English is currently available.
KiCad DISCUSSION
What is a reliable way to share a KiCad project containing custom symbols and footprints? A project can look complete on the original workstation while depending on libraries stored elsewhere.
Which files and paths should be checked before handing the design to another engineer, and how can we distinguish a missing library from a footprint that has changed since placement?
Reference: KiCad 10.0.6 release notes (https://www.kicad.org/blog/2026/08/KiCad-10.0.6-Release/).
Keep the project's custom libraries with the project and use project-relative paths where supported. Include the relevant symbol and footprint library tables and any external models that may be redistributed. Avoid depending on a personal absolute path. A clean checkout on a second environment is a useful test because it exposes dependencies hidden by the original workstation's global configuration.
Distinguish the placed footprint data from its library source. An existing PCB may still display a footprint even if its library is unavailable, while an update-from-library operation can fail or change it later. Review such updates deliberately. Compare pad numbering, dimensions, mask and paste definitions against the intended component before accepting a replacement.
Document the KiCad version and the source of each custom part, including its datasheet revision and any local modifications. Include only the needed libraries when sharing a minimal reproduction, subject to their licenses. The goal is that another person can open, edit, update and regenerate outputs, rather than merely view a board that happens to contain cached geometry.
