← Back to team overview

kicad-developers team mailing list archive

Re: Re: Pwr flag questionable behavior


Dick H. a écrit :
If I change the single pin name and number in the given GND_EARTH
library component from GND to EGND, then the problem goes away.
This I think is a bug.

Not a bug.

Only the pin name is used.
Invisible pins which have the Power In or Power Out electrical caract. are automatically connected. Because your GND_EARTH symbol has a pin named GND, this pin is connected to the GND net. For connection, the name of the symbol is not used (From this point of view, if is only a comment).

A GND_EARTH symbol must be build with a single pin named GND_EARTH. (See Eeschema doc, chapter 10.8)

In order to avoid problems, the flag "Power Symbol" must be set (In libedit, Part Properties).
When this flag is set:
- One cannot edit the symbol name in eeschema.
- The symbol is automatically reannotated when an ERC or a netliste is made.

You can easily create power symbols with the shape you like, because it is a component, like others components.
You cannot create a new power symbol only by editing its name: you must create a new symbol (i.e. a new component), with the shape you want, an a pin which have the same name as the symbol name.

I do not know if advantage is bigger than drawback or drawback is bigger than advantage.
It is only the choice I made for eeschema

JP Charras

Follow ups