With KiCad you can back import Gerbers into Pcbnew, very easily, but it's far from perfect because simply a lot of the information is missing in the gerber files.
What you get is:
* Board outline,
* Placement of mounting holes.
* All the tracks on all the layers.
* SMD pads for all footprints (including original THT components).
* Placement of all the components, (Implicitly in pad locations and track ends).
* Netlist / sort of. (Read on).
As I said, far from perfect, but much better then nothing.
The second step is to remove the loose pads, and put real footprints from KiCad's library on the ends of the tracks.
This will of course generate lots of DRC errors, because there is no netlist to work with.
So the next step is to draw the schematic in Eeschema (Which you have to do anyway), and then, if you import the netlist into Pcbnew, the DRC errors will disappear , because the existing PCB layout coincides with the newly created netlist.
Realise that this is an iterative process, especially if you are a beginner with KiCad. So start with a small corner of the PCB untill you've figured out how to match loose footprints in PCBnew with schematic symbols.
From Eeschema -> Pcbnew it normally goes with timestamp values, which are useless to you. You need to select "update by Reference", which will match the RefDes (U12, R121, etc).
You also do not have to do the footprint assignment in Eeschema. You can export a Footprint Association File with the footprint info of the footprints you have selected in Pcbnew.