Overriding a netname with the pinname is (was) a feature of power symbols.
But normally for this feature the symbol must be specifically defined as power symbol (in the symbol editor).
Just looked into this issue and it seems that alone the definition of a pin as Power Input already is enough to override the netname:
pin as invisible
pin as power input
symbol not as power symbol
→ net already takes the pinname
This looks like a bug - could someone give a second (third) opinion?
I’m not using V9 yet.
But if pin being PowerInput is enough to overwrite net name it have to be a bug, or there is may be some new conception and may be for example IC supply pins no longer are expected to be PowerInput.
Some microcontrolers have separate pins for Analog supply, Internal Digital Supply, Digital I/O buf supply.
I give each of them another name but in most cases connect all them together.
I see in V9 it will be generating by default Warnings.
I have checked - in my digital 1G 2G symbols I used Passive as supply pins. I sometimes supply CMOS gates from uC output pin.
I have now looked into the documentation and into older kicad evrsions as well and the behaviour is correct and follows the manual:
hidden power input pins implicitly define the netname. The flag “power symbol” is not relevant for this behaviour. (manual section " Hidden Power Pins").
The hidden power input pin = global is the legacy behavior, it always has existed specifically to support these specific symbols. I agree that it is not optimal though.
As I understand from this thread it is not new ‘feature’ and it was also in previous versions.
I don’t run ERC so I don’t care about any warnings there.
But I have never (since V4.0.7) noticed anything unusual with power net names. In ICs I’m using Power Input pins with many different names. For example my EFM32GG128B410F1024GQ64 has Power Input pins: “AV”, “IV”, “DV”, “VB”, “G”. But at PCB I see VCC and GND.
Isn’t it so that name of Power Input pin of Power symbol has precedence over name of Power Input pin from symbol being not Power symbol.
If it were such than it would explain why I didn’t noticed any problem ever.
I started with KiCad in a similar version and I also never noticed this. Until I started making custom symbols with stacked pins. This only happens if you set it to invisible and a power pin
Our standard (before EMC our PCBs were designed by someone else) was to have GND pins at symbol bottom, VCC at top and I/O ports distributed at both sides. As practically I connect all I/O pins to bus then bus were going under symbol from one side to the other.
Additionally placing capacitors at top was not so easy.
Recently I was drawing some symbols for not very lot pin microcontrollers and I decided to have top and bottom free from pins. I/O at right, supply, reset, XTAL on the left. VCC pins with some distance between them so capacitors can be one to one.