John
You are welcomed...but I should practice what I preach.   I have been using
this method with 99SE SP6 and have had flawless designs.   Ok until last
week ,  we got a board back with power and gnd were not connected to  the
input connector.    The original  ECO was a minor change, I imported a
netlist,  and since I knew what the ECO was,  made the quick changes.  Ran
DRCs and sent gerbers.     The problem was.....the footprint for the power
connector had duplicate pin numbers.  A second import of  a netlist in
Protel causes all of the pins to disconnect,  at third import will cause
only one of the pins to connect.  Every subsequent import will cause
differnet results . I already was aware of it but didnt see the connector.
This will not show up as an error when you import the netlist either.
Had I stuck with my fool proof method and not taken a shortcut  ( because I
made an assumption)   I wouldnt have had mud in my face.   Clear the
netlist, import the netlist , connect copper, run drcs .....100 percent of
the time and you will never have a problem.     So said the fool of the week
only because I made an assumption.


Mike Reagan



> Hello Mike,
> I tried your fool proof method and everything works great.  Thanks for
> taking the time to help me out.  Take care and have a nice night.....
>
> -----Original Message-----
> From: Mike Reagan [mailto:[EMAIL PROTECTED]]
> Sent: Thursday, February 13, 2003 2:26 PM
> To: Protel EDA Forum
> Subject: Re: [PEDA] A Question About Netlist Compare and Partially
> Matched Nets. Protel 99SE SP6.
>
>
> John,
> You really don't have to do a netlist compare.  I see designers doing this
> all of the time.  This may have developed because of  a mistrust of other
> programs they have used because DRCs couldn't be trusted.  The bottom line
> is the DRC netlist checking in  versions  2.8 - 99SE SP 6 work and work
> quite well.   As far as I know the  errors  that the program will not
check
> for is :  1 if you deleted a component    2:  duplicate pins., 3 it will
> miss split plane problems once in while.
>
> To address your real question, the differences could be attributed to
> several things,   1: the netlist generated from the board does not
> accurately represent the board because of a Protel issue   ( I don't call
> this one a bug because the DRC wasn't designed to work this way) .  2   A
> second netlist generated from the schematic may have different names for
> nets which we not names.  3. Other parts, or pads on the netlist which you
> have connected are now in the netlist,   4: Plane information is not
> accurately generated.    In any case this is not a good method of
> verification
>
> A Fool Proof method for verification:
> Clear all nets,
> Load netlist again
> Update free primitives from pad
> Run your DRCs.
> Review your DRCs , if you have everything set up right it should all read
0
>
> I will guarantee this is 100 percent fool proof.
>
>
> Good Luck
>
> Mike Reagan
> EDSI
> Frederick Md
>
>
>
>
>
>
>
> About Netlist Compare and Partially Matched Nets. Protel 99SE SP6.
>
>
> > Hello All,
> > Have a PCB design that is completely routed.  The board information
report
> > and DRC report state that everything is 100% routed with no violations.
> OK
> > great.
> >
> > In the schematic side I generate a Netlist.  Now  I go to the PCB side
and
> > from Netlist Manager I export the Netlist from PCB.  I then do a Netlist
> > compare and everything is good.
> >
> > I then go to the schematic side again and do a Netlist compare with the
> > same two files.  The report states that I have 2 Partially Matched Nets.
> > How can this be?
> >
> > What exactly is a Partially Matched Net?  To me it sounds like parts of
> the
> > net in question are not completely routed.
> >
> > Has anyone out there had this experience?  Do I have a problem with my
> > design or is this a Protel bug - feature?
> >
> > Any information that you can give me will be greatly appreciated.  Thank
> > you for your time and have a nice day.
> >
> >
> >
> > John Branthoover            :
> > Electrical Design Engineer  :
> > Acutronic  R & D            :Phone  (412) 968-1051
> > 640 Alpha Drive             :Fax    (412) 963-0816
> > Pittsburgh PA 15238         :Email  [EMAIL PROTECTED]
> > USA                         :WEB    http://www.acutronic.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
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *

Reply via email to