kiplot:
  version: 1

preflight:
  # [boolean=false] Zones are filled before doing any operation involving PCB layers
  check_zone_fills: true
  # [list(dict)] A list of entries to filter out ERC/DRC messages
  filters: 
    - filter: 'Filter description'
      number: 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
  # [boolean=false] Runs the DRC (Distance Rules Check). To ensure we have a valid PCB
  run_drc: true
  # [boolean=false] Runs the ERC (Electrical Rules Check). To ensure the schematic is electrically correct
  run_erc: true
  # [boolean=false] Update the XML version of the BoM (Bill of Materials). To ensure our generated BoM is up to date
  update_xml: true

outputs:
  # 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:
      # [string='full'] what to use to indicate the drill places, can be none, small or full (for real scale)
      drill_marks: 'full'
      # [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
      exclude_pads_from_silkscreen: false
      # [boolean=false] include references and values even when they are marked as invisible
      force_plot_invisible_refs_vals: false
      # [boolean=false] use mm instead of inches
      metric_units: false
      # [string=''] output file name, the default KiCad name if empty
      output: ''
      # [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 the auxiliar axis as origin for coordinates
      use_aux_axis_as_origin: false
    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:
      # [dict|string] [hpgl,ps,gerber,dxf,svg,pdf] format for a graphical drill map.
      # Not generated unless a format is specified
      map:
        # [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
      # [boolean=true] generate one file for both, plated holes and non-plated holes, instead of two separated files
      pth_and_npth_single_file: true
      # [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
        filename: ''
      # [boolean=false] use the auxiliar axis as origin for coordinates
      use_aux_axis_as_origin: false

  # 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='pdf'] [hpgl,ps,gerber,dxf,svg,pdf] format for a graphical drill map
        type: 'pdf'
      # [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
        filename: ''
      # [boolean=false] use the auxiliar 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
      # [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
      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-job.%x'] name for the gerber job file
      gerber_job_file: '%f-job.%x'
      # [number=4.6] this the gerber coordinate format, can be 4.5 or 4.6
      gerber_precision: 4.6
      # [number=0.1] [0.02,2] line_width for objects without width [mm]
      line_width: 0.1
      # [string=''] output file name, the default KiCad name if empty
      output: ''
      # [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] substract the solder mask from the silk screen
      subtract_mask_from_silk: false
      # [boolean=true] cover the vias
      tent_vias: true
      # [boolean=false] use the auxiliar 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
      use_gerber_x2_attributes: true
      # [boolean=false] use legacy Protel file extensions
      use_protel_extensions: false
    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:
      # [string='full'] what to use to indicate the drill places, can be none, small or full (for real scale)
      drill_marks: 'full'
      # [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
      exclude_pads_from_silkscreen: false
      # [boolean=false] include references and values even when they are marked as invisible
      force_plot_invisible_refs_vals: false
      # [boolean=false] plot mirrored
      mirror_plot: false
      # [string=''] output file name, the default KiCad name if empty
      output: ''
      # [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
    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*'
      blacklist: ''
      # [boolean=false] Blacklist components with empty value
      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=''] Name of the extra field that indicates do not populate status. Components with this field not empty will be
      # blacklisted
      dnp_field: ''
      # [string=''] Comma separated list of extra fields to pull from netlist or xml file
      extra_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
      name_format: 'ibom'
      # [string=''] Path to netlist or xml file
      netlist_file: ''
      # [boolean=false] Do not blacklist virtual components
      no_blacklist_virtual: 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
      # [boolean=false] Show fabrication layer by default
      show_fabrication: false
      # [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=''] Name of the extra field that stores board variant for component
      variant_field: ''
      # [string=''] List of board variants to exclude from the BOM
      variants_blacklist: ''
      # [string=''] List of board variants to include in the BOM
      variants_whitelist: ''

  # KiBoM (KiCad Bill of Materials):
  # For more information: https://github.com/INTI-CMNB/KiBoM
  # 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='bom.ini'] BoM configuration file, relative to PCB
      conf: 'bom.ini'
      # [string='HTML'] [HTML,CSV] format for the BoM
      format: 'HTML'
      # [number=1] Number of boards to build (components multiplier)
      number: 1
      # [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
      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
      # [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.%x'] name for the generated file
      output: '%f-%i.%x'
      # [boolean=false] show placeholder for missing components
      placeholder: false
      # [dict|None] replacements for PCB references using components (lib:component)
      remap:
      # [string|list(string)] [none,all] list of components to draw, can be also a string for none or all.
      # The default is none
      show_components:
      # [string|dict] PCB style (colors). An internal name, the name of a JSON file or the style options
      style:
        # [string='#4ca06c'] color for the board without copper (covered by solder mask)
        board: '#4ca06c'
        # [string='#9c6b28'] color for the PCB core (not covered by solder mask)
        clad: '#9c6b28'
        # [string='#417e5a'] color for the copper zones (covered by solder mask)
        copper: '#417e5a'
        # [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='#b5ae30'] color for the exposed pads (metal finish)
        pads: '#b5ae30'
        # [string='#f0f0f0'] color for the silk screen
        silk: '#f0f0f0'
        # [string='#bf2600'] color for the V-CUTS
        vcut: '#bf2600'
      # [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 exhange format. Suitable for printing.'
    type: 'pdf'
    dir: 'Example/pdf_dir'
    options:
      # [string='full'] what to use to indicate the drill places, can be none, small or full (for real scale)
      drill_marks: 'full'
      # [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
      exclude_pads_from_silkscreen: false
      # [boolean=false] include references and values even when they are marked as invisible
      force_plot_invisible_refs_vals: false
      # [number=0.1] [0.02,2] for objects without width [mm]
      line_width: 0.1
      # [boolean=false] plot mirrored
      mirror_plot: false
      # [boolean=false] invert black and white
      negative_plot: false
      # [string=''] output file name, the default KiCad name if empty
      output: ''
      # [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
    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 exhange format. Suitable for printing.'
    type: 'pdf_pcb_print'
    dir: 'Example/pdf_pcb_print_dir'
    options:
      # [string='%f.pdf'] filename for the output PDF
      output: '%f.pdf'
      # `output_name` is an alias for `output`
    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 exhange format. Suitable for printing.'
    type: 'pdf_sch_print'
    dir: 'Example/pdf_sch_print_dir'
    options:
      # [string=''] filename for the output PDF (the name of the schematic if empty)
      output: ''

  # Pick & place:
  # This output is what you get from the 'File/Fabrication output/Footprint poistion (.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:
      # [string='ASCII'] [ASCII,CSV] format for the position file
      format: 'ASCII'
      # [boolean=true] only include the surface mount components
      only_smd: true
      # [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] units used for the positions
      units: 'millimeters'

  # 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
      # [string='full'] what to use to indicate the drill places, can be none, small or full (for real scale)
      drill_marks: 'full'
      # [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
      exclude_pads_from_silkscreen: false
      # [boolean=false] include references and values even when they are marked as invisible
      force_plot_invisible_refs_vals: false
      # [number=0.15] [0.02,2] for objects without width [mm]
      line_width: 0.15
      # [boolean=false] plot mirrored
      mirror_plot: false
      # [boolean=false] invert black and white
      negative_plot: false
      # [string=''] output file name, the default KiCad name if empty
      output: ''
      # [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
      # [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

  # 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:
      # [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 auxiliar reference defined by the user.
      # You can define any other origin using the format 'X,Y', i.e. '3.2,-10'
      origin: 'grid'
      # [string=''] name for the generated STEP file (the name of the PCB if empty)
      output: ''

  # 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:
      # [string='full'] what to use to indicate the drill places, can be none, small or full (for real scale)
      drill_marks: 'full'
      # [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
      exclude_pads_from_silkscreen: false
      # [boolean=false] include references and values even when they are marked as invisible
      force_plot_invisible_refs_vals: false
      # [number=0.25] [0.02,2] for objects without width [mm]
      line_width: 0.25
      # [boolean=false] plot mirrored
      mirror_plot: false
      # [boolean=false] invert black and white
      negative_plot: false
      # [string=''] output file name, the default KiCad name if empty
      output: ''
      # [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
    layers: all