gds2kicad

Convert selected GDS geometry into a KiCad .kicad_pcb board file.

The converter uses KLayout to read and polygonize GDS shapes, then writes KiCad PCB objects using kicad-pycbnew. GDS polygons are emitted as KiCad zones with cached filled_polygon data, so downstream exports can use the generated filled geometry without asking KiCad to recalculate zone fills.

Preview

Example output generated from example.gds:

Install

Python 3.12 was used during development. The runtime dependencies are normal Python packages installed from PyPI via pip:

• klayout
• kicad-pycbnew

Create a virtual environment and install the project dependencies from pyproject.toml:

python3 -m venv .venv
. .venv/bin/activate
pip install .

No separate KiCad GUI application package is required to run the converter itself. KiCad is only needed if you want to open the generated .kicad_pcb file graphically or validate/export it with kicad-cli.

Usage

Convert the included example GDS file:

python gds2pcb.py example.gds example.kicad_pcb

If no arguments are provided, the script uses those same defaults:

python gds2pcb.py

Convert another GDS file:

python gds2pcb.py input.gds output.kicad_pcb

Default layer mapping

The current defaults are tailored for the prototype process stack:

GDS layer/datatype	KiCad output
3/0	filled zone on In1.Cu
6/0	filled zone on F.Cu
7/0	filled zone on F.Mask
2/0	blind via from B.Cu to In1.Cu
4/0	blind via from In1.Cu to F.Cu

The default generated net name is empty.

Override mappings

Map GDS polygon layers to KiCad layers:

python gds2pcb.py input.gds output.kicad_pcb \
  --layer-map 3/0=In1.Cu \
  --layer-map 6/0=F.Cu

Map GDS via layers to KiCad via layer pairs:

python gds2pcb.py input.gds output.kicad_pcb \
  --via-map 2/0=B.Cu,In1.Cu \
  --via-map 4/0=In1.Cu,F.Cu

Set a KiCad net name:

python gds2pcb.py input.gds output.kicad_pcb --net-name /GND

Notes

• GDS boxes, polygons, and paths are all converted through KLayout's shape.dpolygon representation.
• KiCad native via objects are circular. For each GDS via polygon, the converter uses the bounding-box center and min(width, height) as the via diameter.
• The via drill defaults to diameter - 10 µm; adjust with --drill-shrink-um.
• Generated zones include both polygon and matching filled_polygon sections. Avoid manually refilling zones in KiCad if you need to preserve the exact GDS-derived fill geometry.
• --flip-y exists for coordinate-system experiments, but the default is no mirroring.

Generate a preview SVG

The converter itself only writes the KiCad PCB file. The preview.svg image in this README was generated from the converted board using KiCad CLI:

python gds2pcb.py example.gds example.kicad_pcb

kicad-cli pcb export svg example.kicad_pcb \
  --output preview.svg \
  --layers F.Cu,In1.Cu,B.Cu,F.Mask \
  --page-size-mode 2 \
  --exclude-drawing-sheet

KiCad / kicad-cli is only needed for opening, validating, or exporting the generated .kicad_pcb file; it is not needed to run gds2pcb.py.