4.3.2. Command open-project

This command opens a LibrePCB project and lets you execute some tasks with it.

Command

  1. $ ./librepcb-cli open-project --help

Output

  1. Usage: ./librepcb-cli [options] open-project [command_options] project
  2. LibrePCB Command Line Interface
  4. Options:
  5.   -h, --help                         Displays this help.
  6.   -v, --version                      Displays version information.
  7.   --verbose                          Verbose output.
  8.   --erc                              Run the electrical rule check, print all
  9.                                      non-approved warnings/errors and report
  10.                                      failure (exit code = 1) if there are
  11.                                      non-approved messages.
  12.   --export-schematics <file>         Export schematics to given file(s).
  13.                                      Existing files will be overwritten.
  14.                                      Supported file extensions: pdf
  15.   --export-bom <file>                Export generic BOM to given file(s).
  16.                                      Existing files will be overwritten.
  17.                                      Supported file extensions: csv
  18.   --export-board-bom <file>          Export board-specific BOM to given
  19.                                      file(s). Existing files will be
  20.                                      overwritten. Supported file extensions: csv
  21.   --bom-attributes <attributes>      Comma-separated list of additional
  22.                                      attributes to be exported to the BOM.
  23.                                      Example: "MANUFACTURER, MPN"
  24.   --export-pcb-fabrication-data      Export PCB fabrication data
  25.                                      (Gerber/Excellon) according the fabrication
  26.                                      output settings of boards. Existing files
  27.                                      will be overwritten.
  28.   --pcb-fabrication-settings <file>  Override PCB fabrication output settings
  29.                                      by providing a *.lp file containing custom
  30.                                      settings. If not set, the settings from the
  31.                                      boards will be used instead.
  32.   --board <name>                     The name of the board(s) to export. Can be
  33.                                      given multiple times. If not set, all
  34.                                      boards are exported.
  35.   --save                             Save project before closing it (useful to
  36.                                      upgrade file format).
  37.   --strict                           Fail if the project files are not strictly
  38.                                      canonical, i.e. there would be changes when
  39.                                      saving the project. Note that this option
  40.                                      is not available for *.lppz files.
  42. Arguments:
  43.   open-project                       Open a project to execute project-related
  44.                                      tasks.
  45.   project                            Path to project file (*.lpp[z]).
Example: Check ERC Messages and Export Schematics & Boards

This command is useful for Continuous Integration of LibrePCB projects because it reports failure if you check in projects with non-approved ERC messages. In addition, it generates all production data so you don’t have to do it manually.

Command

  1. $ ./librepcb-cli open-project \
  2.     --erc \
  3.     --export-schematics="output/{{VERSION}}/{{PROJECT}}_Schematics.pdf" \
  4.     --export-pcb-fabrication-data \
  5.     MyProject.lpp

Output

  1. Open project 'MyProject.lpp'...
  2. Run ERC...
  3.   Approved messages: 7
  4.   Non-approved messages: 2
  5.     - [WARNING] Net signal connected to less than two pins: "CAN_RX"
  6.     - [WARNING] Net signal connected to less than two pins: "JTCK"
  7. Export schematics to 'output/{{VERSION}}/{{PROJECT}}_Schematics.pdf'...
  8.   => 'output/v1/MyProject_Schematics.pdf'
  9. Export PCB fabrication data...
  10.   Board 'default':
  11.     => 'output/v1/gerber/MyProject_DRILLS-PTH.drl'
  12.     => 'output/v1/gerber/MyProject_OUTLINES.gbr'
  13.     => 'output/v1/gerber/MyProject_COPPER-TOP.gbr'
  14.     => 'output/v1/gerber/MyProject_COPPER-BOTTOM.gbr'
  15.     => 'output/v1/gerber/MyProject_SOLDERMASK-TOP.gbr'
  16.     => 'output/v1/gerber/MyProject_SOLDERMASK-BOTTOM.gbr'
  17.     => 'output/v1/gerber/MyProject_SILKSCREEN-TOP.gbr'
  18.     => 'output/v1/gerber/MyProject_SILKSCREEN-BOTTOM.gbr'
  19. Finished with errors!

In this example, the application reported errors and exited with code 1 because there are non-approved ERC messages.