Makefile to create releases of KiCad designs. This project has a branch for each version of versions of KiCad that have the CLI tool (v7, v8, & v9 currently).
At a minimum you'll need the kicad-cli which is available with KiCad 7+ some of the features here are only available in v8+. Depending on how you installed kicad this could be a whole bunch of places. Find it and add the location to your path.
flatpak
KICADCLI=flatpak run --command=kicad-cli org.kicad.KiCadsnap
KICADCLI=/snap/bin/kicad.kicad-clidocker
KICADCLI=docker run -v /tmp/.X11-unix:/tmp/.X11-unix -v ${HOME}:${HOME} -it --rm -e DISPLAY=:0 --name kicad-cli kicad/kicad:8.0 kicad-cliFor python tools you'll also need to set the PYTHONPATH to find the pcbnew.py library. For Ubuntu when using aptitude it should show up in /usr/lib/python3/dist-packages. I add the following to my .zshrc / .bashrc.
PCBNEW_DIR=/usr/lib/python3/dist-packages
export PYTHONPATH=${PYTHONPATH}:${PCBNEW_DIR}Install the subdirectories in the same python environment. If these outputs are not needed then remove the related lines.
git submodule update --init --recursive
cd libs/InteractiveHtmlBom/ && pip install .- Runs DRC & ERC. If these do not pass than the manufacturing files won't be generated.
- Includes both generic and JLCPCB targeted outputs
- PDF Schematic
- SVG board outline (edge cuts)
- Gerbers w/ drill file & zipped gerbers
- Interactive HTML BOM
- STEP model of board
- centroid w/ KiCad and JLCPCB format
- Full BOM and JLCPCB version
- PDF gerber report
- GenCAD
- ODB++
- IPC2581
- Renders of the board
We encourage using semantic numbering for board versions. See the blog post for the versioning scheme. As rolling the subversion number ({Major}.{Minor}.{Subversion}) is done to reflect BOM or manufacturing changes then the released board files will only be tied to the major & minor number. To reflect this we use {Major}.{Minor}.X as the board version. You can use any version number you want though.
You can copy or symlink the makefile into your project however I prefer to point to the file directly with makes -f command. The only usage requirements are:
- All dependencies need to be on your path
- make is called from the project directory
- make finds the Makefile
This is the default target and generates everything.
make -f kicad-make/Makefile PROJECT=<name of kicad project> VERSION=<version number>Try to not do this too often... Exports everything, skipping ERC and DRC check.
make -f kicad-make/Makefile PROJECT=<name of kicad project> VERSION=<version number> no-drcmake -f kicad-make/Makefile PROJECT=<name of kicad project> VERSION=<version number> schematic>> ls
project.kicad_pro project.kicad_sch project.kicad_pcb project.kicad_prl
>> make -f kicad-make/Makefile PROJECT=project VERSION=0.1.X
>> ls
project.kicad_pro project.kicad_sch project.kicad_pcb project.kicad_prl
project_0.1.X.zip project_0.1.X.pdf project_0.1.X_interactive_bom.html fab
mechanicalA Dockerfile example is included to help with setting up your environment.
I prefer to setup the environment locally and would instead recommend setting the tool paths in the Makefile
itself to use the Docker commands. The kicad-cli command has a few examples of how to do that in the Makefile.
From the kicad-make repo directory run:
docker build -t kicad-env .From the kicad-make repo directory run:
docker run -v $(pwd):/home/kicad -it --rm --name t
asd kicad-env make -f /usr/share/kicad-make/Makefile PROJECT=jlcpcb-4Layer-JLC04161H-2116D VER
SION=0.1.X DIR=kicad-setting-boards/jlcpcb-4Layer-JLC04161H-2116D no-drcThis uses the settings board as an example build and uses the makefile in the Docker image.
| Target | Description |
|---|---|
all |
Default target, triggers release. |
clean |
Cleans up generated files and directories. |
release |
Full release process (DRC/ERC, manufacturing, packaging). |
documents |
Generates schematic, BOM, step, IBOM, & gerberpdf |
manufacturing |
Generates manufacturing files (Gerbers, IPC2581, etc.). |
no-drc |
Skips DRC & ERC, completes the rest of the release process |
schematic |
Generates schematic PDF. |
boms |
Generates BOM files (normal and LCSC). |
gerbers |
Generates Gerber files. |
fabzip |
Zips Gerber files and centroids for ordering. |
testpoints |
Generates a testpoint report. |
step |
Generates STEP file of the board. |
ibom |
Generates interactive BOM HTML. |
gerberpdf |
Converts a PDF report with the critical gerber layers |
centroid |
Generates centroid files for assembly. |
drc |
Runs Design Rule Check and saves the report. |
erc |
Runs Electrical Rule Check and saves the report. |
ipc2581 |
Generates IPC2581 files. |
board |
Builds final board (Gerbers, drills, centroid, outline). |
renders |
Generates 3D renders of the PCB (top, bottom, front, back, left, right). |
gencad |
Generates GEN-CAD files. |
odb |
Generates ODB++ files. |
- Add check of critical parts placement