Adom Library

.SchLib  =  OLE2 container
            └── /<ComponentName>/Data   ← record stream
                  ├── text records   <u16 len><u16 flags> |KEY=VAL|KEY=VAL
                  │     RECORD=1  component header (PartCount, AllPinCount…)
                  │     RECORD=14 rectangle (the symbol body)
                  │     RECORD=41 parameter
                  └── binary pin records  <u16 len><u16 flags> + payload[0]=0x02
                        [14]     PinConglomerate (orientation in bits 0..1)
                        [15..17] PinLength      (i16)
                        [17..19] Location.X     (i16)
                        [19..21] Location.Y     (i16)
                        [26..]   length-prefixed strings: Name, Designator

// Parse → symbol JSON { module_name, pin_count, pins:[…], body, part_count }
altium_schlib::parse_altium_schlib_path(&Path) -> Result<serde_json::Value>
altium_schlib::parse_altium_schlib_bytes(&[u8]) -> Result<serde_json::Value>

// Native SVG — draws the symbol directly from the parsed pins (no KiCad).
altium_schlib::render_symbol_svg(&Value) -> String

// Export path — emit a .kicad_sym (rendering uses the SVG above).
altium_schlib::to_kicad_sym(&Value, lib_name: &str) -> String

altium-schlib-json  part.SchLib            # parsed JSON
altium-schlib-svg   part.SchLib            # native symbol SVG → stdout
altium-schlib-kicad part.SchLib [name]     # .kicad_sym → stdout

## What this is

`altium-schlib` is a native Rust crate that reads Altium Designer's **binary
schematic-symbol libraries** — `.SchLib`, and the SchLib stream embedded inside
`.IntLib` — with **no Altium install and no KiCad round-trip**. It is the symbol
counterpart to [`altium-pcblib`](https://wiki.adom.inc/skill/altium-pcblib)
(footprints), and together they let the Adom EDA family read *both halves* of an
Altium library natively.

It emits pins (number, name, position, rotation) and the body as **KiCad-shaped
JSON**, renders a **native SVG** of the symbol, and can emit a **`.kicad_sym`**
for export.

![ADS1263IPWR symbol parsed natively from its Altium .SchLib — 28 pins, both banks, body](screenshots/ads1263-symbol.png)

*The ADS1263IPWR schematic symbol, rendered straight from its Altium `.SchLib` —
28 pins, both banks, correct names + numbers (validated pin-for-pin against KiCad).*

## Why it exists

Altium `.SchLib` is a Microsoft OLE2 / Compound File Binary container, and the
pins inside are **not** the pipe-delimited ASCII records the rest of the file
uses — they're a compact **binary** record format that no public Rust parser
read. Every Adom tool that wanted Altium *symbols* previously had to lean on
KiCad's importer (a lossy conversion that normalises everything to KiCad). This
crate reverse-engineers the binary pin record so a `.SchLib` renders its **own**
geometry — which is the whole point of comparing sources: you can only spot what
disagrees if each format shows its own truth.

## Validation

The binary decode was validated **pin-for-pin** against KiCad 10's Altium
importer on a real part (`ADS1263IPWR`): **28/28** pin numbers and names match —
overbars and all (`C̄S̄`, `R̄ĒS̄ĒT̄`).

![altium-schlib native symbol vs KiCad vs datasheet — pins validated 28/28](screenshots/validation.png)

*Left: the symbol `altium-schlib` parses straight from the `.SchLib`. Middle/right:
KiCad's own render and the datasheet extraction — every pin number and name agrees.*

## The format, briefly

```
.SchLib  =  OLE2 container
            └── /<ComponentName>/Data   ← record stream
                  ├── text records   <u16 len><u16 flags> |KEY=VAL|KEY=VAL
                  │     RECORD=1  component header (PartCount, AllPinCount…)
                  │     RECORD=14 rectangle (the symbol body)
                  │     RECORD=41 parameter
                  └── binary pin records  <u16 len><u16 flags> + payload[0]=0x02
                        [14]     PinConglomerate (orientation in bits 0..1)
                        [15..17] PinLength      (i16)
                        [17..19] Location.X     (i16)
                        [19..21] Location.Y     (i16)
                        [26..]   length-prefixed strings: Name, Designator
```

The OLE2 FAT that Altium writes overshoots the file's real sector count, so the
crate pads the buffer with the CFBF free-sector sentinel (`0xFF`) before opening
— the same trick `altium-pcblib` uses.

## Public API

```rust
// Parse → symbol JSON { module_name, pin_count, pins:[…], body, part_count }
altium_schlib::parse_altium_schlib_path(&Path) -> Result<serde_json::Value>
altium_schlib::parse_altium_schlib_bytes(&[u8]) -> Result<serde_json::Value>

// Native SVG — draws the symbol directly from the parsed pins (no KiCad).
altium_schlib::render_symbol_svg(&Value) -> String

// Export path — emit a .kicad_sym (rendering uses the SVG above).
altium_schlib::to_kicad_sym(&Value, lib_name: &str) -> String
```

## CLI

```bash
altium-schlib-json  part.SchLib            # parsed JSON
altium-schlib-svg   part.SchLib            # native symbol SVG → stdout
altium-schlib-kicad part.SchLib [name]     # .kicad_sym → stdout
```

## Who uses it

`adom-sfconvert` reads Altium symbols through this crate (fully native — no
service round-trip), and `chip-fetcher` shows the result as a per-source
thumbnail next to the KiCad, EAGLE/Fusion, and datasheet symbols so you can
compare what each source actually contains.