X-Authentication-Warning:	delorie.com: mail set sender to geda-user-bounces using -f
X-Recipient:	geda-user AT delorie DOT com
X-Mailer:	exmh version 2.8.0 04/21/2012 (debian 1:2.8.0~rc1-2) with nmh-1.5
X-Exmh-Isig-CompType:	repl
X-Exmh-Isig-Folder:	inbox
From:	karl AT aspodata DOT se
To:	geda-user AT delorie DOT com
Subject:	Re: [geda-user] adding footprints and schematic symbols from CVS
In-reply-to:	<1386690289.1786.689.camel@benjamin-hp>
References:	<1386442454 DOT 1786 DOT 654 DOT camel AT benjamin-hp> <201312071920 DOT rB7JKCT0001853 AT envy DOT delorie DOT com> <20131210131002 DOT 68AAB80459E9 AT turkos DOT aspodata DOT se> <1386687407 DOT 1786 DOT 681 DOT camel AT benjamin-hp> <20131210151644 DOT E723380459E9 AT turkos DOT aspodata DOT se> <1386690289 DOT 1786 DOT 689 DOT camel AT benjamin-hp>
Comments:	In-reply-to "Benjamin L. Naber" <benjamin AT project23d DOT com>
	message dated "Tue, 10 Dec 2013 10:44:49 -0500."
Mime-Version:	1.0
Message-Id:	<20131210192927.C8A8C80459E9@turkos.aspodata.se>
Date:	Tue, 10 Dec 2013 20:29:25 +0100 (CET)
X-Virus-Scanned:	ClamAV using ClamSMTP
Reply-To:	geda-user AT delorie DOT com
Errors-To:	nobody AT delorie DOT com
X-Mailing-List:	geda-user AT delorie DOT com
X-Unsubscribes-To:	listserv AT delorie DOT com

Benjamin:
> This whole process of adding footprints is a real pain, and really
> shouldn't be that much effort involved to add a few or many symbols.

First, you have to realize that gschem and pcb are two different 
programs with separate heritage and history.
 The pcb program are using footprint files, and gschem are using
symbol files.
 To "complicate" things a little more, the pcb program exists in two
versions, a gtk and a lesstif version (I don't know much about the gtk 
version).

> First, how do I change the directory scan depth level?

pcb: coding (in c) or use external program (as I have shown).
gschem: coding in scheme (or ext. program)

> Second, there seems to be poor linking between PCB and gEDA schematic.

There is a weak linkage between the two programs via the gsch2pcb 
program, there is also the possibility to "Import Schematics" directly 
into the pcb program.

> I have used the gsch2pcb and specified some level of foot prints.
> 
> Is there a way, in order NOT to have both PCB and schematic open at the
> same time while drawing the schematic to enter in the component netlist
> and footprint into schematic?

You enter "symbol"s in gschem, you can add a footprint attribute to the
symbol, there is no chooser for that what I know about, you have to 
enter it more or less manually.
 To know what to write into the footprint attribute, it is convenient 
to have the pcb program running, but you can also use look at the file 
names on your disk.

> I've noticed that even after I enter all the necessary component data
> into sch, when using gsch2pcb, many of the components still do not
> populate on the PCB

I use the -d option to tell gsch2pcb where to find the footprints (BTW, 
gsch2pcb call the footprints "pcb file elements"). You can also specify 
it in a gsch2pcb project file.

So I call pcb (lesstif version) in this way:

 pcb  --lib-newlib .:/home/karl/git/openhw/share/pcb:/usr/local/share/pcb/pcblib-newlib:/usr/local/share/pcb/newlib:/home/karl/pcb_cvs_footprints file.pcb

and gsch2pcb in this way:

 gsch2pcb -d . -d /home/karl/git/openhw/share/pcb -d /usr/local/share/pcb/pcblib-newlib -d /usr/local/share/pcb/newlib -d /home/karl/pcb_cvs_footprints file.sch

and for gschem I have this in my .gEDA/gafrc:

(define home (getenv "HOME"))
(component-library-search "/Net/cvs/cvs.gedasymbols.org/www/user" "cvs")
(source-library    "${HOME}/git/openhw/share/gschem/include")
(component-library "${HOME}/git/openhw/share/gschem")

And, yes, it is a little messy.
Maybe someone else can point to a better solution.

Regards,
/Karl Hammar

-----------------------------------------------------------------------
Aspö Data
Lilla Aspö 148
S-742 94 Östhammar
Sweden
+46 173 140 57

- Raw text -