The KiCad 2024 Fund Drive is here!
Donate now Your support is critical to the development of KiCad in 2024
$100,000 TOTAL

Testing: Symbol Library Table Released

The KiCad project recently merged the symbol library table code for accessing symbol libraries into the master branch. This represents a significant change in the way symbol libraries are defined and accessed. It is similar in design and function of the footprint library table and will resolve the long standing issue with symbol library ordering in Eeschema along with some new features such as platform independence and lazy library loading. KiCad users should be familiar with the design and concept so this is not a tutorial on how to configure your symbol library table. It is important information that you need to understand in order to properly convert your existing schematics to use the symbol library table.

Much like the conversion over to the footprint library table, there will be issues and a learning curve. Hopefully, familiarity with the footprint library table will minimize the learning curve. The biggest issues will be with existing projects and users with custom symbol library configurations. Some of these issue will be mitigated by a new symbol library table remapping feature. This feature will be executed whenever a schematic is opened that has not yet been remapped. There are a few steps you should take ahead of time in order for the remapping to be the most effective.

Warning Please note, the remapped schematics will not be compatible with older version of KiCad so make sure to back your project schematic and project files before remapping a schematic just in case things go wrong.
  1. If you get warning about missing libraries when you start your current version of Eeschema, make sure to fix the missing libraries if they contained symbols that are in the schematic before you attempt to remap your schematic. Otherwise, the correct symbol will not be found and you will end up with broken symbol links in your schematic. You can test this by left clicking on a symbol in the schematic and verifying that the symbol is not being loaded from the cache library. If a symbol is being loaded from the cache library, you are already skating on thin ice.

  2. If you have been using a development build of KiCad, copy the full default global symbol library table (sym-lib-table) file from the template folder installed with the KiCad libraries or from the KiCad library repo to your KiCad user configuration folder. This will replace the empty one (most likely) created by Eeschema. If you do not do this, you will most likely end up with a bunch of broken symbol links.

  3. Make sure your default KiCad template project file ( has no entries in the [eeschema/libraries] section or get a copy from the KiCad source repo. If you build from source or are using a nightly build, the update project template file has already been installed. It is imperative that you do not have any symbol libraries in your project files. Otherwise, you could possible be effect by this bug which the symbol library table is designed to resolve.

  4. During the remapping process, symbol libraries not found in the global symbol library table will be used to create a project specific symbol library table. You will have to move them manually to the global symbol library table if that is your preference.

  5. For the most accurate remapping you should create a project library by copying the project cache file (project-name-cache.lib) to a different file and add it to the top of the symbol library list. You must use a version of KiCad prior to the symbol library table implementation in order to do this.

Please be aware that there are also some minor behavioral changes with the introduction of the symbol library table.

  1. When removing the symbol from a library currently being edited in the library editor, the next symbol in the library is not automatically loaded so the canvas will be empty. You will have to select a new symbol to edit.

  2. The cache library is not longer shown in either the symbol library viewer or the symbol library editor. The cache should have never be editable because any edits would get overwritten by the next schematic save. The cache being removed from the symbol library viewer is a minor issue. Given that the cache library is going away when the new schematic file format is completed it was decided that it adding a lot of extra code for something that will soon be obsolete didn’t make much sense.

  3. Symbol naming now follows the same convention as footprint naming. The colon ':' and forward slash '/' characters are illegal and will cause issues with broken symbol links. Please fix any symbol names that contain these characters. It is also a good idea to not use any characters that are not valid file name characters on both Posix and Windows file systems. When the new symbol library file format is implemented, illegal file name characters will cause issues.

This will be one of the last major code changes before the stable 5 release feature freeze so please help test it so we can get the stable 5 release out as soon as possible. Thank you for your patience during this transition.

See Also

Testing: Eagle import plugins

The KiCad project is proud to announce the support for importing Eagle projects. This is the outcome of work to complete the Eagle schematic file plugin and integrate it with the Eagle board file plugin. From the new "Import Project" menu entry in the KiCad launcher users may now select an Eagle schematic or board file and the new project name and location, after which the corresponding Eagle files will be imported respectively into EEschema and PcbNew.

New 3DViewer

After almost 15 months in development and testing, the new 3DViewer developed by Mario Luzeiro has been merged with the product branch in revision 6985 and has since been available in the nightly builds of KiCad. This viewer was written entirely from scratch and takes advantage of the 3D plugin system to provide visualization of all 3D model formats supported by available 3D plugins. Features include: Two new render targets: OpenGL (GPU accelerated), and ray tracing with post-processing effects.