There are now the 3 normally required Power Flags.
I used the @Rene_Poschl 's test circuit because it was easy to use. In the circuit I was creating, instead of using Power Flags I used linear regulator circuits, similar to a LM7805 with the regulated pin set as Electrical Type “Output”. To remove the error in my circuit I had to duplicate the regulator and set it’s regulated pin to Electrical Type “Passive”.
I can not download the current version of KiCad until tomorrow so I can’t test to see if this still exists in V5.0.1 and I was unable to find anything when searching the bug tracker (but I seem to suck at searching it).
The regulator output is a power output, that’s why it’s marked power_out in the component.
For connectors, it is not immediately clear which connector will be used as a power supply, so the connector’s pins are marked passive to ignore the connector for ERC.
If your board is powered through a connector, this means that the power nets would not have a power_out pin on them, which ERC complains about. The fix for that is to place a PWR_FLAG, which behaves like a power_out pin, but doesn’t introduce a component.
This means that PWR_FLAG components are needed only when ERC cannot determine where power comes from, it means “a passive component is supplying power to this net”. If you have a regulator, it is fairly obvious that power comes from the regulator, and connecting another power source to the same net would be wrong. That is why you are getting an error when you connect a PWR_FLAG to a regulator output.
The reason that PWR_FLAGs should be put near to connectors (or rather, the place where the power comes in) is so you can get meaningful error reports on conflicts. In the error message you see, there are two PWR_FLAGs connected to each other, so you have two places where you claim power enters the net. Either that is wrong, and one of these places should not be marked, or you have accidentally connected two supply rails.
I spent way to much time chasing my tail around and around in circles on this problem that I have been having. Somewhere I must have overlooked a mistake as I did in fact attempt to troubleshoot this several different times.
What I also want to mention is that it appears some other legitimate bugs may well have added to the difficulty of working through the issues; as well as some functionality changes to KiCad as the constant development changes the program over time.
I did not know that all Power Symbols are Global. In fact, I (think that I) remember that there was a thread on this forum about Power Symbols really being no different than any other Eeschema library symbol. There was never any mention that the Power Symbols were Global.
Yet, I still want to ask the question, “Is it a bug that Power Symbols placed in hierarchical sheets are automatically assigned to be Global?” Because, I gotta say that, “if so, it’s going to make my printed schematics look goofy in comparison to what others would expect as normal”.
I got misdirected somewhere when trying to figure out what was wrong.
@GyrosGeier thanks for taking your time to help me sort out how I got so far off the planned course!
That last part of your post, with the last portion of it bolded above, was just what I needed to get back on track; you have saved me hours of my own time. Thanks!
