kicad-developers team mailing list archive

[jp charras <jp.charras@xxxxxxxxxx>]

Le 26/08/2015 06:32, Lachlan Audas a écrit :
> Hi, I have a strange problem,   I'm opening a Ealge 6.xx pcb,  saving it,
> then reading the net list from the matching convert eagle sch.
> 
> This works fine, most of the time, but on net list import it prefix's the
> net's with /  and some others is dose not.
> for  example:  the GND net will be split into two net's   GND    and
> /GND,    I can't see any reason for this. the flood fill
> will  keep the GND    while a PAD  GND net will  get  / added to it.   Some
> tracks will be split   SCC  and /SCC.
> 
> I can provided link to a examples if needed.
> 
> Has any one else seen this problem ?
> 
> 
> Lachlan

This is not strange.
Like in others EDA tools, labels can be local or global

"Global Labels" and names of invisible Power pins are global, and have
no prefix.

Other labels (label and hierarchical labels) are local and are prefixed
by their sheet path.

The full name of a local label is /<sheet path name>/label
to avoid names collision between sheets, especially inside a complex
hierarchy.

therefore /GND is the full name of the local label GND inside the root sheet
GND is a global label (name of a "Global Label" or a invisible Power
pin) and are 2 different nets.

An explicit connection should be made between a local label and a
"Global Label" if they belong to the same net.

Label are exactly like variables in C / C++:
they can be local or global exactly for the same reasons.

-- 
Jean-Pierre CHARRAS