X-Authentication-Warning:	delorie.com: mail set sender to geda-user-bounces using -f
Date:	Sat, 26 Jan 2013 14:28:42 -0500
Message-Id:	<201301261928.r0QJSg6W032060@envy.delorie.com>
From:	DJ Delorie <dj AT delorie DOT com>
To:	geda-user AT delorie DOT com
In-reply-to:	<51036C6D.8050808@innocent.com> (message from Gus Fantanas on
	Sat, 26 Jan 2013 00:41:01 -0500)
Subject:	Re: [geda-user] Still Struggling with PCB's Import Feature
References:	<51036C6D DOT 8050808 AT innocent DOT com>
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

Here's what's in one of my pcb files...

Attribute("import::src0" "os-power.sch")
Attribute("import::src1" "os-prog.sch")
Attribute("import::src2" "os-bus.sch")
Attribute("import::src3" "os-ethernet.sch")
Attribute("import::src4" "os-misc.sch")
Attribute("import::src5" "os-usb.sch")
Attribute("import::newX" "171250")
Attribute("import::newY" "54375")
Attribute("import::disperse" "0")

These are outside of any layer or element definition (i.e. they're
layout attributes, not layer attributes).  I use plain File->Import
with it, it pulls in files in the CWD.  (gnetlist is the default, if
you don't override it inside the *.pcb file)

   {"Import Schematics" Import() }

Hmmm... are you invoking pcb from a GUI menu system?  If so, I don't
know what the "current directory" will be for pcb, but the import
works from the current directory.

For gnetlist to work, you need to make sure the gafrc in the "current"
directory hs the paths to the symbols, and pcb's library path must be
correct (before imports, gsch2pcb had pcb's library paths in its
project files).  In my case, I have a file $HOME/.pcb/settings that
contains (among other things I added):

lib-newlib = /envy/dj/geda/gedasymbols/www/user/dj_delorie/footprints:footprints

The "footprints" at the end is "./footprints" in each project
directory, for project-local footprints.

- Raw text -