README.md

Extracting a Bill of Materials

Read a schematic document (.SchDoc) and produce a grouped bill of materials — one line per distinct part, with a quantity and the list of reference designators — as a console table, a CSV file, and an HTML table.

The complete, compiling source for this guide is Program.cs.

Run

# Uses a bundled TestData schematic (TestData/Power Supply.SchDoc)
dotnet run --project examples/ExtractBom

# Point it at your own file
dotnet run --project examples/ExtractBom -- "C:\path\to\MyBoard.SchDoc"

Where the data lives

A schematic component is an ISchComponent. Cast it to the concrete SchComponent to reach the fields a BOM needs. The important gotcha: there is no Designator property — Altium stores the reference designator as a parameter named "Designator".

await using var doc = await AltiumLibrary.OpenSchDocAsync(input);

foreach (var component in doc.Components)
{
    var sc = (SchComponent)component;

    // Designator comes from the parameter collection, not a property.
    var designator = GetParameter(sc, "Designator");
    if (string.IsNullOrWhiteSpace(designator))
        continue;  // power port, net tie or graphic — not a purchasable part

    // Comment is Altium's "Value" field (e.g. "10k", "100nF").
    var value = !string.IsNullOrWhiteSpace(sc.Comment)
        ? sc.Comment!
        : (GetParameter(sc, "Value") ?? "");

    // Footprint: prefer the current PCB implementation link.
    var footprint = GetFootprint(sc) ?? GetParameter(sc, "Footprint") ?? "";
}

static string? GetParameter(SchComponent c, string name)
{
    foreach (var p in c.Parameters)
        if (string.Equals(p.Name, name, StringComparison.OrdinalIgnoreCase))
            return string.IsNullOrEmpty(p.Value) ? null : p.Value;
    return null;
}

Field	Source
Designator	SchComponent.Parameters → "Designator"
Value	SchComponent.Comment (fallback: "Value" parameter)
Footprint	SchComponent.Implementations where ModelType == "PCBLIB" (fallback: "Footprint" parameter)
Manufacturer / MPN	custom parameters; MPN falls back to SchComponent.DesignItemId

Implementations is only on the concrete SchComponent, not the ISchComponent interface — another reason for the cast. Parameters are free-form key/value pairs, so different libraries use different names; the example reads the common ones and is easy to extend.

Sample output

Qty  Value            Footprint              Designators                    MPN
----------------------------------------------------------------------------------
  2  CL10A226MP8NUNE  CAP 0603_1608          C12, C16                       CL10A226MP8NUNE
  2  GCM188R71E105KA… CAP 0603_1608          C13, C15                       GCM188R71E105KA64D
  1  LT1761IS5-5#TRM… AD SOT-23-5 S5 05-08…  IC4                            LT1761IS5-5#TRMPBF
  1  0022272031       MOLEX KK 0022272031    J4                             0022272031

The CSV and HTML are written to a temp folder (the program prints the paths).

Notes

• A BOM needs only component metadata, so the lack of a pin-to-net connectivity API in the schematic model is irrelevant here.
• A top sheet that only contains sub-sheet symbols will report no designated components — run the example against a leaf schematic, or extend it to walk the hierarchy via SheetSymbols (see the planned WalkHierarchy example).

See the guides index for the full set of examples.