How can I find where on my hard drive the schematic symbol for U15 is located?
If I right click on U15 and go to edit properties is has in the “Library Symbol:” field “lightstorm_DAQ_A_ADC-SchDoc-rescue:ADA4807-1AKSZ-R2” which I guess means it is in the library “lightstorm_DAQ_A_ADC-SchDoc-rescue”. But how do I find where this library is located on my hard drive.
Also, I have a similar question about the imported PCB. I can right click on a footprint, go to footprint properties, but I don’t see which footprint library this was imported from and where on the disk it resides.
Kicad does not reference files directly for good reason. That would make your design impossible to share with anybody else.
Inside the schematic (and also pcb) a nickname is used to identify libraries. (typically this nickname is the same as the filename of the library.)
To find out where your files live use the library managers found in the preferences menus of eeschema and pcb_new.
The rescue lib is a special lib. It is created by kicad automatically inside the project directory. It is created if kicad can no longer find the symbol in any of its libraries. (Under normal circumstances) Before any symbol is moved to this lib you are asked in the so called rescue dialog if you want to do that.
In your case i suspect the rescue lib has been created by the tool you used to import the project from altium.
I went to footprint properties for one of the chips that were imported. I then clicked update footprints from library and it says “Update footprints with identifier: LFCSP_64_9x9mm”
So I assume that the name of this footprint is LFCSP_64_9x9mm.
Now, going to the library manager of PCB_NEW this is what I see.
I assume that LFCSP_64_9x9mm isn’t from the KiCAD built in libraries and that my Altium to KiCAD converter made it. Therefore I would think it lives in the myfootprint library which is in E:\KiCad\test\myfootprint.pretty
However, when I navigate to E:/KiCad/test/ I don’t see any folder named myfootprint.pretty.
Footprints are directly included in the pcb_new file header. The altium converter might therefore not even create a separate library. There is some way to get a library out of the pcb_new file. I can not check it now as i do not have access to kicad right now.
Yes. This also means that changing footprints inside the library does not change them in any pcb_new file. Updating footprints from the lib requires direct user action. (Via the update footprints tool in version 5. In version 4 this was done via the change footprints tool.)
This is one feature that is however missing from eeschema.
A valid schema should have all its symbols inside the so called cache lib. (So never ever delete or otherwise manually change this file! Consider it as part of the schematic.)
If something changes inside the library then kicad should ask you via the rescue dialog if you want to update the symbol inside the schematic (meaning copy the new symbol to the cache lib) or if you want to copy the original symbol from the cache into the rescue lib.
This whole process is however a bit error prone and buggy. (Not even the core devs trust it.) The hope is that version 6 will do away with this deficiency. (v6 is however still a few years into the future)
