I agree.
This is the only way I've ever the got the whole Complex Hierarchy thing
working.
Perhaps other readers have had better luck, or understand better about how
to do it.

Damon Kelly
Hardware Engineer


> -----Original Message-----
> From: Bevan Weiss [mailto:[EMAIL PROTECTED]]
> Sent: Tuesday, 24 September 2002 17:14
> To: Protel EDA Forum
> Subject: Re: [PEDA] BOM and complex heirachies
> 
> 
> I thought that the whole idea of having complex hierarchies 
> was to allow
> multiple instances of the same sheet, without having to go to 
> some kind of
> hack like actual document shortcuts...
> I imagine that the multiple instances of the schematic sheet that I've
> created aren't going through to the PCB (netlist) file 
> either... Though I
> haven't confirmed this...
> I'll do it now...
> Don't ya just hate it when you're right about something like this...
> Only 1 listing of components are included in the netlist file.
> So what use is the complex heirarchy??
> Surely if you've only got a single instance of each schematic 
> document, then
> that's just a simple heirarchy and hence no need to convert 
> complex->simple.
> Thus, what exactly does complex->simple do??
> It would seem nothing...
> 
> ----- Original Message -----
> From: "Damon Kelly" <[EMAIL PROTECTED]>
> To: "Protel EDA Forum" <[EMAIL PROTECTED]>
> Sent: Tuesday, September 24, 2002 6:35 PM
> Subject: Re: [PEDA] BOM and complex heirachies
> 
> 
> > The steps that I use for the Complex Hierarchy and Complex-->Simple
> > transformation are:
> >
> > Create "top" level, and _all_ lower sheets as sheet 
> symbols. Identify each
> > sheet symbol as "Channel n", with file name "Channel n.sch" etc...
> > Create one real "master" sheet for the multi-channel sheets 
> (eg. "Channel
> > 1.sch").
> > From the "Documents" folder, use "Copy" then "Paste 
> Shortcut" to create as
> > many shortcuts of this master channel as needed, and rename 
> them "Channel
> > 2.sch", Channel 3.sch" etc...
> > Press F5 in the Explorer panel to rebuild, and you should see the
> Shortcuts
> > (Ch. 2 etc...) fall into place in the hierarchy.
> > Work on master channel only (i.e. Channel 1, the only "real" sheet).
> > When satisfied, run Complex-->Simple. This will replace 
> your shortcuts
> with
> > real sheets.
> >
> > ==> note that there seems to be a bug in the Explorer 
> display such that
> the
> > Shortcut symbol (the little arrow) is not removed until you 
> close the DDB
> > and re-open. Then you should see all the sheets Channel 1, Channel 2
> etc...
> > as real sheets.
> >
> > Re-annotate.
> >
> > BOM should then find all sheets.
> >
> > The crucial parts are that you need "shortcuts" of all 
> sub-sheets (that
> are
> > supposed to be copies of the master channel), and you use 
> Complex-->Simple
> > to convert these to real sheets.
> >
> > Another tip is to keep a copy of the shortcuts (in a sub 
> folder), so that
> if
> > you have to edit the master (and go through the whole 
> Complex-->Simple
> > process), you just copy the shortcuts over the top of the 
> other channel
> > files.
> >
> > Hope that helps!
> >
> >
> > Damon Kelly
> > Hardware Engineer
> >
> >
> > > -----Original Message-----
> > > From: Bevan Weiss [mailto:[EMAIL PROTECTED]]
> > > Sent: Tuesday, 24 September 2002 11:59
> > > To: Protel EDA Forum
> > > Subject: [PEDA] BOM and complex heirachies
> > >
> > >
> > > Hi,
> > > another question.
> > >
> > > When performing a BOM on a complex heirachy schematic layout,
> > > I don't seem
> > > to get components called out right... It's always deficient.
> > > with two sheet symbols (with the same schematic), and a
> > > holding schematic
> > > ie total.sch    ->    audio.sch
> > >                     ->    audio.sch
> > >
> > > I only seem to get the parts for audio.sch reported once, not
> > > the two times
> > > I woudl expect.  This is even after doing a complex to simple
> > > (which doesn't
> > > seem to change anything that I notice).
> > >
> > > Any help?
> > >
> >
> 

* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* To post a message: mailto:[EMAIL PROTECTED]
*
* To leave this list visit:
* http://www.techservinc.com/protelusers/leave.html
*
* Contact the list manager:
* mailto:[EMAIL PROTECTED]
*
* Forum Guidelines Rules:
* http://www.techservinc.com/protelusers/forumrules.html
*
* Browse or Search previous postings:
* http://www.mail-archive.com/proteledaforum@techservinc.com
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *

Reply via email to