Looks like a nice Layout to me!
Here are the first things i noticed:
(1) I really like how you put "GND-Vias" next to each signal via!
(2) I really like how clean your routing is! (Bottom Top-Down, Top Left-Rigth - old school)
(3) I really like how nicely/logically your parts are placed. A good layout starts and ends with good component placement!
(4) In my subjective sense, i can "see" that you put a lot of "pride" in this design! I like it!
What i would change:
(1) The main filter cap GND-connection is only with four little bridges. You can increase the width of these - your ESR at higher frequencys will greatly improve! Also, if the PCB is subject to vibration the capacitor will have a more "ridgid" solder pad. I would remove the thermal-pullback, as this cap wont tombstone
(2) I would give all my SMD-Pads a nice corner rounding. This greatly helps paste-release during production. I would round the IC pads a 100% and all other SMD pads like 25-50%
(3) I would increase my pad and drill diameter on all - especially the gnd - vias. There is more than enough board space available and the reliability of your PCB will increase - also, the cost can go down! I would do a 1mm/0.5mm via.
(4) I would add Layer-Markers into the Copper - not strictly necessary on a two layer board, but why not. This greatly helps service technicians.
(5) I would add some fiducials on the board. They maybe on your panel, but you have the space and this can increase production yield.
(6) I would round over the edges of the PCB chamfers - nicer handling, less burrs.
(7) I would move the tracks ( on both layers ) on the (top view) left and right side inwards a few mm. This makes it possible to put "mouse-bites" in a well-defined place. You can specify this to your board-house. If you need a "clean" edge, you can move these mousebits inward a little. Your assembly cost can decrease.
(8) I would move the bottom layer tracks on the upper edge (top view) somewhat in. This gives you more distance to the edge and this can increase your PCB yield.
(9) I would pullback the copper fills around 1mm from the PCB edge. Same reason as (8)
(10) I would not do "thermal relief" on the single GND pin in the bottom-left. If wave-soldered, there will be no issue. If hand soldered: It will take 1s longer - not big deal. But, your inductance will drop and your realiability (especially when often plugged/unplugged, or if done by a "200 pound gorilla") will increase.
Keep up the good work!