> -----Original Message-----
> From: Dave C [mailto:[EMAIL PROTECTED] 
> Sent: Friday, February 20, 2004 5:18 PM
> To: Forum Protel EDA
> Subject: [PEDA] Complex Hierarchy to PCB layout ?
> Greetings Protel users,
> Scenario: 
>    Schematic design heavily based on complex hierarchy for 
> duplicating certain parts of the design. Sort of like a 
> stereo system with a left and right channel.
> After the design is flattened, every part gets it own 
> designator and it's ready for PCB layout.
> Can anyone suggest a method for replicating the PCB layout 
> (relative placement, tracks, vias, polygons,
> etc.) for these parts of the design which are identical 
> except for the designators and local net names ? 
> I know I can select, copy and paste part the layout.
> The copy will have incremented designators (default), or it 
> may have duplicate designators too. But how can I synchronize 
> this PCB layout copy to the duplicated schematic (say, the 
> left channel) without having to manually rename the 
> designators, which is prone to errors.


This is definitely a case where DXP would save you tons of time (do not
believe I said that, but its true).

Anyhow you can achieve what you want in 99SE but it is a very complex
process and nearly every stage is error prone as you already realise.

In some cases I have done it this way

I made a single channel sheet called AOL.SCH, annotated it with range
100-199. So I have my first channel.
AOL.SCH was then copied and renamed to AOR.SCH. 
The component designators on AOR.SCH were then reset (current sheet only) so
as not to conflict with AOL.SCH
Set the project options for re-annotation so that AOR.SCH is assigned CREFs
Now both channels are in. 
Update your PCB using the synchroniser so component classes are created.
Within the PCB Editor, place each channel in its own room. 
Place & route the first channel AOL.SCH, use a sensible grid and when you
are finished routing you can look to AOR.SCH channel
Move the matching components from channel AOR.SCH (unrouted channel) into
the same location in the room for AOL.SCH (routed channel)
You will get clearance errors but ignore them for now. 
Once all placement is complete you have 2 identical placed component
channels but only one is routed.
At this point make sure there are no active selections by using De-Select
ALL command.
Under Browse PCB panel bring up the component class generated by the
synchroniser for AOR.SCH and click select.
With the AOR.SCH channel parts now selected, move the component group to the
desired location for channel AOR.SCH
Now you have two placed channels that are identical but only one routed.
At this point make sure there are no active selections by using De-Select
ALL command.
Now for the routing, now select all objects within the AOL.SCH area, routes,
parts and all.
Under Browse PCB panel bring up the component class generated by the
synchroniser for AOL.SCH and click select. This will de-select the parts
within the AOL.SCH group but will leave all routing objects selected.
Now use the edit>copy command and select a suitable focus point for the
cut/paste operation that now needs done (always found a component pad was
best to 'snap to'), click on the focus point.
Now use the edit>paste command and click on the identical location point on
the AOR.SCH channel, all routes should now be copied in the exact same place
on the second channel.
As pasted primitives have their net assignments stripped automatically, the
pasted objects should automatically inherit the net names associated to the
component pads on which they are pasted to. If not you can always update
free primitives from component pads.
Pasting of routing objects only works if no routing objects exist in the
paste area already (like polygons and so on)

It's a lot of work, DXP takes care of most of this duplication work for you.

Good luck


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

Reply via email to