I agree with the other answers here but just thought this may help:
I've drawn the 2 high current / high switch frequency loops of most concern in this design.
Green shows the input current loop with the C7/C18 decoupling caps sourcing most of the high frequency current needed. This loop is very large due to poor ground design.
Yellow shows the output current loop, it is also very large.
Perhaps most concerning is that the return currents from both the input and output to the regulator share a single ground return path through the narrow trace leaving C17.
Your ultimate goal here is to minimize the loop area of both of these loops. When doing so remember that high frequency currents, those which are the EMI concern, will follow the path of least inductance to ground, not the path of least resistance.
For example, I've drawn these paths a little wide for clarity but in reality the high frequency components of the ground return path for the output current (yellow) will try to travel directly under the input current path if it can. Its more likely to bend over under L2 on its way back.
EDIT: Update for full ground plane.
Here is an updated drawing of the current loops for your new layout:
This is much better, the ground returns are separated for clarity but the high frequency content will travel along the ground plane as close to directly under the power traces as it can. I added the feedback path in pink and lighter color denotes current traveling on the ground plane.
A few notes:
The paths are still much longer than they need to be. The feedback loop especially is quite long and will travel under the input current. This input is high impedance so any inductive coupling on this trace will have a relatively large impact on your regulation accuracy. You do cross at almost 90 degrees which reduces coupling but the ground currents do not and are an issue for other reasons (see below).
The input power trace crosses a split in the ground plane where the trace for the feedback loop runs. Never ever, ever, cross a split on a ground or power plane on an adjacent layer with a trace that has any chance of carrying high frequencies (which means any trace at all really). This creates a radiating loop as indicated by the light green return path. The end result is a large EMI problem.
I don't know if it is a result of the export to pdf or what but you seem to have lots of vias that will have clearance issues. They are too close together and too close to the component pads. Even with solder mask over the vias the solder mask clearance on the pads looks like it will expose some of the vias causing soldering issues if you use reflow. The vias near D1 for instance will almost certainly be exposed and when the board is reflowed the via will suck all the solder away from the pad leaving D1 either unsoldered or very poorly soldered.
Some vias also don't appear on both layers, such as those under U1.
What I would do:
Setup your PCB design software design rule checking with whatever clearances are required by your PCB fabricator. This will alert you to issues with via-via, via-pad and via-solder mask clearance issues.
Tear the design up and start fresh with component placement knowing that you now have a solid ground plane. Concentrate on minimizing the length of the critical paths and use as much copper as you can for these paths (bar the feedback loop, its low current). If space / layout allows, a ground pour on the surface isn't a bad idea, just make sure you can do it properly. (no orphaned copper, well coupled to the ground plane)
Edit 2:
Not sure if you have this already but here is the reference design / app notes from infineon for a 2 layer board using a solid ground plane on the bottom. They use a fairly long FB trace but keep it well clear of of the dangerous loops.
Much better than before. Perhaps a little overkill on the vias, particularly the vias on the pads for U1 and D2. My main concern is that the vias undeer U1 could suck all the solder away from the pad-- making the GND connection a little unreliable. But if the vias are filled in then that shouldn't be an issue. But in general, it is better to have too many vias than too little.
My only other criticism is the location of C3, and that trace that snakes under L2. L2 is going to put a lot of noise on that trace, which could mess things up. C3 should be placed between U1 and D2, and the traces should be really short-- or at least not routed under L2.
Best Answer
All that copper on the back side (the leftmost of your three pictures) is acting as a heat sink for the switching IC.
If you read the datasheets for this kind of IC, they'll often specify a certain area of copper to be connected to the ground (or possibly the input voltage) pin to give adequate heat dissipation.