On 02:36 PM 12/11/2001 -0500, Sean James said:
>Has anybody out there ever have to upated a schematic's reference 
>designators based on a PCB layout, when there is NOT a netlist to back 
>annotate.

Yes.

>  I have to clean up an engineer's schematics, and he refuses to use an 
> inteligent schematic & layout. He just places the parts on the board and 
> wires them up.

Replace the engineer - I certainly do not accept any engineers work 
(including my own) that is this sloppy.  Engineering is a discipline not a 
place for artisan w*nkers.  The artisans may create good designs but can 
you produce, test and maintain them?  Especially when just a little more 
work would make it easy for someone else to come through and fix up the 
problems.  (This is similar to the difference between a talented software 
hacker and a software engineer - one may be very good at creating code but 
who do you want writing your automobile ABS software?)

Lloyd and Abd ul-Rahman's idea of putting responsibility for sign-off back 
where it belongs (the engineer) is very good, I think. But if the engineer 
involved is the boss then you are stuffed :-).  All you can do is document 
well the time spent so when the issue comes up, due to time to market lag 
or a parts ordering stuffup or whatever, you at least have some 
documentation.  Bum covering is not a good way to operate, I think, but I 
am fully aware that in situation like you could see the engineer may well 
have the bluster and the respect of those above to make your position 
difficult if there is a problem.  I have backed up techs and untrained 
people when engineering colleagues (and engineering managers) started to 
get bombastic and overbearing.

>Not only does this create a situation where I have to clean up the 
>schematics (Ref Des's; missing or incorrect parts; wrong connections, 
>etc.), it is also difficult and time cosuming to go back through the board 
>and assign our company's part numbers.

For cleaning up the layout of the sch - manual operation.  Protel Sch has 
very little in the way of Sch layout intelligence.  The rubber banding is 
poor as well so it can be a very slow operation if you have lots of clean 
up to do.  Even much cheaper packages have better rubber banding.  This has 
been a mark against Protel Sch for a long time, as has the issue of *not* 
merging co-linear line segments, which is something to be wary of when 
doing bulk neatening up.

For adding company info to the sch symbols you may find the spreadsheet 
format is useful as you can block copy similar info quickly and then update 
the Sch.  Use the Export-to-Spread process.  There are issues with how you 
manage the process - basically:
1) do not mess about with the hidden handles (column B, I think, that is 
hidden),
2) Keep the hidden handles sorted with the other columns, as they are the 
association back into the Sch (it is not by designator, which is very 
useful when you have bulk designator changes to do)
3) The hidden handles are not persistent so you must keep the Protel 
session open while doing the edits in the spreadsheet.
4) When you export from the Sch (or PCB) you can then select everything and 
paste into a more capable spreadsheet, do you edits, select all and paste 
back and then update - as long as you observe rule number 1.  (This allows 
you to run more elaborate macros.)

Maybe the database linking function would help as well - but it is reported 
as being deathly slow.

You say there is not a netlist.  Why is this?  You can generate the netlist 
from the PCB and then do a compare with the sch netlist. (as AL offered in 
his recipe).  As I understood it you have a Sch but it needs cleaning 
up.  is the Sch a paper copy of a Protel sch?  If you have a problem with 
the PCB and the Sch designators not matching, then I would get them 
matching using the spreadsheet option or simply double clicking each 
component, using the netlist compare as a help, and the synchronize to 
allow all the other info to be matched - but watch out during 
synchronization that you go the best way - if you got from Sch to PCB you 
will want to make sure that the PCB footprints are not updated.  Then once 
all the value info is correct in the PCB you can transfer the PCB 
footprints back into the Sch using the synch.

You may also find it helpful in doing Abd ul-Rahman's netlist matching to 
make as many multi-pinned components match as possible.  So all the 
manually match as many ICs and some of the R's and C's that are easy - as 
this will make the netlist matching much easier as many of the designators 
in each net will be correct.

Bye,
Ian Wilson

* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* 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