The main thing to keep in mind with the u.FL connector is to ensure a 50 ohm impedance on your RF feedline, and keep it as short as possible. Also most u.FL connectors have a center conductor that sits flush on the PCB but is not normally soldered. It just still carries the RF signal so it shouldn't be too close to GND, so ensure that the GND plane is removed under it on the top layer. I'd still recommend 4 layers with the u.FL connector since it helps you keep the RF trace width smaller. You also want to highlight your RF feedline for your board house and ask them to ensure 50 ohm impedance matching on it. The ground plane surrounding the RF feedline should be stitched down to the GND plane on layer 2 of your 4 layer board as well (it's likely going to tie into GND on the bottom layer as well).
If I had to guess just by looking at your board, I'd say you only have 6/6 mils of trace/clearance on the RF trace? If so that's less than half of what it should be for a 4 layer design (~13 mils trace with 7.5 mil clearance to GND depending on your board specs) and the requirements for 2 layer are even thicker traces with more clearance. Layer 2 is going to be GND, so it should also be about 7.5 mils away from the top layer.