scale, with A1 at the upper left. Reference-designator text is hidden in the KiCad view; pad geometry is unchanged.

| Measured property | KiCad reference | This footprint |
| --- | --- | --- |
| Pad array | 18 × 18 / 324 pads | 18 × 18 / 324 pads |
| Copper pad diameter | 0.40 mm | 0.40 mm |
| Pitch | 0.80 mm | 0.80 mm |
| Outer pad-center span | 13.60 mm | 13.60 mm |
| Ball positions | Reference | All 324 match after Y-axis conversion |
| Courtyard | 15.50 × 15.50 mm | 15.60 × 15.60 mm |

The copper geometry matches. Silkscreen styling differs, and this package uses a slightly larger courtyard to allow 0.25 mm clearance beyond TI's maximum 15.1 mm body. This is a geometry comparison, not an electrical-symbol or assembly qualification. The KiCad footprint is a generic BGA reference; TI's package drawing is the design source.

## Install

```sh
tsci add 0hmX/am3352-zcz-footprint
```

## Use

```tsx
import {
  AM3352ZCZFootprint,
  am3352BallLabels,
} from "@tsci/0hmX.am3352-zcz-footprint"

export default () => (
  <board width={22} height={22} routingDisabled>
    <chip
      name="U1"
      pinLabels={am3352BallLabels}
      footprint={<AM3352ZCZFootprint />}
    />
  </board>
)
```

`AM3352ZCZFootprint` is also the default export. `am3352Balls` and the `AM3352Ball` type are available for custom symbols. Use the matching ball labels to avoid conflicting pin aliases. Numeric identifiers are column-major: pin1=A1, pin2=B1, pin19=A2. Connect by ball name, for example `U1.A1`.

## Geometry

- 324 circular pads, 18 × 18 array, 0.80 mm pitch.
- Copper diameter 0.40 mm; paste diameter 0.40 mm.
- Solder-mask expansion 0.05 mm per side.
- Body 15 × 15 mm nominal; courtyard 15.6 × 15.6 mm.
- Top view: A1 upper left, column numbers increase right, row letters increase down.
- Chamfered fabrication and silkscreen outlines identify A1.

Authored from [TI's ZCZ0324A package drawing](https://www.ti.com/lit/ds/symlink/am3352.pdf), PDF pages 260–262. All 324 pad positions and diameters were checked against the [KiCad BGA geometry reference](https://github.com/KiCad/kicad-footprints/blob/master/Package_BGA.pretty/BGA-324_15.0x15.0mm_Layout18x18_P0.8mm_Ball0.5mm_Pad0.4mm_NSMD.kicad_mod). Electrical signal assignments and manufacturing-process validation are outside this footprint package.