Re: [PEDA] single pin nets
You're right, of course. Looks like either a bug in the program, or incorrect documentation (the one sentence there is). (A copy of this is going to Protel support.) On Design | Rules | Other, "Un-connected Pin Constraint" says "Detects pins that have no connecting tracks." There's no mention of it mattering whether or not the pin is listed in a net. Also, the help file does not document this rule at all. (It does list the other 2 rules on the "Other" tab.) (P99SEsp6) I hope Protel support will comment on what they believe this rule is SUPPOSED to do. Dwight Harm Trax Softworks, Inc. -Original Message- From: Richard Sumner [mailto:[EMAIL PROTECTED]] Sent: Tuesday, September 18, 2001 10:36 AM To: Protel EDA Forum Subject: Re: [PEDA] single pin nets I tried that, it finds all unconnected pins (which I have a lot of) and did not find a named net with only one connection (just a net name on only one unused pin). The single pin net does appear in the netlist (generated from the pcb), so it isn't flagged as an unconnected pin. thanks, Richard At 11:58 AM 9/18/2001 Tuesday, you wrote: >Richard, >This might get you what you want... go to Design | Rules | Other, add >"unconnected pin constraint" with a scope of Whole Board. Then on Tools | >DRC, check "unconnected pins", & you'll get a list of violations for pins >that have no connecting tracks. > >Dwight Harm >Trax Softworks, Inc. > >-Original Message- >From: Richard Sumner [mailto:[EMAIL PROTECTED]] >Sent: Tuesday, September 18, 2001 8:03 AM > >Does anyone know a simple way to find single pin nets on the pcb? I want >to find named nets that have only one pin. I can (and do) export the >netlist from the pcb and look at it, and I really should write a simple >program to do this, but it would be nice if protel could give me a list of >single pin nets. I could probably do it on the schematic using the erc, but >then I would have to put a no erc on all unused pins. That would be a pain >because I do a lot of pin swapping (fpga's are great!) to simplify routing. >Any ideas? > >thanks, >Richard Cheesecote Mountain CAMAC 24 Halley Drive; Pomona, NY 10970 845 364 0211, www.cmcamac.com * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] single pin nets
>Thanks for the replies. While reading and testing them, I realized that >there is a relatively simple way to get protel to help. First, get the netlist status report, and import it into excel, starting on row 3. use spaces and colon (:) as delimiters. Select everything and sort on the column with the length (f). Nets with zero length are now at the top of the list. This is what I want to find, nets that have never been routed, but don't show as unrouted nets in the drc. This is fairly quick, and no harder than exporting the netlist and running a special program. thanks again for the replies Richard >* * * * * * * * * * * * * * * * * * * * * * * * * * * * * * Cheesecote Mountain CAMAC 24 Halley Drive; Pomona, NY 10970 845 364 0211, www.cmcamac.com * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] single pin nets
One way I can think of would be to open the netlist manager highlight the All Nets class and just start keying through the nets listed. The pins connected to it will be shown in the window and single pin nets are very easy to spot there. There may be a better way... but I don't have Protel installed... so I can't check :( Regards, Colby Siemer - Original Message - From: Richard Sumner <[EMAIL PROTECTED]> To: Protel EDA Forum <[EMAIL PROTECTED]> Sent: Tuesday, September 18, 2001 11:36 AM Subject: Re: [PEDA] single pin nets > I tried that, it finds all unconnected pins (which I have a lot of) and > did not find a named net with only one connection (just a net name on only > one unused pin). The single pin net does appear in the netlist (generated > from the pcb), so it isn't flagged as an unconnected pin. > > thanks, > Richard > > At 11:58 AM 9/18/2001 Tuesday, you wrote: > >Richard, > >This might get you what you want... go to Design | Rules | Other, add > >"unconnected pin constraint" with a scope of Whole Board. Then on Tools | > >DRC, check "unconnected pins", & you'll get a list of violations for pins > >that have no connecting tracks. > > > >Dwight Harm > >Trax Softworks, Inc. > > > >-Original Message- > >From: Richard Sumner [mailto:[EMAIL PROTECTED]] > >Sent: Tuesday, September 18, 2001 8:03 AM > > > >Does anyone know a simple way to find single pin nets on the pcb? I want > >to find named nets that have only one pin. I can (and do) export the > >netlist from the pcb and look at it, and I really should write a simple > >program to do this, but it would be nice if protel could give me a list of > >single pin nets. I could probably do it on the schematic using the erc, but > >then I would have to put a no erc on all unused pins. That would be a pain > >because I do a lot of pin swapping (fpga's are great!) to simplify routing. > >Any ideas? > > > >thanks, > >Richard > > Cheesecote Mountain CAMAC > 24 Halley Drive; Pomona, NY 10970 > 845 364 0211, www.cmcamac.com > > > * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] single pin nets
here's a script:
one can download perl for windoze from www.activestate.com... you may also
need the microsoft installer (msi).
I would imagine that the perl script might look something like this:
#!C:\perl\bin\perl
print "\n\nProtel single pin net report v1.0\n\n";
#usage: C:\> perl this_script.pl protel_netlist.txt > results.txt
while(<>)
{
#concatenate each line in one single string including new-lines
$line .= $_;
}
#squash the packaging section of the netlist
#(things in square brackets)
$line =~ s/\[.+\]//gs;
#get each net that begins with an open paren
@nets = split(/\(/, $line);
#shift off the first null net from above split
shift @nets;
#iterate through each net in the @nets list
foreach $net (@nets)
{
#sqaush the net name
$net =~ s/(.+)\n//m;
$net_name = $1;#save the net name
$net =~ s/\)$//s; #squash the ending paren for giggles
#split the nets on newline/carriage returns
@net_pins = split(m/\n/m, $net);
#print if the number of nets split above is less than 2
print "Single pin: @net_pins on Net $net_name\n" if $#net_pins < 2;
}
#done
$count = $#nets + 1;
print "\n\nSearched $count total nets\ndone.\n";
-Original Message-
From: Richard Sumner [mailto:[EMAIL PROTECTED]]
Sent: Tuesday, September 18, 2001 1:36 PM
To: Protel EDA Forum
Subject: Re: [PEDA] single pin nets
I tried that, it finds all unconnected pins (which I have a lot of) and
did not find a named net with only one connection (just a net name on only
one unused pin). The single pin net does appear in the netlist (generated
from the pcb), so it isn't flagged as an unconnected pin.
thanks,
Richard
At 11:58 AM 9/18/2001 Tuesday, you wrote:
>Richard,
>This might get you what you want... go to Design | Rules | Other, add
>"unconnected pin constraint" with a scope of Whole Board. Then on Tools |
>DRC, check "unconnected pins", & you'll get a list of violations for pins
>that have no connecting tracks.
>
>Dwight Harm
>Trax Softworks, Inc.
>
>-Original Message-
>From: Richard Sumner [mailto:[EMAIL PROTECTED]]
>Sent: Tuesday, September 18, 2001 8:03 AM
>
>Does anyone know a simple way to find single pin nets on the pcb? I want
>to find named nets that have only one pin. I can (and do) export the
>netlist from the pcb and look at it, and I really should write a simple
>program to do this, but it would be nice if protel could give me a list of
>single pin nets. I could probably do it on the schematic using the erc, but
>then I would have to put a no erc on all unused pins. That would be a pain
>because I do a lot of pin swapping (fpga's are great!) to simplify routing.
>Any ideas?
>
>thanks,
>Richard
Cheesecote Mountain CAMAC
24 Halley Drive; Pomona, NY 10970
845 364 0211, www.cmcamac.com
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* 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
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] single pin nets
At 01:36 PM 9/18/01 -0400, Richard Sumner wrote: >I tried that, it finds all unconnected pins (which I have a lot of) and >did not find a named net with only one connection (just a net name on >only one unused pin). The single pin net does appear in the netlist >(generated from the pcb), so it isn't flagged as an unconnected pin. Which could be a problem, since checking the NC pin list is a very good place to begin to find possible errors. I was taught this twenty years ago, even before I used a net list (we'd examine a board with all layers in superposition; unconnected pads were easy to spot). Later, I used to routinely deliver the NC pin list with jobs, encouraging the engineer to look it over. One solution to the problem is to remove the net assignments (in Schematic) (net labels) from pins without connections. Thus "single-net" pins will become no-net pins and will appear on the NC report. Schematics with single-net pins can be very confusing to read, since one may look elsewhere on the schematic, trying to find the connection. It is difficult to distinguish between a deliberately single-net pin and one accidentally unconnected, perhaps because of a minor variation in name. Note that there is an "unconnected" parameter in the ERC matrix in Schematic; it is thus possible to generate errors or warnings from single-net pins, which will be treated, as I recall, the same as if there were no net on them. Then the "errors" which are deliberate, whether they are from NC pins with a net name or without, can be suppressed with No-ERC directives. This is my standard practice, I recommend it. This would lead also to another standard practice: place all sections of multipart components, even if only on an additional "unused section" area or page. This is useful for a lot of reasons. I think of many implications and possible reasons why one might want to keep those single-net pins, and for each one of them I imagine I have a better way to suggest, but I'll leave it here for now. But if one insists, I'd recommend generating a net list, massage the net list into a format that will provide one record per net and one field per pin name, and load the formatted net list into Excel or the like. If the field that would hole the second pin name in a net is the third field, then sort the list on the third field; all records with an empty third field will represent single-pin nets and there you have your list. [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 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] single pin nets
I tried that, it finds all unconnected pins (which I have a lot of) and did not find a named net with only one connection (just a net name on only one unused pin). The single pin net does appear in the netlist (generated from the pcb), so it isn't flagged as an unconnected pin. thanks, Richard At 11:58 AM 9/18/2001 Tuesday, you wrote: >Richard, >This might get you what you want... go to Design | Rules | Other, add >"unconnected pin constraint" with a scope of Whole Board. Then on Tools | >DRC, check "unconnected pins", & you'll get a list of violations for pins >that have no connecting tracks. > >Dwight Harm >Trax Softworks, Inc. > >-Original Message- >From: Richard Sumner [mailto:[EMAIL PROTECTED]] >Sent: Tuesday, September 18, 2001 8:03 AM > >Does anyone know a simple way to find single pin nets on the pcb? I want >to find named nets that have only one pin. I can (and do) export the >netlist from the pcb and look at it, and I really should write a simple >program to do this, but it would be nice if protel could give me a list of >single pin nets. I could probably do it on the schematic using the erc, but >then I would have to put a no erc on all unused pins. That would be a pain >because I do a lot of pin swapping (fpga's are great!) to simplify routing. >Any ideas? > >thanks, >Richard Cheesecote Mountain CAMAC 24 Halley Drive; Pomona, NY 10970 845 364 0211, www.cmcamac.com * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] single pin nets
Richard, This might get you what you want... go to Design | Rules | Other, add "unconnected pin constraint" with a scope of Whole Board. Then on Tools | DRC, check "unconnected pins", & you'll get a list of violations for pins that have no connecting tracks. Dwight Harm Trax Softworks, Inc. -Original Message- From: Richard Sumner [mailto:[EMAIL PROTECTED]] Sent: Tuesday, September 18, 2001 8:03 AM Does anyone know a simple way to find single pin nets on the pcb? I want to find named nets that have only one pin. I can (and do) export the netlist from the pcb and look at it, and I really should write a simple program to do this, but it would be nice if protel could give me a list of single pin nets. I could probably do it on the schematic using the erc, but then I would have to put a no erc on all unused pins. That would be a pain because I do a lot of pin swapping (fpga's are great!) to simplify routing. Any ideas? thanks, Richard * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
