The nets VDD and VDDA are connected to each other by both L1 and by R6. Before you added R6 you even shorted L1. I usually put all those power supply caps in a row, that makes it easier to spot how the power is actually distributed.
I also like to draw schematics in a logical order. Currents and signals from west to east (normal reading direction) and voltages from top to bottom (which you've done).
For the power stuff, that would be: Start with the connector J1 on the left side, (and rotate that secton 90 degree CCW), then draw U1 (AMS1117) directly to it, and then put all the decoupling caps on it's 3V3 output.
This gives a logical flow of the whole power delivery system in a single overview, instead of spread around the schematic as it is now.
You've also drawn c1 as a ceramic (or at least unpolarized) 10u cap and C7 & C9 as polarized 100nF caps, while these probably are ceramic.
I do not like SW1 directly over C8. Ceramic capacitors can deliver very high peak currents, and this is of course through the switch when it is still bouncing. Small switches are rated for small currents, and this can and will destroy the switch over time. For a reset switch it's not such a biggie, but for switches that get pushed often (keyboards, mouse buttons) it is definitely a No-No.
I would add some (solder) jumper to the BOOT0 pin, so you have easy access to it on the PCB to put 3V3 on it if and when it's ever needed.
You can use the tacho output, but it will be gated with your PWM output, and therefore needs some finicky programming to get it to work.
But your uC has nothing else to do. But you have to connect the Tacho output to your uC (with suitable resistor divider) to do so of course.
The simplest way to measure RPM is to temporarily disable PWM (Turn the fan ON) and then measure the time between two rising (or falling) flanks of the tacho pin.
At least draw the resistors and wiring in the schematic and on the PCB, If you don't like it later, then you don't have to place the resistor divider.
The "Pin connected to some other pins but no pin to drive it" Is a thing that commonly confuses KiCad beginners.
Short answer: ERC in KiCad checks if the power inputs of IC's are connected to some power output, and if ERC can't find it, it emits that warning.
The warning can be suppressed by indicating that some nets really do have power applied by adding a "PWR_FLAG" symbol to a net.
I usually treat the "PWR_FLAG" symbols as power labels, and place them near the location where the power comes from (such as a connector).
ERC can not look "over" filter capacitors and inductors, so if there is such a component in between a power output (from the LM1117) and a power input, then the ERC warning is issued again.
More about this in the FAQ section of the KiCad users forum:
https://forum.kicad.info/search?q=Pin%20connected%20to%20some%20other%20pins%20but%20no%20pin%20to%20drive%20it%20category%3A19KiCad itself is getting improved at a faster rate then it's documentation is updated, and the FAQ section on the user forum has the most up-to-date info on many subjects.
I also want to suggest to try out your PWM amplifier on a breadboard.
It's quite easy to work with SOT-23 on a breadboard. Just snap of a 3 pin section of a male header and solder the SOT-23 to two of those pins, and add a short wire to the 3rd pin of the SOT-23.