--- In kicad-users@yahoogroups.com, jean-pierre charras - INPG <jean-
[EMAIL PROTECTED]> wrote:
> 1 - Verify in your schematic (not in libedit) the pin number (click
on a
> pin)
> A common mistake is a duplicate component in 2 different libs.
Eeschema
> takes the first (this is a feature: lib order is significant)
> Be absolutely sure eeschema (not libedit) see 1 and 2 (and not A
and B)
> as pin *numbers*
>
> 2 *DO NOT* use spaces in labels, values, references, component
names ...
> This is not a problem in eeschema, but a *lot* of netlist formats
do not
> accept spaces in names.
> I do not know the kicad version you are using.
> The last version replaces spaces in labels in pcbnew netlist, but
it is
> better to avoid spaces in names.
> See (with a text editor) the .net file to verify what is exactly
created.
Here's what is at the beginning of the netlist:
# EESchema Netlist Version 1.1 created 18/9/2008-13:06:32
(
( /48D25246 $noname C3 C {Lib=C}
( B ? )
( A ? )
)
( /48D25243 $noname R6 R {Lib=R}
( B VCC )
( A N-000004 )
)
( /48D25242 $noname R9 R {Lib=R}
( B GND )
( A N-000003 )
You can see why I'm confused. Both the C and R library symbols (which
use ~ for the pin names) show up as having A and B as the pin
numbers. Later in the same netlist my QFP package shows up normally
with pins starting with 1.
Once I checked the list of libraries, it was obvious why I sometimes
had the problem and sometimes didn't. The default location for
additional libraries was at the top of the list. As soon as I
put "device.lib" at the top, my problems went away. When I had added
additional libraries from various websites to the list, the problems
started.
Thanks for your help.
--CG
