PCB Design questions
Probably far from the only issues, but you don't have any supply bypass capacitors and your ground return path from the crystal loading caps to the MCU has a huge loop area.  Put a ground pour on the back side in the area of the oscillator components and MCU ground pins and some vias directly to it.

You may want to rethink that whole side power plane, and instead make most of it ground with a limited power pour capturing the things that needs that.  I'd often start by connecting the power with traces and then pouring a shape to replace them.

It also looks like you may have failed to connect all of the required supply and ground pins to the MCU.  You should probably put the PCB on hold for the moment and make sure the schematic has bypass capacitors and all required power, ground, and reference connections first.

You also seem to have failed to think about how you are going to get your firmware into this.  Even if you're expecting a vendor to program them in a fixture before soldering, having access for ISP will save you lots of frustration in practice.  And you should have a way to connect the UART pins for debug output.  You'll want a way to trigger the reset on pin 29 too, as it's needed both for ISP and to easily get into a serial bootloader.

In general, you should probably review the AVR Hardware Design Considerations Application Note (AVR042)