Warning: symbol ‘GND’ has been modified in library ‘power’
KiCad has some issues with GND (all power) symbols. You should not modify them (as a beginner), but just use them as is. To be sure you use unmodified library symbols for GND, first edit the properties of one of your GND symbols, then use: [ Update Symbol from Library and update all onboard GND symbols from their library defaults.
Error: Symbol U5 has input power pins in units [Unit C] that are not placed
U5, an LM358 has three Units. Two of the units are the opamps themselves, and the third (Unit C) are the power pins. Make sure you place all units on your schematic, connect the power wires (and properly passivate unused opamps). You can change the “Unit” in the properties panel of anyone of the symbols on your schematic.
Error: Input Power pin not driven not driven by any Output Power pins
The net on the +28V power symbol needs a: PWR_FLAG symbol (See below).
You very likely need these PWR_FLAG symbols on most of the power nets. I usually put these power flags near the connectors where power enters the PCB. They allow ERC to verify that you IC’s are getting powered from “somewhere”. Voltage regulators most often have one of their pins set to a power output, and then that net does not need the PWR_FLAG symbol. The use of these PWR_FLAG symbols often leads to some confusion for beginners, and how to use them as been mentioned a lot on this forum. See for example: ErrType(3): Pin connected to some others pins but no pin to drive it