First, you have to have the footprints in KiCad format. There’s no way around that and you can’t make them easily from gerber data. So you must find, make or convert them from some recognizable format first.
You can export a copper or other layer from gerbview to a .kicad_pcb file (not to your actual project pcb file but an extra file). Probably you want copper layers and some guidance layer like silk or fab component outline layer, and edge cuts. Silk or fab layers shouldn’t be exported as that same layer but moved to an extra graphic layer.
In copper layers tracks are probably OK as they are, but zones aren’t, and pads can’t be used at all. Zones must be drawn from scratch and pads come from the footprints. Delete the zones from the exported file (open the .kicad_pcb file in pcbnew in standalone mode).
Update the PCB from the schematic so that you get all the footprints there.
Open pcbnew in standalone mode and open a .kicad_pcb file which has an previously exported layer. Copy the items in the layer. Switch to your project’s pcbnew and paste the data in a place where it doesn’t interfere with anything.
Using the pasted data as guidance create the board outline – or if the outline is now in Edge.Cuts layer use it as it is – and set the helper graphics layer to the correct location.
Place the footprints one by one, using the helper graphics as guidance.
Finally, when you move the tracks as a whole exactly to the right place, they magically receive the nets from the footprint pads.
This is how I remember it, it’s been a while since I did it.