kicad-developers team mailing list archive

[jean-pierre charras <jean-pierre.charras@...>]

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.

Advantage:
You can easily create power symbols with the shape you like, because it 
is a component, like others components.
Drawback:
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