KiPlot

KiPlot is a program which helps you to plot your KiCad PCBs to output formats easily, repeatable, and most of all, scriptably. This means you can use a Makefile to export your KiCad PCBs just as needed.

For example, it's common that you might want for each board rev:

• Check ERC/DRC one last time (using KiCad Automation Scripts)
• Gerbers, drills and drill maps for a fab in their favourite format
• Fab docs for the assembler
• Pick and place files
• PCB 3D model in STEP format

You want to do this in a one-touch way, and make sure everything you need to do so it securely saved in version control, not on the back of an old datasheet.

KiPlot lets you do this.

As a side effect of providing a scriptable plot driver for KiCad, KiPlot also allows functional testing of KiCad plot functions, which would otherwise be somewhat unwieldy to write.

The configuration file

Kiplot uses a configuration file where you can specify what outputs to generate. By default you'll generate all of them, but you can specify which ones from the command line.

The configuration file should be named .kiplot.yaml. The format used is YAML. This is basically a text file with some structure. This file can be compressed using gzip file format.

The header

All configuration files must start with:

kiplot:
  version: 1

This tells to Kiplot that this file is using version 1 of the format.

The preflight section

This section is used to specify tasks that will executed before generating any output. The available tasks are:

• run_erc To run the ERC (Electrical Rules Check). To ensure the schematic is electrically correct.
• run_drc To run the DRC (Distance Rules Check). To ensure we have a valid PCB.
• update_xml To update the XML version of the BoM (Bill of Materials). To ensure our generated BoM is up to date.
• check_zone_fills Zones are filled before doing any operation involving PCB layers.

The run_drc command has the following option:

• ignore_unconnected Ignores the unconnected nets. Useful if you didn't finish the routing.

Here is an example of a preflight section:

preflight:
  run_erc: true
  update_xml: true
  run_drc: true
  check_zone_fills: true
  ignore_unconnected: false

Filtering DRC/ERC errors

Sometimes KiCad reports DRC or ERC errors that you can't get rid off. This could be just because you are part of a team including lazzy people that doesn't want to take the extra effort to solve some errors that aren't in fact errors, just small violations made on purpose. In this case you could exclude some known errors.

For this you must declare filters entry in the preflight section. Then you can add as many filter entries as you want. Each filter entry has an optional description and defines to which error type is applied (number) and a regular expression that the error must match to be ignored (regex). Like this:

  filters:
    - filter: 'Optional filter description'
      number: Numeric_error_type
      regex:  'Expression to match'

Here is an example, suppose you are getting the following errors:

** Found 1 DRC errors **
ErrType(4): Track too close to pad
    @(177.185 mm, 78.315 mm): Track 1.000 mm [Net-(C3-Pad1)] on F.Cu, length: 1.591 mm
    @(177.185 mm, 80.715 mm): Pad 2 of C3 on F.Cu and others

** Found 1 unconnected pads **
ErrType(2): Unconnected items
    @(177.185 mm, 73.965 mm): Pad 2 of C4 on F.Cu and others
    @(177.185 mm, 80.715 mm): Pad 2 of C3 on F.Cu and others

And you want to ignore them. You can add the following filters:

  filters:
    - filter: 'Ignore C3 pad 2 too close to anything'
      number: 4
      regex:  'Pad 2 of C3'
    - filter: 'Ignore unconnected pad 2 of C4'
      number: 2
      regex:  'Pad 2 of C4'

If you need to match text from two different lines in the error message try using (?s)TEXT(.*)TEXT_IN_OTHER_LINE.

If you have two or more different options for a text to match try using (OPTION1|OPTION2).

A complete Python regular expressions explanation is out the scope of this manual. For a complete reference consult the Python manual.

Important note: this will create a file named kiplot_errors.filter in the output directory.

The outputs section

In this section you put all the things that you want to generate. This section contains one or more outputs. Each output contain the following data:

• name a name so you can easily identify it.
• comment a short description of this output.
• type selects which type of output will be generated. Examples are gerbers, drill files and pick & place files
• dir is the directory where this output will be stored.
• options contains one or more options to configure this output.
• layers a list of layers used for this output. Not all outputs needs this subsection.

Important note about the layers: In the original kiplot (from John Beard) the name of the inner layers was Inner.N where N is the number of the layer, i.e. Inner.1 is the first inner layer. This format is supported for compatibility. Note that this generated a lot of confusion because the default KiCad name for the first inner layer is In1.Cu. People filled issues and submitted pull-requests to fix it, thinking that inner layers weren't supported. Currently KiCad allows renaming these layers, so this version of kiplot supports the name used in KiCad. Just use the same name you see in the user interface.

The available values for type are:

• Plot formats:
  • gerber the gerbers for fabrication.
  • ps postscript plot
  • hpgl format for laser printers
  • svg scalable vector graphics
  • pdf portable document format
  • dxf mechanical CAD format
• Drill formats:
  • excellon data for the drilling machine
  • gerb_drill drilling positions in a gerber file
• Pick & place
  • position of the components for the pick & place machine
• Documentation
  • pdf_sch_print schematic in PDF format
  • pdf_pcb_printPDF file containing one or more layer and the page frame
• Bill of Materials
  • kibom BoM in HTML or CSV format generated by KiBoM
  • ibom Interactive HTML BoM generated by InteractiveHtmlBom
• 3D model:
  • step Standard for the Exchange of Product Data for the PCB

Here is an example of a configuration file to generate the gerbers for the top and bottom layers:

kiplot:
  version: 1

preflight:
  run_drc: true

outputs:

  - name: 'gerbers'
    comment: "Gerbers for the board house"
    type: gerber
    dir: gerberdir
    options:
      # generic layer options
      exclude_edge_layer: false
      exclude_pads_from_silkscreen: false
      plot_sheet_reference: false
      plot_footprint_refs: true
      plot_footprint_values: true
      force_plot_invisible_refs_vals: false
      tent_vias: true
      line_width: 0.15

      # gerber options
      use_aux_axis_as_origin: false
      subtract_mask_from_silk: true
      use_protel_extensions: false
      gerber_precision: 4.5
      create_gerber_job_file: true
      use_gerber_x2_attributes: true
      use_gerber_net_attributes: false

    layers:
      - 'F.Cu'
      - 'B.Cu'

Most options are the same you'll find in the KiCad dialogs.

Specifying the layers

You have various ways to specify the layers. If you need to specify just one layer you can just use its name:

    layers: 'F.Cu'

If you want to specify all the available layers:

    layers: 'all'

You can also select the layers you want in KiCad (using File, Plot dialog) and save your PCB. Then you just need to use:

    layers: 'selected'

You can also use any of the following grup of layers:

• copper all the copper layers
• technical all the technical layers (silk sreen, solder mask, paste, adhesive, etc.)
• user all the user layers (draw, comments, eco, margin, edge cuts, etc.)

You can also mix the above definitions using a list:

    layers:
      - 'copper'
      - 'Dwgs.User'

This will select all the copper layers and the user drawings. Note that the above mentioned options will use file name suffixes and descriptions selected automatically. If you want to use a particular suffix and provide better descriptions you can use the following format:

    layers:
      - layer: 'F.Cu'
        suffix: 'F_Cu'
        description: 'Front copper'
      - layer: 'B.Cu'
        suffix: 'B_Cu'
        description: 'Bottom copper'

You can also mix the styles:

    layers:
      - 'copper'
      - layer: 'Cmts.User'
        suffix: 'Cmts_User'
        description: 'User comments'
      - 'Dwgs.User'

If you need to use the same list of layers for various outputs you can use YAML anchors. The first time you define the list of layers just assign an ancho, here is an example:

    layers: &copper_and_cmts
      - copper
      - 'Cmts.User'

Next time you need this list just use an alias, like this:

    layers: *copper_and_cmts

Supported outputs:

• DXF (Drawing Exchange Format)

  • Type: dxf
  • Description: Exports the PCB to 2D mechanical EDA tools (like AutoCAD). This output is what you get from the File/Plot menu in pcbnew.
  • Valid keys:
    • comment: [string=''] A comment for documentation purposes.
    • dir: [string='.'] Output directory for the generated files.
    • layers: [list(dict)|list(string)|string] [all,selected,copper,technical,user] List of PCB layers to plot.
      • Valid keys:
        • description: [string=''] A description for the layer, for documentation purposes.
        • layer: [string=''] Name of the layer. As you see it in KiCad.
        • suffix: [string=''] Suffix used in file names related to this layer. Derived from the name if not specified.
    • name: [string=''] Used to identify this particular output definition.
    • options: [dict] Options for the dxf output.
      • Valid keys:
        • drill_marks: [string='full'] what to use to indicate the drill places, can be none, small or full (for real scale).
        • exclude_edge_layer: [boolean=true] do not include the PCB edge layer.
        • exclude_pads_from_silkscreen: [boolean=false] do not plot the component pads in the silk screen.
        • force_plot_invisible_refs_vals: [boolean=false] include references and values even when they are marked as invisible.
        • metric_units: [boolean=false] use mm instead of inches.
        • plot_footprint_refs: [boolean=true] include the footprint references.
        • plot_footprint_values: [boolean=true] include the footprint values.
        • plot_sheet_reference: [boolean=false] currently without effect.
        • polygon_mode: [boolean=true] plot using the contour, instead of the center line.
        • sketch_plot: [boolean=false] don't fill objects, just draw the outline.
        • tent_vias: [boolean=true] cover the vias.
        • use_aux_axis_as_origin: [boolean=false] use the auxiliar axis as origin for coordinates.

• Excellon drill format

  • Type: excellon
  • Description: This is the main format for the drilling machine. 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.
  • Valid keys:
    • comment: [string=''] A comment for documentation purposes.
    • dir: [string='.'] Output directory for the generated files.
    • name: [string=''] Used to identify this particular output definition.
    • options: [dict] Options for the excellon output.
      • Valid keys:
        • map: [dict|string] [hpgl,ps,gerber,dxf,svg,pdf] format for a graphical drill map. Not generated unless a format is specified.
          • Valid keys:
            • type: [string='pdf'] [hpgl,ps,gerber,dxf,svg,pdf] format for a graphical drill map.
        • metric_units: [boolean=true] use metric units instead of inches.
        • minimal_header: [boolean=false] use a minimal header in the file.
        • mirror_y_axis: [boolean=false] invert the Y axis.
        • pth_and_npth_single_file: [boolean=true] generate one file for both, plated holes and non-plated holes, instead of two separated files.
        • report: [dict|string] name of the drill report. Not generated unless a name is specified.
          • Valid keys:
            • filename: [string=''] name of the drill report. Not generated unless a name is specified.
        • use_aux_axis_as_origin: [boolean=false] use the auxiliar axis as origin for coordinates.

• Gerber drill format

  • Type: gerb_drill
  • Description: This is the information for the drilling machine in gerber 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.
  • Valid keys:
    • comment: [string=''] A comment for documentation purposes.
    • dir: [string='.'] Output directory for the generated files.
    • name: [string=''] Used to identify this particular output definition.
    • options: [dict] Options for the gerb_drill output.
      • Valid keys:
        • map: [dict|string] [hpgl,ps,gerber,dxf,svg,pdf] format for a graphical drill map. Not generated unless a format is specified.
          • Valid keys:
            • type: [string='pdf'] [hpgl,ps,gerber,dxf,svg,pdf] format for a graphical drill map.
        • report: [dict|string] name of the drill report. Not generated unless a name is specified.
          • Valid keys:
            • filename: [string=''] name of the drill report. Not generated unless a name is specified.
        • use_aux_axis_as_origin: [boolean=false] use the auxiliar axis as origin for coordinates.

• Gerber format

  • Type: gerber
  • Description: This is the main fabrication format for the PCB. This output is what you get from the File/Plot menu in pcbnew.
  • Valid keys:
    • comment: [string=''] A comment for documentation purposes.
    • dir: [string='.'] Output directory for the generated files.
    • layers: [list(dict)|list(string)|string] [all,selected,copper,technical,user] List of PCB layers to plot.
      • Valid keys:
        • description: [string=''] A description for the layer, for documentation purposes.
        • layer: [string=''] Name of the layer. As you see it in KiCad.
        • suffix: [string=''] Suffix used in file names related to this layer. Derived from the name if not specified.
    • name: [string=''] Used to identify this particular output definition.
    • options: [dict] Options for the gerber output.
      • Valid keys:
        • create_gerber_job_file: [boolean=true] creates a file with information about all the generated gerbers. You can use it in gerbview to load all gerbers at once.
        • exclude_edge_layer: [boolean=true] do not include the PCB edge layer.
        • exclude_pads_from_silkscreen: [boolean=false] do not plot the component pads in the silk screen.
        • force_plot_invisible_refs_vals: [boolean=false] include references and values even when they are marked as invisible.
        • gerber_precision: [number=4.6] this the gerber coordinate format, can be 4.5 or 4.6.
        • line_width: [number=0.1] [0.02,2] line_width for objects without width [mm].
        • plot_footprint_refs: [boolean=true] include the footprint references.
        • plot_footprint_values: [boolean=true] include the footprint values.
        • plot_sheet_reference: [boolean=false] currently without effect.
        • subtract_mask_from_silk: [boolean=false] substract the solder mask from the silk screen.
        • tent_vias: [boolean=true] cover the vias.
        • use_aux_axis_as_origin: [boolean=false] use the auxiliar axis as origin for coordinates.
        • use_gerber_net_attributes: [boolean=true] include netlist metadata.
        • use_gerber_x2_attributes: [boolean=true] use the extended X2 format.
        • use_protel_extensions: [boolean=false] use legacy Protel file extensions.

• HPGL (Hewlett & Packard Graphics Language)

  • Type: hpgl
  • Description: Exports the PCB for plotters and laser printers. This output is what you get from the File/Plot menu in pcbnew.
  • Valid keys:
    • comment: [string=''] A comment for documentation purposes.
    • dir: [string='.'] Output directory for the generated files.
    • layers: [list(dict)|list(string)|string] [all,selected,copper,technical,user] List of PCB layers to plot.
      • Valid keys:
        • description: [string=''] A description for the layer, for documentation purposes.
        • layer: [string=''] Name of the layer. As you see it in KiCad.
        • suffix: [string=''] Suffix used in file names related to this layer. Derived from the name if not specified.
    • name: [string=''] Used to identify this particular output definition.
    • options: [dict] Options for the hpgl output.
      • Valid keys:
        • drill_marks: [string='full'] what to use to indicate the drill places, can be none, small or full (for real scale).
        • exclude_edge_layer: [boolean=true] do not include the PCB edge layer.
        • exclude_pads_from_silkscreen: [boolean=false] do not plot the component pads in the silk screen.
        • force_plot_invisible_refs_vals: [boolean=false] include references and values even when they are marked as invisible.
        • mirror_plot: [boolean=false] plot mirrored.
        • pen_number: [number=1] [1,16] pen number.
        • pen_speed: [number=20] [1,99] pen speed.
        • pen_width: [number=15] [0,100] pen diameter in MILS, useful to fill areas. However, it is in mm in HPGL files.
        • plot_footprint_refs: [boolean=true] include the footprint references.
        • plot_footprint_values: [boolean=true] include the footprint values.
        • plot_sheet_reference: [boolean=false] currently without effect.
        • scaling: [number=0] scale factor (0 means autoscaling).
        • sketch_plot: [boolean=false] don't fill objects, just draw the outline.
        • tent_vias: [boolean=true] cover the vias.

• IBoM (Interactive HTML BoM)

  • Type: ibom
  • Description: Generates an interactive web page useful to identify the position of the components in the PCB. For more information: https://github.com/INTI-CMNB/InteractiveHtmlBom This output is what you get from the InteractiveHtmlBom plug-in (pcbnew).
  • Valid keys:
    • comment: [string=''] A comment for documentation purposes.
    • dir: [string='.'] Output directory for the generated files.
    • name: [string=''] Used to identify this particular output definition.
    • options: [dict] Options for the ibom output.
      • Valid keys:
        • blacklist: [string=''] List of comma separated blacklisted components or prefixes with . E.g. 'X1,MH'.
        • blacklist_empty_val: [boolean=false] Blacklist components with empty value.
        • board_rotation: [number=0] Board rotation in degrees (-180 to 180). Will be rounded to multiple of 5.
        • bom_view: [string='left-right'] [bom-only,left-right,top-bottom] Default BOM view.
        • checkboxes: [string='Sourced,Placed'] Comma separated list of checkbox columns.
        • dark_mode: [boolean=false] Default to dark mode.
        • dnp_field: [string=''] Name of the extra field that indicates do not populate status. Components with this field not empty will be blacklisted.
        • extra_fields: [string=''] Comma separated list of extra fields to pull from netlist or xml file.
        • hide_pads: [boolean=false] Hide footprint pads by default.
        • hide_silkscreen: [boolean=false] Hide silkscreen by default.
        • highlight_pin1: [boolean=false] Highlight pin1 by default.
        • include_nets: [boolean=false] Include netlist information in output..
        • include_tracks: [boolean=false] Include track/zone information in output. F.Cu and B.Cu layers only.
        • layer_view: [string='FB'] [F,FB,B] Default layer view.
        • name_format: [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.
        • netlist_file: [string=''] Path to netlist or xml file.
        • no_blacklist_virtual: [boolean=false] Do not blacklist virtual components.
        • no_redraw_on_drag: [boolean=false] Do not redraw pcb on drag by default.
        • normalize_field_case: [boolean=false] Normalize extra field name case. E.g. 'MPN' and 'mpn' will be considered the same field.
        • show_fabrication: [boolean=false] Show fabrication layer by default.
        • sort_order: [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.
        • variant_field: [string=''] Name of the extra field that stores board variant for component.
        • variants_blacklist: [string=''] List of board variants to exclude from the BOM.
        • variants_whitelist: [string=''] List of board variants to include in the BOM.

• KiBoM (KiCad Bill of Materials)

  • Type: kibom
  • Description: Used to generate the BoM in HTML or CSV format using the KiBoM plug-in. 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.
  • Valid keys:
    • comment: [string=''] A comment for documentation purposes.
    • dir: [string='.'] Output directory for the generated files.
    • name: [string=''] Used to identify this particular output definition.
    • options: [dict] Options for the kibom output.
      • Valid keys:
        • conf: [string='bom.ini'] BoM configuration file, relative to PCB.
        • format: [string='HTML'] [HTML,CSV] format for the BoM.
        • number: [number=1] Number of boards to build (components multiplier).
        • separator: [string=','] CSV Separator.
        • variant: [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.

• PcbDraw - Beautiful 2D PCB render

  • Type: pcbdraw
  • Description: Exports the PCB as a 2D model (SVG, PNG or JPG). Uses configurable colors. Can also render the components if the 2D models are available
  • Valid keys:
    • comment: [string=''] A comment for documentation purposes.
    • dir: [string='.'] Output directory for the generated files.
    • name: [string=''] Used to identify this particular output definition.
    • options: [dict] Options for the pcbdraw output.
      • Valid keys:
        • bottom: [boolean=false] render the bottom side of the board (default is top side).
        • dpi: [number=300] [10,1200] dots per inch (resolution) of the generated image.
        • format: [string='svg'] [svg,png,jpg] output format. Only used if no output is specified.
        • highlight: [list(string)] list of components to highlight.
        • libs: [list(string)] list of libraries.
        • mirror: [boolean=false] mirror the board.
        • no_drillholes: [boolean=false] do not make holes transparent.
        • output: [string='%f-%i.%x'] name for the generated file.
        • placeholder: [boolean=false] show placeholder for missing components.
        • remap: [dict|None] replacements for PCB references using components (lib:component).
        • show_components: [string|list(string)] [none,all] list of components to draw, can be also a string for none or all. The default is none.
        • style: [string|dict] PCB style (colors). An internal name, the name of a JSON file or the style options.
          • Valid keys:
            • board: [string='#4ca06c'] color for the board without copper (covered by solder mask).
            • clad: [string='#9c6b28'] color for the PCB core (not covered by solder mask).
            • copper: [string='#417e5a'] color for the copper zones (covered by solder mask).
            • highlight_on_top: [boolean=false] highlight over the component (not under).
            • highlight_padding: [number=1.5] [0,1000] how much the highlight extends around the component [mm].
            • highlight_style: [string='stroke:none;fill:#ff0000;opacity:0.5;'] SVG code for the highlight style.
            • outline: [string='#000000'] color for the outline.
            • pads: [string='#b5ae30'] color for the exposed pads (metal finish).
            • silk: [string='#f0f0f0'] color for the silk screen.
            • vcut: [string='#bf2600'] color for the V-CUTS.
        • vcuts: [boolean=false] render V-CUTS on the Cmts.User layer.
        • warnings: [string='visible'] [visible,all,none] using visible only the warnings about components in the visible side are generated.

• PDF (Portable Document Format)

  • Type: pdf
  • Description: Exports the PCB to the most common exhange format. Suitable for printing. 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.
  • Valid keys:
    • comment: [string=''] A comment for documentation purposes.
    • dir: [string='.'] Output directory for the generated files.
    • drill_marks: [string='full'] what to use to indicate the drill places, can be none, small or full (for real scale).
    • exclude_edge_layer: [boolean=true] do not include the PCB edge layer.
    • exclude_pads_from_silkscreen: [boolean=false] do not plot the component pads in the silk screen.
    • force_plot_invisible_refs_vals: [boolean=false] include references and values even when they are marked as invisible.
    • layers: [list(dict)|list(string)|string] [all,selected,copper,technical,user] List of PCB layers to plot.
      • Valid keys:
        • description: [string=''] A description for the layer, for documentation purposes.
        • layer: [string=''] Name of the layer. As you see it in KiCad.
        • suffix: [string=''] Suffix used in file names related to this layer. Derived from the name if not specified.
    • name: [string=''] Used to identify this particular output definition.
    • options: [dict] Options for the pdf output.
      • Valid keys:
        • drill_marks: [string='full'] what to use to indicate the drill places, can be none, small or full (for real scale).
        • exclude_edge_layer: [boolean=true] do not include the PCB edge layer.
        • exclude_pads_from_silkscreen: [boolean=false] do not plot the component pads in the silk screen.
        • force_plot_invisible_refs_vals: [boolean=false] include references and values even when they are marked as invisible.
        • line_width: [number=0.1] [0.02,2] for objects without width [mm].
        • mirror_plot: [boolean=false] plot mirrored.
        • negative_plot: [boolean=false] invert black and white.
        • plot_footprint_refs: [boolean=true] include the footprint references.
        • plot_footprint_values: [boolean=true] include the footprint values.
        • plot_sheet_reference: [boolean=false] currently without effect.
        • tent_vias: [boolean=true] cover the vias.
    • plot_footprint_refs: [boolean=true] include the footprint references.
    • plot_footprint_values: [boolean=true] include the footprint values.
    • plot_sheet_reference: [boolean=false] currently without effect.
    • tent_vias: [boolean=true] cover the vias.

• PDF PCB Print (Portable Document Format)

  • Type: pdf_pcb_print
  • Description: Exports the PCB to the most common exhange format. Suitable for printing. This is the main format to document your PCB. This output is what you get from the 'File/Print' menu in pcbnew.
  • Valid keys:
    • comment: [string=''] A comment for documentation purposes.
    • dir: [string='.'] Output directory for the generated files.
    • layers: [list(dict)|list(string)|string] [all,selected,copper,technical,user] List of PCB layers to include in the PDF.
      • Valid keys:
        • description: [string=''] A description for the layer, for documentation purposes.
        • layer: [string=''] Name of the layer. As you see it in KiCad.
        • suffix: [string=''] Suffix used in file names related to this layer. Derived from the name if not specified.
    • name: [string=''] Used to identify this particular output definition.
    • options: [dict] Options for the pdf_pcb_print output.
      • Valid keys:
        • output_name: [string=''] filename for the output PDF (the name of the PCB if empty).

• PDF Schematic Print (Portable Document Format)

  • Type: pdf_sch_print
  • Description: Exports the PCB to the most common exhange format. Suitable for printing. This is the main format to document your schematic. This output is what you get from the 'File/Print' menu in eeschema.
  • Valid keys:
    • comment: [string=''] A comment for documentation purposes.
    • dir: [string='.'] Output directory for the generated files.
    • name: [string=''] Used to identify this particular output definition.
    • options: [dict] Options for the pdf_sch_print output.
      • Valid keys:
        • output: [string=''] filename for the output PDF (the name of the schematic if empty).

• Pick & place

  • Type: position
  • Description: Generates the file with position information for the PCB components, used by the pick and place machine. This output is what you get from the 'File/Fabrication output/Footprint poistion (.pos) file' menu in pcbnew.
  • Valid keys:
    • comment: [string=''] A comment for documentation purposes.
    • dir: [string='.'] Output directory for the generated files.
    • name: [string=''] Used to identify this particular output definition.
    • options: [dict] Options for the position output.
      • Valid keys:
        • format: [string='ASCII'] [ASCII,CSV] format for the position file.
        • only_smd: [boolean=true] only include the surface mount components.
        • separate_files_for_front_and_back: [boolean=true] generate two separated files, one for the top and another for the bottom.
        • units: [string='millimeters'] [millimeters,inches] units used for the positions.

• PS (Postscript)

  • Type: ps
  • Description: Exports the PCB to a format suitable for printing. This output is what you get from the File/Plot menu in pcbnew.
  • Valid keys:
    • comment: [string=''] A comment for documentation purposes.
    • dir: [string='.'] Output directory for the generated files.
    • layers: [list(dict)|list(string)|string] [all,selected,copper,technical,user] List of PCB layers to plot.
      • Valid keys:
        • description: [string=''] A description for the layer, for documentation purposes.
        • layer: [string=''] Name of the layer. As you see it in KiCad.
        • suffix: [string=''] Suffix used in file names related to this layer. Derived from the name if not specified.
    • name: [string=''] Used to identify this particular output definition.
    • options: [dict] Options for the ps output.
      • Valid keys:
        • a4_output: [boolean=true] force A4 paper size.
        • drill_marks: [string='full'] what to use to indicate the drill places, can be none, small or full (for real scale).
        • exclude_edge_layer: [boolean=true] do not include the PCB edge layer.
        • exclude_pads_from_silkscreen: [boolean=false] do not plot the component pads in the silk screen.
        • force_plot_invisible_refs_vals: [boolean=false] include references and values even when they are marked as invisible.
        • line_width: [number=0.15] [0.02,2] for objects without width [mm].
        • mirror_plot: [boolean=false] plot mirrored.
        • negative_plot: [boolean=false] invert black and white.
        • plot_footprint_refs: [boolean=true] include the footprint references.
        • plot_footprint_values: [boolean=true] include the footprint values.
        • plot_sheet_reference: [boolean=false] currently without effect.
        • scale_adjust_x: [number=1.0] fine grain adjust for the X scale (floating point multiplier).
        • scale_adjust_y: [number=1.0] fine grain adjust for the Y scale (floating point multiplier).
        • scaling: [number=1] scale factor (0 means autoscaling).
        • sketch_plot: [boolean=false] don't fill objects, just draw the outline.
        • tent_vias: [boolean=true] cover the vias.
        • width_adjust: [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.

• STEP (ISO 10303-21 Clear Text Encoding of the Exchange Structure)

  • Type: step
  • Description: Exports the PCB as a 3D model. This is the most common 3D format for exchange purposes. This output is what you get from the 'File/Export/STEP' menu in pcbnew.
  • Valid keys:
    • comment: [string=''] A comment for documentation purposes.
    • dir: [string='.'] Output directory for the generated files.
    • name: [string=''] Used to identify this particular output definition.
    • options: [dict] Options for the step output.
      • Valid keys:
        • metric_units: [boolean=true] use metric units instead of inches.
        • min_distance: [number=-1] the minimum distance between points to treat them as separate ones (-1 is KiCad default: 0.01 mm).
        • no_virtual: [boolean=false] used to exclude 3D models for components with 'virtual' attribute.
        • origin: [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'.
        • output: [string=''] name for the generated STEP file (the name of the PCB if empty).

• SVG (Scalable Vector Graphics)

  • Type: svg
  • Description: Exports the PCB to a format suitable for 2D graphics software. Unlike bitmaps SVG drawings can be scaled without losing resolution. This output is what you get from the File/Plot menu in pcbnew.
  • Valid keys:
    • comment: [string=''] A comment for documentation purposes.
    • dir: [string='.'] Output directory for the generated files.
    • layers: [list(dict)|list(string)|string] [all,selected,copper,technical,user] List of PCB layers to plot.
      • Valid keys:
        • description: [string=''] A description for the layer, for documentation purposes.
        • layer: [string=''] Name of the layer. As you see it in KiCad.
        • suffix: [string=''] Suffix used in file names related to this layer. Derived from the name if not specified.
    • name: [string=''] Used to identify this particular output definition.
    • options: [dict] Options for the svg output.
      • Valid keys:
        • drill_marks: [string='full'] what to use to indicate the drill places, can be none, small or full (for real scale).
        • exclude_edge_layer: [boolean=true] do not include the PCB edge layer.
        • exclude_pads_from_silkscreen: [boolean=false] do not plot the component pads in the silk screen.
        • force_plot_invisible_refs_vals: [boolean=false] include references and values even when they are marked as invisible.
        • line_width: [number=0.25] [0.02,2] for objects without width [mm].
        • mirror_plot: [boolean=false] plot mirrored.
        • negative_plot: [boolean=false] invert black and white.
        • plot_footprint_refs: [boolean=true] include the footprint references.
        • plot_footprint_values: [boolean=true] include the footprint values.
        • plot_sheet_reference: [boolean=false] currently without effect.
        • tent_vias: [boolean=true] cover the vias.

Using KiPlot

If you need a template for the configuration file try:

kiplot --example

This will generate a file named example.kiplot.yaml containing all the available options and comments about them. You can use it to create your own configuration file.

If you want to use the layers of a particular PCB in the example use:

kiplot -b PCB_FILE --example

And if you want to use the same options selected in the plot dialog use:

kiplot -b PCB_FILE -p --example

If the current directory contains only one PCB file and only one configuration file (named *.kiplot.yaml) you can just call kiplot. No arguments needed. The tool will figure out which files to use.

If more than one file is found in the current directory kiplot will use the first found and issue a warning. If you need to use other file just tell it explicitly:

kiplot -b PCB_FILE.kicad_pcb -c CONFIG.kiplot.yaml

A simple target can be added to your makefile, so you can just run make pcb_files or integrate into your current build process.

pcb_files:
    kiplot -b $(PCB) -c $(KIPLOT_CFG)

If you need to supress messages use --quiet or -q and if you need to get more informatio about what's going on use --verbose or -v.

If you want to generate only some of the outputs use:

kiplot OUTPUT_1 OUTPUT_2

If you want to generate all outputs with some exceptions use:

kiplot --invert-sel OUTPUT_1 OUTPUT_2

If you want to skip the DRC and ERC use:

kiplot --skip-pre run_erc,run_drc

If you want to skip all the preflight tasks use:

kiplot --skip-pre all

All outputs are generated using the current directory as base. If you want to use another directory as base use:

kiplot --out-dir OTHER_PLACE

If you want to list the available outputs defined in the configuration file use:

kiplot --list

Command line help

KiPlot: Command-line Plotting for KiCad

Usage:
  kiplot [-b BOARD] [-e SCHEMA] [-c CONFIG] [-d OUT_DIR] [-s PRE]
         [-q | -v...] [-i] [TARGET...]
  kiplot [-c PLOT_CONFIG] --list
  kiplot [-b BOARD] [-d OUT_DIR] [-p | -P] --example
  kiplot [-v] --help-list-outputs
  kiplot --help-output=HELP_OUTPUT
  kiplot --help-outputs
  kiplot --help-preflights
  kiplot -h | --help
  kiplot --version

Arguments:
  TARGET    Outputs to generate, default is all

Options:
  -h, --help                       Show this help message and exit
  -b BOARD, --board-file BOARD     The PCB .kicad-pcb board file
  -c CONFIG, --plot-config CONFIG  The plotting config file to use
  -d OUT_DIR, --out-dir OUT_DIR    The output directory [default: .]
  -e SCHEMA, --schematic SCHEMA    The schematic file (.sch)
  --help-list-outputs              List supported outputs
  --help-output HELP_OUTPUT        Help for this particular output
  --help-outputs                   List supported outputs and details
  --help-preflights                List supported preflights and details
  -i, --invert-sel                 Generate the outputs not listed as targets
  -l, --list                       List available outputs (in the config file)
  -p, --copy-options               Copy plot options from the PCB file
  -P, --copy-and-expand            As -p but expand the list of layers
  -q, --quiet                      Remove information logs
  -s PRE, --skip-pre PRE           Skip preflights, comma separated or `all`
  -v, --verbose                    Show debugging information
  -V, --version                    Show program's version number and exit
  -x, --example                    Create an example configuration file.

Installing

Dependencies

• For ERC, DRC, BoM XML update and PCB/SCH print install KiCad Automation Scripts
• For HTML/CSV BoM install KiBoM
• For interactive BoM install InteractiveHtmlBom

Installation on Ubuntu/Debian:

Get the Debian package from the releases section and run:

sudo apt install ./kiplot.inti-cmnb_*_all.deb

Installation on other targets

• Install KiCad 5.x
• Install Python 3.5 or newer
• Install the Python Yaml module
• Run the script src/kiplot

Using for CI/CD

When using a GitHub or GitLab repo you can use KiPlot to generate all the needed stuff each time you commit a change to the schematic and/or PCB file.

Examples of how to do it can be found here for GitHub and here for GitLab.

In order to run KiPlot on these environments you need a lot of software installed. The usual mechanism to achieve this is using docker. Docker images containing KiPlot, all the supporting scripts and a corresponding KiCad can be found at Docker Hub as setsoft/kicad_auto:latest. This image is based on setsoft/kicad_debian:latest, containing KiCad on Debian GNU/Linux.

For more information about the docker images visit kicad_debian and kicad_auto.