At 07:18 AM 9/18/01 -0500, Robison Michael R CNIN wrote:
>this is just a comment post and not a question.
>
>i wrote about a month ago about a problem i was having with not
>being able to assign multiple names to the same net.  although
>this sounds like an unreasonable, unnecessary, and dubious
>practice, it was actually the result of a simple attempt to redraw
>a non-protel schematic into protel.

Yes, this is where net renaming can become a major issue.

i had the connectors all on the last page, and i used global nets
>to connect them to the other pages.  well, on page 1 there were
>several pins tied to ground.  when i tied several of the global nets
>that represented these pins to ground, i noticed in the netlist that
>all were deleted but one.  the reason is that you can only have
>one name assigned per net.

"Global nets that represented these pins?" It sounds to me that what 
existed were nets naming the pin, such as "J1-25" as a net name. So trying 
to tie these to ground resulted in net renaming, which is a dicey business. 
Protel treats it as an error, which I would consider good, except that I 
would like to have a way to intentionally, visibly and clearly rename a 
net. This is almost a necessity where parts have hidden power pins, say 
VCC, and "VCC" is one net on one sheet and another net on another sheet 
because of isolated power supplies, perhaps even different voltages.

Tango handled this by allow one specific kind of renaming: If one placed a 
power object and connected to the virtual pin of that object a piece of 
wire with a net label, one of those nets was renamed to the other for that 
page only. It worked quite well, the only problem being that I kept 
forgetting which way the nets were renamed; as I recall, the power object 
net became the wire net. If any other nodes were connected to that 
structure, it was treated as a net renaming error.

>it was suggested that i just attach them as non-schematic com-
>ponents, but i feared complications from this approach.

I would too. If it looks like a component, it should be a component. But I 
don't see what would be so difficult about this situation. Where one did 
not want to use the connector pin name net -- assuming this was the problem 
-- as the final net name, one would simply change that net to the power net 
name. It does not have to be a power object, power objects are simply one 
device for creating a named net, explicit naming with a Net Label works 
just as well.

>what i'm thinking about doing is dispensing with the connectors on
>the last page, making the connectors into multi-part components
>with each pin as a part, and doing it that way.  its a trade-off really.
>a component with a hundred parts is something of a mess.

It's not as difficult as it may seem. Being able to independent place pins 
wherever they are appropriate can be very useful; but many designers prefer 
to be able to see the whole connector at once. Sometimes the connectors 
will be placed on the root schematic in a hierarchy; that schematic then 
shows the interface with the outside world plus the internal organization 
of the board; subsheets then give the details of the latter.

When bringing in schematic pieces from other projects, it is a good idea to 
avoid global nets. This forces one to make intersheet connections 
explicitly through ports; what the nets are named on subsheets becomes 
irrelevant (except for power nets, which are global always).

OrCAD Capture, last time I looked, would cheerfully rename nets tied to 
each other, picking one of the names by a less-than-obvious method of 
choice. Problem was that if Net A was connected to Net B on one sheet and 
to Net C on another sheet, the renaming took place at the subsheet level 
before net connections were examined on a higher level, thus it was a 
toss-up whether there ended up being one net or two nets, and the name of 
the final net or nets was not obvious. I received a schematic from a client 
which had been put together from many different projects, and it was a 
one-week job to disentangle the mess.

>   the
>alternative was to break from the older schematic's layout and just
>tie those pins to ground on the final page of connectors.

A pin should be tied to ground only on the page where that pin appears, 
except that one could, maybe, on the highest level schematic, rename a net 
to ground. This is if nets are *not* global, so they may take on the name 
that they are assigned at the highest level. This may not be considered net 
renaming, but I have not tested this where power nets are involved.

I.e., you would have a port and lower level net named J1-26, for example, 
and then that port would be connected to a GND power object at the higher 
level.
I'd test it if I had time today....


[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