At 10:58 PM 3/20/2002 -0500, Bob Wolfe wrote:
> > The documentation on this could be improved, particularly because Sheet
> > Symbol/Sheet Entry is, in my opinion, the best for producing clear and
> > error-free multipage schematics, and this scope also makes design re-use
> > easier.
>I am also using this scope.
>The kicker is the Orcad schematic does produce a correct net list
>and is error free when checked so being that Protel chose to give the
>ability to import
>an OrCAD schematic you would think it would come in with at least proper
>seeing that the connectivity was there in OrCAD with no errors.

It would be extremely difficult to do this. OrCAD and Protel handle 
connectivity a little bit differently. So file import should be considered 
a rough tool, not producing, necessarily, a finished product. Especially if 
a design is not flat (i.e., essentially one large schematic sheet even if 
found on multiple pages), intersheet connectivity may require adjustments.

>Bottom line I need to ERC the design after it comes over.

Yes. Even then there can be problems.

There was a bug in OrCAD Capture v. 7, I don't know if they fixed it later, 
which could cause intersheet connectivity failure. OrCAD allowed net 
renaming. If you tied two nets together, one of the names would be used. It 
was not easy to predict which one. If net A was tied on one sheet to net B 
and on another sheet to net C, one might think that, with nets global 
connectivity, nets A and B and C would all be one big happy net. Not 
necessarily, if the net renaming did not produce a single net name for all 
three. Capture 7 apparently resolved renamed nets one sheet at a time 
instead of globally.

Protel does not so easily allow net renaming simply by tying named nets 
together. It is reported as an error; how it handles the situation I don't 
recall. One can rename nets across sheets by using ports only or sheet 
symbol/port connections, however, and it is precisely controlled, once one 
knows how to use it. It would still be useful to be able to sheetwise 
rename power nets where hidden pins are used. Tango Schematic allowed this 
by placing a short piece of wire on a power object, and placing a net label 
on that wire. I forget which way it went, but it was predictable, so one 
could, for example, rename GND to DGND for one sheet only, i.e., the hidden 
pins would be connected to the renamed net, not to their original native net.

Many of us consider hidden pin connectivity more trouble and danger than it 
is worth. My own opinion, however, is that with proper tools, it could 
still be useful without being dangerous. One tool would be a hidden pin 
connection report; another would be the ability to rename power pin nets. 
Protel presently makes them global always, as it does nets created by power 
objects. This can be a galling restriction, especially in a situation of 
design re-use.

What I would like to see would be a requirement that each sheet with hidden 
pins have some explicit and visible indication regarding the connectivity 
of these on that sheet. This could, at the same time, properly implemented, 
allow renaming of these power nets, such as renaming V+ to +12V.

However, the solution preferred by many of us is simply to make all power 
pins explicit. Power pins should never be hidden for single part symbols. 
When there is more than one part, it is best, in my opinion, if one is 
going to avoid hidden pins, to have a separate power part.

Protel does not have an unused part report, a major oversight. It is my 
opinion that all parts of multipart symbols should be placed; failure to 
place all parts should generate an ERC warning. This, of course, would make 
an unused part report redundant. But if one is going to allow unplaced 
parts, then it should be possible to designate a part as a power part; 
failure to place that part would definitely be an error, to be flagged as such.

Abdulrahman Lomax
Easthampton, Massachusetts USA

* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* To post a message: mailto:[EMAIL PROTECTED]
* To leave this list visit:
* Contact the list manager:
* Forum Guidelines Rules:
* Browse or Search previous postings:
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *

Reply via email to