I come from a different angle. I generally want to move as much responsibility from the circuit designer to the library maintainers. So if the datasheet says two pads must be connected then ensuring this in the symbol makes perfect sense to me. In the current stable version of kicad the only option available is to stack such pins.
It is also the only option to use doubled up output pins with ERC working. If you do not stack them then you have two options
- Have both pins set to output which will result in a false positive ERC message
- Have only one of them set to output which means ERC can not protect you against wrongly connecting the second pin (you get a false negative here)
And from my general philosophy of reducing responsibility i argue working ERC has a high priority so at least for output pins i am forced to use stacked pins.
However, pin stacking is a workaround that is definitely missing some features. For a start it is not easy to see which pins are part of a stack just from the schematic alone (one really needs to have access to the board view in parallel) — I would hope that some future version of kicad will have a better option here (i have not played with current nightly enough to say if there is already something available)
I always use the schematic/pcb cross highlight feature to find pins on the board for debugging so i never missed seeing what pins are part of a stack. Of course if one relies on printouts for debugging then this is a different story. I am not really tempted to use printouts as making a printable design is just too restricting to me (for starters using hierarchical design is not really an option for printable designs – at least not for deep hierarchies like i typically design)
KiCad for legacy reasons uses invisible power input pins as global labels. This allows having power symbols defined without a special pin type and also enforce that any net with a power symbol needs to be driven.
The logic symbols are made with such invisible power input pins also for legacy reasons. In the past when a PCB was a collection of a huge number of logic chips one typically had a single power supply line for all of them which made it seem sensible to have the symbols made such that they automatically connect to power.
However, times have changed. A lot of currently designed boards have multiple power supply systems. This is sadly not supported with the old symbols. Additionally, it is quite hard to convey which decoupling cap should belong to a given IC (and as soon as you place it nearby the IC you already loose the benefits of having the power pins hidden).
Further reading Electrical type of schematic symbol pins (KiCad 4 and KiCad 5) and the power symbol section of Tutorial: How to make a symbol (KiCad v5.1.x) and a very old tutorial (from version 4 times) of how to convert a symbol from hidden power input pins over to having a separate unit for them IC footprint VCC+GND (The symbol editor is now a bit different but the general process is the same)