How to initialize your KiCAD 5 project on the command line

In case you are using KiCAD 6 (released in 2021), this is not the right post for you ! See How to initialize your KiCAD 6 project on the command line

*Note:*This script initializes a KiCAD project in the recommended configuration (i.e. with project-specific footprint and symbol libraries). In case you want to initialize an empty project, see How to initialize an empty KiCAD project on the command line

TL;DR:

Inside the directory where you want to create the project, run

wget -qO- https://techoverflow.net/scripts/kicad-init.sh | bash /dev/stdin MyProject

You should replace MyProject (at the end of the command) with your project name.

*Note:*This will initialize an empty KiCAD project without any libraries. This is equivalent to creating a new project in KiCAD itself (using the GUI).

How it works

Our script is a simple bash script that creates the files that KiCAD creates when manually creating a new project.

It will create these files (MyProject is the default project name, but you can modify it using a command line argument):

MyProject.pro: The project file
MyProject.sch: The empty schematic
MyProject.kicad_pcb: The empty PCB
sym-lib-table: List of schematic symbol libraries for the project
libraries/MyProject.lib: Schematic symbol library
libraries/MyProject.dcm: Metadata for schematic symbols.
fp-lib-table: List of footprint libraries for the project
libraries/footprints: The folder where project-specific footprints (.kicad_mod files) are stored
libraries/3D: This folder should be used to store 3D models (e.g. STEP files)

The files are modelled after KiCAD 5.1.4 but we expect them to work with any recent KiCAD version.

#!/bin/bash
# TechOverflow KiCAD project initializer (with project FP & SYM libraries)
# Usage: $0 
if [ $# -ne 1 ]
then
    echo "Usage: $0 "
    exit 1
fi

# Compute project name and path
proj=$(basename "$1")
dir=$(dirname "$1")

# Create project file
cat < ${1}.pro
update=22/05/2015 07:44:53
version=1
last_client=kicad
[general]
version=1
RootSch=
BoardNm=
[pcbnew]
version=1
LastNetListRead=
UseCmpFile=1
PadDrill=0.600000000000
PadDrillOvalY=0.600000000000
PadSizeH=1.500000000000
PadSizeV=1.500000000000
PcbTextSizeV=1.500000000000
PcbTextSizeH=1.500000000000
PcbTextThickness=0.300000000000
ModuleTextSizeV=1.000000000000
ModuleTextSizeH=1.000000000000
ModuleTextSizeThickness=0.150000000000
SolderMaskClearance=0.000000000000
SolderMaskMinWidth=0.000000000000
DrawSegmentWidth=0.200000000000
BoardOutlineThickness=0.100000000000
ModuleOutlineThickness=0.150000000000
[cvpcb]
version=1
NetIExt=net
[eeschema]
version=1
LibDir=
[eeschema/libraries]
EOT

# Create schematic file
cat < ${1}.sch
EESchema Schematic File Version 2
EELAYER 25 0
EELAYER END
\$EndSCHEMATC
EOT

cat < ${1}.kicad_pcb
(kicad_pcb (version 4) (host kicad "dummy file") )
EOT

#
# Create schematic symbol library mapping
#
mkdir -p ${dir}/libraries
cat < ${dir}/sym-lib-table
(sym_lib_table
  (lib (name ${1})(type Legacy)(uri \${KIPRJMOD}/libraries/${proj}.lib)(options "")(descr ""))
)
EOT

cat < ${dir}/libraries/${proj}.lib
EESchema-LIBRARY Version 2.4
#encoding utf-8
#
#End Library
EOT

cat < ${dir}/libraries/${proj}.dcm
EESchema-DOCLIB  Version 2.0
#
#End Doc Library
EOT

#
# Create footprint library mapping (just an empty directory)
#
mkdir -p ${dir}/libraries/footprints

cat < ${dir}/fp-lib-table
(fp_lib_table
  (lib (name ${proj})(type KiCad)(uri \${KIPRJMOD}/libraries/footprints)(options "")(descr ""))
)
EOT

#
# Create directory for 3D models.
# The search path might need to be configured manually
# since it's not stored in a project
#
mkdir -p ${dir}/libraries/3D

#
# Create .gitignore
#
cat < .gitignore
*-bak
*-cache*
*-bak*
_autosave*
EOT

Run e.g. using

bash kicad-init.sh MyProject