I reordered your questions a bit ...
New Kicad user here... trying to play with this thing.
Questions:
This particular warning always comes up... on power lines, input and output lines. "pin connected to some other pins but no pin to drive it"
Now, for unused pins and input and output lines, I can put an "X" to it, to stop the warning. But what about on power lines? The PWR_FLAG? Why do I need to add another symbol to the power lines? What significance does this do? I may not be getting the big picture/philosophy behind Kicad yet.
Do I always have to attach a PWR_FLAG to my Vcc pins to avoid ERC warnings? The ERC on KiCad seems to be very whiny (compared to Eagle).
It depends. If the VCC pins on your ICs are connected to a net driven by a regulator's power OUTPUT pin, then no, you don't, because that regulator's pin is obviously the power net driver.
But if your power source is from an off-board thing through a connector, and the connector's "power" pin is declared as passive (which is common), then your ICs' power input pins have no power driver so you need to put the PWR_FLAG on that power net so the ERC "knows" that the net has a power driver.
The PWR_FLAG is separate from the usual power symbols in that its lone pin is declared as a power OUTPUT.
(Why do the other power symbols such as VCC have their pins declared as power INPUTs? Simple -- so you don't get the conflict of having a regulator OUTPUT pin connected to a power OUTPUT pin. The point of the power symbols is to make global nets with standard names.)
Another use case for the PWR_FLAG is if you've got a DC-DC converter on your board. The switcher chip doesn't have a power output pin, so no power net is defined by the chip. Instead, the power output is after a diode, perhaps. So whatever net you might consider the rail in that case needs to get a power flag attached to it. The ERC will be happy.
How do I name netnames in the schematic editor? in Eagle, I can name a wire GND, and that particular net will automatically be connected to GND/Gnd plane when I do a PCB design later on. Or I can name a wire "input", or "feedback" so later on during PCB design, I can see the wire's purpose. How do I do this in KiCad?
Look at the EESchema window. On the right-hand side you should see a vertical toolbar. One of the icons is the letter A above a green line. (Place your mouse cursor over it and read the tool tip.) That's the "place local net label" command. (This is different from the "place global net label" command, which is right below the local one.)
-a