SMPS PCB Design Critic 3
The fill areas seem overdone, especially where they fill way out into empty space that's far away from components rather than flowing between components, like at the corners of the board.  I'd put more gap between small traces and large fills since there seems to be room for it - you don't want high-current fills right up against signal traces.  I would not put fill around those standoff holes (TLP1 hole 1), at least not so close, since a wobbly or over-large standoff could scrape away the mask and short to the fill.  Also for EMI you probably don't want a hole in a high-current fill, as those standoffs make.  You've got some thin trace on TLP1 Q1, I'd push the fill below down towards C7/C18 and widen that trace a bit.  You don't want ground running under L3 since you can pick up ground bounce that way.

The component pads need the fill to enter from only one side or otherwise have some thermal separation from the fill, otherwise the component may be hard to solder, as heat will flow away from the pad too quickly compared to small pads and the solder paste won't melt evenly.  Similarly you may want the vias just a little farther from the pad on C14, C20, C21 as they will conduct some heat away to the other plane.  

Don't know if you've considered height and how things are spaced for hand-done rework as you're debugging.  I'd put L3 on TLP2 a little farther out from D3 or L3 will be pretty hard to hand solder without removing D3 first.  If you can't fit a soldering iron tip between two large components they're too close together (if you have room to move them a bit, or can rotate one).  I'd bring the connections to U2 pins 1/2/7/8 out a little like traces and then connect them together, instead of filling them side to side, because if you have to hand cut a trace or something it will be easier.  Just some ideas from a brief look - I haven't considered component placement.