INPUT_FILE_OR_DIR

Footprint (.kicad_mod) or footprint library directory (.pretty) to export.

-h, --help

Hilfe zum Befehl zum Exportieren von Footprint-SVG-Dateien anzeigen.

-o <Ausgabeverzeichnis>, --output <Ausgabeverzeichnis>

Das Ausgabeverzeichnis für die exportierten Dateien. Für jede Ebene jedes Footprints in der Bibliothek wird eine Datei ausgegeben. Wenn --output nicht verwendet wird, werden die Dateien in das aktuelle Verzeichnis exportiert.

-l <Ebenenliste>, --layers <Ebenenliste>

Eine durch Kommas getrennte Liste der Ebenennamen, die aus dem Footprint exportiert werden sollen, z. B. F.Cu,B.Cu. Wenn keine Ebenen angegeben sind, werden alle Ebenen exportiert. Layernamen können als kanonische Layernamen (F.Cu, In.1, F.Fab usw.) oder als benutzerdefinierte Layernamen angegeben werden, wobei benutzerdefinierte Layernamen zuerst abgeglichen werden.

-D <Variablenname>=<Wert>, --define-var <Variablenname>=<Wert>

Projektvariablendefinitionen hinzufügen oder überschreiben. Kann mehrfach verwendet werden, um mehrere Variablen zu definieren.

-t <Themenname>, --theme <Themenname>

Der Name des Themas, das für den Export verwendet werden soll. Wenn kein Thema angegeben ist, wird das derzeit im Footprinteditor ausgewählte Thema verwendet.

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

Der Name des spezifischen Footprints, der aus der Bibliothek exportiert werden soll. Wenn dieses Argument nicht verwendet wird, werden alle Footprints in der Bibliothek exportiert.

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

Pad-Umrisse und deren Nummern auf den vorderen und hinteren Fab-Layern zeichnen.

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

Text und Grafiken von DNP-Footprints nicht auf Fab-Layern plotten.

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

Grafiken von DNP-Footprints im Skizzenmodus auf Fab-Layern zeichnen.

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

Ein „X” über den Hof von DNP-Footprints auf Fab-Layern zeichnen und deren Referenzbezeichnungen durchstreichen.

--black-and-white

Footprints in Schwarz-Weiß exportieren.

INPUT_FILE_OR_DIR

Footprint or footprint library directory to upgrade. For KiCad format footprint libraries, this can be a footprint (.kicad_mod file) or a footprint library (.pretty directory containing .kicad_mod files).

-h, --help

Hilfe zum Upgrade-Befehl anzeigen.

-o <Ausgabeverzeichnis>, --output <Ausgabeverzeichnis>

Das Ausgabeverzeichnis für die aktualisierten Footprints. Wenn --output nicht verwendet wird, werden die ursprünglichen Footprints mit den aktualisierten Footprints überschrieben.

--force

Die Eingabebibliothek erneut speichern, auch wenn sie bereits im aktuellen Dateiformat vorliegt.

INPUT_FILE

Platinendatei, auf der DRC ausgeführt werden soll.

-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

Zu exportierende Platinen-Datei.

-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

Zu exportierende Platinen-Datei.

-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

Zu exportierende Platinen-Datei.

-h, --help

Hilfe für den Befehl zum Exportieren von Bohrdateien anzeigen.

-o <Ausgabeverzeichnis>, --output <Ausgabeverzeichnis>

Das Ausgabeverzeichnis für die Bohrdatei(en). Wenn --output nicht verwendet wird, werden die Bohrdatei(en) im aktuellen Verzeichnis gespeichert.

--format <Format>

Das Bohrdateiformat. Optionen sind excellon (Standard) oder gerber.

--drill-origin <Ursprung>

Der Koordinatenursprung für die Bohrdatei. Optionen sind absolute (Standard) zur Verwendung des absoluten Ursprungs der Platine oder plot zur Verwendung des Bohr-/Platzierungsursprungs der Platine.

--excellon-zeros-format <Format>

Das Nullformat für die Bohrdatei. Optionen sind decimal (Standard), suppressleading, suppresstrailing oder keep. Gilt nur für Bohrdateien im Excellon-Format.

--excellon-oval-format <Format>

Den Bohrmodus für ovale Löcher steuern. Optionen sind route und alternate (Standard). Gilt nur für Bohrdateien im Excellon-Format.

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

Die Einheit für die Bohrdatei. Optionen sind mm (Standard) oder in. Gilt nur für Bohrdateien im Excellon-Format.

--excellon-mirror-y

Die Bohrdatei in Y-Richtung spiegeln. Gilt nur für Bohrdateien im Excellon-Format.

--excellon-min-header

Einen minimalen Header in der Bohrdatei verwenden. Gilt nur für Bohrdateien im Excellon-Format.

--excellon-separate-th

Separate Bohrdateien für durchkontaktierte und nicht durchkontaktierte Bohrungen erstellen. Gilt nur für Bohrdateien im Excellon-Format.

--generate-map

Zusätzlich zur Bohrdatei eine Kartendatei erstellen.

--generate-report

Eine Berichtdatei mit allen Bohrpunkten erstellen.

--report-path <report filename>

Der Ausgabedateiname für die Bohrberichtdatei. Wenn --report-path nicht verwendet wird, entspricht der Dateiname des Berichts dem der Eingabedatei, mit dem Suffix und der Dateiendung -drill.rpt.

--generate-tenting

Separate Bohrdateien für überzeltete Bohrungen generieren. Gilt nur für Bohrdateien im Gerber X2-Format.

--map-format <Format>

Das Format der Map-Datei. Optionen sind pdf (Standard), gerberx2, ps, dxf oder svg.

--gerber-precision <precision>

Die Genauigkeit (Anzahl der Stellen) für die Bohrdatei. Gültige Optionen sind 5 oder 6 (Standard). Gilt nur für Bohrdateien im Gerber-Format.

INPUT_FILE

Zu exportierende Platinen-Datei.

-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.

--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.

--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).

--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

Zu exportierende Platinen-Datei.

-h, --help

Hilfe für den DXF-Exportbefehl anzeigen.

-o <Ausgabedateiname>, --output <Ausgabedateiname>

Der Ausgabedateiname. Wenn --output nicht verwendet wird, entspricht der Ausgabedateiname dem Namen der Eingabedatei mit der Dateiendung .cad.

-D <Variablenname>=<Wert>, --define-var <Variablenname>=<Wert>

Projektvariablendefinitionen hinzufügen oder überschreiben. Kann mehrfach verwendet werden, um mehrere Variablen zu definieren.

-f, --flip-bottom-pads

Untere Footprint-Padstacks umdrehen.

--unique-pins

Eindeutige Pin-Namen generieren.

--unique-footprints

Erzeugt eine neue Form für jede Footprint-Instanz (Formate werden nicht wiederverwendet).

--use-drill-origin

Ursprung der Bohr-/Platzierungsdatei als Ursprung verwenden.

--store-origin-coord

Ursprungskoordinaten in der Datei speichern.

INPUT_FILE

Zu exportierende Platinen-Datei.

-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.

--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.

--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.

--board-plot-params

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

INPUT_FILE

Zu exportierende Platinen-Datei.

-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.

--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 the 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.

--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

Zu exportierende Platinen-Datei.

-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

Zu exportierende Platinen-Datei.

-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

Zu exportierende Platinen-Datei.

-h, --help

Hilfe für den IPC-D-356-Exportbefehl anzeigen.

-o <Ausgabedateiname>, --output <Ausgabedateiname>

Der Name der Ausgabedatei. Wenn --output nicht verwendet wird, entspricht der Name der Ausgabedatei dem Namen der Eingabedatei mit der Dateierweiterung .d356.

INPUT_FILE

Zu exportierende Platinen-Datei.

-h, --help

Hilfe für den ODB++-Exportbefehl anzeigen.

-o <Ausgabedateiname>, --output <Ausgabedateiname>

Der Ausgabedateiname oder Ordnername, wenn keine Komprimierung verwendet wird.

--drawing-sheet <Zeichnungsblattpfad>

Pfad zum Zeichnungsblatt, das beim Plotten verwendet werden soll, wobei das in der Board-Datei angegebene Zeichnungsblatt überschrieben wird

-D <Variablenname>=<Wert>, --define-var <Variablenname>=<Wert>

Projektvariablendefinitionen hinzufügen oder überschreiben. Kann mehrfach verwendet werden, um mehrere Variablen zu definieren.

--precision <Genauigkeit>

Die Genauigkeit (Anzahl der Stellen nach dem Dezimaltrennzeichen) für die exportierte Datei. Der Standardwert ist 2.

--compression <Modus>

Komprimierungsmodus. Optionen sind none, zip (Standard) oder tgz.

--units <Einheit>

In der Ausgabedatei zu verwendende Einheiten. Optionen sind mm (Standard) oder in.

INPUT_FILE

Zu exportierende Platinen-Datei.

-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.

--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.

--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).

--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

Zu exportierende Platinen-Datei.

-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

Zu exportierende Platinen-Datei.

-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).

--variant <variant name>

Board variant for variant-aware filtering (DNP, BOM, position file exclusions).

INPUT_FILE

Zu exportierende Platinen-Datei.

-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 .ps 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-multi

Plot the layers to one or more PS 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

Zu exportierende Platinen-Datei.

-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

Zu exportierende Platinen-Datei.

-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

Zu exportierende Platinen-Datei.

-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

Zu exportierende Platinen-Datei.

-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

Zu exportierende Platinen-Datei.

-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.

--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.

--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).

--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

Zu exportierende Platinen-Datei.

-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

Zu exportierende Platinen-Datei.

-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.

--use-board-stackup-colors

Colors defined in the board stackup override colors from the preset.

--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.

--variant <variant name>

The name(s) of the variant(s) to output. Can be used multiple times to output multiple variants. When specifying multiple variants, use ${VARIANT} in the output path to generate separate files for each variant. When --variant is not used, the default variant is output.

--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.

--variant <variant name>

The name(s) of the variant(s) to output. Can be used multiple times to output multiple variants. When specifying multiple variants, use ${VARIANT} in the output path to generate separate files for each variant. When --variant is not used, the default variant is output.

-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".

--draw-hop-over

Draw hop-overs at wire crossings.

--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.

--variant <variant name>

The name(s) of the variant(s) to output. Can be used multiple times to output multiple variants. When specifying multiple variants, use ${VARIANT} in the output path to generate separate files for each variant. When --variant is not used, the default variant is output.

--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.

--variant <variant name>

The name(s) of the variant(s) to output. Can be used multiple times to output multiple variants. When specifying multiple variants, use ${VARIANT} in the output path to generate separate files for each variant. When --variant is not used, the default variant is output.

-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".

--draw-hop-over

Draw hop-overs at wire crossings.

--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.

--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 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.

--variant <variant name>

The name(s) of the variant(s) to output. Can be used multiple times to output multiple variants. When specifying multiple variants, use ${VARIANT} in the output path to generate separate files for each variant. When --variant is not used, the default variant is output.

-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".

--draw-hop-over

Draw hop-overs at wire crossings.

-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. 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.

--variant <variant name>

The name(s) of the variant(s) to output. Can be used multiple times to output multiple variants. When specifying multiple variants, use ${VARIANT} in the output path to generate separate files for each variant. When --variant is not used, the default variant is output.

-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".

--draw-hop-over

Draw hop-overs at wire crossings.

-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. 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_OR_DIR

Symbol or symbol library to upgrade. This can be an unpacked symbol (.kicad_sym file containing a single symbol), an unpacked symbol library (folder containing .kicad_sym files), or a packed symbol library (.kicad_sym file containing multiple symbols).

-h, --help

Show help for the upgrade command.

-o <output file or directory>, --output <output file or directory>

The output file or directory for the upgraded symbol library. When the output path is a file, the symbols are saved as a single-file ("packed") .kicad_sym library. When the output path is a folder, the symbols are saved as individual ("unpacked") .kicad_sym files in the folder, with one file per symbol. 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.