KiExport

KiExport is a Python application for exporting manufacturing files from KiCad PCB design projects. This is a CLI (Command Line Interface) utility. Commands and arguments can be passed to the script while running or from a JSON configuration file named kiexport.json. You should be familiar working with CLI tools and how to execute commands from a terminal.

KiExport generates the manufacturing files based on the options available in the kiexport.json file, and saves them in an organized way. It renames the files, folders and create ZIP archive files with proper names so that you can send them to a manufacturer or client easily. Since the kiexport.json configuration file can be edited for any project, you only have to create the file once. The Mitayi Pico RP2040 project is added as a sample project to test the script.

Author: Vishnu Mohanan
Version: 0.0.27
Contributors: Dominic Le Blanc (@domleblanc94)

This tool was created with the help of ChatGPT. Thanks to humanity!

Why?

Currently, exporting manufacturing files from KiCad's own UI requires setting so many options correctly and moving through different steps for different types of files.
If you make a mistake in choosing the options correctly, you will end up with a "bad" manufacturing file that will waste your time later.
KiCad currently has no ability to save the export options as presets and it does not always remember the previously used options.
Existing plugins available for KiCad only work for specific types of files and specific set of manufacturing options.
The number and types of files generated from a KiCad project can be quite many. Renaming, organizing and archiving the files manually can be a tedious task. For example, we generate Gerbers, PCB PDF, Schematic PDF, STEP, VRML, CSV BoM, HTML BoM, Position Files, and Preview Images for a typical project. We have to do this every time we make a change to the project to keep consistency across the set of files generated at a time.
KiCad CLI can do almost all of what the KiCad UI can.
Instead of typing the arguments manually to a terminal all the time, we can save the options as a JSON file and call the KiCad CLI every time we want to generate the files.

Requirements

Python 3.x
KiCad 8.x
Git
Interactive HTML BoM Plugin (if you want to generate HTML BoM)
Recommended:
- VS Code
- Windows Terminal

Installation

KiExport relies on the KiCad-CLI tool to generate the files and therefore supports all the features of KiCad-CLI. You should have a KiCad version installed in your system to use this tool. You can download and install the latest version of KiCad from here. After installation, browse to the installation folder and find the bin directory where the kicad-cli.exe file is located. Add the bin folder to your System Path. If you do not know how to add a new path to the System Path variable, check out any tutorials on the internet.

You can clone/fork the project to obtain a copy of the repository in your system using the following command. Git should be installed and available on the path.

git clone https://github.com/vishnumaiea/KiExport.git

Additionally, you can download the project as a ZIP file from the main page or the Releases page and extract it in your system. After getting the files, you can add the project folder to the System Path. If your system opens Python script files with the Python interpreter by default, you can run any python script directly from the terminal even without using the .py extension as shown in the image below.

Example

Following is a tree view of the files generated by KiExport from the Mitayi Pico RP2040 project. A top level revision folder will be created to store the files for that specific revision. Under that, a date-specific folder will be created to store files generated in a specific day. Inside that, file-specific folders are created to store the different types of files. ZIP archives are created for some type of files that are usually sent as a set of files to the manufacturer, for example Gerbers.

If you generate the files multiple times a day, older files will be overwritten except for any files with a sequence number at the end of the filename. For example, ZIP files have a sequence number at the end of the filename after the date string. A new file with a new sequence number will be created when multiple files are generated.

\---R0.6
    \---2024-10-26
        +---3D
        |       Mitayi-Pico-RP2040-R0.6-STEP-26102024-1.step
        |       Mitayi-Pico-RP2040-R0.6-VRML-26102024-1.wrl
        |
        +---Assembly
        |       Mitayi-Pico-RP2040-R0.6-Pos-All.csv
        |       Mitayi-Pico-RP2040-R0.6-Pos-Back.csv
        |       Mitayi-Pico-RP2040-R0.6-Pos-Front.csv
        |       Mitayi-Pico-RP2040-R0.6-Position-Files-26102024-1.zip
        |
        +---BoM
        |       Mitayi-Pico-RP2040-R0.6-BoM-CSV-26102024-1.csv
        |       Mitayi-Pico-RP2040-R0.6-BoM-HTML-26102024-1.html
        |
        +---Gerber
        |       Mitayi-Pico-RP2040-R0.6-B_Courtyard.gbr
        |       Mitayi-Pico-RP2040-R0.6-B_Cu.gbr
        |       Mitayi-Pico-RP2040-R0.6-B_Fab.gbr
        |       Mitayi-Pico-RP2040-R0.6-B_Mask.gbr
        |       Mitayi-Pico-RP2040-R0.6-B_Paste.gbr
        |       Mitayi-Pico-RP2040-R0.6-B_Silkscreen.gbr
        |       Mitayi-Pico-RP2040-R0.6-Edge_Cuts.gbr
        |       Mitayi-Pico-RP2040-R0.6-F_Courtyard.gbr
        |       Mitayi-Pico-RP2040-R0.6-F_Cu.gbr
        |       Mitayi-Pico-RP2040-R0.6-F_Fab.gbr
        |       Mitayi-Pico-RP2040-R0.6-F_Mask.gbr
        |       Mitayi-Pico-RP2040-R0.6-F_Paste.gbr
        |       Mitayi-Pico-RP2040-R0.6-F_Silkscreen.gbr
        |       Mitayi-Pico-RP2040-R0.6-Gerber-26102024-1.zip
        |       Mitayi-Pico-RP2040-R0.6-job.gbrjob
        |       Mitayi-Pico-RP2040-R0.6-NPTH-drl_map.pdf
        |       Mitayi-Pico-RP2040-R0.6-NPTH.drl
        |       Mitayi-Pico-RP2040-R0.6-PTH-drl_map.pdf
        |       Mitayi-Pico-RP2040-R0.6-PTH.drl
        |       Mitayi-Pico-RP2040-R0.6-User_Comments.gbr
        |       Mitayi-Pico-RP2040-R0.6-User_Drawings.gbr
        |
        +---PCB
        |       Mitayi-Pico-RP2040-R0.6-B_Courtyard.pdf
        |       Mitayi-Pico-RP2040-R0.6-B_Cu.pdf
        |       Mitayi-Pico-RP2040-R0.6-B_Fab.pdf
        |       Mitayi-Pico-RP2040-R0.6-B_Mask.pdf
        |       Mitayi-Pico-RP2040-R0.6-B_Paste.pdf
        |       Mitayi-Pico-RP2040-R0.6-B_Silkscreen.pdf
        |       Mitayi-Pico-RP2040-R0.6-Edge_Cuts.pdf
        |       Mitayi-Pico-RP2040-R0.6-F_Courtyard.pdf
        |       Mitayi-Pico-RP2040-R0.6-F_Cu.pdf
        |       Mitayi-Pico-RP2040-R0.6-F_Fab.pdf
        |       Mitayi-Pico-RP2040-R0.6-F_Mask.pdf
        |       Mitayi-Pico-RP2040-R0.6-F_Paste.pdf
        |       Mitayi-Pico-RP2040-R0.6-F_Silkscreen.pdf
        |       Mitayi-Pico-RP2040-R0.6-PCB-PDF-26102024-1.zip
        |       Mitayi-Pico-RP2040-R0.6-PCB-PDF-All-26102024-1.pdf
        |       Mitayi-Pico-RP2040-R0.6-User_Comments.pdf
        |       Mitayi-Pico-RP2040-R0.6-User_Drawings.pdf
        |
        +---SCH
        |       Mitayi-Pico-RP2040-R0.6-SCH-26102024-1.pdf
        |
        \---SVG
                Mitayi-Pico-RP2040-R0.6-SVG-26102024-1.svg

Usage

You can run the Python script directly from the source folder with the following command. Python should be installed and available on the path.

python kiexport.py <command> <arguments>

In addition, you can also run the Windows executable kiexport.exe with the following command. The dist folder should be added to the path in order for this to work.

kiexport <command> <arguments>

You can automate running multiple commands with a batch script. Refer to the export.bat file for an example. Run the script to see KiExport in action.

@REM @echo off

:: Set variables
set OUTPUT_DIR=Export
set SCH_FILE=Mitayi-Pico-RP2040.kicad_sch
set PCB_FILE=Mitayi-Pico-RP2040.kicad_pcb

:: Execute commands
kiexport sch_pdf -od "%OUTPUT_DIR%" -if "%SCH_FILE%"
kiexport bom -od "%OUTPUT_DIR%" -if "%SCH_FILE%"
kiexport ibom -od "%OUTPUT_DIR%" -if "%PCB_FILE%"
kiexport pcb_pdf -od "%OUTPUT_DIR%" -if "%PCB_FILE%"
kiexport gerbers -od "%OUTPUT_DIR%" -if "%PCB_FILE%"
kiexport positions -od "%OUTPUT_DIR%" -if "%PCB_FILE%"
kiexport ddd -od "%OUTPUT_DIR%" -if "%PCB_FILE%" -t "STEP"
kiexport ddd -od "%OUTPUT_DIR%" -if "%PCB_FILE%" -t "VRML"

pause

Commands

`version`

Run the following command to show the version of the tool.

kiexport -v

kiexport --version

`help`

Show the help menu.

kiexport -h

kiexport --help

You can include the command to get the help menu of a specific command. For example,

kiexport gerbers -h

`gerbers`

Export Gerbers.

kiexport gerbers -if <input_file> -od <output_dir>

-if: Path to the input .kicad_pcb file. Required.
-od: Path to the output directory. Required.

`positions`

Export Position or Centroid files for PCB assembly (PCBA).

kiexport positions -if <input_file> -od <output_dir>

-if: Path to the input .kicad_pcb file. Required.
-od: Path to the output directory. Required.

Example:

kiexport positions -if "Mitayi-Pico-D1/Mitayi-Pico-RP2040.kicad_pcb" -od "Mitayi-Pico-D1/Export"

`pcb_pdf`

Export the PCB layers as individual PDF.

kiexport pcb_pdf -if <input_file> -od <output_dir>

-if: Path to the input .kicad_pcb file. Required.
-od: Path to the output directory. Required.

Example:

kiexport pcb_pdf -if "Mitayi-Pico-D1/Mitayi-Pico-RP2040.kicad_pcb" -od "Mitayi-Pico-D1/Export"

`sch_pdf`

Export the schematic as PDF.

kiexport sch_pdf -if <input_file> -od <output_dir>

-if: Path to the input .kicad_sch file. Required.
-od: Path to the output directory. Required.

Example:

kiexport sch_pdf -if "Mitayi-Pico-D1/Mitayi-Pico-RP2040.kicad_sch" -od "Mitayi-Pico-D1/Export"

`ddd`

Export the 3D files.

kiexport ddd -if <input_file> -od <output_dir> -t <type>

-if: Path to the input .kicad_pcb file. Required.
-od: Path to the output directory. Required.
-t: The type of 3D file to export. Possible values are STEP and VRML. Required.

Example:

kiexport ddd -if "Mitayi-Pico-D1/Mitayi-Pico-RP2040.kicad_pcb" -od "Mitayi-Pico-D1/Export" -t STEP

`svg`

Export the PCB as SVG files.

kiexport svg -if <input_file> -od <output_dir>

-if: Path to the input .kicad_pcb file. Required.
-od: Path to the output directory. Required.

Example:

kiexport svg -if "Mitayi-Pico-D1/Mitayi-Pico-RP2040.kicad_pcb" -od "Mitayi-Pico-D1/Export"

`bom`

Export the bill of materials files.

kiexport bom -if <input_file> -od <output_dir> -t <type>

-if: Path to the input .kicad_sch file. Required.
-od: Path to the output directory. Required.
-t: The type of bill of materials to export. Possible values are CSV. Optional.

Example:

kiexport bom -if "Mitayi-Pico-D1/Mitayi-Pico-RP2040.kicad_sch" -od "Mitayi-Pico-D1/Export" -t CSV

`ibom`

Export an HTML BoM with the help of the Interactive HTML BoM plugin for KiCad. The plugin should be available in your PC. You need to add the paths to generate_interactive_bom.py script and the KiCad Python path ("C:\Program Files\KiCad\8.0\bin\python.exe" for example) to the JSON configuration file. Check the configuration file available in the Mitayi-Pico-D1 folder for an example.

kiexport ibom -od <output_dir> -if <input_file>

-od: Path to the output directory. Required.
-if: Path to the input .kicad_pcb file. Required.

Example:

kiexport ibom -od "Mitayi-Pico-D1/Export" -if "Mitayi-Pico-D1/Mitayi-Pico-RP2040.kicad_pcb"

`run`

This command can be used to generate multiple types of files by providing just a valid JSON configuration file. Unlike other commands which will look specifically for the kiexport.json file, this command will accept a JSON file with any name. This is useful when you need different configurations for different manufacturers and use-cases. You can create a configuration file for each manufacturer and use them with the run command individually.

Since the run command does not accept any other arguments, everything needed to generate the manufacturing files should be in the JSON configuration file.

kiexport run <config_file>

<config_file>: Path to the JSON configuration file. Required.

Example:

kiexport run Mitayi-Pico-D1/kiexport.json

Configuration File

KiExport supports a JSON configuration file called kiexport.json. The name of the file should be exact when running the all of the generic commands except run. The run command will accept a configuration file with any name. The configuration file should be placed in the root folder of your KiCad project where the main .kicad_sch and .kicad_pcb files are located. Check the Mitayi-Pico-D1 folder for an example. A copy of the default configuration file is integrated into the script to use as the default one. So if any of the input parameters are missing from your configuration file, the script will use the default values.

To create a configuration file for your own project, add the project_name, the required commands under commands. The commands can be a simple list of strings, or a nested list. You can add any number of instances of the same command. The data for the commands should be added under data. All keys that starts with -- are directly passed to the KiCad-CLI and anything that starts with kie_ is a data for the KiExport application.

Limitations

KiExport can only do as much as the KiCad CLI can do.
Can not generate PCB preview images from the 3D viewer. Currently this is not supported by the KiCad CLI.

License

This project is licensed under the MIT license.

Name		Name	Last commit message	Last commit date
Latest commit History 60 Commits
Mitayi-Pico-D1		Mitayi-Pico-D1
dist		dist
resources		resources
.gitignore		.gitignore
Changes.md		Changes.md
Readme.md		Readme.md
kiexport.py		kiexport.py

Provide feedback

Saved searches

Use saved searches to filter your results more quickly

Repository files navigation

KiExport

Table of Contents

Why?

Requirements

Installation

Example

Usage

Commands

`version`

`help`

`gerbers`

`positions`

`pcb_pdf`

`sch_pdf`

`ddd`

`svg`

`bom`

`ibom`

`run`

Configuration File

Limitations

License

References

About

Releases 1

Packages

Languages

vishnumaiea/KiExport

Folders and files

Latest commit

History

Repository files navigation

KiExport

Table of Contents

Why?

Requirements

Installation

Example

Usage

Commands

version

help

gerbers

positions

pcb_pdf

sch_pdf

ddd

svg

bom

ibom

run

Configuration File

Limitations

License

References

About

Resources

Stars

Watchers

Forks

Releases 1

Packages 0

Languages

`version`

`help`

`gerbers`

`positions`

`pcb_pdf`

`sch_pdf`

`ddd`

`svg`

`bom`

`ibom`

`run`

Packages