Export

The ExportOperations module handles generating manufacturing outputs.

board = kicad.get_board()
export = board.export

Gerber Files

gerbers(output_dir, ...)

Generates Gerber files for all layers.

board.export.gerbers("/path/to/output/")

gerbers_with_options(output_dir, **options)

Generates Gerbers with custom options.

board.export.gerbers_with_options(
    "/path/to/output/",
    format="gerber_x2",      # or "gerber_rs274x"
    use_protel_extensions=True,
    include_edge_cuts=True,
    include_netlist=True,
    plot_references=True,
    plot_values=True,
    plot_footprint_mode="plot"  # or "none", "sketch"
)

Drill Files

drill(output_dir, ...)

Generates drill files.

board.export.drill("/path/to/output/")

drill_with_options(output_dir, **options)

Generates drill files with custom options.

board.export.drill_with_options(
    "/path/to/output/",
    format="excellon",        # or "gerber_x2"
    units="mm",              # or "inches"
    zeros="decimal",         # or "leading", "trailing"
    merge_pth_npth=False,    # Separate plated/non-plated
    minimal_header=False
)

Position File (Pick and Place)

position(output_path, ...)

Generates component position file.

board.export.position("/path/to/output/positions.csv")

position_with_options(output_path, **options)

Generates position file with options.

board.export.position_with_options(
    "/path/to/output/positions.csv",
    format="csv",            # or "gerber", "ascii"
    units="mm",
    side="both",            # or "front", "back"
    exclude_through_hole=False,
    exclude_smd=False
)

BOM (Bill of Materials)

bom(output_path, ...)

Generates bill of materials.

board.export.bom("/path/to/output/bom.csv")

bom_with_options(output_path, **options)

Generates BOM with options.

board.export.bom_with_options(
    "/path/to/output/bom.csv",
    format="csv",
    group_by="value",       # or "footprint"
    include_dnp=False,
    sort_by="reference"
)

3D Model

step(output_path)

Exports 3D STEP model.

board.export.step("/path/to/output/board.step")

step_with_options(output_path, **options)

Exports STEP with options.

board.export.step_with_options(
    "/path/to/output/board.step",
    include_tracks=True,
    include_zones=True,
    include_silkscreen=True,
    substitute_models=True
)

DRC Report

drc_report(output_path)

Generates DRC report.

board.export.drc_report("/path/to/output/drc.txt")

PDF/SVG

pdf(output_path, layers)

Exports layers as PDF.

from kipy.board import BoardLayer

board.export.pdf(
    "/path/to/output/board.pdf",
    layers=[BoardLayer.BL_F_Cu, BoardLayer.BL_F_SilkS]
)

svg(output_path, layers)

Exports layers as SVG.

board.export.svg(
    "/path/to/output/board.svg",
    layers=[BoardLayer.BL_F_Cu]
)

Example: Full Manufacturing Export

from kipy import KiCad
import os

kicad = KiCad()
board = kicad.get_board()

# Create output directory
output_dir = "/path/to/fab_output"
os.makedirs(output_dir, exist_ok=True)

# Generate Gerbers
board.export.gerbers_with_options(
    output_dir,
    format="gerber_x2",
    use_protel_extensions=True
)
print("Gerbers generated")

# Generate drill files
board.export.drill_with_options(
    output_dir,
    format="excellon",
    units="mm",
    merge_pth_npth=False
)
print("Drill files generated")

# Generate position file
board.export.position_with_options(
    os.path.join(output_dir, "positions.csv"),
    format="csv",
    units="mm"
)
print("Position file generated")

# Generate BOM
board.export.bom_with_options(
    os.path.join(output_dir, "bom.csv"),
    format="csv",
    group_by="value"
)
print("BOM generated")

# Generate 3D model
board.export.step(os.path.join(output_dir, "board.step"))
print("3D model generated")

print(f"\nManufacturing files exported to: {output_dir}")

Example: Generate Review PDFs

from kipy.board import BoardLayer

# Front side review
board.export.pdf(
    "/path/to/review_front.pdf",
    layers=[
        BoardLayer.BL_F_Cu,
        BoardLayer.BL_F_SilkS,
        BoardLayer.BL_Edge_Cuts
    ]
)

# Back side review
board.export.pdf(
    "/path/to/review_back.pdf",
    layers=[
        BoardLayer.BL_B_Cu,
        BoardLayer.BL_B_SilkS,
        BoardLayer.BL_Edge_Cuts
    ]
)

# Assembly drawing
board.export.pdf(
    "/path/to/assembly.pdf",
    layers=[
        BoardLayer.BL_F_Fab,
        BoardLayer.BL_F_CrtYd,
        BoardLayer.BL_Edge_Cuts
    ]
)

File Extensions

Standard Gerber file extensions:

Layer	Extension
Front Copper	`.gtl` or `F_Cu.gbr`
Back Copper	`.gbl` or `B_Cu.gbr`
Front Mask	`.gts` or `F_Mask.gbr`
Back Mask	`.gbs` or `B_Mask.gbr`
Front Silk	`.gto` or `F_SilkS.gbr`
Back Silk	`.gbo` or `B_SilkS.gbr`
Edge Cuts	`.gm1` or `Edge_Cuts.gbr`
Drill	`.drl` or `.xln`