i am new to KiCad and so I am currentliy familiarizing myself with KiCad. Basically, I get along pretty well with KiCad. Now I am stuck trying to update schematic symbols in the schematic editor which I have moved from one symbol libaray to another.
I create all my symbols / footprints in “quarantine” or “test” libraries. So I created a schematic symbol (MCP2551) in a library called “user_symbol_quarantine”. Afterwards I used the symbol in the schematic. Now someone else reviews the symbol / footprint created by me and corrects wrong things and when the review is done the symbol / footprint is moved by the other person into the specific library (user_symbol_ic …).
Now I am trying to update the symbol in the schematic editor but it seams not to work. I select “Update symbols matching library identifier: user_symbol_ic:MCP2551”. In the “user_symbol_ic” I can select MCP2551. But when press on “Update”. Nothing happens. No report.
You are misinterpreting the “update Symbols from Library” function.
Since KiCad V6 all schematic symbols are embedded in the schematic file itself, but they also have a link to the library where that symbol originated from. You can load the copy of a symbol that is in the schematic directly in the Schematic Symbol Editor by hovering over it and pressing [Ctrl + e], and changes you made are saved directy into the schematic.
The Update symbols from Libary reverts the changes you made to the copies in the schematic, and re-loads a fresh copy from the same library that the schematic symbol originally came from.
Thus, your schematic symbols keep linked to the same library with this method, and that is not your intention.
What you want is to change the links to the library for a schematic symbol. You can do that with: Schematic Editor / Tools / Edit Symbol Library Links
There is something extra you may not be aware of:
KiCad does not search for libraries, and to be able to use a new library, you have to add it to the library table first. You can do this with: Schematic Editor / Preferences / Manage Symbol Libraries.
Thank you for the detailed reply. After updating the link to the specific library I could reload the symbol including the changes made to the symbol in the library. So the process would be:
Create symbol in the Quarantine library
Use in schematic
Symbol and footprint are reviewed
Move footprint to specific “reviewed” library
update footprint link inside symbol with the symbol editor
move symbol to specific “reviewed” library
update symbol link inside schematic editor
reload updated symbol through the “update symbol from library”