John, Well, thanks a lot, really. That is a very good suggestion, it makes a lot of sense. It still takes some redundant work, but it may not be as bad as renaming all of the parts' designators.
I'm trying it as of now, though it's taking time to match the parts and place them. I was about to annotate the schematics in increments of 100s like you did, but I didn't at the end... I should have. My parts are all numbered sequentially now. It sure would help a lot having all parts in the duplicated sections to be numbered with just an offset of 100, that way it would be a lot faster the matching of the parts in the layout. Next week I'll post a follow up on this.. see how it works. Thanks. David --- "John A. Ross [RSDTV]" <[EMAIL PROTECTED]> wrote: > > 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 > 200-299. > 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 > > John __________________________________ Do you Yahoo!? Yahoo! Mail SpamGuard - Read only the mail you want. http://antispam.yahoo.com/tools * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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/[EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *