GerberOptions parameters

  • create_gerber_job_file : [boolean] (default: true) Creates a file with information about all the generated gerbers. You can use it in gerbview to load all gerbers at once.

  • output : [string] (default: '%f-%i%I%v.%x') Output file name, the default KiCad name if empty. IMPORTANT! KiCad will always create the file using its own name and then we can rename it. For this reason you must avoid generating two variants at the same directory when one of them uses the default KiCad name. Affected by global options.

  • plot_sheet_reference : [boolean] (default: false) Include the frame and title block. Only available for KiCad 6+ and you get a poor result (i.e. always the default worksheet style, also problems expanding text variables). The pcb_print output can do a better job for PDF, SVG, PS, EPS and PNG outputs.

  • subtract_mask_from_silk : [boolean] (default: false) Subtract the solder mask from the silk screen.

  • use_gerber_net_attributes : [boolean] (default: true) Include netlist metadata.

  • use_gerber_x2_attributes : [boolean] (default: true) Use the extended X2 format (otherwise use X1 formerly RS-274X).

  • use_protel_extensions : [boolean] (default: false) Use legacy Protel file extensions.

  • custom_reports : [CustomReport parameters] [list(dict)] (default: []) A list of customized reports for the manufacturer.

  • disable_aperture_macros : [boolean] (default: false) Disable aperture macros (workaround for buggy CAM software) (KiCad 6).

  • dnf_filter : [string | list(string)] (default: '_null') Name of the filter to mark components as not fitted. A short-cut to use for simple cases where a variant is an overkill.

  • edge_cut_extension : [string] (default: '') Used to configure the edge cuts layer extension for Protel mode. Include the dot.

  • exclude_edge_layer : [boolean] (default: true) Do not include the PCB edge layer.

  • exclude_pads_from_silkscreen : [boolean] (default: false) Do not plot the component pads in the silk screen (KiCad 5.x only).

  • force_plot_invisible_refs_vals : [boolean] (default: false) Include references and values even when they are marked as invisible.

  • gerber_job_file : [string] (default: '%f-%i%I%v.%x') Name for the gerber job file (%i=’job’, %x=’gbrjob’). Affected by global options.

  • gerber_precision : [number] (default: 4.6) (choices: 4.5, 4.6) This is the gerber coordinate format, can be 4.5 or 4.6.

  • inner_extension_pattern : [string] (default: '') Used to change the Protel style extensions for inner layers. The replacement pattern can contain %n for the inner layer number and %N for the layer number. Example ‘.g%n’.

  • line_width : [number] (default: 0.1) (range: 0.02 to 2) Line_width for objects without width [mm] (KiCad 5).

  • plot_footprint_refs : [boolean] (default: true) Include the footprint references.

  • plot_footprint_values : [boolean] (default: true) Include the footprint values.

  • pre_transform : [string | list(string)] (default: '_null') Name of the filter to transform fields before applying other filters. A short-cut to use for simple cases where a variant is an overkill.

  • sketch_pad_line_width : [number] (default: 0.1) Line width for the sketched pads [mm], see sketch_pads_on_fab_layers (KiCad 6+) Note that this value is currently ignored by KiCad (6.0.9).

  • sketch_pads_on_fab_layers : [boolean] (default: false) Draw only the outline of the pads on the \*.Fab layers (KiCad 6+).

  • tent_vias : [boolean] (default: true) Cover the vias.

Warning

KiCad 8 has a bug that ignores this option. Set it from KiCad GUI.

  • uppercase_extensions : [boolean] (default: false) Use uppercase names for the extensions.

  • use_aux_axis_as_origin : [boolean] (default: false) Use the auxiliary axis as origin for coordinates.

  • variant : [string] (default: '') Board variant to apply.

Used dicts