Hi, I designed a footprint for a display which shall be plugged on a board.
After placing this footprint to my board I added some labels (visible) in the footprint with the footprint editor and saved it.
In the footprint editor there is a function “insert footprint into actual board” which adds the new footprint to the layout. But I only want to update the footprint in my layout, not add an additional footprint.
I also reassigned the new footprint to the display symbol in the schematic and then in the layout editor clicked the function “transfer changes in the schematic to layout” (F8). But the new labels are not visible in my layout.
The only possible way seems to be delete the old footprint in the layout and after that add the new one from within footprint editor.
Layout editor???
and then in the layoutschematic editor clicked the function “transfer changes in the schematic to layout” (F8).
Do you mean “Update PCB from Schematic F8”?
F8 should work if you also remembered to press OK.
Also, hovering the mouse cursor above a footprint (or selecting it) in the PCB Editor and then pressing [Ctrl + e] loads that footprint directly in the footprint editor, and when you save it then in the footprint editor, it updates the used footprint on the PCB directly. You can also just close the footprint editor, and then KiCad asks you whether you want to update the footprint on the PCB.
Clicking F8 only offers"Update board" and “close window”, but there is no OK button.
I tried “Update board” several times without success.
Button “update footprint from library” within property window was successful.
It’s not possible to use the “Update PCB from Schematic” dialog to reload footprints from libraries. It can only change from one footprint to another, i.e. it changes the footprints when library IDs have been changed in the schematic.
Updating footprints which have been edited in the footprint libraries can be initiated from the Footprint properties dialog, or from Tools → Update Footprints from Library, or from the context menu on a footprint → Update Footprint. They all open the same dialog.
It’s unfortunate that the difference between updating the footprints re-assigned in the schematic and updating footprints on the board from their libraries is difficult to understand for those who don’t know it already, and it’s difficult to to find totally unambiguous and self-evident wording for it in English to be used in the UI, but IMO it has been made as clear as possible in the dialogs and UI strings. See Misleading "Update footprints" text in "Update PCB from Schematic" (lp:#1838551) (#3149) · Issues · KiCad / KiCad Source Code / kicad · GitLab if you are interested in details.