X-Authentication-Warning: delorie.com: mail set sender to geda-user-bounces using -f
X-Recipient: geda-user AT delorie DOT com
DKIM-Signature: v=1; a=rsa-sha256; c=relaxed/relaxed;
        d=gmail.com; s=20120113;
        h=mime-version:in-reply-to:references:date:message-id:subject:from:to
         :content-type;
        bh=nHTNq5t2yxj4a3A0NtpD0CO3F105IyzhQWyAyXy6rzA=;
        b=DRkA+GAAk2z74UQ2H4MlPZoejtq34luS0KXKeXDsArq9ThapjmnriKs7tDB1ra/Ro3
         8BTy8xmehTEgheY1ZGUBo/51pisELdsD8aWufsLa0QRK8y3n9kY6qxnUZOMww1vmAf+c
         QwWD4InSoWiO2REiUR6Bp9hBSZu1cEiHHYfZok7HcHS7fuUuRm59segq+tadN/pbrgE8
         URN7uV7ErRwkwJQgObARvvymN4spNUqjWk5mOnxrvrQjgUxwJ+b7tAQlSZhYHUJXz6/y
         Eb4d4V0nsSZ6sadRRrknBH3ykb0kBpDwnLfKYIq6Q79pBO3pSNeXUIlAPjzXqTojHjti
         kwPw==
MIME-Version: 1.0
X-Received: by 10.42.39.203 with SMTP id i11mr37612714ice.23.1402403833437;
 Tue, 10 Jun 2014 05:37:13 -0700 (PDT)
In-Reply-To: <CAOFvGD6Q-XnRme-tDwDacQKzY1Ragp94hpe+G7Mk4Qzfob6rdA@mail.gmail.com>
References: <CAOFvGD6Q-XnRme-tDwDacQKzY1Ragp94hpe+G7Mk4Qzfob6rdA AT mail DOT gmail DOT com>
Date: Tue, 10 Jun 2014 08:37:13 -0400
Message-ID: <CAOuGh8_8FvwUWcaKsbrzn5R2Sf30=HZHS6gOHtfp92Zr2daQfA@mail.gmail.com>
Subject: Re: [geda-user] Using PCB with a EDIF/Protel/PADS format netlist
 generated by ORCAD?
From: Bob Paddock <graceindustries AT gmail DOT com>
To: geda-user AT delorie DOT com
Content-Type: text/plain; charset=UTF-8
Reply-To: geda-user AT delorie DOT com
Errors-To: nobody AT delorie DOT com
X-Mailing-List: geda-user AT delorie DOT com
X-Unsubscribes-To: listserv AT delorie DOT com
Precedence: bulk

On Mon, Jun 9, 2014 at 9:17 PM, Jason White
<whitewaterssoftwareinfo AT gmail DOT com> wrote:
> Hello, recently I began using ORCAD at work. Long story short, the
> schematic capture side works like a dream, but the layout side is a
> mess. The schematic capture side supports exporting to something like
>>25 different formats and that leaves me wondering if there are any
> scripts floating around out there to convert one of them into the gEDA
> netlist format?

Some cryptic notes I wrote to myself about doing this years ago:

OrCAD Integra format netlist looks like this:

%PART
+3V             BT1
0.1uF           C1
...
%NET
N06426                  R8-2 Q3-BASE
N00495                  R13-2 Q6-COLLECTOR C2-1 Q7-COLLECTOR
*                       R11-2
N08216                  DS2-ANODE R2-2
N08220                  DS3-ANODE R3-2
$

PCB wants to see this:
N06426                  R8-2 Q3-1
N00495                  R13-2 Q6-3 C2-1 Q7-3 \
                        R11-2
N08216                  DS2-2 R2-2
N08220                  DS3-2 R3-2

In other words remove everything before, and including
%NET, and remove the final $.

Then change all <LF>"* text" to "text \"<LF>.

In other words change leading * to trailing backslash
on the previous line.

Change words like BASE/GATE to the appropriate PCB footprint number.
2N4401 are 1=Base 2=Emitter 3=Collector etc.

If your netlist is wrong as far as words vs numbers, then your board
will be wrong.