Some tips requested to import symbol and lib files from another project

[rvamerongen]

Hello

I have found a basic project an did redraw/redesign this to my needs with several added components. Works fine.
But the basic project got some symbol, cache lib and .lib files that I would like tom import and use.

How should I do that? I would like them internal in my project because off uploading the project into git.

Any suggestions?

[paulvdh]

What KiCad version are you using?

The [Project]-cache.lib file is a remnant of KiCad V5. After a project is converted to a newer KiCad version this file can be deleted. You probably also have a [Project].pro file from KiCad V5, and a [project].kicad_pro file from a newer KiCad version. That old file can also be deleted.

If you want to work with git. Start with learning which files in your project are important and which should be ignored. Recently I stumbled onto a 500MB git repository for a 20MB project. There were over 30 zipped up KiCad backups and 10+ sets of gerber files in the git repository.

[rvamerongen]

Hi Paul,

Thank you for your Reply.
Indeed, the original files are from a older project. Not really mentioned but thats was a reason to start from scratch.

Is there a way to create project.lib symbol part files in the project ( folder / Project ) from the used parts/pretty footprint to keep them together? I would like to have them in the project folder.

I know about the zip files and yes you don’t want them into your repo. Side note: I copy them using a BU app as a kind repo for now.

[paulvdh]

In KiCad V6 an newer, there is no need to have libraries in your project. Even without any libraries the project is mostly OK. The only thing is that ERC and/or DRC starts nagging about missing libraries or differences between symbols (footprints) used in the schematic (PCB) and the libraries. That system is mostly important for people who use database driven libraries and need to verify that the used library parts are compatible with what is in the database. But KiCad has copies of all parts (Except 3D models) inside the schematic and PCB files itself, so you can not loose them. For hobbyists and occasional users, I see it as a perfectly valid workflow to collect some parts from external sources to cobble a project together, and just disable the ERC and DRC warnings for library parts.

But when you do some more projects, it becomes advantageous to do some library management too. You can create a library from all parts used in a project with:
Schematic Editor / File / Export / Symbols to New Library and with:
PCB Editor / File / Export / Footprints to New Library.

When you do this with footprints there are two extra steps:

1. During the export, KiCad asks whether you want to update the parts on the PCB to link to the new library. Answer with [Yes] to that question.
2. Use PCB Editor / Tools / Update Schematic from PCB to push the changes back to the schematic. (This is the other way around from the regular workflow). This updates the links in the schematic symbols to refer to your newly created footprint library and this is needed because the schematic symbols are the source of the whole design chain in KiCad.

[rvamerongen]

Thank you very much.

The points are great info.
Sometimes I search for something but don’t know or forgot the terms and then…. searching from one void into another void.