Voltage regulators.
Add 0.1 uF or 0.01 uF ceramic capacitors on the input of both +15v and -15v regulators.
Add a small electrolytic input capacitor on both +15v and -15v regulators ... small as in let's say 10..100uF, anything higher won't help more
No idea why you went with 2.2uF , it's a weird value and unnecessarily small.
Below some uF value all capacitors will have the same diameter and height, so you're not saving pcb space and you don't have to be exactly as the datasheet minimums recommend.
I'd suggest going with a value that you're gonna reuse in the circuit somewhere else... for example 22uF 35v rated electrolytic capacitors which you can use for the opamps as well.
I'd add output capacitors to both +15v and -15v regulators... again, don't understand why go with 100nF on one and 1uF on the other... I'd go with 10uF 25v electrolytic on both, or reuse 22uF 35v you already picked for the input and output and opamps.
I wouldn't use electrolytic capacitors with less than 10uF capacitance, and if I have to I'd use ones with high voltage rating, like 35v..50v, to get better specifications.
If the 5v regulator's gonna be physically very close to the 15v regulator output, then you don't need input capacitors for it, as the output capacitor of that regulator will provide the capacitance and the voltage should be smooth enough to not require decoupling capacitors.
The opamps ... the 22k resistors bother me a bit ... do you have to use 22k or could you maybe deal with 10k (in which case you could use 2 10k in series and simplify your bom by having only 10k resistors)
the actual layout ... i'd use thick traces for +25v and -25v and i'd route them horizontally to the left of the connector, and rotate by 90 degrees both regulators so if you wanted to you could place heatsinks on the edge of the board. Probably your board doesn't consume that much current, but never hurts to have the option.
The 5v regulator could fit between the +15v one and the input power connector which could be moved a bit to the right.
Then you'd have room to move up that mcp4231 and not have such long traces from the arduino to it.
I'D move the bass and treble headers to the left edge, like the out terminal, and maybe rotate 90 degree the opamps to have the traces go directly to it.
I see you have footprints for ceramic capacitors for 22uF ... I hope you're aware capacitance of ceramic caps varies with voltage and also that 22uF capacitors with high enough voltage rating will be expensive.
If you need the 22uF may be better to use electrolytic capacitors or maybe consider having 2-3 footprints for 10uF ceramics in parallel.
Rotate ir header and rotary header so they're on the edge
do something with the shift registers and the 7segment header ... move a bit to the right, rotate the shift registers, use resistor arrays if you have to or smaller footprint resistors