Reference manual

This document is Copyright © 2023-2024 by its contributors as listed below. You may distribute it and/or modify it under the terms of either the GNU General Public License (http://www.gnu.org/licenses/gpl.html), version 3 or later, or the Creative Commons Attribution License (http://creativecommons.org/licenses/by/3.0/), version 3.0 or later.

All trademarks within this guide belong to their legitimate owners.

Contributors

Graham Keeth

Feedback

The KiCad project welcomes feedback, bug reports, and suggestions related to the software or its documentation. For more information on how to sumbit feedback or report an issue, please see the instructions at https://www.kicad.org/help/report-an-issue/

1. Introduction to the KiCad Command-Line Interface

KiCad provides a command-line interface, which is available by running the kicad-cli binary. With the command-line interface, you can perform a number of actions on schematics, PCBs, symbols, and footprints in an automated fashion, such as plotting Gerber files from a PCB design or upgrading a symbol library from a legacy file format to a modern format.

Note
On macOS, the kicad-cli executable is located at /Applications/KiCad/KiCad.app/Contents/MacOS/kicad-cli.

2. kicad-cli commands

The kicad-cli command has 5 subcommands: fp, pcb, sch, sym, and version. Each subcommand may have its own subcommands and arguments. For example, to export Gerber files from a PCB you could run kicad-cli pcb export gerbers example.kicad_pcb.

You can add the --help or -h flag to see information about each subcommand. For example, running kicad-cli pcb -h prints usage information about the pcb subcommand, and kicad-cli pcb export gerbers -h prints usage information specifically for the pcb export gerbers subcommand.

2.1. Footprint

The fp subcommand exports footprints to another format or upgrades the footprint libraries to the current version of the KiCad footprint file format.

2.1.1. Footprint export

The fp export svg command exports one or more footprints from the specified library into SVG files.

Usage: kicad-cli fp export svg [--help] [--output OUTPUT_FILE] [--layers LAYER_LIST] [--define-var KEY=VALUE] [--theme VAR] [--footprint FOOTPRINT_NAME] [--black-and-white] INPUT_DIR

Positional arguments:

INPUT_DIR

Footprint library directory to export (.pretty).

Optional arguments:

-h, --help

Show help for the footprint SVG export command.

-o <output dir>, --output <output dir>

The output directory for the exported files. When this argument is not used, the files are exported to the current directory.

-l <layer list>, --layers <layer list>

A comma-separated list of layer names to export from the footprint, such as F.Cu,B.Cu. If no layers are given, all layers are exported.

-D <variable name>=<value>, --define-var <variable_name>=<value>

Add or override project variable definitions. Can be used multiple times to define multiple variables.

-t <theme name>, --theme <theme name>

The name of the theme to use for export. If no theme is given, the footprint editor’s currently selected theme is used.

--fp <footprint>, --footprint <footprint>

The name of the specific footprint to export from the library. When this argument is not used, all footprints in the library are exported.

--black-and-white

Export footprints in black and white.

2.1.2. Footprint upgrade

The fp upgrade command upgrades the the specified footprint library from a legacy footprint format to the native format for the current version of KiCad. If the input library is already in the current file format, no action is taken.

Usage: kicad-cli fp upgrade [-h] [--output OUTPUT_DIR] [--force] INPUT_DIR

Positional arguments:

INPUT_DIR

Footprint library directory to upgrade (.pretty).

Optional arguments:

-h, --help

Show help for the footprint upgrade command.

-o <output dir>, --output <output dir>

The output directory for the upgraded footprints. When this argument is not used, the upgraded footprints are saved over the original footprints.

--force

Re-save the input library even if it is already in the current file format.

2.2. PCB

The pcb command runs a design rule check or exports a board to various other file formats, including fabrication and 3D files.

2.2.1. PCB DRC

The pcb drc command runs a design rule check on a board and generates a report.

Usage: kicad-cli pcb drc [--help] [--output OUTPUT_FILE] [--define-var KEY=VALUE] [--format FORMAT] [--all-track-errors] [--schematic-parity] [--units UNITS] [--severity-all] [--severity-error] [--severity-warning] [--severity-exclusions] [--exit-code-violations] INPUT_FILE

Positional arguments:

INPUT_FILE

Board file to run DRC on.

-h, --help

Show help for the DRC command.

-o <output filename>, `--output <output filename>

Output filename for the generated DRC report. When this argument is not used, the output filename will be the same as the input file, with the .rpt or .json file extension, depending on the selected format.

-D <variable name>=<value>, --define-var <variable_name>=<value>

Add or override project variable definitions. Can be used multiple times to define multiple variables.

--format <format>

Report file format. Options are report (default) or json.

--all-track-errors

Report all errors for each track.

--schematic-parity

Test for parity between PCB and schematic.

--units <unit>

Units to use in the report. Options are mm (default), in, or mils.

--severity-all

Report all DRC violations. This is equivalent to using all of the other DRC severity options.

--severity-error

Report all error-level DRC violations. This can be combined with the other DRC severity options.

--severity-warning

Report all warning-level DRC violations. This can be combined with the other DRC severity options.

--severity-exclusions

Report all excluded DRC violations. This can be combined with the other DRC severity options.

--exit-code-violations

Return an exit code depending on whether or not DRC violations exist. The exit code is 0 if no violations are found, and 5 if any violations are found.

2.2.2. PCB drill file export

The pcb export drill command exports a drill file from a board.

Usage: kicad-cli pcb export drill [--help] [--output OUTPUT_DIR] [--format FORMAT] [--drill-origin DRILL_ORIGIN] [--excellon-zeros-format ZEROS_FORMAT] [--excellon-oval-format OVAL_FORMAT] [--excellon-units UNITS] [--excellon-mirror-y] [--excellon-min-header] [--excellon-separate-th] [--generate-map] [--map-format MAP_FORMAT] [--gerber-precision VAR] INPUT_FILE

Positional arguments:

INPUT_FILE

Board file to export.

Optional arguments:

-h, --help

Show help for the drill file export command.

-o <output dir>, --output <output dir>

The output directory for the drill file. When this argument is not used, the drill file is saved in the current directory.

--format <format>

The drill file format. Options are excellon (default) or gerber.

--drill-origin <origin>

The coordinate origin for the drill file. Options are absolute (default) to use the board’s absolute origin or plot to use the board’s drill/placement origin.

--excellon-zeros-format <format>

The zeros format for the drill file. Options are decimal (default), suppressleading, suppresstrailing, or keep. Only applies to Excellon format drill files.

--excellon-oval-format <format>

The command to use for oval holes. Options are route (default) or alternate.

-u <units>, --excellon-units <units>

The units for the drill file. Options are mm (default) or in. Only applies to Excellon format drill files.

--excellon-mirror-y

Mirror the drill file in the Y direction. Only applies to Excellon format drill files.

--excellon-min-header

Use a minimal header in the drill file. Only applies to Excellon format drill files.

--excellon-separate-th

Generate separate drill files for plated and non-plated through holes. Only applies to Excellon format drill files.

--excellon-oval-format <format>

Control the oval holes drill mode. Options are route (default) and alternate. Only applies to Excellon format drill files.

--generate-map

Generate a map file in addition to the drill file.

--map-format <format>

The map file format. Options are pdf (default), gerberx2, ps, dxf, or svg.

--gerber-precision <precision>

The precision (number of digits) for the drill file. Valid options are 5 or 6 (default). Only applies to Gerber format drill files.

2.2.3. PCB DXF export

The pcb export dxf command exports a board design to a DXF file.

Usage: kicad-cli pcb export dxf [--help] [--output OUTPUT_FILE] [--layers LAYER_LIST] [--drawing-sheet SHEET_PATH] [--define-var KEY=VALUE] [--exclude-refdes] [--exclude-value] [--use-contours] [--include-border-title] [--output-units UNITS] INPUT_FILE

Positional arguments:

INPUT_FILE

Board file to export.

Optional arguments:

-h, --help

Show help for the DXF export command.

-o <output filename>, --output <output filename>

The output filename. When this argument is not used, the output filename will be the same as the input file, with the .dxf file extension.

--drawing-sheet <sheet path>

Path to drawing sheet to use in plot, overriding the drawing sheet specified in the board file.

-D <variable name>=<value>, --define-var <variable_name>=<value>

Add or override project variable definitions. Can be used multiple times to define multiple variables.

-l <layer list>, --layers <layer list>

A comma-separated list of layer names to export from the footprint, such as F.Cu,B.Cu. At least one layer must be given.

--erd, --exclude-refdes

Exclude footprint reference designators from plot.

--ev, --exclude-value

Exclude footprint values from plot.

--uc, --use-contours

Plot graphic items using their contours.

-ibt, --include-border-title

Include sheet border and title block in plot.

--ou <unit>, --output-units <unit>

Output units. Options are mm or in (default).

2.2.4. PCB Gerber export: one layer per file

The pcb export gerbers command exports a board design to Gerber files, with one layer per file.

Note
Be aware that there are two distinct Gerber export commands, gerber and gerbers. The gerber command plots multiple PCB layers to a single Gerber file, while the gerbers command plots multiple Gerber files, with one PCB layer per file. The gerbers command is typically the correct command to use for having a PCB fabricated.

Usage: kicad-cli pcb export gerbers [--help] [--output OUTPUT_FILE] [--layers LAYER_LIST] [--drawing-sheet SHEET_PATH] [--define-var KEY=VALUE] [--exclude-refdes] [--exclude-value] [--include-border-title] [--no-x2] [--no-netlist] [--subtract-soldermask] [--disable-aperture-macros] [--use-drill-file-origin] [--precision PRECISION] [--no-protel-ext] [--common-layers COMMON_LAYER_LIST] [--board-plot-params] INPUT_FILE

Positional arguments:

INPUT_FILE

Board file to export.

Optional arguments:

-h, --help

Show help for the Gerber export command.

-o <output dir>, --output <output dir>

The output folder for the exported files. When this argument is not used, the files are exported to the current directory.

-l <layer list>, --layers <layer list>

A comma-separated list of layer names to plot from the board, such as F.Cu,B.Cu. If this argument is not used, all layers will be plotted.

--drawing-sheet <sheet path>

Path to drawing sheet to use in plot, overriding the drawing sheet specified in the board file.

-D <variable name>=<value>, --define-var <variable_name>=<value>

Add or override project variable definitions. Can be used multiple times to define multiple variables.

--erd, --exclude-refdes

Exclude footprint reference designators from plot.

--ev, --exclude-value

Exclude footprint values from plot.

--ibt, --include-border-title

Include the sheet border and title block.

--no-x2

Do not use the extended X2 format.

--no-netlist

Do not include netlist attributes.

--subtract-soldermask

Remove silkscreen from areas without soldermask.

--disable-aperture-macros

Disable aperture macros.

--use-drill-file-origin

Use drill/place file origin instead of absolute origin.

--precision <precision>

The precision (number of digits) for the Gerber files. Valid options are 5 or 6 (default).

--no-protel-ext

Use .gbr file extension instead of Protel file extensions (.gbl, .gtl, etc.).

--cl <layer list>, --common-layers <layer list>

A comma-separated list of layer names to plot on all layers, such as F.Cu,B.Cu.

--board-plot-params

Use the Gerber plot settings already configured in the board file.

2.2.5. PCB Gerber export: multiple layers per file

The pcb export gerber command exports one or more board layers to a single Gerber file.

Note
Be aware that there are two distinct Gerber export commands, gerber and gerbers. The gerber command plots multiple PCB layers to a single Gerber file, while the gerbers command plots multiple Gerber files, with one PCB layer per file. The gerbers command is typically the correct command to use for having a PCB fabricated.

Usage: kicad-cli pcb export gerber [--help] [--output OUTPUT_FILE] [--layers LAYER_LIST] [--drawing-sheet SHEET_PATH] [--define-var KEY=VALUE] [--exclude-refdes] [--exclude-value] [--include-border-title] [--no-x2] [--no-netlist] [--subtract-soldermask] [--disable-aperture-macros] [--use-drill-file-origin] [--precision PRECISION] [--no-protel-ext] INPUT_FILE

Positional arguments:

INPUT_FILE

Board file to export.

Optional arguments:

-h, --help

Show help for the Gerber export command.

-o <output filename>, --output <output filename>

The output filename. When this argument is not used, the output filename will be the same as the input file, with the .gbr file extension.

-l <layer list>, --layers <layer list>

A comma-separated list of layer names to plot from the board, such as F.Cu,B.Cu. All layers will be plotted in the output file. At least one layer must be given.

--drawing-sheet <sheet path>

Path to drawing sheet to use in plot, overriding the drawing sheet specified in the board file.

-D <variable name>=<value>, --define-var <variable_name>=<value>

Add or override project variable definitions. Can be used multiple times to define multiple variables.

--erd, --exclude-refdes

Exclude footprint reference designators from plot.

--ev, --exclude-value

Exclude footprint values from plot.

--ibt, --include-border-title

Include the sheet border and title block.

--no-x2

Do not use the extended X2 format.

--no-netlist

Do not include netlist attributes.

--subtract-soldermask

Remove silkscreen from areas without soldermask.

--disable-aperture-macros

Disable aperture macros.

--use-drill-file-origin

Use drill/place file origin instead of absolute origin.

--precision <precision>

The precision (number of digits) for the Gerber files. Valid options are 5 or 6 (default).

--no-protel-ext

Use .gbr file extension instead of Protel file extensions (.gbl, .gtl, etc.).

2.2.6. PCB GLB export

The pcb export glb command exports a board design to a GLB (binary GLTF) 3D file.

Usage: kicad-cli pcb export glb [--help] [--output OUTPUT_FILE] [--define-var KEY=VALUE] [--force] [--grid-origin] [--drill-origin] [--no-unspecified] [--no-dnp] [--subst-models] [--board-only] [--include-tracks] [--include-zones] [--min-distance MIN_DIST] [--user-origin VAR] INPUT_FILE

Positional arguments:

INPUT_FILE

Board file to export.

Optional arguments:

-h, --help

Show help for the GLB export command.

-o <output filename>, --output <output filename>

The output filename. When this argument is not used, the output filename will be the same as the input file, with the .glb file extension.

-D <variable name>=<value>, --define-var <variable_name>=<value>

Add or override project variable definitions. Can be used multiple times to define multiple variables.

-f, --force

Overwrite output file.

--grid-origin

Use grid origin as origin of output file.

--drill-origin

Use drill origin as origin of output file.

--no-unspecified

Exclude 3D models of components with 'unspecified' footprint type.

--no-dnp

Exclude 3D models of components with 'Do not populate' attribute.

--subst-models

Replace VRML models in footprints with STEP models of the same name, if they exist.

--board-only

Only include the board itself in the generated model; exclude all component models.

--include-tracks

Include tracks in export (time consuming).

--include-zones

Include zones in export (time consuming).

--min-distance <min distance>

Tolerance for considering two points to be in the same location. Default: 0.01mm.

--user-origin <output origin>

Specify a custom origin for the output file, with X and Y coordinates. For example, 1x1in, 1x1inch, or 25.4x25.4mm. The default unit is millimeters.

2.2.7. PCB IPC-2581 export

The pcb export ipc2581 command exports a board design in IPC-2581 format.

Usage: kicad-cli pcb export ipc2581 [--help] [--output OUTPUT_FILE] [--drawing-sheet SHEET_PATH] [--define-var KEY=VALUE] [--precision PRECISION] [--compress] [--version VAR] [--units VAR] [--bom-col-int-id FIELD_NAME] [--bom-col-mfg-pn FIELD_NAME] [--bom-col-mfg FIELD_NAME] [--bom-col-dist-pn FIELD_NAME] [--bom-col-dist FIELD_NAME] INPUT_FILE

INPUT_FILE

Board file to export.

Optional arguments:

-h, --help

Show help for the IPC-2581 export command.

-o <output filename>, --output <output filename>

The output filename. When this argument is not used, the output filename will be the same as the input file, with the .xml file extension.

--drawing-sheet <sheet path>

Path to drawing sheet to use in plot, overriding the drawing sheet specified in the board file.

-D <variable name>=<value>, --define-var <variable_name>=<value>

Add or override project variable definitions. Can be used multiple times to define multiple variables.

--precision <precision>

The precision (number of digits after the decimal separator) for the exported file. The default is 3.

--compress

Compress output file as a ZIP file.

--version <IPC-2581 standard version>

IPC-2581 standard version to use. Options are B or C (default).

--units

Units to use in export. Options are mm (default) or in.

--bom-col-int-id

Name of the part field to use for the Bill of Materials Internal ID column. This can be any footprint field, or blank to omit this column.

--bom-col-mfg-pn

Name of the part field to use for the Bill of Materials Manufacturer Part Number column. This can be any footprint field, or blank to omit this column.

--bom-col-mfg

Name of the part field to use for the Bill of Materials Manufacturer column. This can be any footprint field, or blank to omit this column.

--bom-col-dist-pn

Name of the part field to use for the Bill of Materials Distributor Part Number column. This can be any footprint field, or blank to omit this column.

--bom-col-dist

Name of the part field to use for the Bill of Materials Distributor column. This can be any footprint field, or blank to omit this column.

2.2.8. PCB PDF export

The pcb export pdf command exports a board design to a PDF file.

Usage: kicad-cli pcb export pdf [--help] [--output OUTPUT_FILE] [--layers LAYER_LIST] [--drawing-sheet SHEET_PATH] [--define-var KEY=VALUE] [--mirror] [--exclude-refdes] [--exclude-value] [--include-border-title] [--negative] [--black-and-white] [--theme THEME_NAME] [--drill-shape-opt VAR] INPUT_FILE

Positional arguments:

INPUT_FILE

Board file to export.

Optional arguments:

-h, --help

Show help for the PDF export command.

-o <output filename>, --output <output filename>

The output filename. When this argument is not used, the output filename will be the same as the input file, with the .pdf file extension.

-l <layer list>, --layers <layer list>

A comma-separated list of layer names to export from the board, such as F.Cu,B.Cu. At least one layer must be given.

--drawing-sheet <sheet path>

Path to drawing sheet to use in plot, overriding the drawing sheet specified in the board file.

-D <variable name>=<value>, --define-var <variable_name>=<value>

Add or override project variable definitions. Can be used multiple times to define multiple variables.

-m, --mirror

Mirror the board. This can be useful for showing bottom layers.

--erd, --exclude-refdes

Exclude footprint reference designators from plot.

--ev, --exclude-value

Exclude footprint values from plot.

--ibt, --include-border-title

Include the sheet border and title block.

-n, --negative

Plot in negative.

--black-and-white

Plot in black and white.

-t <theme name>, --theme <theme name>

The name of the theme to use for export. If no theme is given, the board editor’s currently selected theme is used.

--drill-shape-opt

The shape of drill marks in the plot. Options are 0 for no drill marks, 1 for small marks, or 2 for actual size marks (default).

2.2.9. PCB position file export

The pcb export pos command exports a position file from a board design.

Usage: kicad-cli pcb export pos [--help] [--output OUTPUT_FILE] [--side VAR] [--format FORMAT] [--units UNITS] [--bottom-negate-x] [--use-drill-file-origin] [--smd-only] [--exclude-fp-th] [--exclude-dnp] [--gerber-board-edge] INPUT_FILE

Positional arguments:

INPUT_FILE

Board file to export.

Optional arguments:

-h, --help

Show help for the position file export command.

-o <output filename>, --output <output filename>

The output filename. When this argument is not used, the output filename will be the same as the input file, with the .pos file extension.

--side <side>

The side of the board to export. Options are front, back, or both (default). Gerber format does not support both.

--format <format>

The position file format. Options are ascii (default), csv, or gerber.

--units <unit>

Units for position file. Options are in (default) or mm. This option has no effect for Gerber format.

--bottom-negate-x

Use negative X coordinates for footprints on the bottom layer. This option has no effect for Gerber format.

--use-drill-file-origin

Use drill/place file origin instead of absolute origin. This option has no effect for Gerber format.

--smd-only

Include only surface-mount components. This option has no effect for Gerber format.

--exclude-fp-th

Exclude all footprints with through-hole pads. This option has no effect for Gerber format.

--exclude-dnp

Exclude all footprints with "Do not populate" attribute.

--gerber-board-edge

Include board edge layer in export (Gerber format only).

2.2.10. PCB STEP export

The pcb export step command exports a board design to a STEP file.

Usage: kicad-cli pcb export step [--help] [--output OUTPUT_FILE] [--define-var KEY=VALUE] [--force] [--grid-origin] [--drill-origin] [--no-unspecified] [--no-dnp] [--subst-models] [--board-only] [--include-tracks] [--include-zones] [--min-distance MIN_DIST] [--no-optimize-step] [--user-origin VAR] INPUT_FILE

Positional arguments:

INPUT_FILE

Board file to export.

Optional arguments:

-h, --help

Show help for the STEP file export command.

-o <output filename>, --output <output filename>

The output filename. When this argument is not used, the output filename will be the same as the input file, with the .step file extension.

-D <variable name>=<value>, --define-var <variable_name>=<value>

Add or override project variable definitions. Can be used multiple times to define multiple variables.

-f, --force

Overwrite output file.

--grid-origin

Use grid origin as origin of output file.

--drill-origin

Use drill origin as origin of output file.

--no-unspecified

Exclude 3D models of components with 'unspecified' footprint type.

--no-dnp

Exclude 3D models of components with 'Do not populate' attribute.

--subst-models

Replace VRML models in footprints with STEP models of the same name, if they exist.

--board-only

Only include the board itself in the generated model; exclude all component models.

--include-tracks

Include tracks in export (time consuming).

--include-zones

Include zones in export (time consuming).

--min-distance <min distance>

Tolerance for considering two points to be in the same location. Default: 0.01mm.

--no-optimize-step

Do not optimize STEP file. This enables writing parametric curves, which reduces file sizes and write/read times, but may reduce compatibility with other software.

--user-origin <output origin>

Specify a custom origin for the output file, with X and Y coordinates. For example, 1x1in, 1x1inch, or 25.4x25.4mm. The default unit is millimeters.

2.2.11. PCB SVG export

The pcb export svg command exports a board design to an SVG file.

Usage: kicad-cli pcb export svg [--help] [--output OUTPUT_FILE] [--layers LAYER_LIST] [--drawing-sheet SHEET_PATH] [--define-var KEY=VALUE] [--mirror] [--theme THEME_NAME] [--negative] [--black-and-white] [--page-size-mode MODE] [--exclude-drawing-sheet] [--drill-shape-opt SHAPE_OPTION] INPUT_FILE

Positional arguments:

INPUT_FILE

Board file to export.

Optional arguments:

-h, --help

Show help for the SVG file export command.

-o <output filename>, --output <output filename>

The output filename. When this argument is not used, the output filename will be the same as the input file, with the .svg file extension.

-l <layer list>, --layers <layer list>

A comma-separated list of layer names to export from the board, such as F.Cu,B.Cu. At least one layer must be given.

--drawing-sheet <sheet path>

Path to drawing sheet to use in plot, overriding the drawing sheet specified in the board file.

-D <variable name>=<value>, --define-var <variable_name>=<value>

Add or override project variable definitions. Can be used multiple times to define multiple variables.

-m, --mirror

Mirror the board. This can be useful for showing bottom layers.

-t <theme name>, --theme <theme name>

The name of the theme to use for export. If no theme is given, the board editor’s currently selected theme is used.

-n, --negative

Plot in negative.

--black-and-white

Plot in black and white.

--page-size-mode <mode>

Set page sizing mode. Options are 0 (default), 1, or 2. 0 sets the output page size to fit the entire sheet, including drawing sheet frame and title block. 1 sets the output page size to match the current page size. 2 sets the output page size to the size of the board itself.

--exclude-drawing-sheet

Plot SVG without a drawing sheet.

--drill-shape-opt

The shape of drill marks in the plot. Options are 0 for no drill marks, 1 for small marks, or 2 for actual size marks (default).

2.2.12. PCB VRML export

The pcb export vrml command exports a board design to a VRML 3D file.

Usage: kicad-cli pcb export vrml [--help] [--output OUTPUT_FILE] [--define-var KEY=VALUE] [--force] [--user-origin VAR] [--units VAR] [--models-dir VAR] [--models-relative] INPUT_FILE

Positional arguments:

INPUT_FILE

Board file to export.

Optional arguments:

-h, --help

Show help for the VRML export command.

-o <output filename>, --output <output filename>

The output filename. When this argument is not used, the output filename will be the same as the input file, with the .wrl file extension.

-D <variable name>=<value>, --define-var <variable_name>=<value>

Add or override project variable definitions. Can be used multiple times to define multiple variables.

-f, --force

Overwrite output file.

--user-origin <output origin>

Specify a custom origin for the output file, with X and Y coordinates. For example, 1x1in, 1x1inch, or 25.4x25.4mm. The default unit is millimeters. If this option is not given, the board center is used.

--units <units>

Units to use in the output file. Options are mm, m, in (default), or tenths (tenths of an inch).

--models-dir <output model directory>

Name of output directory to copy component models into. If not used, component models are embedded into the output file.

--models-relative

With --models-dir, use relative paths in the output file.

2.3. Schematic

The sch command runs an electrical rule check, exports a schematic to various other file formats, or exports a bill of materials or netlist. Each subcommand has its own options.

2.3.1. Schematic ERC

The sch erc command runs an electrical rule check on a schematic and generates a report.

Usage: kicad-cli sch erc [--help] [--output OUTPUT_FILE] [--define-var KEY=VALUE] [--format VAR] [--units VAR] [--severity-all] [--severity-error] [--severity-warning] [--severity-exclusions] [--exit-code-violations] INPUT_FILE

Positional arguments:

INPUT_FILE

Schematic file to run ERC on.

-h, --help

Show help for the ERC command.

-o <output filename>, `--output <output filename>

Output filename for the generated ERC report. When this argument is not used, the output filename will be the same as the input file, with the .rpt or .json file extension, depending on the selected format.

-D <variable name>=<value>, --define-var <variable_name>=<value>

Add or override project variable definitions. Can be used multiple times to define multiple variables.

--format <format>

Report file format. Options are report (default) or json.

--units <unit>

Units to use in the report. Options are mm (default), in, or mils.

--severity-all

Report all ERC violations. This is equivalent to using all of the other ERC severity options.

--severity-error

Report all error-level ERC violations. This can be combined with the other ERC severity options.

--severity-warning

Report all warning-level ERC violations. This can be combined with the other ERC severity options.

--severity-exclusions

Report all excluded ERC violations. This can be combined with the other ERC severity options.

--exit-code-violations

Return an exit code depending on whether or not ERC violations exist. The exit code is 0 if no violations are found, and 5 if any violations are found.

2.3.2. Schematic bill of materials export

The sch export bom command exports a BOM from a schematic. The BOM export has a number of options for controlling the format and included fields. This export method is equivalent to exporting a BOM from the symbol fields table.

Note
To export a BOM using the legacy XML and Python BOM script workflow, use the sch export python-bom command.

Usage: kicad-cli sch export bom [--help] [--output OUTPUT_FILE] [--preset PRESET] [--format-preset FMT_PRESET] [--fields FIELDS] [--labels LABELS] [--group-by GROUP_BY] [--sort-field SORT_BY] [--sort-asc] [--filter FILTER] [--exclude-dnp] [--field-delimiter FIELD_DELIM] [--string-delimiter STR_DELIM] [--ref-delimiter REF_DELIM] [--ref-range-delimiter REF_RANGE_DELIM] [--keep-tabs] [--keep-line-breaks] INPUT_FILE

Positional arguments:

INPUT_FILE

Schematic file to export.

Optional arguments:

-h, --help

Shows help message and exits

-o <output filename>, --output <output filename>

The output filename. When this argument is not used, the output filename will be the same as the input file, with a .csv file extension.

--preset <preset>

Use a named BOM preset setting from the schematic, e.g. "Grouped By Value".

--format-preset <format preset>

Use a named BOM format preset setting from the schematic, e.g. CSV.

--fields <fields>

An ordered list of fields to export. * includes all fields. Special symbol fields such as DNP or Exclude from board can be accessed with ${DNP} or ${EXCLUDE_FROM_BOARD}, respectively (see the text variable documentation for a list of fields). Default: "Reference,Value,Footprint,${QUANTITY},${DNP}".

--labels <labels>

An ordered list of labels to apply the exported fields (default: "Refs,Value,Footprint,Qty,DNP").

--group-by <fields>

Fields to group references by when field values match.

--sort-field <fields>

Field name to sort by (default: "Reference").

--sort-asc

If given, sort in ascending order. If not given, sort in descending order.

--filter <filter>

Filter string to remove output lines.

--exclude-dnp

Exclude symbols with the "Do not populate" attribute.

--field-delimiter <delimiter>

Separator between output fields/columns (default: ",").

--string-delimiter <delimiter>

Character to surround fields with (none by default).

--ref-delimiter <delimiter>

Character to place between individual references (default: ",").

--ref-range-delimiter <delimiter>

Character to place in ranges of references (default: "-"). Leave blank for no ranges.

--keep-tabs

Keep tab characters from input fields. Stripped by default.

--keep-line-breaks

Keep line break characters from input fields. Stripped by default.

2.3.3. Schematic DXF export

The sch export dxf command exports a schematic to a DXF file. Each sheet in the design is exported to its own file.

Usage: kicad-cli sch export dxf [--help] [--output OUTPUT_DIR] [--drawing-sheet SHEET_PATH] [--define-var KEY=VALUE] [--theme THEME_NAME] [--black-and-white] [--exclude-drawing-sheet] [--pages PAGE_LIST] INPUT_FILE

Positional arguments:

INPUT_FILE

Schematic file to export.

Optional arguments:

-h, --help

Show help for the DXF file export command.

-o <output dir>, --output <output dir>

The output folder for the exported files. When this argument is not used, the files are exported to the current directory.

--drawing-sheet <sheet path>

Path to drawing sheet to use in plot, overriding the drawing sheet specified in the schematic file.

-D <variable name>=<value>, --define-var <variable_name>=<value>

Add or override project variable definitions. Can be used multiple times to define multiple variables.

-t <theme name>, --theme <theme name>

The name of the theme to use for export. If no theme is given, the schematic editor’s currently selected theme is used.

-b, --black-and-white

Export schematic in black and white.

-e, --exclude-drawing-sheet

Plot DXF without a drawing sheet.

--pages <page list>

Comma-separated list of pages to export. Blank or unspecified means all pages.

2.3.4. Schematic HPGL export

The sch export hpgl command exports a schematic to an HPGL file for a pen plotter. Each sheet in the design is exported to its own file.

Usage: kicad-cli sch export hpgl [--help] [--output OUTPUT_DIR] [--drawing-sheet SHEET_PATH] [--define-var KEY=VALUE] [--exclude-drawing-sheet] [--pages PAGE_LIST] [--pen-size PEN_SIZE] [--origin ORIGIN] INPUT_FILE

Positional arguments:

INPUT_FILE

Schematic file to export.

Optional arguments:

-h, --help

Show help for the HPGL file export command.

-o <output dir>, --output <output dir>

The output folder for the exported files. When this argument is not used, the files are exported to the current directory.

--drawing-sheet <sheet path>

Path to drawing sheet to use in plot, overriding the drawing sheet specified in the schematic file.

-D <variable name>=<value>, --define-var <variable_name>=<value>

Add or override project variable definitions. Can be used multiple times to define multiple variables.

-e, --exclude-drawing-sheet

Plot HPGL without a drawing sheet.

--pages <page list>

Comma-separated list of pages to export. Blank or unspecified means all pages.

-p <pen size>, --pen-size <pen size>

Set the pen width. The default pen size is 0.5 mm.

-r <origin>, --origin <origin>

Set plotter origin and scale. Options are 0, 1 (default), 2, or 3. 0 sets the origin to the bottom left and uses plotter units. 1 sets the origin to the center and uses plotter units. 2 scales to the page, and 3 scales to the content within the page.

2.3.5. Schematic netlist export

The sch export netlist command exports a netlist in various formats from a schematic.

Usage: kicad-cli sch export netlist [--help] [--output OUTPUT_FILE] [--format FORMAT] INPUT_FILE

Positional arguments:

INPUT_FILE

Schematic file to export.

Optional arguments:

-h, --help

Show help for the netlist export command.

-o <output filename>, --output <output filename>

The output filename. When this argument is not used, the output filename will be the same as the input file, with a .net file extension.

-f <format>, --format <format>

The netlist output format. Options are kicadsexpr (default), kicadxml, cadstar, orcadpcb2, spice, or spicemodel.

2.3.6. Schematic PDF export

The sch export pdf command exports a schematic to a PDF file. Each sheet in the design is exported to its own page in the PDF file.

Usage: kicad-cli sch export pdf [--help] [--output OUTPUT_FILE] [--drawing-sheet SHEET_PATH] [--define-var KEY=VALUE] [--theme THEME_NAME] [--black-and-white] [--exclude-drawing-sheet] [--exclude-pdf-property-popups] [--no-background-color] [--pages PAGE_LIST] INPUT_FILE

Positional arguments:

INPUT_FILE

Schematic file to export.

Optional arguments:

-h, --help

Show help for the PDF file export command.

-o <output filename>, --output <output filename>

The output filename. When this argument is not used, the output filename will be the same as the input file, with a .pdf file extension.

--drawing-sheet <sheet path>

Path to drawing sheet to use in plot, overriding the drawing sheet specified in the schematic file.

-D <variable name>=<value>, --define-var <variable_name>=<value>

Add or override project variable definitions. Can be used multiple times to define multiple variables.

-t <theme name>, --theme <theme name>

The name of the theme to use for export. If no theme is given, the schematic editor’s currently selected theme is used.

-b, --black-and-white

Export schematic in black and white.

-e, --exclude-drawing-sheet

Plot PDF without a drawing sheet.

--exclude-pdf-property-popups

Do not generate property popups in PDF.

-n, --no-background-color

Export schematic without a background color, regardless of theme.

--pages <page list>

Comma-separated list of pages to export. Blank or unspecified means all pages.

2.3.7. Schematic PostScript export

The sch export ps command exports a schematic to a PostScript file. Each sheet in the design is exported to its own file.

Usage: kicad-cli sch export ps [--help] [--output OUTPUT_DIR] [--drawing-sheet SHEET_PATH] [--define-var KEY=VALUE] [--theme THEME_NAME] [--black-and-white] [--exclude-drawing-sheet] [--no-background-color] [--pages PAGE_LIST] INPUT_FILE

Positional arguments:

INPUT_DIR

Schematic file to export.

Optional arguments:

-h, --help

Show help for the PS file export command.

-o <output dir>, --output <output dir>

The output folder for the exported files. When this argument is not used, the files are exported to the current directory.

--drawing-sheet <sheet path>

Path to drawing sheet to use in plot, overriding the drawing sheet specified in the schematic file.

-D <variable name>=<value>, --define-var <variable_name>=<value>

Add or override project variable definitions. Can be used multiple times to define multiple variables.

-t <theme name>, --theme <theme name>

The name of the theme to use for export. If no theme is given, the schematic editor’s currently selected theme is used.

-b, --black-and-white

Export schematic in black and white.

-e, --exclude-drawing-sheet

Plot PS without a drawing sheet.

-n, --no-background-color

Export schematic without a background color, regardless of theme.

--pages <page list>

Comma-separated list of pages to export. Blank or unspecified means all pages.

2.3.8. Schematic bill of materials export (legacy BOM scripts)

The sch export python-bom command exports an XML BOM file from a schematic. The XML BOM file can then be processed into your desired BOM format using a custom script or one of the scripts described in the schematic BOM export documentation.

Usage: kicad-cli sch export python-bom [--help] [--output OUTPUT_FILE] INPUT_FILE

Positional arguments:

INPUT_FILE

Schematic file to export.

Optional arguments:

-h, --help

Show help for the BOM export command.

-o <output filename>, --output <output filename>

The output filename. When this argument is not used, the output filename will be the same as the input file, with a -bom.xml suffix and file extension.

2.3.9. Schematic SVG export

The sch export svg command export a schematic to an SVG file. Each sheet in the design is exported to its own file.

Usage: kicad-cli sch export svg [--help] [--output OUTPUT_DIR] [--drawing-sheet SHEET_PATH] [--define-var KEY=VALUE] [--theme THEME_NAME] [--black-and-white] [--exclude-drawing-sheet] [--no-background-color] [--pages PAGE_LIST] INPUT_FILE

Positional arguments:

INPUT_FILE

Schematic file to export.

Optional arguments:

-h, --help

Show help for the SVG file export command.

-o <output dir>, --output <output dir>

The output folder for the exported files. When this argument is not used, the files are exported to the current directory.

--drawing-sheet <sheet path>

Path to drawing sheet to use in plot, overriding the drawing sheet specified in the schematic file.

-D <variable name>=<value>, --define-var <variable_name>=<value>

Add or override project variable definitions. Can be used multiple times to define multiple variables.

-t <theme name>, --theme <theme name>

The name of the theme to use for export. If no theme is given, the schematic editor’s currently selected theme is used.

-b, --black-and-white

Export schematic in black and white.

-e, --exclude-drawing-sheet

Plot SVG without a drawing sheet.

-n, --no-background-color

Export schematic without a background color, regardless of theme.

--pages <page list>

Comma-separated list of pages to export. Blank or unspecified means all pages.

2.4. Symbol

The sym subcommand exports symbols to another format or upgrades symbol libraries to the current version of the KiCad symbol file format.

2.4.1. Symbol export

The sym export svg command exports one or more symbols from the specified library into SVG files.

Usage: kicad-cli sym export svg [--help] [--output OUTPUT_DIR] [--theme THEME_NAME] [--symbol SYMBOL] [--black-and-white] [--include-hidden-pins] [--include-hidden-fields] INPUT_FILE

Positional arguments:

INPUT_FILE

Symbol library file to use for export.

Optional arguments:

-h, --help

Show help for the symbol SVG export command.

-o <output dir>, --output <output dir>

The output folder for the exported files. When this argument is not used, the files are exported to the current directory.

-t <theme name>, --theme <theme name>

The name of the theme to use for export. If no theme is given, the symbol editor’s currently selected theme is used.

-s <symbol name>, --symbol <symbol name>

The specific symbol to export from the library. When this argument is not used, all symbols in the library are exported.

--black-and-white

Export symbols in black and white.

--include-hidden-pins

Export hidden pins in the exported SVG.

--include-hidden-fields

Export hidden symbol fields in the exported SVG.

2.4.2. Symbol upgrade

The sym upgrade command upgrades the the specified symbol library from a legacy symbol format to the native format for the current version of KiCad. If the input library is already in the current file format, no action is taken.

Usage: kicad-cli sym upgrade [--help] [--output OUTPUT_FILE] [--force] INPUT_FILE

Positional arguments:

INPUT_FILE

Symbol library to upgrade.

Optional arguments:

-h, --help

Show help for the symbol upgrade command.

-o <output filename>, --output <output filename>

The output filename for the upgraded symbol library. When this argument is not used, the upgraded symbol library is saved over the original library.

--force

Re-save the input library even if it is already in the current file format.

2.5. Version

The version subcommand prints the KiCad version. Without any arguments, it simply prints the version number, for example 7.0.7. You can print the version in several other formats using the --format argument.

Note
Use kicad-cli version --format about for version information to include when submitting bug reports or feature requests on Gitlab.

Usage: kicad-cli version [--help] [--format VAR]

Optional arguments:

--format <format>

Format of the version number. Options are plain (default), commit, or about. plain prints the version number (e.g. 7.0.7), which is the default if the --format argument is not used. commit prints the hash of the git commit for the build of KiCad you are using. about prints the full version information, including library versions and basic system information. You can use the about version information in bug reports.