My first though is that it looks like you have a switching DCDC converter, not sure of the current/power requirements but if it was me I would try connect each component that is part of the power path with a thicker track or a plane like this:
Yes I thought that might come up. I'm just not quite sure how to do it in Altium other than by literally drawing the polygons, and I can see them ending up rather ugly :-)
I might have a go though.
It's an AP5724 DC to DC converter. http://www.internetsomething.com/lcd/AP5724%20backlight%20driver.pdf
There's 6 LEDs in series, at 20mA, 18v total, so 360mw total. They say the above driver chip is 84% efficient, so expected draw of 430mw. Call it 500mw. I'm not really sure I know enough about this stuff, but I gather it's current that matters. So the 500mw should pull 151mA from the 3.3v supply. I've used 10 mil traces which an online calculator says should be good for 450mA with 1oz copper. The LCD panel itself pulls 15mA. So I'm at about 165mA.
What do you think? I suppose it makes sense for me to learn how to do the job properly though doesn't it..
The way I see it if the LED's expect to consume 360mW and the converter is 84% efficient then this means 70mW will be dissipated as heat in the SOT23-6 package. Given that θJA is 162°C/W this means that IC will rise by ~11°C above ambient. Not that bad but for the sake of it I would still use a polygon to help dissipate the heat, and give the current a much less resistance pathway (lower ohmic loss, not that it matters that much with your current draw).
As for polygons you can either manually place them down and adjust as you go like:
Or you could use another layer (like MECH 1) to define the shape and then create a polygon on copper layer, like (Create Polygon from Selected Primitives): https://www.altium.com/documentation/15.1/display/ADES/PCB_Cmd-ConvertSelected((ConvertSelected))_AD
Also I think your latest iteration with polygons looks better, but there is still room for improvement. To get an idea of a good layout have a look at the appnote:
https://www.diodes.com/diodes-part-files/AC/AP5724/User%20Guides%20and%20EV%20Boards/AP5724-EVM.pdf
Notice how all components part of the power path (inductor, diode, filter caps, IC...) are all connected via a large polygon
The current paths in that SMPS look unnecessarily long. You want the high currents to have short, uninterrupted current paths from the input capacitors to the output capacitors.
You could improve this by rotating the inductor by 90° clockwise and move those input capacitors closer to the output caps. Also, fatten the traces up around the diode.
I think they mean trace area going into SW pin, if you have a look at reference design they still have a wide traces for all components it's only when they funnel into the IC that they become smaller (design constraint of pin positions).
Also Dave made a good point. Think of a transient happening on the Vout and suddenly you must supply additional current to get the voltage back up, how you have C4 positioned makes it harder for the circuit to respond faster.
If J1 is a single sided flex cable connector, the pins where you length equalize extended the traces may travel into the connector to the flex cable with a little more length inside the connector compared to the pins right under the connector. Have you taken this into account when extending those 2 traces to their length on the PCB?
I realise you now have your boards back (and they work! awesome! ) so it's probably a bit too late, but... why do you have thermal relief on your stitching vias?
That has worked out remarkably well for a first PCB. In the future I would suggest using thicker traces in the switching regulator area, and keeping everything as short as possible there but it seems it has worked out ok in this case.