Building library for an import project

[Kickadjob]

Hello Kicad experts!

I imported a complete schematic from Altium and downloaded the footprints of all the components from multiple websites and its not clear how to create a library for the whole project and assign each component a foot prin from the downloaded files.

Is this possible? Or its just possible to import a one by one?

Thank you!

[craftyjon]

@Kickadjob

how to create a library for the whole project

File > Export > Symbols to New Library (for the imported schematic)

@Kickadjob

assign each component a foot prin from the downloaded files

Create a new footprint library in the footprint library editor. Import each downloaded file into this library. Then go over to the schematic editor, and use the Assign Footprints tool to go through and map the footprints onto the symbols (alternatively, open up the symbol library you created earlier, go through and assign the footprints at the library level, and then do Update Symbols from Library. This method will mean that you can place new copies of the symbols in the library and they will automatically have the right footprints assigned).

[paulvdh]

craftyjon 's method seems a bit complicated.
Edit, oops. I interpreted it as importing a whole project (schematic + PCB), and indeed, if you only imported a schematic, my method below does not make much sense.

I suggest you start from the other end:

1. PCB Editor / Export / Footprints to new library.
2. At some point, KiCad asks you whether to update the links in the PCB editor to link to the new library. Answer that question with Yes.
3. PCB Editor / Tools / Update Schematic from PCB Editor This is the other way around from the normal workflow, and it pushes the changed footprint links back to the schematic. The Schematic is always the “first” reference for anything in KiCad.
4. Schematic Editor / Export / Symbols to New Library. Do this after the links from the PCB editor have been pushed to the schematic. This way the schematic library directly has links to the new footprint library.

But also consider that these steps are not absolutely necessary. Both the schematic and the PCB files have local copies of the used symbols and footprints inside their files. It does make the project more robust though. If you do not do this, and then attempt to update symbols or footprints from libraries, KiCad probably does nothing for parts it can not find, but it may update things to who knows what if those links point to “somewhere”.

[craftyjon]

@paulvdh

@craftyjon 's method is a bit complicated.

What about it is complicated? But, OP said they only imported a schematic. Your suggestion doesn’t make sense in that light.

[paulvdh]

@craftyjon

But, OP said they only imported a schematic.

Oops I missed that.

If only a schematic is imported, I usually start with a cleanup step. replace the resistors and capacitors with KiCad’s default symbols, maybe more, depending on how well it has been drawn.

Footprint libraries are pretty simple in KiCad. It is just a directory, but you have to add it to: Project Manager / Preferences / Manage Footprint Libraries. After that you can simply copy footprint files into that directory. I don’t know if KiCad has a “file watcher” on such files, so it’s safest to close KiCad before you start dumping footprint files into that library / directory / folder.