INPUT_DIR

Footprint library directory to export (.pretty).

-h, --help

Show help for the footprint SVG export command.

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

The output folder for the exported files. One file is output for each layer of each footprint in the library. When --output 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. Layer names can be specified as canonical layer names (F.Cu, In.1, F.Fab, etc.) or as user-defined (custom) layer names, but user-defined layer names are matched first.

-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.

--sp, --sketch-pads-on-fab-layers

Draw pad outlines and their numbers on front and back fab layers.

--hdnp, --hide-DNP-footprints-on-fab-layers

Don’t plot text and graphics of DNP footprints on fab layers.

--sdnp, --sketch-DNP-footprints-on-fab-layers

Plot graphics of DNP footprints in sketch mode on fab layers.

--cdnp, --crossout-DNP-footprints-on-fab-layers

Plot an "X" over the courtyard of DNP footprints on fab layers, and strikeout their reference designators.

--black-and-white

Export footprints in black and white.

INPUT_DIR

Footprint library directory to upgrade. For KiCad format footprint libraries, this is the .pretty directory, not a .kicad_mod file.

-h, --help

Show help for the upgrade command.

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

The output directory for the upgraded footprints. When --output 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.

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 --output 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.

--refill-zones

Refill all zones before running DRC. The board will not be saved after refilling zones unless --save-board is also used.

--save-board

Save the board after running DRC. The board will not be saved unless --refill-zones is also used.

INPUT_FILE

Board file to export.

-h, --help

Show help for the 3D PDF export command.

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

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

--no-unspecified

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

--no-dnp

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

--grid-origin

Use grid origin as origin of output file.

--drill-origin

Use drill origin as origin of output file.

--subst-models

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

--board-only

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

--cut-vias-in-body

Cut via holes in board body even if conductor layers are not exported.

--no-board-body

Exclude board body.

--no-components

Exclude 3D models for components.

--component-filter <reference designator list>

Only include component 3D models matching this list of reference designators (comma-separated, wildcards supported)

--include-tracks

Include tracks and vias on outer conductor layers in export (time consuming).

--include-pads

Include pads in export (time consuming).

--include-zones

Include zones in export (time consuming).

--include-inner-copper

Include elements on inner conductor layers in export.

--include-silkscreen

Include silkscreen graphics in export as a set of flat faces.

--include-soldermask

Include solder mask layers in export as a set of flat faces.

--fuse-shapes

Fuse overlapping geometry together in export (time consuming).

--fill-all-vias

Don’t cut via holes in conductor layers.

--no-extra-pad-thickness

Disable adding additional metal thickness to pads. When not used, pads have 0.005mm added to their metal thickness, which causes pads to be separate faces in the exported model, distinct from the surrounding metal.

--min-distance <min distance>

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

--net-filter <net filter>

Only include copper items belonging to nets matching this wildcard.

--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.

INPUT_FILE

Board file to export.

-h, --help

Show help for the BREP export command.

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

The output filename. When --output is not used, the output filename will be the same as the input file, with the .brep 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.

--no-unspecified

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

--no-dnp

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

--grid-origin

Use grid origin as origin of output file.

--drill-origin

Use drill origin as origin of output file.

--subst-models

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

--board-only

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

--cut-vias-in-body

Cut via holes in board body even if conductor layers are not exported.

--no-board-body

Exclude board body.

--no-components

Exclude 3D models for components.

--component-filter <reference designator list>

Only include component 3D models matching this list of reference designators (comma-separated, wildcards supported)

--include-tracks

Include tracks and vias on outer conductor layers in export (time consuming).

--include-pads

Include pads in export (time consuming).

--include-zones

Include zones in export (time consuming).

--include-inner-copper

Include elements on inner conductor layers in export.

--include-silkscreen

Include silkscreen graphics in export as a set of flat faces.

--include-soldermask

Include solder mask layers in export as a set of flat faces.

--fuse-shapes

Fuse overlapping geometry together in export (time consuming).

--fill-all-vias

Don’t cut via holes in conductor layers.

--no-extra-pad-thickness

Disable adding additional metal thickness to pads. When not used, pads have 0.005mm added to their metal thickness, which causes pads to be separate faces in the exported model, distinct from the surrounding metal.

--min-distance <min distance>

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

--net-filter <net filter>

Only include copper items belonging to nets matching this wildcard.

--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.

INPUT_FILE

Board file to export.

-h, --help

Show help for the drill file export command.

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

The output directory for the drill file(s). When --output is not used, the drill file(s) are 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>

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

-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.

--generate-map

Generate a map file in addition to the drill file.

--generate-report

Generate a report file listing all drill hits.

--report-path <report filename>

The output filename for the drill report file. When --report-path is not used, the report filename will be the same as the input file, with the -drill.rpt suffix and file extension.

--generate-tenting

Generate separate drill files for tented drill hits. Only applies to Gerber X2 format drill files.

--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.

INPUT_FILE

Board file to export.

-h, --help

Show help for the DXF export command.

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

The output folder or filename for the exported files. When --mode-single is used, this is the output filename. If --output is not used, the output filename will be the same as the input file, with the .pdf file extension. When --mode-multi is used, this is the output directory. If --output 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. At least one layer must be given. Layer names can be specified as canonical layer names (F.Cu, In.1, F.Fab, etc.) or as user-defined (custom) layer names, but user-defined layer names are matched first.

--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.

--sp, --sketch-pads-on-fab-layers

Draw pad outlines and their numbers on front and back fab layers.

--hdnp, --hide-DNP-footprints-on-fab-layers

Don’t plot text and graphics of DNP footprints on fab layers.

--sdnp, --sketch-DNP-footprints-on-fab-layers

Plot graphics of DNP footprints in sketch mode on fab layers.

--cdnp, --crossout-DNP-footprints-on-fab-layers

Plot an "X" over the courtyard of DNP footprints on fab layers, and strikeout their reference designators.

--subtract-soldermask

Remove silkscreen from areas without soldermask.

--uc, --use-contours

Plot graphic items using their contours.

--udo, --use-drill-origin

Plot using the drill/place file origin.

-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).

--drill-shape-opt <shape>

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).

--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. Layer names can be specified as canonical layer names (F.Cu, In.1, F.Fab, etc.) or as user-defined (custom) layer names, but user-defined layer names are matched first.

--mode-single

Generates a single file with the output arg path acting as the complete directory and filename path. COMMON_LAYER_LIST does not function in this mode. Instead LAYER_LIST controls all layers plotted.

--mode-multi

Plot the layers to one or more DXF files, with each file representing a single layer from LAYER_LIST. The output path specifies the directory in which the files will be written.

--plot-invisible-text

Force plotting of values and references, even if they are invisible. This argument is deprecated as of KiCad 9.0.1 and has no effect. It will be removed in a future version of KiCad. To plot invisible text, edit the board so that the text is no longer invisible.

--scale <scale>

A scaling factor to use for plotting the PCB. The border and title block are not scaled. A scale factor of 0 autoscales the plot.

--check-zones

Check zone fills and refill zones, if required, prior to export. Any zone fill updates are not saved in the board file.

INPUT_FILE

Board file to export.

-h, --help

Show help for the DXF export command.

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

The output filename. When --output is not used, the output filename will be the same as the input file, with the .cad 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, --flip-bottom-pads

Flip bottom footprint padstacks.

--unique-pins

Generate unique pin names.

--unique-footprints

Generate a new shape for each footprint instance (do not reuse shapes).

--use-drill-origin

Use drill/place file origin as origin.

--store-origin-coord

Save the origin coordinates in the file.

INPUT_FILE

Board file to export.

-h, --help

Show help for the Gerber export command.

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

The output folder for the exported files. One file is output for each layer. When --output 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. A seperate output file is plotted for each layer. Layer names can be specified as canonical layer names (F.Cu, In.1, F.Fab, etc.) or as user-defined (custom) layer names, but user-defined layer names are matched first.

--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.

--sp, --sketch-pads-on-fab-layers

Draw pad outlines and their numbers on front and back fab layers.

--hdnp, --hide-DNP-footprints-on-fab-layers

Don’t plot text and graphics of DNP footprints on fab layers.

--sdnp, --sketch-DNP-footprints-on-fab-layers

Plot graphics of DNP footprints in sketch mode on fab layers.

--cdnp, --crossout-DNP-footprints-on-fab-layers

Plot an "X" over the courtyard of DNP footprints on fab layers, and strikeout their reference designators.

--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.).

--plot-invisible-text

Force plotting of values and references, even if they are invisible. This argument is deprecated as of KiCad 9.0.1 and has no effect. It will be removed in a future version of KiCad. To plot invisible text, edit the board so that the text is no longer invisible.

--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. Each layer specified is included in every output file. Layer names can be specified as canonical layer names (F.Cu, In.1, F.Fab, etc.) or as user-defined (custom) layer names, but user-defined layer names are matched first.

--check-zones

Check zone fills and refill zones, if required, prior to export. Any zone fill updates are not saved in the board file.

--board-plot-params

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

INPUT_FILE

Board file to export.

-h, --help

Show help for the Gerber export command.

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

The output filename. When --output 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. Layer names can be specified as canonical layer names (F.Cu, In.1, F.Fab, etc.) or as user-defined (custom) layer names, but user-defined layer names are matched first.

--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.

--sp, --sketch-pads-on-fab-layers

Draw pad outlines and their numbers on front and back fab layers.

--hdnp, --hide-DNP-footprints-on-fab-layers

Don’t plot text and graphics of DNP footprints on fab layers.

--sdnp, --sketch-DNP-footprints-on-fab-layers

Plot graphics of DNP footprints in sketch mode on fab layers.

--cdnp, --crossout-DNP-footprints-on-fab-layers

Plot an "X" over the courtyard of DNP footprints on fab layers, and strikeout their reference designators.

--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.).

--plot-invisible-text

Force plotting of values and references, even if they are invisible. This argument is deprecated as of KiCad 9.0.1 and has no effect. It will be removed in a future version of KiCad. To plot invisible text, edit the board so that the text is no longer invisible.

--check-zones

Check zone fills and refill zones, if required, prior to export. Any zone fill updates are not saved in the board file.

INPUT_FILE

Board file to export.

-h, --help

Show help for the GLB export command.

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

The output filename. When --output 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.

--no-unspecified

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

--no-dnp

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

--grid-origin

Use grid origin as origin of output file.

--drill-origin

Use drill origin as origin of output file.

--subst-models

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

--board-only

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

--cut-vias-in-body

Cut via holes in board body even if conductor layers are not exported.

--no-board-body

Exclude board body.

--no-components

Exclude 3D models for components.

--component-filter <reference designator list>

Only include component 3D models matching this list of reference designators (comma-separated, wildcards supported)

--include-tracks

Include tracks and vias on outer conductor layers in export (time consuming).

--include-pads

Include pads in export (time consuming).

--include-zones

Include zones in export (time consuming).

--include-inner-copper

Include elements on inner conductor layers in export.

--include-silkscreen

Include silkscreen graphics in export as a set of flat faces.

--include-soldermask

Include solder mask layers in export as a set of flat faces.

--fuse-shapes

Fuse overlapping geometry together in export (time consuming).

--fill-all-vias

Don’t cut via holes in conductor layers.

--no-extra-pad-thickness

Disable adding additional metal thickness to pads. When not used, pads have 0.005mm added to their metal thickness, which causes pads to be separate faces in the exported model, distinct from the surrounding metal.

--min-distance <min distance>

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

--net-filter <net filter>

Only include copper items belonging to nets matching this wildcard.

--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.

INPUT_FILE

Board file to export.

-h, --help

Show help for the IPC-2581 export command.

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

The output filename. When --output 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 6.

--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.

INPUT_FILE

Board file to export.

-h, --help

Show help for the IPC-D-356 export command.

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

The output filename. When --output is not used, the output filename will be the same as the input file, with the .d356 file extension.

INPUT_FILE

Board file to export.

-h, --help

Show help for the ODB++ export command.

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

The output filename, or folder name if no compression is used.

--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 2.

--compression <mode>

Compression mode. Options are none, zip (default), or tgz.

--units <unit>

Units to use in the output file. Options are mm (default) or in.

INPUT_FILE

Board file to export.

-h, --help

Show help for the PDF export command.

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

The output folder or filename for the exported files. When --mode-single or --mode-multipage is used, this is the output filename. If this argument is not used, the output filename will be the same as the input file, with the .pdf file extension. When --mode-separate is used, this is the output directory. If --output 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 board, such as F.Cu,B.Cu. At least one layer must be given. Layer names can be specified as canonical layer names (F.Cu, In.1, F.Fab, etc.) or as user-defined (custom) layer names, but user-defined layer names are matched first.

--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.

--subtract-soldermask

Remove silkscreen from areas without soldermask.

--sp, --sketch-pads-on-fab-layers

Draw pad outlines and their numbers on front and back fab layers.

--hdnp, --hide-DNP-footprints-on-fab-layers

Don’t plot text and graphics of DNP footprints on fab layers.

--sdnp, --sketch-DNP-footprints-on-fab-layers

Plot graphics of DNP footprints in sketch mode on fab layers.

--cdnp, --crossout-DNP-footprints-on-fab-layers

Plot an "X" over the courtyard of DNP footprints on fab layers, and strikeout their reference designators.

-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).

--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. Layer names can be specified as canonical layer names (F.Cu, In.1, F.Fab, etc.) or as user-defined (custom) layer names, but user-defined layer names are matched first.

--plot-invisible-text

Force plotting of values and references, even if they are invisible. This argument is deprecated as of KiCad 9.0.1 and has no effect. It will be removed in a future version of KiCad. To plot invisible text, edit the board so that the text is no longer invisible.

--mode-single

Generates a single file with the output arg path acting as the complete directory and filename path. COMMON_LAYER_LIST does not function in this mode. Instead LAYER_LIST controls all layers plotted. All specified layers are plotted on a single page.

--mode-separate

Plot the layers to one or more PDF files, with each file representing a single layer from LAYER_LIST. The output path specifies the directory in which the files will be written.

--mode-multipage

Plot the layers to a single PDF file with multiple pages, with each page representing a single layer from LAYER_LIST. The output path specifies the complete directory and filename path.

--scale <scale>

A scaling factor to use for plotting the PCB. The border and title block are not scaled. A scale factor of 0 autoscales the plot.

--bg-color <color>

A background color for the plot. The format can be hex (#rrggbb or #rrggbbaa) or CSS (rgb(r,g,b) or rgba(r,g,b,a)).

--check-zones

Check zone fills and refill zones, if required, prior to export. Any zone fill updates are not saved in the board file.

INPUT_FILE

Board file to export.

-h, --help

Show help for the PLY export command.

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

The output filename. When --output is not used, the output filename will be the same as the input file, with the .ply 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.

--no-unspecified

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

--no-dnp

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

--grid-origin

Use grid origin as origin of output file.

--drill-origin

Use drill origin as origin of output file.

--subst-models

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

--board-only

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

--cut-vias-in-body

Cut via holes in board body even if conductor layers are not exported.

--no-board-body

Exclude board body.

--no-components

Exclude 3D models for components.

--component-filter <reference designator list>

Only include component 3D models matching this list of reference designators (comma-separated, wildcards supported)

--include-tracks

Include tracks and vias on outer conductor layers in export (time consuming).

--include-pads

Include pads in export (time consuming).

--include-zones

Include zones in export (time consuming).

--include-inner-copper

Include elements on inner conductor layers in export.

--include-silkscreen

Include silkscreen graphics in export as a set of flat faces.

--include-soldermask

Include solder mask layers in export as a set of flat faces.

--fuse-shapes

Fuse overlapping geometry together in export (time consuming).

--fill-all-vias

Don’t cut via holes in conductor layers.

--no-extra-pad-thickness

Disable adding additional metal thickness to pads. When not used, pads have 0.005mm added to their metal thickness, which causes pads to be separate faces in the exported model, distinct from the surrounding metal.

--min-distance <min distance>

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

--net-filter <net filter>

Only include copper items belonging to nets matching this wildcard.

--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.

INPUT_FILE

Board file to export.

-h, --help

Show help for the position file export command.

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

The output filename. When --output 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).

INPUT_FILE

Board file to export.

-h, --help

Show help for the PS export command.

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

The output folder or filename for the exported files. When --mode-single is used, this is the output filename. If --output is not used, the output filename will be the same as the input file, with the .pdf file extension. When --mode-multi is used, this is the output directory. If --output 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 board, such as F.Cu,B.Cu. At least one layer must be given. Layer names can be specified as canonical layer names (F.Cu, In.1, F.Fab, etc.) or as user-defined (custom) layer names, but user-defined layer names are matched first.

--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. Each layer specified is included in every output file. Layer names can be specified as canonical layer names (F.Cu, In.1, F.Fab, etc.) or as user-defined (custom) layer names, but user-defined layer names are matched first.

--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.

--subtract-soldermask

Remove silkscreen from areas without soldermask.

--sp, --sketch-pads-on-fab-layers

Draw pad outlines and their numbers on front and back fab layers.

--hdnp, --hide-DNP-footprints-on-fab-layers

Don’t plot text and graphics of DNP footprints on fab layers.

--sdnp, --sketch-DNP-footprints-on-fab-layers

Plot graphics of DNP footprints in sketch mode on fab layers.

--cdnp, --crossout-DNP-footprints-on-fab-layers

Plot an "X" over the courtyard of DNP footprints on fab layers, and strikeout their reference designators.

-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).

--mode-single

Generates a single file with the output arg path acting as the complete directory and filename path. COMMON_LAYER_LIST does not function in this mode. Instead LAYER_LIST controls all layers plotted.

--mode-multipage

Plot the layers to one or more PDF files, with each file representing a single layer from LAYER_LIST. The output path specifies the directory in which the files will be written.

--C, --track-width-correction

A global correction, in millimeters, that is added to the size of tracks, vias, and pads when plotted. This correction can be used to correct for errors in the PostScript output device to achieve an exact-scale output.

--X, --x-scale-factor

X scale adjust for exact scale.

--Y, --y-scale-factor

Y scale adjust for exact scale.

--A, --force-a4

Force A4 paper size.

--scale <scale>

A scaling factor to use for plotting the pcb. The border and title block are not scaled. A scale factor of 0 autoscales the plot.

--check-zones

Check zone fills and refill zones, if required, prior to export. Any zone fill updates are not saved in the board file.

INPUT_FILE

Board file to export statistics from.

-h, --help

Show help for the statistics command.

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

Output filename for the generated statistics report. When --output is not used, the output filename will be the same as the input file, with a _statistics suffix and the .rpt or .json file extension, depending on the selected format.

--format <format>

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

--units <unit>

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

--exclude-footprints-without-pads

Exclude footprints that do not contain any pads from component counts.

--subtract-holes-from-board

Subtract the area of holes from the total board area.

--subtract-holes-from-copper

Subtract the area of holes from the total copper area.

INPUT_FILE

Board file to export.

-h, --help

Show help for the STEP file export command.

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

The output filename. When --output 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.

--no-unspecified

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

--no-dnp

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

--grid-origin

Use grid origin as origin of output file.

--drill-origin

Use drill origin as origin of output file.

--subst-models

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

--board-only

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

--cut-vias-in-body

Cut via holes in board body even if conductor layers are not exported.

--no-board-body

Exclude board body.

--no-components

Exclude 3D models for components.

--component-filter <reference designator list>

Only include component 3D models matching this list of reference designators (comma-separated, wildcards supported)

--include-tracks

Include tracks and vias on outer conductor layers in export (time consuming).

--include-pads

Include pads in export (time consuming).

--include-zones

Include zones in export (time consuming).

--include-inner-copper

Include elements on inner conductor layers in export.

--include-silkscreen

Include silkscreen graphics in export as a set of flat faces.

--include-soldermask

Include solder mask layers in export as a set of flat faces.

--fuse-shapes

Fuse overlapping geometry together in export (time consuming).

--fill-all-vias

Don’t cut via holes in conductor layers.

--no-extra-pad-thickness

Disable adding additional metal thickness to pads. When not used, pads have 0.005mm added to their metal thickness, which causes pads to be separate faces in the exported model, distinct from the surrounding metal.

--min-distance <min distance>

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

--net-filter <net filter>

Only include copper items belonging to nets matching this wildcard.

--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.

INPUT_FILE

Board file to export.

-h, --help

Show help for the STL export command.

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

The output filename. When --output is not used, the output filename will be the same as the input file, with the .stl 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.

--no-unspecified

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

--no-dnp

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

--grid-origin

Use grid origin as origin of output file.

--drill-origin

Use drill origin as origin of output file.

--subst-models

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

--board-only

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

--cut-vias-in-body

Cut via holes in board body even if conductor layers are not exported.

--no-board-body

Exclude board body.

--no-components

Exclude 3D models for components.

--component-filter <reference designator list>

Only include component 3D models matching this list of reference designators (comma-separated, wildcards supported)

--include-tracks

Include tracks and vias on outer conductor layers in export (time consuming).

--include-pads

Include pads in export (time consuming).

--include-zones

Include zones in export (time consuming).

--include-inner-copper

Include elements on inner conductor layers in export.

--include-silkscreen

Include silkscreen graphics in export as a set of flat faces.

--include-soldermask

Include solder mask layers in export as a set of flat faces.

--fuse-shapes

Fuse overlapping geometry together in export (time consuming).

--fill-all-vias

Don’t cut via holes in conductor layers.

--no-extra-pad-thickness

Disable adding additional metal thickness to pads. When not used, pads have 0.005mm added to their metal thickness, which causes pads to be separate faces in the exported model, distinct from the surrounding metal.

--min-distance <min distance>

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

--net-filter <net filter>

Only include copper items belonging to nets matching this wildcard.

--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.

INPUT_FILE

Board file to export.

-h, --help

Show help for the STEPZ file export command.

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

The output filename. When --output is not used, the output filename will be the same as the input file, with the .stpz 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.

--no-unspecified

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

--no-dnp

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

--grid-origin

Use grid origin as origin of output file.

--drill-origin

Use drill origin as origin of output file.

--subst-models

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

--board-only

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

--cut-vias-in-body

Cut via holes in board body even if conductor layers are not exported.

--no-board-body

Exclude board body.

--no-components

Exclude 3D models for components.

--component-filter <reference designator list>

Only include component 3D models matching this list of reference designators (comma-separated, wildcards supported)

--include-tracks

Include tracks and vias on outer conductor layers in export (time consuming).

--include-pads

Include pads in export (time consuming).

--include-zones

Include zones in export (time consuming).

--include-inner-copper

Include elements on inner conductor layers in export.

--include-silkscreen

Include silkscreen graphics in export as a set of flat faces.

--include-soldermask

Include solder mask layers in export as a set of flat faces.

--fuse-shapes

Fuse overlapping geometry together in export (time consuming).

--fill-all-vias

Don’t cut via holes in conductor layers.

--no-extra-pad-thickness

Disable adding additional metal thickness to pads. When not used, pads have 0.005mm added to their metal thickness, which causes pads to be separate faces in the exported model, distinct from the surrounding metal.

--min-distance <min distance>

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

--net-filter <net filter>

Only include copper items belonging to nets matching this wildcard.

--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.

INPUT_FILE

Board file to export.

-h, --help

Show help for the 3D PDF export command.

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

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

--no-unspecified

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

--no-dnp

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

--grid-origin

Use grid origin as origin of output file.

--drill-origin

Use drill origin as origin of output file.

--subst-models

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

--board-only

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

--cut-vias-in-body

Cut via holes in board body even if conductor layers are not exported.

--no-board-body

Exclude board body.

--no-components

Exclude 3D models for components.

--component-filter <reference designator list>

Only include component 3D models matching this list of reference designators (comma-separated, wildcards supported)

--include-tracks

Include tracks and vias on outer conductor layers in export (time consuming).

--include-pads

Include pads in export (time consuming).

--include-zones

Include zones in export (time consuming).

--include-inner-copper

Include elements on inner conductor layers in export.

--include-silkscreen

Include silkscreen graphics in export as a set of flat faces.

--include-soldermask

Include solder mask layers in export as a set of flat faces.

--fuse-shapes

Fuse overlapping geometry together in export (time consuming).

--fill-all-vias

Don’t cut via holes in conductor layers.

--no-extra-pad-thickness

Disable adding additional metal thickness to pads. When not used, pads have 0.005mm added to their metal thickness, which causes pads to be separate faces in the exported model, distinct from the surrounding metal.

--min-distance <min distance>

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

--net-filter <net filter>

Only include copper items belonging to nets matching this wildcard.

--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.

INPUT_FILE

Board file to export.

-h, --help

Show help for the SVG file export command.

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

The output folder or filename for the exported files. When --mode-single is used, this is the output filename. If --output is not used, the output filename will be the same as the input file, with the .pdf file extension. When --mode-multi is used, this is the output directory. If --output 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 board, such as F.Cu,B.Cu. At least one layer must be given. Layer names can be specified as canonical layer names (F.Cu, In.1, F.Fab, etc.) or as user-defined (custom) layer names, but user-defined layer names are matched first.

--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.

--subtract-soldermask

Remove silkscreen from areas without soldermask.

-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.

--sp, --sketch-pads-on-fab-layers

Draw pad outlines and their numbers on front and back fab layers.

--hdnp, --hide-DNP-footprints-on-fab-layers

Don’t plot text and graphics of DNP footprints on fab layers.

--sdnp, --sketch-DNP-footprints-on-fab-layers

Plot graphics of DNP footprints in sketch mode on fab layers.

--cdnp, --crossout-DNP-footprints-on-fab-layers

Plot an "X" over the courtyard of DNP footprints on fab layers, and strikeout their reference designators.

--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.

--fit-page-to-board

Set the SVG size to match the board outline. This is equivalent to --page-size-mode 2.

--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).

--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. Layer names can be specified as canonical layer names (F.Cu, In.1, F.Fab, etc.) or as user-defined (custom) layer names, but user-defined layer names are matched first.

--mode-single

Generates a single file with the output arg path acting as the complete directory and filename path. COMMON_LAYER_LIST does not function in this mode. Instead LAYER_LIST controls all layers plotted.

--mode-multi

Plot the layers to one or more SVG files, with each file representing a single layer from LAYER_LIST. The output path specifies the directory in which the files will be written.

--plot-invisible-text

Force plotting of values and references, even if they are invisible. This argument is deprecated as of KiCad 9.0.1 and has no effect. It will be removed in a future version of KiCad. To plot invisible text, edit the board so that the text is no longer invisible.

--scale <scale>

A scaling factor to use for plotting the PCB. The border and title block are not scaled. A scale factor of 0 autoscales the plot.

--check-zones

Check zone fills and refill zones, if required, prior to export. Any zone fill updates are not saved in the board file.

INPUT_FILE

Board file to export.

-h, --help

Show help for the VRML export command.

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

The output filename. When --output 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.

--no-unspecified

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

--no-dnp

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

--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.

INPUT_FILE

Board file to export.

-h, --help

Show help for the XAO export command.

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

The output filename. When --output is not used, the output filename will be the same as the input file, with the .xao 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.

--no-unspecified

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

--no-dnp

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

--grid-origin

Use grid origin as origin of output file.

--drill-origin

Use drill origin as origin of output file.

--subst-models

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

--board-only

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

--cut-vias-in-body

Cut via holes in board body even if conductor layers are not exported.

--no-board-body

Exclude board body.

--no-components

Exclude 3D models for components.

--component-filter <reference designator list>

Only include component 3D models matching this list of reference designators (comma-separated, wildcards supported)

--include-tracks

Include tracks and vias on outer conductor layers in export (time consuming).

--include-pads

Include pads in export (time consuming).

--include-zones

Include zones in export (time consuming).

--include-inner-copper

Include elements on inner conductor layers in export.

--include-silkscreen

Include silkscreen graphics in export as a set of flat faces.

--include-soldermask

Include solder mask layers in export as a set of flat faces.

--fuse-shapes

Fuse overlapping geometry together in export (time consuming).

--fill-all-vias

Don’t cut via holes in conductor layers.

--no-extra-pad-thickness

Disable adding additional metal thickness to pads. When not used, pads have 0.005mm added to their metal thickness, which causes pads to be separate faces in the exported model, distinct from the surrounding metal.

--min-distance <min distance>

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

--net-filter <net filter>

Only include copper items belonging to nets matching this wildcard.

--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.

INPUT_FILE

Board file to render.

-h, --help

Show help for the render command.

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

The output filename. This argument must be given. The file extension given in this argument determines the output image file format. The filename must end with either .png (for PNG files) or .jpg/.jpeg (for JPG files).

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

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

-w <width>, --width <width>

Image width in pixels. Default: 1600.

-h <height>, --height <height>

Image height in pixels. Default: 900.

--side <side>

The side of the board to render. Options are top (default), bottom, left, right, front, or back.

--background <background>

Image background. Options are default (default), transparent, or opaque. For PNG files, default is transparent. For JPG files, default is opaque.

--quality <quality>

Render quality. Options are basic (default), high, user. When user is specified, the render settings stored in the project are used.

--preset <color preset>

Color preset. Options are follow_pcb_editor, follow_plot_settings (default), or legacy_preset_flag.

--floor

Enables floor, shadows and post-processing, even if disabled in quality preset.

--perspective

Use perspective projection instead of orthogonal.

--zoom <zoom level>

Camera zoom factor as an integer. Default: 1.

--pan <camera pan>

Set camera pan location, in millimeters, with the format 'X,Y,Z', e.g. '3,0,0'.

--pivot <pivot>

Set pivot point relative to the board center in centimeters, with the format 'X,Y,Z' e.g. '-10,2,0'.

--rotate <rotation>

Set board rotation around pivot point, in degrees, with the format 'X,Y,Z', e.g. '-45,0,45' for isometric view.

--light-top <intensity>

Top light intensity, format 'R,G,B' or a single number, range: 0-1.

--light-bottom <intensity>

Bottom light intensity, format 'R,G,B' or a single number, range: 0-1.

--light-side <intensity>

Side lights intensity, format 'R,G,B' or a single number, range: 0-1.

--light-camera <intensity>

Camera light intensity, format 'R,G,B' or a single number, range: 0-1.

--light-side-elevation <elevation>

Side lights elevation angle in degrees, range: 0-90.

INPUT_FILE

Board file to upgrade.

-h, --help

Show help for the upgrade command.

--force

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

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 --output 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.

INPUT_FILE

Schematic file to export.

-h, --help

Shows help message and exits

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

The output filename. When --output 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.

--include-excluded-from-bom

Include symbols marked "Exclude from BOM". This argument is deprecated as of KiCad 10.0 and has no effect.

--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.

INPUT_FILE

Schematic file to export.

-h, --help

Show help for the DXF file export command.

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

The output folder for the exported files. One file is output for each sheet. When --output 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.

--default-font <font name>

Default font name. Default: "KiCad Font".

-p <page list>, --pages <page list>

Comma-separated list of pages to export. Blank or unspecified means all pages. To plot specific pages, give the root sheet as INPUT_FILE and specify the desired output pages with the --pages argument.

INPUT_FILE

Schematic file to export.

-h, --help

Show help for the netlist export command.

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

The output filename. When --output 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, spicemodel, pads, or allegro.

INPUT_FILE

Schematic file to export.

-h, --help

Show help for the PDF file export command.

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

The output filename. When --output 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.

--default-font <font name>

Default font name. Default: "KiCad Font".

--exclude-pdf-property-popups

Do not generate property popups in PDF.

--exclude-pdf-hierarchical-links

Do not generate clickable links for hierarchical elements in PDF.

--exclude-pdf-metadata

Do not generate PDF metadata from AUTHOR and SUBJECT variables.

-n, --no-background-color

Export schematic without a background color, regardless of theme.

-p <page list>, --pages <page list>

Comma-separated list of pages to export. Blank or unspecified means all pages. To plot specific pages, give the root sheet as INPUT_FILE and specify the desired output pages with the --pages argument.

INPUT_DIR

Schematic file to export.

-h, --help

Show help for the PS file export command.

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

The output folder for the exported files. One file is output for each sheet. When --output 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.

--default-font <font name>

Default font name. Default: "KiCad Font".

-n, --no-background-color

Export schematic without a background color, regardless of theme.

-p <page list>, --pages <page list>

Comma-separated list of pages to export. Blank or unspecified means all pages. To plot specific pages, give the root sheet as INPUT_FILE and specify the desired output pages with the --pages argument.

INPUT_FILE

Schematic file to export.

-h, --help

Show help for the BOM export command.

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

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

INPUT_FILE

Schematic file to export.

-h, --help

Show help for the SVG file export command.

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

The output folder for the exported files. When --output 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.

--default-font <font name>

Default font name. Default: "KiCad Font".

-n, --no-background-color

Export schematic without a background color, regardless of theme.

-p <page list>, --pages <page list>

Comma-separated list of pages to export. Blank or unspecified means all pages. To plot specific pages, give the root sheet as INPUT_FILE and specify the desired output pages with the --pages argument.

INPUT_FILE

Schematic file to upgrade.

-h, --help

Show help for the upgrade command.

--force

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

INPUT_FILE

Symbol library file to use for export.

-h, --help

Show help for the symbol SVG export command.

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

The output folder for the exported files. Each symbol in the input library is output to a separate file. When --output 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.

INPUT_FILE

Symbol library to upgrade.

-h, --help

Show help for the upgrade command.

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

The output filename for the upgraded symbol library. When --output 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.