Usage¶
kmake - collection of command line KiCad automation utilites. Program must be run in project workdir.
usage: kmake [-h] [--debug]
{aux-origin,bom,clean,dnp,gerber,get-ignore,globlib,impedance,init-project,kibuzzard-to-graphic,loclib,logos,netlist,pcb-filter,pnp,prettify,rename,sch,set-drc,stackup-export,step,version,wireframe}
...
Named Arguments¶
- --debug, --verbose, --dbg
increase verbosity, keep temp files
Default:
False
Subcommands¶
- subcommand
Possible choices: aux-origin, bom, clean, dnp, gerber, get-ignore, globlib, impedance, init-project, kibuzzard-to-graphic, loclib, logos, netlist, pcb-filter, pnp, prettify, rename, sch, set-drc, stackup-export, step, version, wireframe
To display help for specific subcommand use “kmake SUBCOMMAND -h”
Sub-commands¶
aux-origin¶
Set drill origin to bounding box corner or given x,y coordinate.
kmake aux-origin [-h] (-r | -s {tl,tr,bl,br} | -p x_pos y_pos)
Named Arguments¶
- -r, --reset
Reset position of auxilary origin to (0,0).
Default:
False- -s, --side
Possible choices: tl, tr, bl, br
Edge of the PCB bounding box to place aux origin, default: bl.
- -p, --position
Position for aux origin to be placed.
bom¶
Generate Bill-of-Materials (BOM). Include ONLY populated components by default.Default format is default .None of the options include blacklisted components unless –no-ignore flag is passed.
kmake bom [-h] [-d | -a] [--no-ignore] [--fields FIELDS [FIELDS ...]] [-g]
[-o OUTPUT]
Named Arguments¶
- -d, --dnp
Include ONLY DNP components.
Default:
False- -a, --all
Include populated and DNP components.
Default:
False- --no-ignore
Don’t ignore blacklisted components.
Default:
False- --fields
Change BoM field. Available fields: Reference Designators Reference Quantity Value Footprint Manufacturer Manufacturer Part Number MPN DNP Description. When not provided default setup is selected (Reference Quantity Value Footprint Manufacturer MPN)
- -g, --group-references
Group references of components into single line
Default:
True- -o, --output
Output file name
clean¶
Clean redundant project files from project’s directory.
kmake clean [-h]
dnp¶
Fix discrepancies between DNP, exclude-from-bom and exclude-from-board atributes in schematic symbols and footprints.
kmake dnp [-h] [-l] [-rp] [-sp] [-atp] [-rtp]
Named Arguments¶
- -l, --list-broken
List references of malformed DNP schematic components, do not modify.
Default:
False- -rp, --remove-dnp-paste
Remove solder paste from DNP components footprints.
Default:
False- -sp, --restore-dnp-paste
Restore solder paste on DNP components footprints.
Default:
False- -atp, --add-tht-paste
Add solder paste on THT components footprints.
Default:
False- -rtp, --restore-tht-paste
Restore no solder paste on THT components footprints.
Default:
False
gerber¶
Generate production files of PCB layers and drills in Gerber format.
kmake gerber [-h] [-e] [-x] [--drill-origin {absolute,plot}]
Named Arguments¶
- -e, --noedge
Do not copy content of Edge.Cuts to other layers.
Default:
False- -x, --excellon
Set drill file format to Excellon.
Default:
False- --drill-origin
Possible choices: absolute, plot
Set drill file origin to absolute origin or plot (relative).
Default:
'absolute'
get-ignore¶
Copy .gitignore file from template.
kmake get-ignore [-h]
globlib¶
Link symbols and footprints to global libraries.
kmake globlib [-h] [--include-kicad-lib] [--exclude-pcb] [--update-all]
[--update-properties] [-s [SCH ...]]
Named Arguments¶
- --include-kicad-lib
Use also KiCad official libraries (if installed).
Default:
False- --exclude-pcb
Do not propagate footprint links from schematic to PCB
Default:
False- --update-all
Include symbols that already link to global libraries
Default:
False- --update-properties
Update all properties of symbols/footprints based on global library
Default:
False- -s, --sch
Specify list of schematic files to update, this option also enables –exclude-pcb
impedance¶
Generate impedance maps in Gerber format.
kmake impedance [-h]
init-project¶
Initialize KiCad project.
kmake init-project [-h] [-c COMPANY] -t [TITLE ...] [--force-title] [-s SIZE]
[-r]
Named Arguments¶
- -c, --company
Company name.
- -t, --title
Project title.
- --force-title
Everride existing title.
Default:
False- -s, --size
Page size, default A3.
Default:
'A3'- -r, --reload
Remove project info except: company name, page size, and project title
Default:
False
kibuzzard-to-graphic¶
Convert Kibuzzard footprints to graphical polygons
kmake kibuzzard-to-graphic [-h]
loclib¶
Create local project library and link symbols/footprint/3D models to this library.
kmake loclib [-h] [-f] [-c]
Named Arguments¶
- -f, --force, --force-override
Rewrite local library.
Default:
False- -c, --cleanup, --cleanup-lib-symbols
Remove unrefferenced lib_symbols, footprints and 3D models.
Default:
False
logos¶
Adds selected logo to the schematic.
kmake logos [-h] [-s SIZE] [-p PATH] [--list] [<logo file> ...]
Positional Arguments¶
- <logo file>
Name of the logo file.
Named Arguments¶
- -s, --size
Size of the logos.
Default:
180- -p, --path
Custom path to logos folder.
Default:
'/home/runner/.local/share/kmake/logos/'- --list
List available logos.
Default:
False
netlist¶
Create KiCad netlist file.
kmake netlist [-h]
pcb-filter¶
Create *.kicad_pcb
kmake pcb-filter [-h] [-o OUTFILE] [-i INFILE] [-c] [-x REF_FILTER]
[-xo REF_FILTER_OTHER] [-s {top,bottom}] [--std-edge] [-st]
[-d] [-t] [-z] [--vias] [-r] [-v] [-l ALLOWED_LAYERS]
[-lf ALLOWED_LAYERS_FULL] [--generate-frame]
[--std-dimension] [--mirror-bottom]
Named Arguments¶
- -o, --outfile
Name of output file (defaults to filtred.kicad_pcb)
Default:
'filtred.kicad_pcb'- -i, --infile
Name of input file (defaults to {$PRO_NAME}.kicad_pcb)
- -c, --cascade
If output file exists use it as input, simplifies cascaded calls
Default:
False- -x, --ref-filter
- Pattern based component filter
eg. -x “+J+D-D1” - remove components other than connectors(J) and diodes(D), diode D1 will also be removed, eg. -x=”-J-D+D1” - remove connectors(J) and diodes(D), other components and diode D1 will left untouched (note = when first character is -)
- -xo, --ref-filter-other
–ref-filter filter used on side opposite to –side
- -s, --side
Possible choices: top, bottom
Leave only components from selected layer
- --std-edge
Copy edge.cuts from footprints to pcb; Set all Edge.Cuts graphics thickness
Default:
False- -st, --stackup
Remove stackup table
Default:
False- -d, --dimensions
Remove dimensions (dimmensions should be added on User.Drawings layer)
Default:
False- -t, --tracks
Remove tracks
Default:
False- -z, --zones
Remove cooper & keepout zones
Default:
False- --vias
Remove vias
Default:
False- -r, --references
Remove footprint references
Default:
False- -v, --values
Remove footprint values
Default:
False- -l, --allowed-layers
Remove all graphic/footprint elements except those on specified layers (leaves knockout text untouched)
- -lf, --allowed-layers-full
Remove all graphic/footprint elements except those on specified layers (removes also knockout text)
- --generate-frame
Generate output that is rectangle created from board outline b-box expanded by 60mm
Default:
False- --std-dimension
Standardize/add main dimensions
Default:
False- --mirror-bottom
Mirror text if side is bottom
Default:
False
pnp¶
Create footprint position files.
kmake pnp [-h] [-t] [-v] [-o] [-e]
Named Arguments¶
- -t, --tht
Include THT components in output.
Default:
False- -v, --virtual
Include Virtual components in output.
Default:
False- -o, --other
Include Other type components in output.
Default:
False- -e, --excluded
Include components excluded from position files in output.
Default:
False
prettify¶
Pretify files to conform with KiCad formatter
kmake prettify [-h]
rename¶
Rename project files.
kmake rename [-h] <new_name>
Positional Arguments¶
- <new_name>
New name of project.
sch¶
Generate schematics in PDF format.
kmake sch [-h] [-t [THEME]]
Named Arguments¶
- -t, --theme
Theme to use for the schematic (default: schematic settings).
Default:
''
set-drc¶
Sets DRC and custom DRC rules from provided template.
kmake set-drc [-h] [-s [S]] [--no-dru] [-u [U]]
Named Arguments¶
- -s
Manufacturer DRC rules set.
Default:
''- --no-dru
Do not set custom rules.
Default:
False- -u
Set custom rules only.
Default:
''
stackup-export¶
Export stackup information to file.
kmake stackup-export [-h] [-o OUTPUT_FILENAME] [--legacy-csv]
Named Arguments¶
- -o
Change export file name/location.
- --legacy-csv
Export as csv with legacy format.
Default:
False
step¶
Export 3D models of PCB in STEP format.
kmake step [-h]
version¶
Print kmake, kiutils & kicad version
kmake version [-h]
wireframe¶
Split outline layer to top/bottom and optionally export it as .svg and .gbr files.
kmake wireframe [-h] [-r] [-i INPUT]
[-p {simple,dimensions,descriptions,assembly_drawing,margin_frame}]
[-sr] [-f PCB_FILTER_ARGS] [-a] [-x REF_FILTER]
[-xo REF_FILTER_OTHER]
Named Arguments¶
- -r, --reset
Reset layer of outline items to User.9 .
Default:
False- -i, --input
Use specified *.kicad_pcb file as input
- -p, --preset
Possible choices: simple, dimensions, descriptions, assembly_drawing, margin_frame
Generate SVG according to preset
- -sr, --set-ref
Set footprint references to certain state (reset position, set size, ..)
Default:
False- -f, --pcb-filter-args
- Additional arguments to be passed to pcb-filter;
(overrides argument value from preset, unless –pcb-filter-args-append specified) eg. -f ‘{“allowed_layers”:”+J+D-D1”}’
Default:
{}- -a, --pcb-filter-args-append
- Lists/strings, that are passed to pcb-filter (pcb-filter-args, ref-filter, ref-filter-other)
will be appended to ones defined in preset
Default:
False- -x, --ref-filter
- Argument passed to pcb-filter: Pattern based component filter
eg. -x “+J+D-D1” - remove components other than connectors(J) and diodes(D), diode D1 will also be removed, eg. -x=”-J-D+D1” - remove connectors(J) and diodes(D), other components and diode D1 will left untouched (note = when first character is -)
- -xo, --ref-filter-other
Argument passed to pcb-filter: –ref-filter filter used on side opposite to –side