KICAD questions

[makebit]

Hi,
Is there any way i can set up a project in KICAD and have a schem library and a footprint library in that project?
So that i can just copy paste it and send it to another computer to work on it there and still have the libraries available.
I wish the libraries to be "global".

I am making a library up at the moment, and i seem to be able to save symbols to it from a schematic, but i am not sure where this library is....i am able to save symbols to it.....but its strange because i dont know where this library actually is in my laptops folder structure.

In Altium, i had a project, and that project contained a schem lib and a footprint lib, but one doesnt seem to be able to set kicad up in this way?

[Benta]

KiCad later than V7 stores all used symbols and footprints within the project. You don't need the libraries.
Those can be transferred separately if you like.

[golden_labels]

All symbols are stored in the schematic file, which uses them. That is the file with “.kicad_sch” extension.
All footprints are stored in the PCB file, which uses them. That is the file with “.kicad_pcb” extension.

In addition to the above and independently of the project, any library file with custom symbols and footprints you created is stored where you created that library. Those are files with “.kicad_sym” and “.pretty” extensions.

[Doctorandus_P]

As has already been mentioned (twice), for KiCad V6 and newer all needed information is inside the schematic (and PCB file for footprints) and this makes it easy enough to move your project to another PC and work on it. But you are likely to get error messages about missing libraries on that other PC.

You also mention you do not know where the library is you created. You can see the full path to a library from: Preferences / Manage Symbol Libraries (Ditto for the footprint libraries). KiCad does not do any searching for library locations, so if you want to use a custom library on two PC's you have to copy the library itself to that other PC, and also add the library to the library table on that other PC. The library tables are in the sym-lib-table and fp-lib-table files. These files can be in your project (for the project specific libraries) or in your configuration directory (for global directories).

On Linux, the configuration directory is in: ~/.config/kicad/9.0 (Where 9.0 is the KiCad version you are using) The configuration directory holds a lot of personalized settings, and you can copy that whole directory to another PC, or use a source code merge program such as meldmerge to transfer only a few settings. If you plan on doing manual edits, I suggest you first make a backup copy of the whole directory. If you make a big mistake, you can also simply delete the whole configuration directory. If you start KiCad and there is no configuration directory for that specific KiCad version, then KiCad assumes it has just been installed, and it creates a configuration directory with defaults.

[ksjh]

Newer version of KiCad also allow to export all symbols used in a schematic into a new library and change the symbols in the schematic to reference the new library (File > Export > Symbols to New Library...). The footprints of a PCB layout can be exported and referenced the same way (File > Export > Footprints to New Library...). In both cases, you can specify the name and location of the new libraries.

UPDATE, forgot to mention: Once you have done both, you can use (Tools > Update Schematic from PCB...) in the Schmatic editor to update the association between the symbols and the footprints in the new footprint library.

[Doctorandus_P]

Newer version of KiCad also allow to export ...

Yes, that is also an option. If you want to go full circle then I recommend to to it in this order:

• In the PCB editor export the footprints.
• Accept it when KiCad suggests to update the library links of the used footprints.
• Use: PCB Editor / tools / Update schematic from PCB with the Footprint Assignments checkbox checked to get the changes back to the schematic editor.
• Export the schematic symbols to a new library.

[makebit]

Value field in kicad symbol
Thanks, also, if i have copied a kicad resistor into a library, and its value is say 100nF, but i want it to be blank so i can assign its value after i have put it in the schem...do i just call its value "~".

[tggzzz]

Caution.

It is believed that makebit==Treez/Faringdon/ocset/zenerbjt etc etc

[jkazda]

Hi, I'm new here and I have a question about VIA pads and alignment. When I select a pad from a footprint and try to align it with a VIA, the function behaves a bit strangely — it only moves the pad, not the entire footprint. Is this normal, or am I doing something wrong?
Normally, I use alignment between footprints and it works without any issues.

[Benta]

Please start a new thread instead of hijacking an existing one.

[golden_labels]

Blame OP for poorly naming the thread.

Now we’ll all be notified each time somebody thinks this is the place to ask KiCad questions.