Mail Archives: geda-user/2018/07/23/13:15:38
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 -