The “name” is Reference, i.e. reference designator, by default it’s REF**. Just change it in the Properties of the placed footprint.
The nets can be managed in View → Panels → Net Inspector. On that, context menu → Add Net.
Updating the schematic from the PCB works if you already have the schematic and the symbols in it, and updating is limited in certain ways. KiCad can’t read your mind to know what symbol each footprint needs. In the normal workflow you add symbols first and define the footprints for them in the symbol properties. Then KiCad knows what footprints must be added to the board for each symbol. The same doesn’t work in the other way: you can’t add a symbol to a footprint.
So, you have two possibilities:
- After doing the PCB, add the corresponding symbols to the schematic and give them the correct reference designators. Then update the schematic from the PCB, using the option to use the reference designators:
Or
2. Because you are going to have the schematic anyway, why not to start with the schematic? You know all the components and what they are, so add the symbols to the schematic, choose the footprints for them in each symbol’s Properties and update the PCB normally from the schematic. If it’s easier to reverse engineer the connections in the PCB, continue by adding the nets and tracks in the PCB, then do the backannotation to the schematic, but without using the reference designators:
In any case KiCad can’t automatically draw wires in the schematic, but with backannotation you should be able to add the labels to symbols.
Here’s a very simple example where I added a symbol to the schematic, changed its reference designator (C1) according to the PCB where I had put the footprint with Reference C1, added a net and changed the net of both pins. After KiCad has updated the schematic there are the net labels in the pins. Now you can move the symbols (with the labels) and wire the schematic.
Probably the most important piece of knowledge you have missed is how the symbols and footprints are connected in KiCad, and you have also to understand that the pins must match between the symbol and the footprint. KiCad doesn’t have “parts” as some other EDAs have, it has loosely connected symbols and footprints.
Please see (Start Here) Frequently Asked Questions if the KiCad’s library system, i.e. connecting symbols with footprints, is still unclear to you.