KiExport

KiExport is a Python application for automating the manufacturing files generation process 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 and date stamps 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. You can also create multiple configuration files according to different manufacturing requirements.

The Mitayi Pico RP2040 project is added as a sample project to test the script. If you are on Windows, you can run the EXPORT-ALL.bat batch script to automatically generate the manufacturing files with a double-click.

Author: Vishnu Mohanan
Version: 0.1.8
Contributors: Dominic Le Blanc (@domleblanc94)

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

KiExport
- Table of Contents
- Why?
- Why not KiCad Jobsets?
- Requirements
- Installation
- Example
- Usage
- Commands
  - version
  - help
  - pcb_drc
  - gerbers
  - drills
  - positions
  - pcb_pdf
  - pcb_render
  - sch_pdf
  - ddd
  - svg
  - bom
  - run
- Configuration File
- Log File
- License
- References

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, XLS 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.

Why not KiCad Jobsets?

KiCad V9 added support for Jobsets which allow you to generate manufacturing files in an automated way. However, the feature is in its early stages and causes freezes and crashes often (at least when I tried it last time). Until the feature matures enough, the development on KiExport will continue.

Requirements

This software was developed and tested on Windows 11. It should work on other platforms as well, but it is not tested. The following software should be installed in your system to use this tool.

Python 3.x
KiCad 8.x or later
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 variable. 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.

If you are going to run the app as a Python script, install the dependencies using the following command.

pip install -r requirements.txt

Check if the app is working by checking the version of the tool. Open a terminal and run the following command.

kiexport -v

If you see the version printed, the installation is successful. Otherwise, follow the installation procedure again.

Example

Following is a tree view of the files generated by KiExport from the Mitayi-Pico-D1 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
        |
        +---Position
        |       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-XLS-26102024-1.xlsx
        |       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
        |
        +---Render
        |       Mitayi-Pico-RP2040-R0.6-Top-26102024-1.png
        |       Mitayi-Pico-RP2040-R0.6-Bottom-26102024-1.png
        |       Mitayi-Pico-RP2040-R0.6-Front-26102024-1.png
        |       Mitayi-Pico-RP2040-R0.6-Back-26102024-1.png
        |
        +---Report
        |       Mitayi-Pico-RP2040-R0.6-DRC-26102024-1.rpt
        |       Mitayi-Pico-RP2040-R0.6-DRC-26102024-1.json
        |
        +---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 system Path in order for this to work.

kiexport <command> <arguments>

You can automate running multiple commands with a batch script if you are on Windows. Refer to the EXPORT-ALL.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
@REM kiexport pcb_drc -od "%OUTPUT_DIR%" -if "%PCB_FILE%" -t "report"
@REM kiexport sch_pdf -od "%OUTPUT_DIR%" -if "%SCH_FILE%"
@REM kiexport bom -od "%OUTPUT_DIR%" -if "%SCH_FILE%" -t "CSV"
@REM kiexport bom -od "%OUTPUT_DIR%" -if "%SCH_FILE%" -t "XLS"
@REM kiexport bom -od "%OUTPUT_DIR%" -if "%PCB_FILE%" -t "HTML"
@REM kiexport pcb_pdf -od "%OUTPUT_DIR%" -if "%PCB_FILE%"
@REM kiexport pcb_render -od "%OUTPUT_DIR%" -if "%PCB_FILE%"
@REM kiexport gerbers -od "%OUTPUT_DIR%" -if "%PCB_FILE%"
@REM kiexport positions -od "%OUTPUT_DIR%" -if "%PCB_FILE%"
@REM kiexport ddd -od "%OUTPUT_DIR%" -if "%PCB_FILE%" -t "STEP"
@REM kiexport ddd -od "%OUTPUT_DIR%" -if "%PCB_FILE%" -t "VRML"

pause

You can also create a batch file for running the run command as shown below. You can then double-click on the script every time you want to generate new files, saving you from typing the same commands over and over.

kiexport run Mitayi-Pico-D1/kiexport.json

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

`pcb_drc`

Runs a DRC (Design Rule Check) on the PCB file. If there are errors in the design, evaluated as per the DRC rules, the command will return the type and number of errors found. It will also generate a report file and save it to the output directory. When ran as part of the run command, you can choose to skip other commands if there are DRC errors. The configruation for this command can be specified in the configuration file under the pcb_drc section. If a format type is specified in the CLI command, it will override the type specified in the configuration file.

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

-if: Path to the input .kicad_pcb file. Required.
-od: Path to the output directory where the report will be saved. Required.
-t: The type of report to generate. Possible values are report, and json. Optional. Defaults to the type specified in the configuration file.
- report - Generates a text report file with .rpt extension.
- json - Generates a JSON report file with .json extension.

`gerbers`

Export the Gerber files. Gerber files export does not include the drill files by default. If you want to generate the drill files as well, you can either manually run the drills command or enable the drill file generation in the JSON configuration file using the kie_include_drill flag.

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

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

Example:

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

`drills`

Generate the drill files. If you are generating drill files along with the gerbers command, you don't need to run this command again. Otherwise, the drill files will be generated twice.

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

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

Example:

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

`positions`

Export the 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"

`pcb_render`

Export the PCB as a rendered image.

kiexport pcb_render -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_render -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. Generating STEP files can take some time when the PCB is large. Wait for the process to complete. VRML file generation is faster.

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. The list of layers can be specified in the config file. You can also define common layers to be used when generating each layer. A ZIP file is created at the end while keeping the original files intact. Each run of the command will overwrite the standalone files but will create a new ZIP file with a new sequence number.

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/kicad_pcb file. Required.
-od: Path to the output directory. Required.
-t: The type of bill of materials to export. Possible values are CSV, XLS, and HTML. Optional. Defaults to CSV.
- CSV & XLS - Requires .kicad_sch file.
- HTML - Requires .kicad_pcb file.

Example:

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

Exporting the HTML BoM requires the Interactive HTML BoM plugin for KiCad. The plugin should be available in your PC. You need to add the paths to the generate_interactive_bom.py script and the KiCad Python ("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.

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. Check out the kiexport.json file for an example configuration file.

Since the run command does not accept any configuration parameters directly, everything needed to generate the manufacturing files should be in the JSON configuration file. Additionally, run can also accept a subset of commands to run from the supplied configuration file. This can be useful when you do not want to run the commands individually.

kiexport run <config_file> <commands>

<config_file>: Path to the JSON configuration file. Required.
<commands>: A list of commands to run from the configuration file. Optional. The list of commands should be a comma separated string in the same format as the commands key in the configuration file. Do not use quotes for individual commands in this case.

Example:

kiexport run Mitayi-Pico-D1/kiexport.json

kiexport run Mitayi-Pico-D1/kiexport.json "gerbers, positions"
kiexport run Mitayi-Pico-D1/kiexport.json "pcb_pdf, sch_pdf"
kiexport run Mitayi-Pico-D1/kiexport.json "gerbers, [ddd, STEP], [ddd, VRML]"

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.

If you want to disable any of the commands in the commands list, you can simply prefix or suffix them with, for example _, and KiExport will ignore such invalid commands. This is better than deleting the commands.

Log File

KiExport will generate a log file in a directory specified in the configuration file. This log can be used to check what commands were run and what files were created in the last run. The log file can be specified in the configuration file as follows for example:

"kiexport_log_path": "Export\\kiexport.log"

License

This project is licensed under the MIT license.

Name		Name	Last commit message	Last commit date
Latest commit History 118 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
requirements.txt		requirements.txt

Provide feedback

Saved searches

Use saved searches to filter your results more quickly

Uh oh!

Repository files navigation

KiExport

Table of Contents

Why?

Why not KiCad Jobsets?

Requirements

Installation

Example

Usage

Commands

`version`

`help`

`pcb_drc`

`gerbers`

`drills`

`positions`

`pcb_pdf`

`pcb_render`

`sch_pdf`

`ddd`

`svg`

`bom`

`run`

Configuration File

Log File

License

References

About

Uh oh!

Releases 1

Packages

Uh oh!

Contributors 2

Uh oh!

Languages

vishnumaiea/KiExport

Folders and files

Latest commit

History

Repository files navigation

KiExport

Table of Contents

Why?

Why not KiCad Jobsets?

Requirements

Installation

Example

Usage

Commands

version

help

pcb_drc

gerbers

drills

positions

pcb_pdf

pcb_render

sch_pdf

ddd

svg

bom

run

Configuration File

Log File

License

References

About

Resources

Uh oh!

Stars

Watchers

Forks

Releases 1

Packages 0

Uh oh!

Contributors 2

Uh oh!

Languages

`version`

`help`

`pcb_drc`

`gerbers`

`drills`

`positions`

`pcb_pdf`

`pcb_render`

`sch_pdf`

`ddd`

`svg`

`bom`

`run`

Packages