[Author Prev][Author Next][Thread Prev][Thread Next][Author Index][Thread Index]

Re: gEDA-user: An opportunity to fix the symbol library

Karl Hammar wrote:

> I already have checked out cvs.gedasymbols.org, how do I integrate
> it withing gschem and pcb?

Let the config files point to where your preferred symbols and 
footprints are stored. Unfortunately, gschem does not descend
into subdirectories. So you have to give each and every dir in 
the config.

Snippet from my $HOME/.gEDA/gafrc: 
; Allow to source symbols from the local copy of geda-symbols
(define gedasymbols "/home/kmk/geda/gedasymbols/www/user/kai_martin_knaak/symbols")
(component-library (build-path gedasymbols "titleblock"))
(component-library (build-path gedasymbols "power"))
(component-library (build-path gedasymbols "misc"))
(component-library (build-path gedasymbols "digital"))
(component-library (build-path gedasymbols "connector"))
(component-library (build-path gedasymbols "block"))
(component-library (build-path gedasymbols "analog/diode"))
(component-library (build-path gedasymbols "analog"))

When searching for footprint files, gnetlist does descend into subdirs.
So you only need to give the path of the top dir of the footprints. 
For some reason xgsch2pcb does not read the footprint search path from 
gafrc files (maybe I did not understand how to set it up properly). I
tell it about my preferred footprints with an option in the project file.

A project file of mine looks like this: 
schematics pidpeltier.sch
output-name pidpeltier
elements-dir /home/kmk/geda/footprints

Note, that this still falls back to the default lib of footprints if
a search at the path given by elements-dir fails. I found no way to 
disable this potentially detrimental fall-back short of moving the 
default lib out of sight. Also note, that there can be only one 
elements-dir. (Please enlighten me, if there is a way to give more)

If you want to browse the local footprints in PCB, you can tell the 
GUI where to look for them. From $HOME/.pcb/preferences 
library-newlib = ~/geda/footprints:/usr/local/lib/luciani:./packages:.
The path ~/geda/footprints is a symlink to my section of the local 
gedasymbols repository. This search path can be set in the GUI of 
PCB in the preferences dialog.

I am not sure, where the import function of PCB can be configured. 
Last time I checked, it seemed to use the paths given in $HOME/.pcb/preferences
But schematic import did not play nice with hierarchical layout. 
So I still stick with gsch2pcb. 

Kai-Martin Knaak
Email: kmk@xxxxxxxxxxxxxxx
Ãffentlicher PGP-SchlÃssel:

geda-user mailing list