/pcb-export

pcb — board exports and render

Input is a .kicad_pcb file. pcb drc is documented separately in references/checks.md.

pcb export gerbers — fabrication gerbers (one layer per file)

kicad-cli pcb export gerbers [-o OUTPUT_DIR] [-l LAYER_LIST] [options] INPUT.kicad_pcb

--output is a directory. Preferred over the deprecated singular gerber.

Key flags:

• --layers / -l — comma-separated layers, e.g. F.Cu,B.Cu,F.SilkS,B.SilkS,F.Mask,B.Mask,Edge.Cuts
• --common-layers — layers added to every output file
• --precision 5|6 — Gerber coordinate precision
• --no-x2 (X1 attributes instead of X2), --no-netlist (omit netlist attributes), --no-protel-ext (don't use Protel filename extensions)
• --subtract-soldermask, --use-drill-file-origin, --disable-aperture-macros
• --board-plot-params — use plot params stored in the board file (overrides --layers)
• DNP/fab: --exclude-refdes, --exclude-value, --include-border-title, --sketch-pads-on-fab-layers, --hide-DNP-footprints-on-fab-layers, --sketch-DNP-footprints-on-fab-layers, --crossout-DNP-footprints-on-fab-layers, --plot-invisible-text

kicad-cli pcb export gerbers -o gerbers/ \
  -l "F.Cu,B.Cu,F.Paste,B.Paste,F.SilkS,B.SilkS,F.Mask,B.Mask,Edge.Cuts" \
  board.kicad_pcb

pcb export gerber (singular, single multi-layer file) is deprecated in 9.0, removed in 10.0. Use gerbers.

pcb export drill

kicad-cli pcb export drill [-o OUTPUT_DIR] [options] INPUT.kicad_pcb — --output is a directory.

• --format excellon|gerber (default excellon)
• --drill-origin absolute|plot
• --excellon-units mm|in (-u)
• --excellon-zeros-format decimal|suppressleading|suppresstrailing|keep
• --excellon-oval-format route|alternate
• --excellon-mirror-y, --excellon-min-header, --excellon-separate-th (separate plated/non-plated holes)
• --generate-map + --map-format pdf|gerberx2|ps|dxf|svg — also produce a drill map
• --gerber-precision

kicad-cli pcb export drill -o gerbers/ --excellon-separate-th \
  --generate-map --map-format pdf board.kicad_pcb

pcb export pos — pick-and-place / position file

kicad-cli pcb export pos [-o OUTPUT_FILE] [options] INPUT.kicad_pcb — --output is a file.

• --side front|back|both
• --format ascii|csv|gerber
• --units in|mm
• --smd-only, --exclude-fp-th (exclude through-hole), --exclude-dnp
• --bottom-negate-x, --use-drill-file-origin, --gerber-board-edge

kicad-cli pcb export pos -o board-pos.csv --side both --format csv --units mm --exclude-dnp board.kicad_pcb

pcb export pdf

--output is a file. Choose a mode:

• --mode-single — all selected layers on one page
• --mode-separate — one PDF per layer
• --mode-multipage — one PDF, one page per layer

Other flags: --layers/-l, --mirror/-m, --negative/-n, --black-and-white, --theme/-t, --include-border-title, --subtract-soldermask, --drill-shape-opt, --common-layers, DNP/fab flags, --plot-invisible-text.

kicad-cli pcb export pdf -l "F.Cu,B.Cu,Edge.Cuts" --mode-multipage -o board.pdf board.kicad_pcb

pcb export svg

--layers is optional (default = all layers). --mode-single (single file, --output is full path) vs --mode-multi (one SVG per layer). Extras: --page-size-mode 0|1|2, --fit-page-to-board, --mirror, --negative, --black-and-white, --theme, --exclude-drawing-sheet, --drill-shape-opt, --common-layers.

pcb export dxf

--layers required. --output-units mm|in (--ou), --use-contours (--uc), --use-drill-origin (--udo), --mode-single/--mode-multi, --include-border-title, plus DNP/fab flags.

3D model exports

pcb export step — STEP (--output is a file)

• --subst-models — substitute STEP/IGS models of the same name for VRML models
• --board-only — board only, no components; --no-components — exclude components
• --no-dnp — exclude DNP models; --no-unspecified — exclude "unspecified" components
• --include-tracks, --include-pads, --include-zones, --include-inner-copper, --include-silkscreen, --include-soldermask (tracks/zones are "time consuming")
• --user-origin VAR (e.g. 25.4x25.4mm, 1x1in), --grid-origin, --drill-origin
• --min-distance MIN_DIST (point-merge tolerance, default 0.01mm)
• --cut-vias-in-body, --no-board-body, --fuse-shapes, --fill-all-vias, --component-filter VAR, --net-filter VAR
• --no-optimize-step (parametric curves; smaller, less compatible), --force/-f (overwrite)

kicad-cli pcb export step --subst-models --no-dnp --force -o board.step board.kicad_pcb

pcb export glb — binary glTF

Same option set as step minus --no-optimize-step.

pcb export vrml

• --units mm|m|in|tenths
• --models-dir DIR, --models-relative — where component models are written/referenced
• --no-dnp, --no-unspecified, --user-origin, --force

Other mesh/CAD formats

pcb export brep, stl, ply, gencad, xao exist and share most of the step/glb 3D options. gencad adds --flip-bottom-pads/-f, --unique-pins, --unique-footprints, --use-drill-origin, --store-origin-coord. Confirm obscure flags with -h on the target install.

Assembly / data exchange

pcb export ipc2581

• --version B|C, --units mm|in, --precision, --compress
• --bom-col-int-id, --bom-col-mfg-pn, --bom-col-mfg, --bom-col-dist-pn, --bom-col-dist — map schematic field names to IPC-2581 BOM columns

pcb export ipcd356

kicad-cli pcb export ipcd356 [-o OUTPUT_FILE] INPUT.kicad_pcb — IPC-D-356 netlist (minimal options).

pcb export odb — ODB++

• --compression none|zip|tgz, --units mm|in, --precision

pcb render — raytraced PNG/JPEG

Output format from the --output extension (.png/.jpg).

Defaults: --width 1600, --height 900, --side top (also bottom/left/right/front/back), --background default (transparent for PNG, opaque for JPG; force transparent/opaque), --quality basic (high/user), --preset follow_plot_settings, --zoom 1.

Camera: --rotate X,Y,Z, --pan X,Y,Z, --pivot X,Y,Z, --perspective, --floor. Lights: --light-top/-bottom/-side/-camera COLOR, --light-side-elevation ANGLE.

kicad-cli pcb render --side top --quality high -w 3000 -o render.png board.kicad_pcb