# ATTENTION! THIS ISN'T A FULLY FUNCTIONAL EXAMPLE. # You should take portions of this example and edit the options to make # them suitable for your use. # This file is useful to know all the available options. kibot: version: 1 preflight: # [boolean=false] Annotates all power components. # This preflight modifies the schematic, use it only in revision control environments. # Used to solve ERC problems when using filters that remove power reference numbers. annotate_power: true # [boolean=false] Zones are filled before doing any operation involving PCB layers. check_zone_fills: true # [boolean=false] Option for `run_erc`. ERC warnings are considered errors. erc_warnings: false # [list(dict)] A list of entries to filter out ERC/DRC messages. filters: - filter: 'Filter description' error: '10' regex: 'Regular expression to match' # [boolean=false] Option for `run_drc`. Ignores the unconnected nets. Useful if you didn't finish the routing. ignore_unconnected: false # [dict] Replaces tags in the schematic. I.e. to insert the git hash or last revision date. # This pre-flight modifies the PCB. Even when a back-up is done use it carefully. pcb_replace: date_command: "git log -1 --format='%as' -- $KIBOT_PCB_NAME" replace_tags: - tag: '@git_hash@' command: 'git log -1 --format="%h" $KIBOT_PCB_NAME' before: 'Git hash: <' after: '>' # [boolean=false] Runs the DRC (Distance Rules Check). To ensure we have a valid PCB. # The report file name is controlled by the global output pattern (%i=drc %x=txt). run_drc: true # [boolean=false] Runs the ERC (Electrical Rules Check). To ensure the schematic is electrically correct. # The report file name is controlled by the global output pattern (%i=erc %x=txt). run_erc: true # [dict] Replaces tags in the schematic. I.e. to insert the git hash or last revision date. # This pre-flight modifies the schematics. Even when a back-up is done use it carefully. sch_replace: date_command: "git log -1 --format='%as' -- $KIBOT_SCH_NAME" replace_tags: - tag: '@git_hash@' command: 'git log -1 --format="%h" $KIBOT_SCH_NAME' before: 'Git hash: <' after: '>' # [boolean=false] Update the QR codes. # Complements the `qr_lib` output. # The KiCad 6 files and the KiCad 5 PCB needs manual update, generating a new library isn't enough. update_qr: true # [boolean=false] Update the XML version of the BoM (Bill of Materials). # To ensure our generated BoM is up to date. # Note that this isn't needed when using the internal BoM generator (`bom`). update_xml: true outputs: # BoardView: # This format allows simple pads and connections navigation, mainly for circuit debug. # The output can be loaded using Open Board View (https://openboardview.org/) - name: 'boardview_example' comment: 'Exports the PCB in board view format.' type: 'boardview' dir: 'Example/boardview_dir' options: # [string='%f-%i%I%v.%x'] Filename for the output (%i=boardview, %x=brd). Affected by global options output: '%f-%i%I%v.%x' # BoM (Bill of Materials): # This output can generate XYRS files (pick and place files). # Is compatible with KiBoM, but doesn't need to update the XML netlist because the components # are loaded from the schematic. # Important differences with KiBoM output: # - All options are in the main `options` section, not in `conf` subsection. # - The `Component` column is named `Row` and works just like any other column. # This output is what you get from the 'Tools/Generate Bill of Materials' menu in eeschema. - name: 'bom_example' comment: 'Used to generate the BoM in CSV, HTML, TSV, TXT, XML or XLSX format using the internal BoM.' type: 'bom' dir: 'Example/bom_dir' options: # [list(dict)] Add components from other projects aggregate: # [string=''] Name of the schematic to aggregate - file: '' # [string=''] Name to identify this source. If empty we use the name of the schematic name: '' # [number=1] Number of boards to build (components multiplier). Use negative to subtract number: 1 # [string=''] A prefix to add to all the references from this project ref_id: '' # [boolean=true] Always use positive values for the footprint rotation angle_positive: true # [boolean=false] Use negative X coordinates for footprints on bottom layer (for XYRS) bottom_negative_x: false # [list(dict)|list(string)] List of columns to display. # Can be just the name of the field columns: # [string=''] Used as explanation for this column. The XLSX output uses it - comment: '' # [string=''] Name of the field to use for this column field: 'Row' # [list(dict)|list(string)|string=''] List of fields to join to this column join: # [string=''] Name of the field - field: 'Voltage' # [string=''] Text to use instead of a field. This option is incompatible with the `field` option. # Any space to separate it should be added in the text. # Use \n for newline and \t for tab text: '' # [string=''] Text to add after the field content. Will be added only if the field isn't empty. # Any space to separate it should be added in the text. # Use \n for newline and \t for tab text_after: '' # [string=''] Text to add before the field content. Will be added only if the field isn't empty. # Any space to separate it should be added in the text. # Use \n for newline and \t for tab text_before: '' # [number=0] Used to group columns. The XLSX output uses it to collapse columns level: 0 # [string=''] Name to display in the header. The field is used when empty name: 'Line' # [list(list(string))] A series of values which are considered to be equivalent for the part name. # Each entry is a list of equivalen names. Example: ['c', 'c_small', 'cap' ] # will ensure the equivalent capacitor symbols can be grouped together. # If empty the following aliases are used: # - ['r', 'r_small', 'res', 'resistor'] # - ['l', 'l_small', 'inductor'] # - ['c', 'c_small', 'cap', 'capacitor'] # - ['sw', 'switch'] # - ['zener', 'zenersmall'] # - ['d', 'diode', 'd_small'] component_aliases: [['r', 'r_small', 'res', 'resistor'], ['l', 'l_small', 'inductor'], ['c', 'c_small', 'cap', 'capacitor'], ['sw', 'switch'], ['zener', 'zenersmall'], ['d', 'diode', 'd_small']] # [list(dict)|list(string)] List of columns to add to the global section of the cost. # Can be just the name of the field cost_extra_columns: # [string=''] Used as explanation for this column. The XLSX output uses it - comment: '' # [string=''] Name of the field to use for this column field: 'Row' # [list(dict)|list(string)|string=''] List of fields to join to this column join: # [string=''] Name of the field - field: 'Voltage' # [string=''] Text to use instead of a field. This option is incompatible with the `field` option. # Any space to separate it should be added in the text. # Use \n for newline and \t for tab text: '' # [string=''] Text to add after the field content. Will be added only if the field isn't empty. # Any space to separate it should be added in the text. # Use \n for newline and \t for tab text_after: '' # [string=''] Text to add before the field content. Will be added only if the field isn't empty. # Any space to separate it should be added in the text. # Use \n for newline and \t for tab text_before: '' # [number=0] Used to group columns. The XLSX output uses it to collapse columns level: 0 # [string=''] Name to display in the header. The field is used when empty name: 'Line' # [boolean=false] Show the stats about how many of the components are SMD/THT. You must provide the PCB count_smd_tht: false # [dict] Options for the CSV, TXT and TSV formats csv: # [boolean=false] Hide the header line (names of the columns) hide_header: false # [boolean=false] Hide project information hide_pcb_info: false # [boolean=false] Hide statistics information hide_stats_info: false # [boolean=false] Enclose all values using double quotes quote_all: false # [string=','] CSV Separator. TXT and TSV always use tab as delimiter separator: ',' # [string|list(string)] Include this distributors list. Default is all the available distributors: # [string|list(string)='_kibom_dnc'] Name of the filter to mark components as 'Do Not Change'. # The default filter marks components with a DNC value or DNC in the Config field dnc_filter: '_kibom_dnc' # [string|list(string)='_kibom_dnf'] Name of the filter to mark components as 'Do Not Fit'. # The default filter marks components with a DNF value or DNF in the Config field dnf_filter: '_kibom_dnf' # [string|list(string)='_mechanical'] Name of the filter to exclude components from BoM processing. # The default filter excludes test points, fiducial marks, mounting holes, etc exclude_filter: '_mechanical' # [string='Config'] Field name used for internal filters fit_field: 'Config' # [string|list(string)='no,yes'] Values for the `Footprint Populate` column footprint_populate_values: 'no,yes' # [string|list(string)='SMD,THT,VIRTUAL'] Values for the `Footprint Type` column footprint_type_values: 'SMD,THT,VIRTUAL' # [string=''] [HTML,CSV,TXT,TSV,XML,XLSX] format for the BoM. # Defaults to CSV or a guess according to the options. format: 'CSV' # [boolean=true] Connectors with the same footprints will be grouped together, independent of the name of the connector group_connectors: true # [list(string)] List of fields used for sorting individual components into groups. # Components which match (comparing *all* fields) will be grouped together. # Field names are case-insensitive. # If empty: ['Part', 'Part Lib', 'Value', 'Footprint', 'Footprint Lib', # 'Voltage', 'Tolerance', 'Current', 'Power'] is used group_fields: ['part', 'part lib', 'value', 'footprint', 'footprint lib', 'voltage', 'tolerance', 'current', 'power'] # [list(string)] List of fields to be used when the fields in `group_fields` are empty. # The first field in this list is the fallback for the first in `group_fields`, and so on group_fields_fallbacks: # [dict] Options for the HTML format html: # [boolean=true] Use colors to show the field type col_colors: true # [string=''] Column with links to the datasheet datasheet_as_link: '' # [string|list(string)=''] Column/s containing Digi-Key part numbers, will be linked to web page digikey_link: '' # [boolean=true] Generate a separated section for DNF (Do Not Fit) components generate_dnf: true # [boolean=false] Hide project information hide_pcb_info: false # [boolean=false] Hide statistics information hide_stats_info: false # [boolean=true] Use a color for empty cells. Applies only when `col_colors` is `true` highlight_empty: true # [string|boolean=''] PNG file to use as logo, use false to remove logo: '' # [string='modern-blue'] Page style. Internal styles: modern-blue, modern-green, modern-red and classic. # Or you can provide a CSS file name. Please use .css as file extension. style: 'modern-blue' # [string='KiBot Bill of Materials'] BoM title title: 'KiBot Bill of Materials' # [boolean=true] Exclude DNF (Do Not Fit) components ignore_dnf: true # [boolean=true] Component quantities are always expressed as integers. Using the ceil() function int_qtys: true # [boolean=true] Component groups with blank fields will be merged into the most compatible group, where possible merge_blank_fields: true # [boolean=true] When creating groups two components with empty/missing field will be interpreted as with the same value merge_both_blank: true # [list(string)] List of fields where we tolerate conflicts. # Use it to avoid undesired warnings. # By default the field indicated in `fit_field`, the field used for variants and # the field `part` are excluded no_conflict: ['Config', 'Part'] # [string|list(string)] Exclude this distributors list. They are removed after computing `distributors` no_distributors: # [boolean=false] When normalizing values use the locale decimal point normalize_locale: false # [boolean=false] Try to normalize the R, L and C values, producing uniform units and prefixes normalize_values: false # [number=1] Number of boards to build (components multiplier) number: 1 # [string='%f-%i%I%v.%x'] filename for the output (%i=bom). Affected by global options output: '%f-%i%I%v.%x' # [string=''] A prefix to add to all the references from this project. Used for multiple projects ref_id: '' # [string=' '] Separator used for the list of references ref_separator: ' ' # [string='type_value'] [type_value,type_value_ref,ref] Sorting criteria sort_style: 'type_value' # [boolean=false] Generate the `Source BoM` column using the reference ID instead of the project name source_by_id: false # [string='millimeters'] [millimeters,inches,mils] Units used for the positions ('Footprint X' and 'Footprint Y' columns). # Affected by global options units: 'millimeters' # [boolean=false] Print grouped references in the alternate compressed style eg: R1-R7,R18 use_alt: false # [boolean=true] Use the auxiliary axis as origin for coordinates (KiCad default) (for XYRS) use_aux_axis_as_origin: true # [string=''] Board variant, used to determine which components # are output to the BoM. variant: '' # [dict] Options for the XLSX format xlsx: # [boolean=true] Use colors to show the field type col_colors: true # [string=''] Column with links to the datasheet datasheet_as_link: '' # [string|list(string)=''] Column/s containing Digi-Key part numbers, will be linked to web page digikey_link: '' # [boolean=true] Generate a separated section for DNF (Do Not Fit) components generate_dnf: true # [boolean=false] Hide project information hide_pcb_info: false # [boolean=false] Hide statistics information hide_stats_info: false # [boolean=true] Use a color for empty cells. Applies only when `col_colors` is `true` highlight_empty: true # [boolean=false] Enable KiCost worksheet creation kicost: false # [string|boolean=''] PNG file to use as logo, use false to remove logo: '' # [number=2] Scaling factor for the logo. Note that this value isn't honored by all spreadsheet software logo_scale: 2 # [number=60] [20,999] Maximum column width (characters) max_col_width: 60 # [string='modern-blue'] Head style: modern-blue, modern-green, modern-red and classic style: 'modern-blue' # [string='KiBot Bill of Materials'] BoM title title: 'KiBot Bill of Materials' # Archiver (files compressor): # This is used to generate groups of files in compressed file format. - name: 'compress_example' comment: 'Generates a compressed file containing output files.' type: 'compress' dir: 'Example/compress_dir' options: # [string='auto'] [auto,stored,deflated,bzip2,lzma] Compression algorithm. Use auto to let KiBot select a suitable one compression: 'auto' # [list(dict)] Which files will be included files: # [string=''] Destination directory inside the archive, empty means the same of the file - dest: '' # [string='.*'] A regular expression that source files must match filter: '.*' # [boolean=false] Use the current working directory instead of the dir specified by `-d` from_cwd: false # [string=''] Collect files from the selected output. # When used the `source` option is ignored from_output: '' # [string='*'] File names to add, wildcards allowed. Use ** for recursive match. # By default this pattern is applied to the output dir specified with `-d` command line option. # See the `from_cwd` option source: '*' # [string='ZIP'] [ZIP,TAR,RAR] Output file format format: 'ZIP' # [string='%f-%i%I%v.%x'] Name for the generated archive (%i=name of the output %x=according to format). Affected by global options output: '%f-%i%I%v.%x' # Datasheets downloader: - name: 'download_datasheets_example' comment: 'Downloads the datasheets for the project' type: 'download_datasheets' dir: 'Example/download_datasheets_dir' options: # [boolean=false] Include the DNF components dnf: false # [string|list(string)='_none'] Name of the filter to mark components as not fitted. # A short-cut to use for simple cases where a variant is an overkill dnf_filter: '_none' # [string='Datasheet'] Name of the field containing the URL field: 'Datasheet' # [boolean=true] Instead of download things we already downloaded use symlinks link_repeated: true # [string='${VALUE}.pdf'] Name used for the downloaded datasheet. # ${FIELD} will be replaced by the FIELD content output: '${VALUE}.pdf' # [boolean=false] Download URLs that we already downloaded. # It only makes sense if the `output` field makes their output different repeated: false # [string=''] Board variant to apply variant: '' # DXF (Drawing Exchange Format): # This output is what you get from the File/Plot menu in pcbnew. - name: 'dxf_example' comment: 'Exports the PCB to 2D mechanical EDA tools (like AutoCAD).' type: 'dxf' dir: 'Example/dxf_dir' options: # [list(dict)] A list of customized reports for the manufacturer custom_reports: # [string=''] Content for the report. Use ${basename} for the project name without extension. # Use ${filename(LAYER)} for the file corresponding to LAYER - content: '' # [string='Custom_report.txt'] File name for the custom report output: 'Custom_report.txt' # [string|list(string)='_none'] Name of the filter to mark components as not fitted. # A short-cut to use for simple cases where a variant is an overkill dnf_filter: '_none' # [string='full'] what to use to indicate the drill places, can be none, small or full (for real scale) drill_marks: 'full' # [string=''] Used to configure the edge cuts layer extension for Protel mode. Include the dot edge_cut_extension: '' # [boolean=true] Do not include the PCB edge layer exclude_edge_layer: true # [boolean=false] Do not plot the component pads in the silk screen (KiCad 5.x only) exclude_pads_from_silkscreen: false # [boolean=false] Include references and values even when they are marked as invisible force_plot_invisible_refs_vals: false # [string=''] 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' inner_extension_pattern: '' # [boolean=false] Use mm instead of inches metric_units: false # [string='%f-%i%I%v.%x'] Output file name, the default KiCad name if empty. Affected by global options output: '%f-%i%I%v.%x' # [boolean=true] Include the footprint references plot_footprint_refs: true # [boolean=true] Include the footprint values plot_footprint_values: true # [boolean=false] Currently without effect plot_sheet_reference: false # [boolean=true] Plot using the contour, instead of the center line polygon_mode: true # [boolean=false] Don't fill objects, just draw the outline sketch_plot: false # [boolean=true] Cover the vias tent_vias: true # [boolean=false] Use uppercase names for the extensions uppercase_extensions: false # [boolean=false] Use the auxiliary axis as origin for coordinates use_aux_axis_as_origin: false # [string=''] Board variant to apply variant: '' layers: all # Excellon drill format: # You can create a map file for documentation purposes. # This output is what you get from the 'File/Fabrication output/Drill Files' menu in pcbnew. - name: 'excellon_example' comment: 'This is the main format for the drilling machine.' type: 'excellon' dir: 'Example/excellon_dir' options: # [number=0] number of digits for integer part of coordinates (0 is auto) left_digits: 0 # [dict|string] [hpgl,ps,gerber,dxf,svg,pdf] Format for a graphical drill map. # Not generated unless a format is specified map: # [string='%f-%i%I%v.%x'] Name for the map file, KiCad defaults if empty (%i='PTH_drill_map'). Affected by global options output: '%f-%i%I%v.%x' # [string='pdf'] [hpgl,ps,gerber,dxf,svg,pdf] Format for a graphical drill map type: 'pdf' # [boolean=true] Use metric units instead of inches metric_units: true # [boolean=false] Use a minimal header in the file minimal_header: false # [boolean=false] Invert the Y axis mirror_y_axis: false # [string] Force this replacement for %i when generating NPTH files npth_id: null # [string='%f-%i%I%v.%x'] name for the drill file, KiCad defaults if empty (%i='PTH_drill'). Affected by global options output: '%f-%i%I%v.%x' # [boolean=true] Generate one file for both, plated holes and non-plated holes, instead of two separated files pth_and_npth_single_file: true # [string] Force this replacement for %i when generating PTH and unified files pth_id: null # [dict|string] Name of the drill report. Not generated unless a name is specified report: # [string=''] Name of the drill report. Not generated unless a name is specified. # (%i='drill_report' %x='txt') filename: '' # [number=0] number of digits for mantissa part of coordinates (0 is auto) right_digits: 0 # [boolean=true] Use route command for oval holes (G00), otherwise use G85 route_mode_for_oval_holes: true # [boolean=false] Use the auxiliary axis as origin for coordinates use_aux_axis_as_origin: false # [string='DECIMAL_FORMAT'] [DECIMAL_FORMAT,SUPPRESS_LEADING,SUPPRESS_TRAILING,KEEP_ZEROS] How to handle the zeros zeros_format: 'DECIMAL_FORMAT' # Gerber drill format: # You can create a map file for documentation purposes. # This output is what you get from the 'File/Fabrication output/Drill Files' menu in pcbnew. - name: 'gerb_drill_example' comment: 'This is the information for the drilling machine in gerber format.' type: 'gerb_drill' dir: 'Example/gerb_drill_dir' options: # [dict|string] [hpgl,ps,gerber,dxf,svg,pdf] Format for a graphical drill map. # Not generated unless a format is specified map: # [string='%f-%i%I%v.%x'] Name for the map file, KiCad defaults if empty (%i='PTH_drill_map'). Affected by global options output: '%f-%i%I%v.%x' # [string='pdf'] [hpgl,ps,gerber,dxf,svg,pdf] Format for a graphical drill map type: 'pdf' # [string] Force this replacement for %i when generating NPTH files npth_id: null # [string='%f-%i%I%v.%x'] name for the drill file, KiCad defaults if empty (%i='PTH_drill'). Affected by global options output: '%f-%i%I%v.%x' # [string] Force this replacement for %i when generating PTH and unified files pth_id: null # [dict|string] Name of the drill report. Not generated unless a name is specified report: # [string=''] Name of the drill report. Not generated unless a name is specified. # (%i='drill_report' %x='txt') filename: '' # [boolean=false] Use the auxiliary axis as origin for coordinates use_aux_axis_as_origin: false # Gerber format: # This output is what you get from the File/Plot menu in pcbnew. - name: 'gerber_example' comment: 'This is the main fabrication format for the PCB.' type: 'gerber' dir: 'Example/gerber_dir' options: # [boolean=true] Creates a file with information about all the generated gerbers. # You can use it in gerbview to load all gerbers at once create_gerber_job_file: true # [list(dict)] A list of customized reports for the manufacturer custom_reports: # [string=''] Content for the report. Use ${basename} for the project name without extension. # Use ${filename(LAYER)} for the file corresponding to LAYER - content: '' # [string='Custom_report.txt'] File name for the custom report output: 'Custom_report.txt' # [boolean=false] Disable aperture macros (workaround for buggy CAM software) (KiCad 6) disable_aperture_macros: false # [string|list(string)='_none'] Name of the filter to mark components as not fitted. # A short-cut to use for simple cases where a variant is an overkill dnf_filter: '_none' # [string=''] Used to configure the edge cuts layer extension for Protel mode. Include the dot edge_cut_extension: '' # [boolean=true] Do not include the PCB edge layer exclude_edge_layer: true # [boolean=false] Do not plot the component pads in the silk screen (KiCad 5.x only) exclude_pads_from_silkscreen: false # [boolean=false] Include references and values even when they are marked as invisible force_plot_invisible_refs_vals: false # [string='%f-%i%I%v.%x'] Name for the gerber job file (%i='job', %x='gbrjob'). Affected by global options gerber_job_file: '%f-%i%I%v.%x' # [number=4.6] This the gerber coordinate format, can be 4.5 or 4.6 gerber_precision: 4.6 # [string=''] 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' inner_extension_pattern: '' # [number=0.1] [0.02,2] Line_width for objects without width [mm] (KiCad 5) line_width: 0.1 # [string='%f-%i%I%v.%x'] Output file name, the default KiCad name if empty. Affected by global options output: '%f-%i%I%v.%x' # [boolean=true] Include the footprint references plot_footprint_refs: true # [boolean=true] Include the footprint values plot_footprint_values: true # [boolean=false] Currently without effect plot_sheet_reference: false # [boolean=false] Subtract the solder mask from the silk screen subtract_mask_from_silk: false # [boolean=true] Cover the vias tent_vias: true # [boolean=false] Use uppercase names for the extensions uppercase_extensions: false # [boolean=false] Use the auxiliary axis as origin for coordinates use_aux_axis_as_origin: false # [boolean=true] Include netlist metadata use_gerber_net_attributes: true # [boolean=true] Use the extended X2 format (otherwise use X1 formerly RS-274X) use_gerber_x2_attributes: true # [boolean=false] Use legacy Protel file extensions use_protel_extensions: false # [string=''] Board variant to apply variant: '' layers: all # HPGL (Hewlett & Packard Graphics Language): # This output is what you get from the File/Plot menu in pcbnew. - name: 'hpgl_example' comment: 'Exports the PCB for plotters and laser printers.' type: 'hpgl' dir: 'Example/hpgl_dir' options: # [list(dict)] A list of customized reports for the manufacturer custom_reports: # [string=''] Content for the report. Use ${basename} for the project name without extension. # Use ${filename(LAYER)} for the file corresponding to LAYER - content: '' # [string='Custom_report.txt'] File name for the custom report output: 'Custom_report.txt' # [string|list(string)='_none'] Name of the filter to mark components as not fitted. # A short-cut to use for simple cases where a variant is an overkill dnf_filter: '_none' # [string='full'] what to use to indicate the drill places, can be none, small or full (for real scale) drill_marks: 'full' # [string=''] Used to configure the edge cuts layer extension for Protel mode. Include the dot edge_cut_extension: '' # [boolean=true] Do not include the PCB edge layer exclude_edge_layer: true # [boolean=false] Do not plot the component pads in the silk screen (KiCad 5.x only) exclude_pads_from_silkscreen: false # [boolean=false] Include references and values even when they are marked as invisible force_plot_invisible_refs_vals: false # [string=''] 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' inner_extension_pattern: '' # [boolean=false] Plot mirrored mirror_plot: false # [string='%f-%i%I%v.%x'] Output file name, the default KiCad name if empty. Affected by global options output: '%f-%i%I%v.%x' # [number=1] [1,16] Pen number pen_number: 1 # [number=20] [1,99] Pen speed pen_speed: 20 # [number=15] [0,100] Pen diameter in MILS, useful to fill areas. However, it is in mm in HPGL files pen_width: 15 # [boolean=true] Include the footprint references plot_footprint_refs: true # [boolean=true] Include the footprint values plot_footprint_values: true # [boolean=false] Currently without effect plot_sheet_reference: false # [number=0] Scale factor (0 means autoscaling) scaling: 0 # [boolean=false] Don't fill objects, just draw the outline sketch_plot: false # [boolean=true] Cover the vias tent_vias: true # [boolean=false] Use uppercase names for the extensions uppercase_extensions: false # [string=''] Board variant to apply variant: '' layers: all # IBoM (Interactive HTML BoM): # For more information: https://github.com/INTI-CMNB/InteractiveHtmlBom # This output is what you get from the InteractiveHtmlBom plug-in (pcbnew). - name: 'ibom_example' comment: 'Generates an interactive web page useful to identify the position of the components in the PCB.' type: 'ibom' dir: 'Example/ibom_dir' options: # [string=''] List of comma separated blacklisted components or prefixes with *. E.g. 'X1,MH*'. # IBoM option, avoid using in conjunction with KiBot variants/filters blacklist: '' # [boolean=false] Blacklist components with empty value. # IBoM option, avoid using in conjunction with KiBot variants/filters blacklist_empty_val: false # [number=0] Board rotation in degrees (-180 to 180). Will be rounded to multiple of 5 board_rotation: 0 # [string='left-right'] [bom-only,left-right,top-bottom] Default BOM view bom_view: 'left-right' # [string='Sourced,Placed'] Comma separated list of checkbox columns checkboxes: 'Sourced,Placed' # [boolean=false] Default to dark mode dark_mode: false # [string|list(string)='_none'] Name of the filter to mark components as not fitted. # A short-cut to use for simple cases where a variant is an overkill. # Avoid using it in conjunction with with IBoM native filtering options dnf_filter: '_none' # [string=''] Name of the extra field that indicates do not populate status. # Components with this field not empty will be blacklisted. # IBoM option, avoid using in conjunction with KiBot variants/filters dnp_field: '' # [string=''] Path to netlist or xml file. You can use '%F.xml' to avoid specifying the project name. # Leave it blank for most uses, data will be extracted from the PCB extra_data_file: '' # [string=''] Comma separated list of extra fields to pull from netlist or xml file. # Using 'X,Y' is a shortcut for `show_fields` and `group_fields` with values 'Value,Footprint,X,Y' extra_fields: '' # [string=''] Comma separated list of fields that components will be grouped by. # Value and Footprint are used when nothing is specified group_fields: '' # [boolean=false] Hide footprint pads by default hide_pads: false # [boolean=false] Hide silkscreen by default hide_silkscreen: false # [boolean=false] Highlight pin1 by default highlight_pin1: false # [boolean=false] Include netlist information in output. include_nets: false # [boolean=false] Include track/zone information in output. F.Cu and B.Cu layers only include_tracks: false # [string='FB'] [F,FB,B] Default layer view layer_view: 'FB' # [string='ibom'] Output file name format supports substitutions: # %f : original pcb file name without extension. # %p : pcb/project title from pcb metadata. # %c : company from pcb metadata. # %r : revision from pcb metadata. # %d : pcb date from metadata if available, file modification date otherwise. # %D : bom generation date. # %T : bom generation time. # Extension .html will be added automatically. # Note that this name is used only when output is '' name_format: 'ibom' # `netlist_file` is an alias for `extra_data_file` # [boolean=false] Do not blacklist virtual components. # IBoM option, avoid using in conjunction with KiBot variants/filters no_blacklist_virtual: false # [boolean=false] Disable compression of pcb data no_compression: false # [boolean=false] Do not redraw pcb on drag by default no_redraw_on_drag: false # [boolean=false] Normalize extra field name case. E.g. 'MPN' and 'mpn' will be considered the same field normalize_field_case: false # [string='%f-%i%I%v.%x'] Filename for the output, use '' to use the IBoM filename (%i=ibom, %x=html). Affected by global options output: '%f-%i%I%v.%x' # [boolean=false] Show fabrication layer by default show_fabrication: false # [string=''] Comma separated list of fields to show in the BOM. # Value and Footprint are displayed when nothing is specified show_fields: '' # [string='C,R,L,D,U,Y,X,F,SW,A,~,HS,CNN,J,P,NT,MH'] Default sort order for components. Must contain '~' once sort_order: 'C,R,L,D,U,Y,X,F,SW,A,~,HS,CNN,J,P,NT,MH' # [string=''] Board variant to apply. # Avoid using it in conjunction with with IBoM native filtering options variant: '' # [string=''] Name of the extra field that stores board variant for component. # IBoM option, avoid using in conjunction with KiBot variants/filters variant_field: '' # [string=''] List of board variants to exclude from the BOM. # IBoM option, avoid using in conjunction with KiBot variants/filters variants_blacklist: '' # [string=''] List of board variants to include in the BOM. # IBoM option, avoid using in conjunction with KiBot variants/filters variants_whitelist: '' # KiBoM (KiCad Bill of Materials): # For more information: https://github.com/INTI-CMNB/KiBoM # Note that this output is provided as a compatibility tool. # We recommend using the `bom` output instead. # This output is what you get from the 'Tools/Generate Bill of Materials' menu in eeschema. - name: 'kibom_example' comment: 'Used to generate the BoM in HTML or CSV format using the KiBoM plug-in.' type: 'kibom' dir: 'Example/kibom_dir' options: # [string|dict] BoM configuration file, relative to PCB. # You can also define the configuration here, will be stored in `config.kibom.ini` conf: # [list(dict)|list(string)] List of columns to display. # Can be just the name of the field columns: # [string=''] Name of the field to use for this column - field: 'Row' # [list(string)|string=''] List of fields to join to this column join: '' # [string=''] Name to display in the header. The field is used when empty name: 'Line' # [list(list(string))] A series of values which are considered to be equivalent for the part name. # Each entry is a list of equivalen names. Example: ['c', 'c_small', 'cap' ] # will ensure the equivalent capacitor symbols can be grouped together. # If empty the following aliases are used: # - ['r', 'r_small', 'res', 'resistor'] # - ['l', 'l_small', 'inductor'] # - ['c', 'c_small', 'cap', 'capacitor'] # - ['sw', 'switch'] # - ['zener', 'zenersmall'] # - ['d', 'diode', 'd_small'] component_aliases: [['r', 'r_small', 'res', 'resistor'], ['l', 'l_small', 'inductor'], ['c', 'c_small', 'cap', 'capacitor'], ['sw', 'switch'], ['zener', 'zenersmall'], ['d', 'diode', 'd_small']] # [string=''] Column with links to the datasheet (HTML only) datasheet_as_link: '' # [string|list(string)=''] Column/s containing Digi-Key part numbers, will be linked to web page (HTML only) digikey_link: '' # [list(dict)] A series of regular expressions used to exclude parts. # If a component matches ANY of these, it will be excluded. # Column names are case-insensitive. # If empty the following list is used: # - column: References # regex: '^TP[0-9]*' # - column: References # regex: '^FID' # - column: Part # regex: 'mount.*hole' # - column: Part # regex: 'solder.*bridge' # - column: Part # regex: 'test.*point' # - column: Footprint # regex 'test.*point' # - column: Footprint # regex: 'mount.*hole' # - column: Footprint # regex: 'fiducial' exclude_any: # [string=''] Name of the column to apply the regular expression - column: '' # `field` is an alias for `column` # [string=''] Regular expression to match regex: '' # `regexp` is an alias for `regex` # [string='Config'] Field name used to determine if a particular part is to be fitted (also DNC and variants) fit_field: 'Config' # [boolean=true] Connectors with the same footprints will be grouped together, independent of the name of the connector group_connectors: true # [list(string)] List of fields used for sorting individual components into groups. # Components which match (comparing *all* fields) will be grouped together. # Field names are case-insensitive. # If empty: ['Part', 'Part Lib', 'Value', 'Footprint', 'Footprint Lib'] is used group_fields: ['Part', 'Part Lib', 'Value', 'Footprint', 'Footprint Lib'] # [boolean=false] Hide column headers hide_headers: false # [boolean=false] Hide project information hide_pcb_info: false # [boolean=true] Generate a separated section for DNF (Do Not Fit) components (HTML only) html_generate_dnf: true # [boolean=true] Exclude DNF (Do Not Fit) components ignore_dnf: true # [list(dict)] A series of regular expressions used to select included parts. # If there are any regex defined here, only components that match against ANY of them will be included. # Column names are case-insensitive. # If empty all the components are included include_only: # [string=''] Name of the column to apply the regular expression - column: '' # `field` is an alias for `column` # [string=''] Regular expression to match regex: '' # `regexp` is an alias for `regex` # [boolean=true] Component groups with blank fields will be merged into the most compatible group, where possible merge_blank_fields: true # [boolean=true] First column is the row number number_rows: true # [string=' '] Separator used for the list of references ref_separator: ' ' # [boolean=true] Each component group will be tested against a number of regular-expressions (see ``). test_regex: true # [boolean=false] Print grouped references in the alternate compressed style eg: R1-R7,R18 use_alt: false # [string='HTML'] [HTML,CSV,XML,XLSX] format for the BoM format: 'HTML' # [number=1] Number of boards to build (components multiplier) number: 1 # [string='%f-%i%I%v.%x'] filename for the output (%i=bom). Affected by global options output: '%f-%i%I%v.%x' # [string=','] CSV Separator separator: ',' # [string=''] Board variant(s), used to determine which components # are output to the BoM. To specify multiple variants, # with a BOM file exported for each variant, separate # variants with the ';' (semicolon) character. # This isn't related to the KiBot concept of variants variant: '' # KiCost (KiCad Cost calculator): # For more information: https://github.com/INTI-CMNB/KiCost # This output is what you get from the KiCost plug-in (eeschema). - name: 'kicost_example' comment: 'Generates a spreadsheet containing components costs.' type: 'kicost' dir: 'Example/kicost_dir' options: # [list(dict)] Add components from other projects aggregate: # `board_qty` is an alias for `number` # [string=''] Name of the XML to aggregate - file: '' # [number=100] Number of boards to build (components multiplier) number: 100 # [string=' '] Variant for this project variant: ' ' # `board_qty` is an alias for `number` # [string|list(string)=USD] Currency priority. Use ISO4217 codes (i.e. USD, EUR) currency: USD # [string|list(string)] Include this distributors list. Default is all the available distributors: # [string|list(string)='_none'] Name of the filter to mark components as not fitted. # A short-cut to use for simple cases where a variant is an overkill. # Don't use the `kicost_variant` when using internal variants/filters dnf_filter: '_none' # [string|list(string)] List of fields to be added to the global data section fields: # [string|list(string)] List of fields that can be different for a group. # Parts with differences in these fields are grouped together, but displayed individually group_fields: # [string|list(string)] List of fields to be ignored ignore_fields: # [string=''] Regular expression to match the variant field (KiCost option, not internal variants) kicost_variant: '' # [boolean=false] Do not collapse the part references (collapse=R1-R4) no_collapse: false # [string|list(string)] Exclude this distributors list. They are removed after computing `distributors` no_distributors: # [boolean=false] Do not look for components price. For testing purposes no_price: false # [number=100] Number of boards to build (components multiplier) number: 100 # [string='%f-%i%I%v.%x'] Filename for the output (%i=kicost, %x=xlsx). Affected by global options output: '%f-%i%I%v.%x' # [boolean=false] Include the catalogue links in the catalogue code show_cat_url: false # [string|list(string)] Declare part fields to include in multipart split process split_extra_fields: # [list(dict)] Fields to rename (KiCost option, not internal filters) translate_fields: # [string=''] Name of the field to rename - field: 'mpn' # [string=''] New name name: 'manf#' # [string=''] Board variant to apply. # Don't use the `kicost_variant` when using internal variants/filters variant: '' # PcbDraw - Beautiful 2D PCB render: # Uses configurable colors. # Can also render the components if the 2D models are available - name: 'pcbdraw_example' comment: 'Exports the PCB as a 2D model (SVG, PNG or JPG).' type: 'pcbdraw' dir: 'Example/pcbdraw_dir' options: # [boolean=false] Render the bottom side of the board (default is top side) bottom: false # [string|list(string)='_none'] Name of the filter to mark components as not fitted. # A short-cut to use for simple cases where a variant is an overkill dnf_filter: '_none' # [number=300] [10,1200] Dots per inch (resolution) of the generated image dpi: 300 # [string='svg'] [svg,png,jpg] Output format. Only used if no `output` is specified format: 'svg' # [list(string)=[]] List of components to highlight highlight: [] # [list(string)=[]] List of libraries libs: [] # [boolean=false] Mirror the board mirror: false # [boolean=false] Do not make holes transparent no_drillholes: false # [string='%f-%i%I%v.%x'] Name for the generated file. Affected by global options output: '%f-%i%I%v.%x' # [boolean=false] Show placeholder for missing components placeholder: false # [dict|None] Replacements for PCB references using components (lib:component) remap: # [list(string)|string=none] [none,all] List of components to draw, can be also a string for none or all. # The default is none show_components: none # [string|dict] PCB style (colors). An internal name, the name of a JSON file or the style options style: # [string='#208b47'] color for the board without copper (covered by solder mask) board: '#208b47' # [string='#cabb3e'] color for the PCB core (not covered by solder mask) clad: '#cabb3e' # [string='#285e3a'] color for the copper zones (covered by solder mask) copper: '#285e3a' # [boolean=false] highlight over the component (not under) highlight_on_top: false # [number=1.5] [0,1000] how much the highlight extends around the component [mm] highlight_padding: 1.5 # [string='stroke:none;fill:#ff0000;opacity:0.5;'] SVG code for the highlight style highlight_style: 'stroke:none;fill:#ff0000;opacity:0.5;' # [string='#000000'] color for the outline outline: '#000000' # [string='#8b898c'] color for the exposed pads (metal finish) pads: '#8b898c' # [string='#d5dce4'] color for the silk screen silk: '#d5dce4' # [string='#bf2600'] color for the V-CUTS vcut: '#bf2600' # [string=''] Board variant to apply variant: '' # [boolean=false] Render V-CUTS on the Cmts.User layer vcuts: false # [string='visible'] [visible,all,none] Using visible only the warnings about components in the visible side are generated warnings: 'visible' # PDF (Portable Document Format): # Note that this output isn't the best for documating your project. # This output is what you get from the File/Plot menu in pcbnew. - name: 'pdf_example' comment: 'Exports the PCB to the most common exchange format. Suitable for printing.' type: 'pdf' dir: 'Example/pdf_dir' options: # [list(dict)] A list of customized reports for the manufacturer custom_reports: # [string=''] Content for the report. Use ${basename} for the project name without extension. # Use ${filename(LAYER)} for the file corresponding to LAYER - content: '' # [string='Custom_report.txt'] File name for the custom report output: 'Custom_report.txt' # [string|list(string)='_none'] Name of the filter to mark components as not fitted. # A short-cut to use for simple cases where a variant is an overkill dnf_filter: '_none' # [string='full'] what to use to indicate the drill places, can be none, small or full (for real scale) drill_marks: 'full' # [string=''] Used to configure the edge cuts layer extension for Protel mode. Include the dot edge_cut_extension: '' # [boolean=true] Do not include the PCB edge layer exclude_edge_layer: true # [boolean=false] Do not plot the component pads in the silk screen (KiCad 5.x only) exclude_pads_from_silkscreen: false # [boolean=false] Include references and values even when they are marked as invisible force_plot_invisible_refs_vals: false # [string=''] 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' inner_extension_pattern: '' # [number=0.1] [0.02,2] For objects without width [mm] (KiCad 5) line_width: 0.1 # [boolean=false] Plot mirrored mirror_plot: false # [boolean=false] Invert black and white negative_plot: false # [string='%f-%i%I%v.%x'] Output file name, the default KiCad name if empty. Affected by global options output: '%f-%i%I%v.%x' # [boolean=true] Include the footprint references plot_footprint_refs: true # [boolean=true] Include the footprint values plot_footprint_values: true # [boolean=false] Currently without effect plot_sheet_reference: false # [boolean=true] Cover the vias tent_vias: true # [boolean=false] Use uppercase names for the extensions uppercase_extensions: false # [string=''] Board variant to apply variant: '' layers: all # PDF PCB Print (Portable Document Format): # This is the main format to document your PCB. # This output is what you get from the 'File/Print' menu in pcbnew. - name: 'pdf_pcb_print_example' comment: 'Exports the PCB to the most common exchange format. Suitable for printing.' type: 'pdf_pcb_print' dir: 'Example/pdf_pcb_print_dir' options: # [string|list(string)='_none'] Name of the filter to mark components as not fitted. # A short-cut to use for simple cases where a variant is an overkill dnf_filter: '_none' # [string='full'] What to use to indicate the drill places, can be none, small or full (for real scale) drill_marks: 'full' # [boolean=true] Only useful for KiCad 6 when printing in one page, you can disable the edge here. # KiCad 5 forces it by default, and you can't control it from config files. # Same for KiCad 6 when printing to separated pages force_edge_cuts: true # [boolean=false] Hide components in the Fab layer that are marked as excluded by a variant hide_excluded: false # [boolean=false] Print mirrored (X axis inverted). ONLY for KiCad 6 mirror: false # [boolean=false] Print in black and white monochrome: false # [string='%f-%i%I%v.%x'] Filename for the output PDF (%i=layers, %x=pdf). Affected by global options output: '%f-%i%I%v.%x' # `output_name` is an alias for `output` # [boolean=true] Include the title-block plot_sheet_reference: true # [number=1.0] Scale factor (0 means autoscaling) scaling: 1.0 # [boolean=false] Print layers in separated pages separated: false # [string=''] Text used to replace the sheet title. %VALUE expansions are allowed. # If it starts with `+` the text is concatenated title: '' # [string=''] Board variant to apply variant: '' layers: all # PDF Schematic Print (Portable Document Format): # This is the main format to document your schematic. # This output is what you get from the 'File/Print' menu in eeschema. - name: 'pdf_sch_print_example' comment: 'Exports the PCB to the most common exchange format. Suitable for printing.' type: 'pdf_sch_print' dir: 'Example/pdf_sch_print_dir' options: # [string|list(string)='_none'] Name of the filter to mark components as not fitted. # A short-cut to use for simple cases where a variant is an overkill dnf_filter: '_none' # [boolean=true] Include the frame and title block frame: true # [boolean=false] Generate a monochromatic PDF monochrome: false # [string='%f-%i%I%v.%x'] Filename for the output PDF (%i=schematic %x=pdf). Affected by global options output: '%f-%i%I%v.%x' # [string=''] Board variant to apply. # Not fitted components are crossed variant: '' # PDF joiner: # This is just a PDF joiner, using `pdfunite` from Poppler Utils. - name: 'pdfunite_example' comment: 'Generates a new PDF from other outputs.' type: 'pdfunite' dir: 'Example/pdfunite_dir' options: # [string='%f-%i%I%v.%x'] Name for the generated PDF (%i=name of the output %x=pdf). Affected by global options output: '%f-%i%I%v.%x' # [list(dict)] Which files will be included outputs: # [string='.*\.pdf'] A regular expression that source files must match - filter: '.*\.pdf' # [boolean=false] Use the current working directory instead of the dir specified by `-d` from_cwd: false # [string=''] Collect files from the selected output. # When used the `source` option is ignored from_output: '' # [string='*.pdf'] File names to add, wildcards allowed. Use ** for recursive match. # By default this pattern is applied to the output dir specified with `-d` command line option. # See the `from_cwd` option source: '*.pdf' # Pick & place: # This output is what you get from the 'File/Fabrication output/Footprint position (.pos) file' menu in pcbnew. - name: 'position_example' comment: 'Generates the file with position information for the PCB components, used by the pick and place machine.' type: 'position' dir: 'Example/position_dir' options: # [boolean=false] Use negative X coordinates for footprints on bottom layer bottom_negative_x: false # [list(dict)|list(string)] Which columns are included in the output columns: # [string=''] [Ref,Val,Package,PosX,PosY,Rot,Side] Internal name - id: 'Ref' # [string=''] Name to use in the output file. The id is used when empty name: 'Reference' # [string|list(string)='_none'] Name of the filter to mark components as not fitted. # A short-cut to use for simple cases where a variant is an overkill dnf_filter: '_none' # [string='ASCII'] [ASCII,CSV] Format for the position file format: 'ASCII' # [boolean=false] Include virtual components. For special purposes, not pick & place include_virtual: false # [boolean=true] Only include the surface mount components only_smd: true # [string='%f-%i%I%v.%x'] Output file name (%i='top_pos'|'bottom_pos'|'both_pos', %x='pos'|'csv'). Affected by global options output: '%f-%i%I%v.%x' # [boolean=true] Generate two separated files, one for the top and another for the bottom separate_files_for_front_and_back: true # [string='millimeters'] [millimeters,inches,mils] Units used for the positions. Affected by global options units: 'millimeters' # [boolean=true] Use the auxiliary axis as origin for coordinates (KiCad default) use_aux_axis_as_origin: true # [string=''] Board variant to apply variant: '' # PS (Postscript): # This output is what you get from the File/Plot menu in pcbnew. - name: 'ps_example' comment: 'Exports the PCB to a format suitable for printing.' type: 'ps' dir: 'Example/ps_dir' options: # [boolean=true] force A4 paper size a4_output: true # [list(dict)] A list of customized reports for the manufacturer custom_reports: # [string=''] Content for the report. Use ${basename} for the project name without extension. # Use ${filename(LAYER)} for the file corresponding to LAYER - content: '' # [string='Custom_report.txt'] File name for the custom report output: 'Custom_report.txt' # [string|list(string)='_none'] Name of the filter to mark components as not fitted. # A short-cut to use for simple cases where a variant is an overkill dnf_filter: '_none' # [string='full'] what to use to indicate the drill places, can be none, small or full (for real scale) drill_marks: 'full' # [string=''] Used to configure the edge cuts layer extension for Protel mode. Include the dot edge_cut_extension: '' # [boolean=true] Do not include the PCB edge layer exclude_edge_layer: true # [boolean=false] Do not plot the component pads in the silk screen (KiCad 5.x only) exclude_pads_from_silkscreen: false # [boolean=false] Include references and values even when they are marked as invisible force_plot_invisible_refs_vals: false # [string=''] 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' inner_extension_pattern: '' # [number=0.15] [0.02,2] For objects without width [mm] (KiCad 5) line_width: 0.15 # [boolean=false] Plot mirrored mirror_plot: false # [boolean=false] Invert black and white negative_plot: false # [string='%f-%i%I%v.%x'] Output file name, the default KiCad name if empty. Affected by global options output: '%f-%i%I%v.%x' # [boolean=true] Include the footprint references plot_footprint_refs: true # [boolean=true] Include the footprint values plot_footprint_values: true # [boolean=false] Currently without effect plot_sheet_reference: false # [number=1.0] Fine grain adjust for the X scale (floating point multiplier) scale_adjust_x: 1.0 # [number=1.0] Fine grain adjust for the Y scale (floating point multiplier) scale_adjust_y: 1.0 # [number=1] Scale factor (0 means autoscaling) scaling: 1 # [boolean=false] Don't fill objects, just draw the outline sketch_plot: false # [boolean=true] Cover the vias tent_vias: true # [boolean=false] Use uppercase names for the extensions uppercase_extensions: false # [string=''] Board variant to apply variant: '' # [number=0] This width factor is intended to compensate PS printers/plotters that do not strictly obey line width settings. # Only used to plot pads and tracks width_adjust: 0 layers: all # QR_Lib: # This output creates a library containing a symbol and footprint for a QR code. # To refresh the generated symbols and footprints use the `update_qr` preflight. # The workflow is as follows: # - Create the symbol and footprints using this output. # - Use them in your schematic and PCB. # - To keep them updated add the `update_qr` preflight - name: 'qr_lib_example' comment: 'Generates a QR code symbol and footprint.' type: 'qr_lib' dir: 'Example/qr_lib_dir' options: # [string='QR'] Short name for the library lib: 'QR' # [string='%f-%i%I%v.%x'] Filename for the output (%i=qr, %x=lib). Affected by global options output: '%f-%i%I%v.%x' # [list(dict)] QR codes to include in the library qrs: # [string='low'] [low,medium,quartile,high] Error correction level - correction_level: 'low' # [string='silk'] [silk,copper] Layer for the footprint layer: 'silk' # [string='QR'] Name for the symbol/footprint name: 'QR' # [boolean=false] Generate a negative image for the PCB pcb_negative: false # [number=15] Size of the QR footprint size_pcb: 15 # [number=15] Size of the QR symbol size_sch: 15 # [string='millimeters'] [millimeters,inches] Units used for the size size_units: 'millimeters' # [string='%p %r'] Text to encode as QR text: '%p %r' # [string='QR'] The reference prefix reference: 'QR' # [boolean=true] Generate the libs relative to the schematic/PCB dir use_sch_dir: true # 3D render of the PCB: - name: 'render_3d_example' comment: "Exports the image generated by KiCad's 3D viewer." type: 'render_3d' dir: 'Example/render_3d_dir' options: # [string='#66667F'] First color for the background gradient background1: '#66667F' # [string='#CCCCE5'] Second color for the background gradient background2: '#CCCCE5' # [string='#332B16'] Color for the board without copper or solder mask board: '#332B16' # [string='#8b898c'] Color for the copper copper: '#8b898c' # [string|list(string)='_none'] Name of the filter to mark components as not fitted. # A short-cut to use for simple cases where a variant is an overkill dnf_filter: '_none' # [boolean=true] Downloads missing 3D models from KiCad git. Only applies to models in KISYS3DMOD download: true # [number=720] Image height (aprox.) height: 720 # [string='https://gitlab.com/kicad/libraries/kicad-packages3D/-/raw/master/'] Base URL for the KiCad 3D models kicad_3d_url: 'https://gitlab.com/kicad/libraries/kicad-packages3D/-/raw/master/' # [number=0] Steps to move in the X axis, positive is to the right. # Just like pressing the right arrow in the 3D viewer move_x: 0 # [number=0] Steps to move in the Y axis, positive is up. # Just like pressing the up arrow in the 3D viewer move_y: 0 # [boolean=false] Used to exclude 3D models for surface mount components no_smd: false # [boolean=false] Used to exclude 3D models for through hole components no_tht: false # [boolean=false] Used to exclude 3D models for components with 'virtual' attribute no_virtual: false # [boolean=false] Enable the orthographic projection mode (top view looks flat) orthographic: false # [string='%f-%i%I%v.%x'] Name for the generated image file (%i='3D_$VIEW' %x='png'). Affected by global options output: '%f-%i%I%v.%x' # [boolean=false] Enable the ray tracing. Much better result, but slow, and you'll need to adjust `wait_rt` ray_tracing: false # [string='#d5dce4'] Color for the silk screen silk: '#d5dce4' # [string='#208b47'] Color for the solder mask solder_mask: '#208b47' # [string='#808080'] Color for the solder paste solder_paste: '#808080' # [string=''] Board variant to apply variant: '' # [string='top'] [top,bottom,front,rear,right,left,z,Z,y,Y,x,X] Point of view view: 'top' # [number=-600] How many seconds we must wait before capturing the ray tracing render. # Lamentably KiCad can save an unfinished image. Enlarge it if your image looks partially rendered. # Use negative values to enable the auto-detect using CPU load. # In this case the value is interpreted as a time-out. wait_ray_tracing: -600 # [number=1280] Image width (aprox.) width: 1280 # [number=0] Zoom steps. Use positive to enlarge, get closer, and negative to reduce. # Same result as using the mouse wheel in the 3D viewer zoom: 0 # Design report: # Mainly oriented to be sent to the manufacturer or check PCB details. - name: 'report_example' comment: 'Generates a report about the design.' type: 'report' dir: 'Example/report_dir' options: # [string='%f-%i%I%v.%x'] Output file name (%i='report', %x='txt'). Affected by global options output: '%f-%i%I%v.%x' # [string='full'] Name for one of the internal templates (full, simple) or a custom template file template: 'full' # Schematic with variant generator: # This copy isn't intended for development. # Is just a tweaked version of the original where you can look at the results. - name: 'sch_variant_example' comment: 'Creates a copy of the schematic with all the filters and variants applied.' type: 'sch_variant' dir: 'Example/sch_variant_dir' options: # [string|list(string)='_none'] Name of the filter to mark components as not fitted. # A short-cut to use for simple cases where a variant is an overkill dnf_filter: '_none' # [string=''] Board variant to apply variant: '' # STEP (ISO 10303-21 Clear Text Encoding of the Exchange Structure): # This is the most common 3D format for exchange purposes. # This output is what you get from the 'File/Export/STEP' menu in pcbnew. - name: 'step_example' comment: 'Exports the PCB as a 3D model.' type: 'step' dir: 'Example/step_dir' options: # [string|list(string)='_none'] Name of the filter to mark components as not fitted. # A short-cut to use for simple cases where a variant is an overkill dnf_filter: '_none' # [boolean=true] Downloads missing 3D models from KiCad git. Only applies to models in KISYS3DMOD download: true # [string='https://gitlab.com/kicad/libraries/kicad-packages3D/-/raw/master/'] Base URL for the KiCad 3D models kicad_3d_url: 'https://gitlab.com/kicad/libraries/kicad-packages3D/-/raw/master/' # [boolean=true] Use metric units instead of inches metric_units: true # [number=-1] The minimum distance between points to treat them as separate ones (-1 is KiCad default: 0.01 mm) min_distance: -1 # [boolean=false] Used to exclude 3D models for components with 'virtual' attribute no_virtual: false # [string='grid'] Determines the coordinates origin. Using grid the coordinates are the same as you have in the design sheet. # The drill option uses the auxiliary reference defined by the user. # You can define any other origin using the format 'X,Y', i.e. '3.2,-10' origin: 'grid' # [string='%f-%i%I%v.%x'] Name for the generated STEP file (%i='3D' %x='step'). Affected by global options output: '%f-%i%I%v.%x' # [boolean=true] Substitute STEP or IGS models with the same name in place of VRML models subst_models: true # [string=''] Board variant to apply variant: '' # SVG (Scalable Vector Graphics): # Unlike bitmaps SVG drawings can be scaled without losing resolution. # This output is what you get from the File/Plot menu in pcbnew. - name: 'svg_example' comment: 'Exports the PCB to a format suitable for 2D graphics software.' type: 'svg' dir: 'Example/svg_dir' options: # [list(dict)] A list of customized reports for the manufacturer custom_reports: # [string=''] Content for the report. Use ${basename} for the project name without extension. # Use ${filename(LAYER)} for the file corresponding to LAYER - content: '' # [string='Custom_report.txt'] File name for the custom report output: 'Custom_report.txt' # [string|list(string)='_none'] Name of the filter to mark components as not fitted. # A short-cut to use for simple cases where a variant is an overkill dnf_filter: '_none' # [string='full'] what to use to indicate the drill places, can be none, small or full (for real scale) drill_marks: 'full' # [string=''] Used to configure the edge cuts layer extension for Protel mode. Include the dot edge_cut_extension: '' # [boolean=true] Do not include the PCB edge layer exclude_edge_layer: true # [boolean=false] Do not plot the component pads in the silk screen (KiCad 5.x only) exclude_pads_from_silkscreen: false # [boolean=false] Include references and values even when they are marked as invisible force_plot_invisible_refs_vals: false # [string=''] 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' inner_extension_pattern: '' # [number=0.25] [0.02,2] For objects without width [mm] (KiCad 5) line_width: 0.25 # [boolean=false] Plot mirrored mirror_plot: false # [boolean=false] Invert black and white negative_plot: false # [string='%f-%i%I%v.%x'] Output file name, the default KiCad name if empty. Affected by global options output: '%f-%i%I%v.%x' # [boolean=true] Include the footprint references plot_footprint_refs: true # [boolean=true] Include the footprint values plot_footprint_values: true # [boolean=false] Currently without effect plot_sheet_reference: false # [boolean=true] Cover the vias tent_vias: true # [boolean=false] Use uppercase names for the extensions uppercase_extensions: false # [string=''] Board variant to apply variant: '' layers: all # SVG PCB Print (Scalable Vector Graphics): # This output is what you get from the 'File/Print' menu in pcbnew. - name: 'svg_pcb_print_example' comment: 'Exports the PCB to the scalable vector graphics format.' type: 'svg_pcb_print' dir: 'Example/svg_pcb_print_dir' options: # [string|list(string)='_none'] Name of the filter to mark components as not fitted. # A short-cut to use for simple cases where a variant is an overkill dnf_filter: '_none' # [string='full'] What to use to indicate the drill places, can be none, small or full (for real scale) drill_marks: 'full' # [boolean=true] Enable workaround for KiCad 6 bug #11033 enable_ki6_page_fix: true # [boolean=true] Only useful for KiCad 6 when printing in one page, you can disable the edge here. # KiCad 5 forces it by default, and you can't control it from config files. # Same for KiCad 6 when printing to separated pages force_edge_cuts: true # [boolean=false] Hide components in the Fab layer that are marked as excluded by a variant hide_excluded: false # [boolean=false] Print mirrored (X axis inverted). ONLY for KiCad 6 mirror: false # [boolean=false] Print in black and white monochrome: false # [string='%f-%i%I%v.%x'] Filename for the output SVG (%i=layers, %x=svg). Affected by global options output: '%f-%i%I%v.%x' # `output_name` is an alias for `output` # [boolean=true] Include the title-block plot_sheet_reference: true # [number=1.0] Scale factor (0 means autoscaling) scaling: 1.0 # [boolean=false] Print layers in separated pages separated: false # [string=''] Text used to replace the sheet title. %VALUE expansions are allowed. # If it starts with `+` the text is concatenated title: '' # [string=''] Board variant to apply variant: '' layers: all # SVG Schematic Print: # This is a format to document your schematic. - name: 'svg_sch_print_example' comment: 'Exports the PCB. Suitable for printing.' type: 'svg_sch_print' dir: 'Example/svg_sch_print_dir' options: # [string|list(string)='_none'] Name of the filter to mark components as not fitted. # A short-cut to use for simple cases where a variant is an overkill dnf_filter: '_none' # [string='%f-%i%I%v.%x'] Filename for the output SVG (%i=schematic %x=svg). Affected by global options output: '%f-%i%I%v.%x' # [string=''] Board variant to apply. # Not fitted components are crossed variant: ''