At 11:44 AM 12/28/2001 +1100, Thomas wrote:
>Someone recently posted a question to this list, asking weather a schematic
>should represent the electrical or physical layout, I was of the firm
>opinion - electrical, now I'm not so sure.

A schematic is intended to represent the electrical layout of a single 
subassembly. The project in question involves two subassemblies, so it is 
not an exception. Each PCB should have its own schematic, *that* schematic 
is a representation of the "electrical layout" of that PCB.

One might possibly want to represent a higher-level assembly with a single 
schematic on a single sheet, but this is not useful for design of the 
individual subassemblies; further, a prime use of a schematic is for field 
service or other technical work with the PCB, and the technician will want 
to know the circuit partitioning. I don't recommend it.

>So, do I scrap the easy to interpret logical electrical layout in favour of
>a physical one?

The "easy to interpret" quality of the integrated schematic is illusory. It 
is easy to interpret for the purpose of understanding the assembly 
function, but not for understanding the function of each individual PCB and 
for identifying which specific components are involved.

Normally, if your partitioning of the circuitry into the two PCBs is 
rational (typically one minimizes interconnects, and/or functional blocks 
are grouped to minimize noise and other signal integrity problems), each 
schematic will make sense by itself, especially if the interconnecting 
signals are given functional names.

However, it is possible to have it both ways.

>I'm still not sure. They both have their merits. Electrical layout with
>annotations pointing to the physical layout is the easiest to use when
>trying to understand the design, but physical layout would be easier to
>generate the netlists for layout and thus manufacturing.

Remember, the annotations would be a chore to create and a nightmare to 
maintain, plus netlisting would require additional time-consuming work. And 
the result will not be any more useful, even for the purpose of 
transmitting understanding of the design, than another approach.

>I'm having another look at the design to see If I can come to a better
>compromise, perhaps by adding another sheet, for the distributed display
>components, but then how do I represent this on the master sheet (if I stay
>with schematic = electrical design) if the master sheet is only to be used
>for generating the netlst for the other ccts? A rectangle object instead of
>a sheet symbol for the display cct perhaps?

First of all, if you use port only connectivity, the master sheet only 
calls out the two subsheets, it would not actually implement the 
connections. Its only function, really, would be to tell the netlister to 
look at both subsheets. In fact, the project sheet is not really necessary 
at all, since one of the subsheets could contain the reference (sheet 
symbol) to the other subsheet. One would use "ports only" to make sheet 
interconnection completely clear. But, in fact, the only purpose of the 
ports is to cause the creation of a complete netlist for the combination of 
the two sheets, which can be compared with the original project to make 
sure that every connection is the same.

Once the new set of schematics matches the original single schematic, the 
ports would be replaced with connectors. I'd put net labels on the 
connector pins. (Using net labels and ports global later one would still 
produce a complete net list.) The reference to the second sheet from the 
first could also be deleted, at least for the purpose of generating a net 
list from the first sheet alone. Yes, replacing that sheet symbol with a 
rectangle and perhaps arranging the connectors around that rectangle might 
make things easier for a technician later on.

>What I would really like is to be able to select a list of sheets to be
>netlisted instead of all or only one. This has the potential to create more
>problems than it would solve though (how could I be sure the whole design
>was netlisted?).

No, this is how it works now, if you use a project sheet. The "list of 
sheets" is a project schematic with sheet symbols for all the sheets to be 
included.

[EMAIL PROTECTED]
Abdulrahman Lomax
Easthampton, Massachusetts USA

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