thank you for your comments, mr. lomax.  you are right about it
being somewhat messy using global nets for connector pins.  i
had to call the connector C1, and then the global nets P1-XXX,
and there would be a one-to-one correspondence between the
C1-XXX and the P1-XXX.  

i am presently reworking the schematic and connecting grounds
to the pins themselves on the last two pages (the connectors), 
but i've retained the global nets elsewhere.  the old schematic 
had no qualms about connecting P1-45 to a chip and then a
global net for connections on other pages.  i'm in the process of
going thru and replacing any redundant global nets with just one.

to verify the schematic redraw in protel, i've decided to bail out 
on a comparison of the two schematics, and just generate a
netlist in protel and bounce it against the older schematic.

again, thanks.  


> -----Original Message-----
> From: Abd ul-Rahman Lomax [SMTP:[EMAIL PROTECTED]]
> Sent: Tuesday, September 18, 2001 2:34 PM
> To:   Protel EDA Forum; '[EMAIL PROTECTED]'
> Subject:      Re: [PEDA] fix for no multi-named nets
> 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....
> 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