Ian, I always print my schematics in colour, this way I avoid the confusion
of having only 4 power ports for six ground nets (same port styles with
different nets are assigned different colours). Also I have never yet used
all six on one schematic.
-----Original Message-----
From: Ian Wilson [mailto:[EMAIL PROTECTED]]
Sent: Wednesday, 16 May 2001 8:46 PM
To: Protel EDA Forum
Subject: Re: [PEDA] Suggestion for Net Names on all Power Symbols
I suspect I know what Paul is on about.
Just as many designs have multiple supplies - some have multiple
grounds. In these days of tighter EMC requirements common mode chokes and
isolated RF/analog ground etc a single circuit ground is no longer always
the case. As well you have earth, chassis ground, and maybe a frame ground
etc etc...
An ground symbol can mean any one of several different grounds. Looking at
the schematic a simple power symbol does not really show what the netlister
will make of it. Remember the power symbol does not convey connectivity -
only the net associated with each power port does that.
I am increasingly finding that companies are forbidding the use of anything
but the bar power port to ensure that the net is shown and there is
consistency. I think, Paul, may desire this same absolutely clear
information on the schematic *but* he prefers the traditional earth/ground
symbols.
Having toolbar buttons that ease the placement of power ports, and that
even set the net name, does not absolutely ensure that the net is correct -
it can easily be edited. The netlist could easily become very wrong.
I think I will probably stick to the bars but I think the suggestion has
merit. Can't be very hard to implement either. I think PCAD does/did this.
Thomas, you say that you use the four ground power symbols across six nets
you regularly use - there is some chance of confusion here and this is
exactly what I, and I suspect Paul, is worried about.
Ian Wilson
On 05:41 PM 16/05/2001 +1000, Thomas said:
>Another option would be to edit the 'power objects' toolbar.
>
>Setting the parameter: S=text, where 'text' is the net name you wish that
>type of port to connect to for a number of different ground ports makes
life
>allot easier.
>
>I have six buttons that I use regularly, GND, PGND, SGND, DGND, CHASSIS and
>EARTH set for the four main types of ground symbol.
>
>I also set the colour parameter for ground ports differently (in the
>associated toolbar buttons' parameter field) to tell the ones that have the
>same symbol apart.
>
>Here's a sample of two of the parameter fields:
>
>S=GND|Color=32768|Orientation=3|Style=1|$Description=GND power port
>S=EARTH|Color=32768|Orientation=3|Style=6|$Description=Earth power port
>
>You could also alter the toolbar button bitmap to show what net each ground
>symbols netlist parameter is set to.
>
>It does take a bit of work to set this all up but I have found it to be a
>worthwhile solution to the problem.
>
>The 'info' button next to the parameter text box associated with each
button
>is quite useful and does give lots of info on how to alter power object
>parameters.
>
>If all this tinkering worries you, back up your CLIENT99SE.rcs file first.
>
>
>Regards,
>
>Tom L.
>
>
>-----Original Message-----
>From: [EMAIL PROTECTED]
>[mailto:[EMAIL PROTECTED]]
>Sent: Wednesday, 16 May 2001 8:15 AM
>To: proteledaforum
>Subject: [PEDA] Suggestion for Net Names on all Power Symbols
>
>
>I would like to make a suggestion that net names be made visible on all
>protel power symbols (eg. the net name could optionally appear below the
>ground symbol). The problem with the current implementation is that it is
>very easy to have a power object like an earth, power or signal ground
>unintentionally connected to an incorrect net like VCC. It is not possible
>to easily check for this without having to clicking on the symbol. I am
>aware that many companies have circumvented this problem by always using
the
>bar power symbols. However I believe that the power ground, frame and
signal
>ground symbols increase the readability of a schematic. I am also aware
that
>it is possible to place a net label somewhere near the symbol but this is
>not always easy to locate or read. I would like to retain the use of ground
>power symbols without having to compromise the accuracy of my schematic or
>be forced to check all the symbols manually.
>
>Regards Paul
>Electronics Design Engineer
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* To post a message: mailto:[EMAIL PROTECTED]
*
* To leave this list visit:
* http://www.techservinc.com/protelusers/subscrib.html
* - or email -
* mailto:[EMAIL PROTECTED]?body=leave%20proteledaforum
*
* Contact the list manager:
* mailto:[EMAIL PROTECTED]
*
* Browse or Search previous postings:
* http://www.mail-archive.com/[email protected]
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
