Re: gEDA-user: Hierarchical Design

[Ales Hvezda <ahvezda@seul.org>]

Hi,

[snip]
>1. Upper level
>
>Create a symbol somewhere along the "component-library" search path, defined
>in gschemrc. The name of the symbol should be the same as the name of the
>lower level schematic, but with the extension "*.sym":

	The names actually no longer matter.  I need to update the doc which
states this.  


[snip]
>Attach the the following attributes to each pin of the symbol:
>
>pinlabel=<signal_name>, visible
>pinnumber=1, 2, IN, Out, ...;  comment only
>pinseq=1, 2. ...; invisible, comment only
>
>
>Place the symbol in the upper level schematic.


	Yes.   And, very importantly, you need to attach an attribute
called source=filename.sch to the placed symbol in the toplevel schematic.
This ties together the placed symbol to the underlying schematic.
You can test this by selecting the symbol and then picking "Hierarchy/Down
Schematic..." off of the menu.


[snip]
>Create a new schematic called <lower_level_schematic_name.sch>. This must
> be
>in the somewhere in the "source-library" search path defined in gschemrc.
>
>Example definition:
>
>(source-library ".")

	Yes.

>
>
>Use the symbol "in-1" or "out-1" form the library "IO", connect it to a n
>et.
>Change the value of the refdes attribute to <signal_name>. The signal nam
>e
>must be the same as the pinlable propertys on the previous crated symbol.


	Yes.

>
>
>Alternatively you can create your own symbol. The symbol needs one pin wi
>th
>the following attributes:
>
>refdes=<signal_name>; visible
>
>optional:
>device=input, output, ...; invisible.
>
>pin attributes:
>pinnumber=1; invisible
>pinseq=1; invisible

	Yes.


			-Ales