delorie.com/archives/browse.cgi   search  
Mail Archives: geda-user/2018/07/23/13:15:38

X-Authentication-Warning: delorie.com: mail set sender to geda-user-bounces using -f
X-Recipient: geda-user AT delorie DOT com
Date: Mon, 23 Jul 2018 19:14:13 +0200 (CEST)
From: Roland Lutz <rlutz AT hedmen DOT org>
To: "Luis de Arquer (ldearquer AT gmail DOT com) [via geda-user AT delorie DOT com]" <geda-user AT delorie DOT com>
Subject: Re: [geda-user] gschem multiple pages
In-Reply-To: <CAGqyy=bsRdbA8r8q1MTX7pG9ASZiqpsw1-kbj=geTwLoWaz1sA@mail.gmail.com>
Message-ID: <alpine.DEB.2.20.1807231835450.1641@nimbus>
References: <CAGqyy=bsRdbA8r8q1MTX7pG9ASZiqpsw1-kbj=geTwLoWaz1sA AT mail DOT gmail DOT com>
User-Agent: Alpine 2.20 (DEB 67 2015-01-07)
MIME-Version: 1.0
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

On Mon, 23 Jul 2018, Luis de Arquer (ldearquer AT gmail DOT com) [via 
geda-user AT delorie DOT com] wrote:
> I have an schematic split in 6 pages, but I am unable to tell gschem the 
> pages are related.

gEDA/gaf doesn't have a concept of top-level schematic files "belonging 
together".  When you create a netlist, all file names given on the command 
line are treated as top-level schematics.  The same applies when invoking 
gschem: all file names given on the command line will be loaded as 
top-level schematics.  (You may want to create an alias, script, or 
shortcut for convenience.)


On Mon, 23 Jul 2018, Nicklas Karlsson (nicklas DOT karlsson17 AT gmail DOT com) [via 
geda-user AT delorie DOT com] wrote:
> You add the source=filename.sch attribute to any symbol. Then you could 
> traverse the hierachy with "Hd" or right click and chose "Down 
> schematic".

This is a different mechanism: hierarchical schematics.  If the toplevel 
schematic(s) contain components on which the source= attribute is set, 
these are treated as subschematics.

This is explained here: http://wiki.geda-project.org/geda:hierarchy


On Mon, 23 Jul 2018, karl AT aspodata DOT se wrote:
> the page manager just lists one file at the startup, I have to go down 
> to all subpages for it to list them. Is that what it is supposed to 
> work, isn't there a "scan hierarchy" so that all pages show up in the 
> page manager without me actually traversing the whole the hierarchy ?

AFAICT, the purpose of the page manager is to track the files which you 
have visited and their relation to each other, not to represent a 
"complete" hierarchy.  This concept is hard to define: for example, if a 
file is referenced as a subschematic by multiple pages, where should it be 
placed in the page manager?

> How to you do that, or are you just using a "cable" top page referencing 
> actual "board" subpages ?

There are multiple ways to represent connections between pages.  In the 
simplest case, you could disable netname=/net= mangling and draw a purely 
human-readable "overview page".  All nets called "foo" on all pages will 
connect to each other, so you can use netname= attributes either on the 
net objects itself or on special symbols ("power symbols", a somewhat 
unfortunate name because these are not limited to power nets).  You can 
either specify the individual schematic pages as top-level pages on the 
command line, or use hierarchy and specify them via pin-less subschematic 
symbols on the overview page.

If you want to have separate net namespaces for the individual pages and 
require the connections between them to be explicit, you can enable 
netname=/net= mangling and use subschematic symbols with pins.

- Raw text -


  webmaster     delorie software   privacy  
  Copyright © 2019   by DJ Delorie     Updated Jul 2019