It almost feels like you want to turn a bicycle into a racing car by exchanging parts one by one. It can be done, but it’s not a very efficient method.
Similar with KiCad.
In KiCad the main reference is the schematic with it’s schematic symbols. If you want to change things, then do not delete a schematic symbol and place a new one. If you do that, then the link between the schematic symbol and the PCB gets broken. (But it can be repaired).
If you want to change a schematic symbol, then just select it, press e to edit it’s properties and use the Change Symbol button.
Alternatively, you can also use Schematic editor / Tools / Edit Symbol Library Links. Either method can be used to swap a single schematic symbol or groups of them, depending on how you use the dialogs.
Changing footprints is very similar. You can either edit the Footprint … link in the symbol properties, or use Schematic Editor / Tools / Edit Symbol fields. You can also use the Schematic Editor / Tools / Assign Footprints tool, and probably some more methods. After you’ve changed a footprint link in the schematic, you have to run Schematic Editor / Tools / Update PCB from Schematic [F8] again to push your changes to the PCB. You have to pay some attention to the dialog and make sure that Options / Replace footprints with those specified in the schematic is turned on.
The mapping between schematic pins and footprint pads is done directly with pin numbers in KiCad. It is a very simple and straight forward connection. Disadvantage is that different IC packages can have pins at different locations. Especially when you change from a DIP footprint to some small SMT variant, the pin numbering can be different. The normal way in KiCad to solve this is to have different schematic symbols for such parts (The ATMEGA328 is an example of such a part).
If you have such parts, then the smarter option may be to just delete the schematic symbol and place a new one. This will leave an “unused” footprint on the PCB, and the F8 process will add the new footprint also to the PCB. The “Unused” footprint has to be deleted manually. (If you leave it on the PCB, it will generate DRC violations, because it’s no longer part of the netlist)
It’s also possible to change footprints on the PCB, and then push those back to the schematic, but this answer is already long enough. (I also skipped over some other details).