templates
/
KiBot
1
0
Fork 0
Code Issues Pull Requests Packages Projects Releases Wiki Activity
KiBot/docs/samples/generic_plot.kibot.yaml

1842 lines
96 KiB
YAML
Raw Blame History

# 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:
# [dict] Annotates the PCB according to physical coordinates.
# This preflight modifies the PCB and schematic, use it only in revision control environments.
# Used to assign references according to footprint coordinates.
# The project must be fully annotated first.
annotate_pcb:
- top_main_axis: y
- top_main_ascending: true
- top_secondary_ascending: true
- top_start: 1
- bottom_main_axis: y
- bottom_main_ascending: true
- bottom_secondary_ascending: true
- bottom_start: 101
- use_position_of: 'footprint'
- grid: 1.0
# [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.
# The original PCB remains unchanged.
check_zone_fills: true
# [boolean=false] Option for `run_erc`. ERC warnings are considered errors.
erc_warnings: false
# [boolean=false] Fill all zones again and save the PCB.
fill_zones: true
# [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 PCB. I.e. to insert the git hash or last revision date.
# This is useful for KiCad 5, use `set_text_variables` when using KiCad 6.
# This preflight 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 is useful for KiCad 5, use `set_text_variables` when using KiCad 6.
# This preflight 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: '>'
# [dict|list(dict)] Defines KiCad 6 variables.
# They are expanded using ${VARIABLE}, and stored in the project file.
# This preflight replaces `pcb_replace` and `sch_replace` when using KiCad 6.
# The KiCad project file is modified.
set_text_variables:
- name: 'git_hash'
command: 'git log -1 --format="%h" $KIBOT_PCB_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.
# This option is for simple cases, consider using a full variant for complex cases
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.
# This option is for simple cases, consider using a full variant for complex cases
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.
# This option is for simple cases, consider using a full variant for complex cases
exclude_filter: '_mechanical'
# [boolean=true] Expand KiCad 6 text variables after applying all filters and variants.
# This is done using a **_expand_text_vars** filter.
# If you need to customize the filter, or apply it before, you can disable this option and
# add a custom filter to the filter chain
expand_text_vars: true
# [string='Config'] Field name used for internal filters (not for variants)
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: ''
# [string|list(string)=''] Information to put after the title and before the pcb and stats info
extra_info: ''
# [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: ''
# [string|list(string)=''] Information to put after the title and before the pcb and stats info
extra_info: ''
# [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|list(string)=''] List of KiCost APIs to disable
kicost_api_disable: ''
# [string|list(string)=''] List of KiCost APIs to enable
kicost_api_enable: ''
# [string=''] KiCost configuration file. It contains the keys for the different distributors APIs.
# The regular KiCost config is used when empty
kicost_config: ''
# [boolean=false] Used to add a column with the distributor's description. So you can check this is the right component
kicost_dist_desc: 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
# [boolean=false] Enable Specs worksheet creation. Contains specifications for the components.
# Works with only some KiCost APIs
specs: false
# [list(dict)|list(string)] Which columns are included in the Specs worksheet. Use `References` for the references,
# 'Row' for the order and 'Sep' to separate groups at the same level. By default all are included.
# Column names are distributor specific, the following aren't: '_desc', '_value', '_tolerance', '_footprint',
# '_power', '_current', '_voltage', '_frequency', '_temp_coeff', '_manf', '_size'
specs_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'
# [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: '*'
# [boolean=true] Store the file pointed by symlinks, not the symlink
follow_links: true
# [string='ZIP'] [ZIP,TAR,RAR] Output file format
format: 'ZIP'
# [boolean=false] Move the files to the archive. In other words: remove the files after adding them to the archive
move_files: false
# [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'
# `remove_files` is an alias for `move_files`
# Diff:
# Recursive git submodules aren't supported (submodules inside submodules)
- name: 'diff_example'
comment: 'Generates a PDF with the differences between two PCBs or schematics.'
type: 'diff'
dir: 'Example/diff_dir'
options:
# [boolean=false] When enabled we create a symlink to the output file with a name that contains the
# git hashes involved in the comparison. If you plan to compress the output don't
# forget to disable the `follow_links` option
add_link_id: false
# [string=''] Directory to cache the intermediate files. Leave it blank to disable the cache
cache_dir: ''
# [boolean=false] Modifies the behavior of `add_link_id` to create a copy of the file instead of a
# symlink. Useful for some Windows setups
copy_instead_of_link: false
# [string='red_green'] [red_green,stats] In the `red_green` mode added stuff is green and red when removed.
# The `stats` mode is used to meassure the amount of difference. In this mode all
# changes are red, but you can abort if the difference is bigger than certain threshold
diff_mode: 'red_green'
# [boolean=false] When `old_type` and/or `new_type` are `git` KiBot will checkout the indicated point.
# Before doing it KiBot will stash any change. Under some circumstances git could fail
# to do a checkout, even after stashing, this option can workaround the problem.
# Note that using it you could potentially lose modified files. For more information
# read https://stackoverflow.com/questions/1248029/git-pull-error-entry-foo-not-uptodate-cannot-merge
force_checkout: false
# [number=5] [0,100] Color tolerance (fuzzyness) for the `stats` mode
fuzz: 5
# [string|list(string)] The file you want to compare. Leave it blank for the current PCB/SCH.
# A list is accepted only for the `multivar` type
new: ''
# [string='file'] [git,file,output,multivar] How to interpret the `new` name. Use `git` for a git hash, branch, etc.
# Use `file` for a file name. Use `output` to specify the name of a `pcb_variant`/`sch_variant` output.
# Use `multivar` to compare a set of variants, in this mode `new` is the list of variants.
# If `old` is also `multivar` then it becomes the reference, otherwise we compare using pairs of variants
new_type: 'file'
# [string='HEAD'] Reference file. When using git use `HEAD` to refer to the last commit.
# Use `HEAD~` to refer the previous to the last commit.
# As `HEAD` is for the whole repo you can use `KIBOT_LAST-n` to make
# reference to the changes in the PCB/SCH. The `n` value is how many
# changes in the history you want to go back. A 0 is the same as `HEAD`,
# a 1 means the last time the PCB/SCH was changed, etc
old: 'HEAD'
# [string='git'] [git,file,output,multivar] How to interpret the `old` name. Use `git` for a git hash, branch, etc.
# Use `file` for a file name. Use `output` to specify the name of a `pcb_variant`/`sch_variant` output.
# Use `multivar` to specify a reference file when `new_type` is also `multivar`
old_type: 'git'
# [string='%f-%i%I%v.%x'] Filename for the output (%i=diff_pcb/diff_sch, %x=pdf). Affected by global options
output: '%f-%i%I%v.%x'
# [boolean=true] Compare the PCB, otherwise compare the schematic
pcb: true
# [number=0] [0,1000000] Error threshold for the `stats` mode, 0 is no error. When specified a
# difference bigger than the indicated value will make the diff fail
threshold: 0
layers: all
# 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'] [none,small,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] Include the frame and title block. Only available for KiCad 6 and you get a poor result
# The `pcb_print` output can do a better job for PDF, SVG, PS, EPS and PNG outputs
plot_sheet_reference: false
# [boolean=true] Plot using the contour, instead of the center line.
# You must disable it to get the dimensions (See https://gitlab.com/kicad/code/kicad/-/issues/11901)
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'
# GenCAD:
# This format is interpreted by some CADCAM software and helps certain
# manufacturers
- name: 'gencad_example'
comment: 'Exports the PCB in GENCAD format.'
type: 'gencad'
dir: 'Example/gencad_dir'
options:
# [boolean=false] Use auxiliary axis as origin
aux_origin: false
# [boolean=false] Flip bottom footprint padstacks
flip_bottom_padstacks: false
# [boolean=false] Generate a new shape for each footprint instance (Do not reuse shapes)
no_reuse_shapes: false
# [string='%f-%i%I%v.%x'] Filename for the output (%i=gencad, %x=cad). Affected by global options
output: '%f-%i%I%v.%x'
# [boolean=false] Save the origin coordinates in the file
save_origin: false
# [boolean=false] Generate unique pin names
unique_pin_names: 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='%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] Include the frame and title block. Only available for KiCad 6 and you get a poor result
# The `pcb_print` output can do a better job for PDF, SVG, PS, EPS and PNG outputs
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'] [none,small,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] Include the frame and title block. Only available for KiCad 6 and you get a poor result
# The `pcb_print` output can do a better job for PDF, SVG, PS, EPS and PNG outputs
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 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 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: ''
# Info:
# It can be used to know more about the environment used to generate the files.
# Please don't rely on the way things are reported, its content could change,
# adding or removing information
- name: 'info_example'
comment: 'Records information about the current run.'
type: 'info'
dir: 'Example/info_dir'
options:
# [string='names'] [names,none,full] List environment variables.
# IMPORTANT: Don't use `full` unless you know you are not leaking sensitive information
environment: 'names'
# [string='%f-%i%I%v.%x'] Filename for the output (%i=info, %x=txt). Affected by global options
output: '%f-%i%I%v.%x'
# 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. Environment variables and ~ allowed.
# 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: ''
# Navigate Results:
- name: 'navigate_results_example'
comment: 'Generates a web page to navigate the generated outputs'
type: 'navigate_results'
dir: 'Example/navigate_results_dir'
options:
# [string=''] The name of a file to create at the main output directory linking to the home page
link_from_root: ''
# [string='%f-%i%I%v.%x'] Filename for the output (%i=html, %x=navigate). Affected by global options
output: '%f-%i%I%v.%x'
# Netlist:
# The netlist can be generated in the classic format and in IPC-D-356 format,
# useful for board testing
- name: 'netlist_example'
comment: 'Generates the list of connections for the project.'
type: 'netlist'
dir: 'Example/netlist_dir'
options:
# [string='classic'] [classic,ipc] The `classic` format is the KiCad internal format, and is generated
# from the schematic. The `ipc` format is the IPC-D-356 format, useful for PCB
# testing, is generated from the PCB
format: 'classic'
# [string='%f-%i%I%v.%x'] Filename for the output (%i=netlist/IPC-D-356, %x=net/d356). Affected by global options
output: '%f-%i%I%v.%x'
# PCB Print:
# Supports PDF, SVG, PNG, EPS and PS formats.
# KiCad 5: including the frame is slow.
# KiCad 6: for custom frames use the `enable_ki6_frame_fix`, is slow.
- name: 'pcb_print_example'
comment: 'Prints the PCB using a mechanism that is more flexible than `pdf_pcb_print` and `svg_pcb_print`.'
type: 'pcb_print'
dir: 'Example/pcb_print_dir'
options:
# [boolean=false] Add a background to the pages, see `background_color`
add_background: false
# [string='#FFFFFF'] Color for the background when `add_background` is enabled
background_color: '#FFFFFF'
# [string=''] Background image, must be an SVG, only when `add_background` is enabled
background_image: ''
# [string=''] Color used for blind/buried `colored_vias`
blind_via_color: ''
# [string='_builtin_classic'] Selects the color theme. Only applies to KiCad 6.
# To use the KiCad 6 default colors select `_builtin_default`.
# Usually user colors are stored as `user`, but you can give it another name
color_theme: '_builtin_classic'
# [boolean=true] Plot through-hole in a different color. Like KiCad GUI does
colored_pads: true
# [boolean=true] Plot vias in a different color. Like KiCad GUI does
colored_vias: true
# [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=360] [36,1200] Resolution (Dots Per Inch) for the output file. Most objects are vectors, but thing
# like the the solder mask are handled as images by the conversion tools
dpi: 360
# [string='full'] [none,small,full] What to use to indicate the drill places, can be none, small or full (for real scale)
drill_marks: 'full'
# [boolean=false] Add the `Edge.Cuts` to all the pages
force_edge_cuts: false
# [string=''] Color used for the `force_edge_cuts` option
forced_edge_cuts_color: ''
# [string='PDF'] [PDF,SVG,PNG,EPS,PS] Format for the output file/s.
# Note that for PS you need `ghostscript` which isn't part of the default docker images
format: 'PDF'
# [string='internal'] [gui,internal,plot] Plotting the frame from Python is problematic.
# This option selects a workaround strategy.
# gui: uses KiCad GUI to do it. Is slow but you get the correct frame.
# But it can't keep track of page numbers.
# internal: KiBot loads the `.kicad_wks` and does the drawing work.
# Best option, but some details are different from what the GUI generates.
# plot: uses KiCad Python API. Only available for KiCad 6.
# You get the default frame and some substitutions doesn't work
frame_plot_mechanism: 'internal'
# [boolean=false] Hide components in the Fab layer that are marked as excluded by a variant
hide_excluded: false
# [boolean=false] Store the temporal page and layer files in the output dir and don't delete them
keep_temporal_files: false
# [string=''] Color used for micro `colored_vias`
micro_via_color: ''
# [string='%f-%i%I%v.%x'] Filename for the output (%i=assembly, %x=pdf/ps)/(%i=assembly_page_NN, %x=svg/png/eps).
# Consult the `page_number_as_extension` and `page_id` options. Affected by global options
output: '%f-%i%I%v.%x'
# `output_name` is an alias for `output`
# [string=''] Color used for `colored_pads`
pad_color: ''
# [boolean=false] When enabled the %i is always `assembly`, the %x will be NN.FORMAT (i.e. 01.png).
# Note: page numbers can be customized using the `page_id` option for each page
page_number_as_extension: false
# [list(dict)] List of pages to include in the output document.
# Each page contains one or more layers of the PCB
pages:
# [boolean=true] Change the drill holes to be colored instead of white
- colored_holes: true
# [boolean=false] Do not plot the component pads in the silk screen (KiCad 5.x only)
exclude_pads_from_silkscreen: false
# [string='#000000'] Color used for the holes when `colored_holes` is enabled
holes_color: '#000000'
# [list(dict)|list(string)|string] List of layers printed in this page.
# Order is important, the last goes on top.
# You can reuse other layers lists, some options aren't used here, but they are valid
layers:
# [string=''] Color used for this layer
- color: ''
# [string=''] A description for the layer, for documentation purposes
description: ''
# [boolean=false] Include references and values even when they are marked as invisible
force_plot_invisible_refs_vals: false
# [string=''] Name of the layer. As you see it in KiCad
layer: ''
# [boolean=true] Include the footprint references
plot_footprint_refs: true
# [boolean=true] Include the footprint values
plot_footprint_values: true
# [string=''] Suffix used in file names related to this layer. Derived from the name if not specified
suffix: ''
# [number=0.1] [0.02,2] For objects without width [mm] (KiCad 5)
line_width: 0.1
# [boolean=false] Print mirrored (X axis inverted)
mirror: false
# [boolean=false] Print in gray scale
monochrome: false
# [boolean=false] Invert black and white. Only useful for a single layer
negative_plot: false
# [string='%02d'] Text to differentiate the pages. Use %d (like in C) to get the page number
page_id: '%02d'
# [number=1.0] Scale factor (0 means autoscaling)
scaling: 1.0
# [string='Assembly'] Text to use for the `sheet` in the title block
sheet: 'Assembly'
# [string=''] Color to use for the frame and title block
sheet_reference_color: ''
# [boolean=false] Try to sort the layers in the same order that uses KiCad for printing
sort_layers: false
# [boolean=true] Cover the vias
tent_vias: true
# [string=''] Text used to replace the sheet title. %VALUE expansions are allowed.
# If it starts with `+` the text is concatenated
title: ''
# [boolean=true] Include the title-block (worksheet, frame, etc.)
plot_sheet_reference: true
# [number=1280] [0,7680] Width of the PNG in pixels. Use 0 to use as many pixels as the DPI needs for the page size
png_width: 1280
# [boolean=true] Try to draw the solder mask as a real solder mask, not the negative used for fabrication.
# In order to get a good looking select a color with transparency, i.e. '#14332440'.
# PcbDraw must be installed in order to use this option
realistic_solder_mask: true
# [number=1.0] Default scale factor (0 means autoscaling)
scaling: 1.0
# [string=''] Worksheet file (.kicad_wks) to use. Leave empty to use the one specified in the project
sheet_reference_layout: ''
# [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: ''
# [string=''] Color used for through-hole `colored_vias`
via_color: ''
# PCB 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: 'pcb_variant_example'
comment: 'Creates a copy of the PCB with all the filters and variants applied.'
type: 'pcb_variant'
dir: 'Example/pcb_variant_dir'
options:
# [boolean=true] Copy the KiCad project to the destination directory
copy_project: true
# [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=false] Hide components in the Fab layer that are marked as excluded by a variant
hide_excluded: false
# [string='%f-%i%I%v.%x'] Filename for the output (%i=variant, %x=kicad_pcb). Affected by global options
output: '%f-%i%I%v.%x'
# [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: ''
# 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.
# The `pcb_print` is usually a better alternative.
- 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'] [none,small,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] Include the frame and title block. Only available for KiCad 6 and you get a poor result
# The `pcb_print` output can do a better job for PDF, SVG, PS, EPS and PNG outputs
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.
# The `pcb_print` is usually a better alternative.
- 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='_builtin_classic'] Selects the color theme. Onlyu applies to KiCad 6.
# To use the KiCad 6 default colors select `_builtin_default`.
# Usually user colors are stored as `user`, but you can give it another name
color_theme: '_builtin_classic'
# [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'] [none,small,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). You should disable `plot_sheet_reference` when using it
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:
# [boolean=true] Generate with all hierarchical sheets
all_pages: true
# [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'
# [boolean=false] Use the `pdfunite` tool instead of PyPDF2 Python module
use_external_command: false
# 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').
# Important: when using separate files you must use `%i` to differentiate them. 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.
# The `pcb_print` is usually a better alternative.
- 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'] [none,small,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] Include the frame and title block. Only available for KiCad 6 and you get a poor result
# The `pcb_print` output can do a better job for PDF, SVG, PS, EPS and PNG outputs
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
# [number=0] Steps to rotate around the X axis, positive is clockwise.
# Each step is currently 10 degrees. Only for KiCad 6
rotate_x: 0
# [number=0] Steps to rotate around the Y axis, positive is clockwise.
# Each step is currently 10 degrees. Only for KiCad 6
rotate_y: 0
# [number=0] Steps to rotate around the Z axis, positive is clockwise.
# Each step is currently 10 degrees. Only for KiCad 6
rotate_z: 0
# [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'
# `wait_ray_tracing` is an alias for `wait_render`
# [number=-600] How many seconds we must wait before capturing the render (ray tracing or normal).
# 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_render: -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='markdown'] Original format for the report conversion. Current templates are `markdown`. See `do_convert`
convert_from: 'markdown'
# [string='pdf'] Target format for the report conversion. See `do_convert`
convert_to: 'pdf'
# [string='%f-%i%I%v.%x'] Converted output file name (%i='report', %x=`convert_to`).
# Note that the extension should match the `convert_to` value. Affected by global options
converted_output: '%f-%i%I%v.%x'
# [boolean=false] Run `Pandoc` to convert the report. Note that Pandoc must be installed.
# The conversion is done assuming the report is in `convert_from` format.
# The output file will be in `convert_to` format.
# The available formats depends on the `Pandoc` installation.
# In CI/CD environments: the `kicad_auto_test` docker image contains it.
# In Debian/Ubuntu environments: install `pandoc`, `texlive-latex-base` and `texlive-latex-recommended`
do_convert: false
# [string='10F'] Which Eurocircuits class are we aiming at
eurocircuits_class_target: '10F'
# [number=0.45] When computing the Eurocircuits category: Final holes sizes smaller or equal to this given
# diameter can be reduced to accommodate the correct annular ring values.
# Use 0 to disable it
eurocircuits_reduce_holes: 0.45
# [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, full_svg, simple) or a custom template file.
# Environment variables and ~ are allowed.
# Note: when converting to PDF PanDoc can fail on some Unicode values (use `simple_ASCII`)
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:
# [boolean=false] Copy the KiCad project to the destination directory.
# Disabled by default for compatibility with older versions
copy_project: 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=''] 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.
# The `pcb_print` is usually a better alternative.
- 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'] [none,small,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] Include the frame and title block. Only available for KiCad 6 and you get a poor result
# The `pcb_print` output can do a better job for PDF, SVG, PS, EPS and PNG outputs
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.
# The `pcb_print` is usually a better alternative.
- 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='_builtin_classic'] Selects the color theme. Onlyu applies to KiCad 6.
# To use the KiCad 6 default colors select `_builtin_default`.
# Usually user colors are stored as `user`, but you can give it another name
color_theme: '_builtin_classic'
# [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'] [none,small,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 5 bug
enable_ki5_page_fix: true
# [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). You should disable `plot_sheet_reference` when using it
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:
# [boolean=true] Generate with all hierarchical sheets
all_pages: true
# [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 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: ''
Reference in New Issue View Git Blame Copy Permalink