Adom Library

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 (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.

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).

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

// 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

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.