These are .SVG files and unfortunately web browsers have been extremely slow in implementing that standard, and apparently also not much effort is put into web browsers (frameworks) to show them at different sizes etc. Quite a shame because I quite like the .SVG vector format. The schematic has āBoard1.svgā as filename. This is not a very meaningful filename.
For the schematic. I donāt like the blue boxes around all schematic sections. It does nothing what a bit of whitespace does not do and itās an extra bore to maintain them. Sometimes these can be useful to put a bit of emphasis onto something special, but not for all sections. I do like the use of titles above schematic sections, but normally draw them in a lot bigger font. Both to put more emphasis on the titles, and to make them readable when zoomed out.
The schematic symbols are also āweirdā at best. For most, they do follow common conventions (voltages top - down, and signals from left to right), but the wide bodies take up a lot of space. U16 also does not follow this convention. Putting pins in pin number order on the schematic is a bad practice. Schematic symbols should be designed to display itās function.
What does the ā/NOPBā mean in the schematic symbols? They appear to be part of the reason the schematic symbols are so big. Usually texts are placed just outside of the symbols, so the boxes can be made much smaller.
Why didnāt you just use KiCadās native symbols for the LM1117?
(Also see PCB remarks below).
![image](//kicad-info.s3.dualstack.us-west-2.amazonaws.com/original/3X/9/0/90d6e067532350079f644d3fdd57aba170552148.png)
700 Ohm (R21, R22, R23) in series with a power supply output?
There are also two sections that are implemented twice. KiCad has āhierarchical sheetsā for this. Basically you just draw such a circuit once in KiCad, and then include two copies of the sheet it is on. This makes maintenance easier, because with hierarchical sheets, the copies will always be the same. Even if you for example change a 5uF capacitor for a 4.7uF capacitor.
For the PCB. It only shows a single layer. I do see some test points, but no viaās.
Pin mapping to the SOT223 devices (LM1117) looks wrong. Pins 1 and 2 should not be shorted. You also used thermal reliefs for the big ātabā pins, while these are supposed to be soldered to some copper to act as a heatsink.
It looks like you put some effort in the PCB layout itself, but itās hard to see whether the decoupling capacitors are placed properly. Yellow text on red and white background is also hard to read, especially with the very thin and small texts. These texts also look too small to be readable as silk screen text.
How do you want to connect the outputs? Soldering wires to those small SMT pads is a nuisance.