KiCad silkscreen export substitutes wider text metrics and a fixed 0.15 mm stroke

Versions: @tscircuit/cli 0.1.2057, @tscircuit/core 0.0.1892, circuit-to-svg 0.0.413; KiCad 10.0.2. Linux/WSL2.

A silkscreentext with fontSize=0.8 is exported as native KiCad text with (size 0.8 0.8) and a fixed (thickness 0.15). The source preview allocates 0.6 * fontSize per character, but the substituted KiCad font has a materially different width. Text clear in the SVG can overlap adjacent silkscreen or run off the PCB in the exported project.

Minimal reproduction:

export default () => <board width={10.4} height={10.4}>
  <silkscreentext text="SN74LVC1G17DCKR" pcbX={0} pcbY={0} fontSize={0.8}/>
</board>

Run tsci build lib/index.tsx --svgs --kicad-project, compare the PCB SVG against the exported KiCad text's effective shape, then run native DRC. In our real small-board fixture this produced silk_edge_clearance and text-to-text silk_overlap even after increasing the nominal text height to 0.8 mm.

Expected: preserve the source font or export native text with equivalent metrics and stroke, so layout/clearance review transfers to the exported board. Expose/document any unavoidable font substitution. Do not lower text-height rules or hide warnings.

Local workaround implemented in the family exporter: preserve native text height, use a 0.10-mm stroke, and fit the native text width to the source allocation using KiCad's measured bounding box. No upstream PR is open from this work; this issue remains available for an upstream implementation.

Start with the family exporter used by tsci build lib/index.tsx --svgs --kicad-project, then compare the source PCB SVG with the exported KiCad text's effective shape. Reproduce the small-board case and run native KiCad DRC, checking silk_edge_clearance and silk_overlap. Done means exported text preserves or documents equivalent metrics without suppressing clearance warnings.