.. Automatically generated by KiBot, please don't edit this file - global - Valid keys: - ``aliases_for_3d_models`` :index:`: ` [list(dict)] List of aliases for the 3D models (KiCad 6). KiCad stores 3D aliases with the user settings, not locally. This makes impossible to create self contained projects. You can define aliases here to workaround this problem. The values defined here has precedence over the KiCad configuration. Related to https://gitlab.com/kicad/code/kicad/-/issues/3792. - Valid keys: - *alias* :index:`: ` Alias for name. - ``name`` :index:`: ` [string=''] Name of the alias. - *text* :index:`: ` Alias for value. - ``value`` :index:`: ` [string=''] Path to the 3D model. - *variable* :index:`: ` Alias for name. - ``allow_blind_buried_vias`` :index:`: ` [boolean=true] Allow the use of buried vias. This value is only used for KiCad 7+. For KiCad 5 and 6 use the design rules settings, stored in the project. - ``allow_microvias`` :index:`: ` [boolean=true] Allow the use of micro vias. This value is only used for KiCad 7+. For KiCad 5 and 6 use the design rules settings, stored in the project. - ``cache_3d_resistors`` :index:`: ` [boolean=false] Use a cache for the generated 3D models of colored resistors. Will save time, but you could need to remove the cache if you need to regenerate them. - ``castellated_pads`` :index:`: ` [boolean=false] Has the PCB castellated pads? KiCad 6: you should set this in the Board Setup -> Board Finish -> Has castellated pads. - ``colored_tht_resistors`` :index:`: ` [boolean=true] Try to add color bands to the 3D models of KiCad THT resistors. - *copper_finish* :index:`: ` Alias for pcb_finish. - ``copper_thickness`` :index:`: ` [number|string] Copper thickness in micrometers (1 Oz is 35 micrometers). KiCad 6: you should set this in the Board Setup -> Physical Stackup. - ``cross_footprints_for_dnp`` :index:`: ` [boolean=true] Draw a cross for excluded components in the `Fab` layer. - ``cross_no_body`` :index:`: ` [boolean=false] Cross components even when they don't have a body. Only for KiCad 6 and internal cross. - ``cross_using_kicad`` :index:`: ` [boolean=true] When using KiCad 7+ let KiCad cross the components. - ``csv_accept_no_ref`` :index:`: ` [boolean=false] Accept aggregating CSV files without references (Experimental). - ``date_format`` :index:`: ` [string='%Y-%m-%d'] Format used for the day we started the script. Is also used for the PCB/SCH date formatting when `time_reformat` is enabled (default behavior). Uses the `strftime` format. - ``date_time_format`` :index:`: ` [string='%Y-%m-%d_%H-%M-%S'] Format used for the PCB and schematic date when using the file timestamp. Uses the `strftime` format. - ``default_resistor_tolerance`` :index:`: ` [number=20] When no tolerance is specified we use this value. Note that I know 5% is a common default, but technically speaking 20% is the default. Used while creating colored resistors. - ``dir`` :index:`: ` [string=''] Default pattern for the output directories. It also applies to the preflights, unless `use_dir_for_preflights` is disabled. - ``disable_3d_alias_as_env`` :index:`: ` [boolean=false] Disable the use of environment and text variables as 3D models aliases. - ``drc_exclusions_workaround`` :index:`: ` [boolean=false] KiCad 6 introduced DRC exclusions. They are stored in the project but ignored by the Python API. This is reported as bug number 11562 (https://gitlab.com/kicad/code/kicad/-/issues/11562). If you really need exclusions enable this option, this will use the GUI version of the DRC (slower). Current KiCad version is 6.0.7 and the bug is still there. - ``drill_size_increment`` :index:`: ` [number=0.05] This is the difference between drill tools in millimeters. A manufacturer with 0.05 of increment has drills for 0.1, 0.15, 0.2, 0.25, etc.. - ``edge_connector`` :index:`: ` [string='no'] [yes,no,bevelled] Has the PCB edge connectors? KiCad 6: you should set this in the Board Setup -> Board Finish -> Edge card connectors. - ``edge_plating`` :index:`: ` [boolean=false] Has the PCB a plated board edge? KiCad 6: you should set this in the Board Setup -> Board Finish -> Plated board edge. - ``environment`` :index:`: ` [dict] Used to define environment variables used by KiCad. The values defined here are exported as environment variables and has more precedence than KiCad paths defined in the GUI. You can make reference to any OS environment variable using `${VARIABLE}`. The KIPRJMOD is also available for expansion. - Valid keys: - ``define_old`` :index:`: ` [boolean=false] Also define legacy versions of the variables. Useful when using KiCad 6+ and some libs uses old KiCad 5 names. - ``extra_os`` :index:`: ` [list(dict)] Extra variables to export as OS environment variables. Note that you can also define them using `- NAME: VALUE`. - Valid keys: - **name** :index:`: ` [string=''] Name of the variable. - **value** :index:`: ` [string=''] Value for the variable. - ``footprints`` :index:`: ` [string=''] System level footprints (aka modules) dir. KiCad 5: KICAD_FOOTPRINT_DIR and KISYSMOD. KiCad 6: KICAD6_FOOTPRINT_DIR. - ``models_3d`` :index:`: ` [string=''] System level 3D models dir. KiCad 5: KISYS3DMOD. KiCad 6: KICAD6_3DMODEL_DIR. - ``symbols`` :index:`: ` [string=''] System level symbols dir. KiCad 5: KICAD_SYMBOL_DIR. KiCad 6: KICAD6_SYMBOL_DIR. - ``templates`` :index:`: ` [string=''] System level templates dir. KiCad 5: KICAD_TEMPLATE_DIR. KiCad 6: KICAD6_TEMPLATE_DIR. - ``third_party`` :index:`: ` [string=''] 3rd party dir. KiCad 6: KICAD6_3RD_PARTY. - ``user_templates`` :index:`: ` [string=''] User level templates dir. KiCad 5/6: KICAD_USER_TEMPLATE_DIR. - ``erc_grid`` :index:`: ` [number=50] Grid size used for the ERC. This value must be in mils. This is needed for KiCad 7 in order to run the off grid check. Shouldn't be needed in KiCad 8. https://gitlab.com/kicad/code/kicad/-/issues/14110. - ``extra_pth_drill`` :index:`: ` [number=0.1] How many millimeters the manufacturer will add to plated holes. This is because the plating reduces the hole, so you need to use a bigger drill. For more information consult: https://www.eurocircuits.com/pcb-design-guidelines/drilled-holes/. - ``field_3D_model`` :index:`: ` [string='_3D_model'] Name for the field controlling the 3D models used for a component. - ``field_lcsc_part`` :index:`: ` [string=''] The name of the schematic field that contains the part number for the LCSC/JLCPCB distributor. When empty KiBot will try to discover it. - ``field_package`` :index:`: ` [string|list(string)] Name/s of the field/s used for the package, not footprint. I.e. 0805, SOT-23, etc. Used for the value split filter. The default is ['package', 'pkg']. - ``field_power`` :index:`: ` [string|list(string)] Name/s of the field/s used for the power raiting. Used for the value split filter. The default is ['power', 'pow']. - ``field_temp_coef`` :index:`: ` [string|list(string)] Name/s of the field/s used for the temperature coefficient. I.e. X7R, NP0, etc. Used for the value split filter. The default is ['temp_coef', 'tmp_coef']. - ``field_tolerance`` :index:`: ` [string|list(string)] Name/s of the field/s used for the tolerance. Used while creating colored resistors and for the value split filter. The default is ['tolerance', 'tol']. - ``field_voltage`` :index:`: ` [string|list(string)] Name/s of the field/s used for the voltage raiting. Used for the value split filter. The default is ['voltage', 'v']. - ``filters`` :index:`: ` [list(dict)] KiBot warnings to be ignored. - Valid keys: - ``error`` :index:`: ` [string=''] Error id we want to exclude. - *error_number* :index:`: ` Alias for number. - ``filter`` :index:`: ` [string=''] Name for the filter, for documentation purposes. - *filter_msg* :index:`: ` Alias for filter. - ``number`` :index:`: ` [number=0] Error number we want to exclude. - ``regex`` :index:`: ` [string=''] Regular expression to match the text for the error we want to exclude. - *regexp* :index:`: ` Alias for regex. - ``git_diff_strategy`` :index:`: ` [string='worktree'] [worktree,stash] When computing a PCB/SCH diff it configures how do we preserve the current working state. The *worktree* mechanism creates a separated worktree, that then is just removed. The *stash* mechanism uses *git stash push/pop* to save the current changes. Using *worktree* is the preferred mechanism. - ``hide_excluded`` :index:`: ` [boolean=false] Default value for the `hide_excluded` option of various PCB outputs. - ``impedance_controlled`` :index:`: ` [boolean=false] The PCB needs specific dielectric characteristics. KiCad 6: you should set this in the Board Setup -> Physical Stackup. - ``include_components_from_pcb`` :index:`: ` [boolean=true] Include components that are only in the PCB, not in the schematic, for filter and variants processing. Note that version 1.6.3 and older ignored them. - ``invalidate_pcb_text_cache`` :index:`: ` [string='auto'] [auto,yes,no] Remove any cached text variable in the PCB. This is needed in order to force a text variables update when using `set_text_variables`. You might want to disable it when applying some changes to the PCB and create a new copy to send to somebody without changing the cached values. The `auto` value will remove the cached values only when using `set_text_variables`. - ``kiauto_time_out_scale`` :index:`: ` [number=0.0] Time-out multiplier for KiAuto operations. - ``kiauto_wait_start`` :index:`: ` [number=0] Time to wait for KiCad in KiAuto operations. - ``kicad_dnp_applied`` :index:`: ` [boolean=true] The KiCad v7 PCB flag *Do Not Populate* is applied to our fitted flag before running any filter. - ``kicad_dnp_applies_to_3D`` :index:`: ` [boolean=true] The KiCad v7 PCB flag *Do Not Populate* is applied to our fitted flag for 3D models, even when no filter/variant is specified. Disabling `kicad_dnp_applied` also disables this flag. - ``layer_defaults`` :index:`: ` [list(dict)] Used to indicate the default suffix and description for the layers. Note that the name for the layer must match exactly, no aliases. - Valid keys: - ``description`` :index:`: ` [string=''] A description for the layer, for documentation purposes. A default can be specified using the `layer_defaults` global option. - ``layer`` :index:`: ` [string=''] Name of the layer. As you see it in KiCad. - ``suffix`` :index:`: ` [string=''] Suffix used in file names related to this layer. Derived from the name if not specified. A default can be specified using the `layer_defaults` global option. - ``out_dir`` :index:`: ` [string=''] Base output dir, same as command line `--out-dir`. - ``output`` :index:`: ` [string='%f-%i%I%v.%x'] Default pattern for output file names. Affected by global options. - ``pcb_finish`` :index:`: ` [string='HAL'] Finishing used to protect pads. Currently used for documentation and to choose default colors. KiCad 6: you should set this in the Board Setup -> Board Finish -> Copper Finish option. Currently known are None, HAL, HASL, HAL SnPb, HAL lead-free, ENIG, ENEPIG, Hard gold, ImAg, Immersion Silver, Immersion Ag, ImAu, Immersion Gold, Immersion Au, Immersion Tin, Immersion Nickel, OSP and HT_OSP. - ``pcb_material`` :index:`: ` [string='FR4'] PCB core material. Currently used for documentation and to choose default colors. Currently known are FR1 to FR5. - ``remove_adhesive_for_dnp`` :index:`: ` [boolean=true] When applying filters and variants remove the adhesive (glue) for components that won't be included. - ``remove_solder_mask_for_dnp`` :index:`: ` [boolean=false] When applying filters and variants remove the solder mask apertures for components that won't be included. - ``remove_solder_paste_for_dnp`` :index:`: ` [boolean=true] When applying filters and variants remove the solder paste for components that won't be included. - ``resources_dir`` :index:`: ` [string='kibot_resources'] Directory where various resources are stored. Currently we support colors and fonts. They must be stored in sub-dirs. I.e. kibot_resources/fonts/MyFont.ttf Note this is mainly useful for CI/CD, so you can store fonts and colors in your repo. Also note that the fonts are installed using a mechanism known to work on Debian, which is used by the KiBot docker images, on other OSs *your mileage may vary*. - ``restore_project`` :index:`: ` [boolean=false] Restore the KiCad project after execution. Note that this option will undo operations like `set_text_variables`. Starting with 1.6.4 it also restores the PRL (Project Local Settings) and DRU (Design RUles) files. - ``set_text_variables_before_output`` :index:`: ` [boolean=false] Run the `set_text_variables` preflight before running each output that involves variants. This can be used when a text variable uses the variant and you want to create more than one variant in the same run. Note that this could be slow because it forces a board reload each time you run an output that uses variants. - ``silk_screen_color`` :index:`: ` [string='white'] Color for the markings. Currently used for documentation and to choose default colors. KiCad 6: you should set this in the Board Setup -> Physical Stackup. Currently known are black and white. - ``silk_screen_color_bottom`` :index:`: ` [string=''] Color for the bottom silk screen. When not defined `silk_screen_color` is used. Read `silk_screen_color` help. - ``silk_screen_color_top`` :index:`: ` [string=''] Color for the top silk screen. When not defined `silk_screen_color` is used. Read `silk_screen_color` help. - ``solder_mask_color`` :index:`: ` [string='green'] Color for the solder mask. Currently used for documentation and to choose default colors. KiCad 6: you should set this in the Board Setup -> Physical Stackup. Currently known are green, black, white, yellow, purple, blue and red. - ``solder_mask_color_bottom`` :index:`: ` [string=''] Color for the bottom solder mask. When not defined `solder_mask_color` is used. Read `solder_mask_color` help. - ``solder_mask_color_top`` :index:`: ` [string=''] Color for the top solder mask. When not defined `solder_mask_color` is used. Read `solder_mask_color` help. - ``time_format`` :index:`: ` [string='%H-%M-%S'] Format used for the time we started the script. Uses the `strftime` format. - ``time_reformat`` :index:`: ` [boolean=true] Tries to reformat the PCB/SCH date using the `date_format`. This assumes you let KiCad fill this value and hence the time is in ISO format (YY-MM-DD). - ``units`` :index:`: ` [string=''] [millimeters,inches,mils] Default units. Affects `position`, `bom` and `panelize` outputs. Also KiCad 6 dimensions. - ``use_dir_for_preflights`` :index:`: ` [boolean=true] Use the global `dir` as subdir for the preflights. - ``use_os_env_for_expand`` :index:`: ` [boolean=true] In addition to KiCad text variables also use the OS environment variables when expanding `${VARIABLE}`. - ``variant`` :index:`: ` [string=''] Default variant to apply to all outputs.