X-Authentication-Warning: delorie.com: mail set sender to geda-user-bounces using -f
X-Recipient: geda-user AT delorie DOT com
Date: Tue, 17 Jul 2018 22:56:48 +0200 (CEST)
From: Roland Lutz <rlutz AT hedmen DOT org>
To: "Rob Butts (r DOT butts2 AT gmail DOT com) [via geda-user AT delorie DOT com]" <geda-user AT delorie DOT com>
Subject: Re: [geda-user] How to define for an exposed pad to connect to 3
 pins/pads
In-Reply-To: <CALSZ9gqcUsDbq4j6fpPSBb5dV+_mqhYxBSNb1WuWNQygru8=wg@mail.gmail.com>
Message-ID: <alpine.DEB.2.20.1807172230250.2555@nimbus>
References: <xnmuuy6a7j DOT fsf AT envy DOT delorie DOT com> <910e5ecd-24a2-fdb6-432a-0fa913cf3559 AT neurotica DOT com> <0dd0f101-93ae-1126-ab61-7d9d16886f78 AT ecosensory DOT com> <CALSZ9gqBHoCnie-Cuk3wV2nvMW9-cK3gWN-ZKKGsYFKBnPPLrQ AT mail DOT gmail DOT com> <CALSZ9gqwgiumLniqndvBx2wTcwWEJfY2YxgALUQ7Kp-dUZPwBg AT mail DOT gmail DOT com>
 <s6nlgahj3ih DOT fsf AT falbala DOT ieap DOT uni-kiel DOT de> <CALSZ9go7WnqUnU0y2uhnBJQP2=LBfV=Z8di=9nhrJG_q6Khp6g AT mail DOT gmail DOT com> <CALSZ9gpzRD4-m21HXkoRdLUbewYPrsJcMapSKBPj3ek2LQAnBg AT mail DOT gmail DOT com> <20180711180601 DOT 764ace616542cb8e00831933 AT gmail DOT com>
 <CALSZ9grtHiS67asvOfEpQvtd+0V0x0ga-9xGcYwxLWq7T0G=hA AT mail DOT gmail DOT com> <CALSZ9gqcUsDbq4j6fpPSBb5dV+_mqhYxBSNb1WuWNQygru8=wg AT mail DOT gmail DOT com>
User-Agent: Alpine 2.20 (DEB 67 2015-01-07)
MIME-Version: 1.0
Content-Type: multipart/mixed; BOUNDARY="8323329-1082386632-1531861008=:2555"
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

  This message is in MIME format.  The first part should be readable text,
  while the remaining parts are likely unreadable without MIME-aware tools.

--8323329-1082386632-1531861008=:2555
Content-Type: text/plain; charset=UTF-8; format=flowed
Content-Transfer-Encoding: 8BIT

On Tue, 17 Jul 2018, Rob Butts (r DOT butts2 AT gmail DOT com) [via 
geda-user AT delorie DOT com] wrote:
> So now I have an 8 pin mosfet where the D is pins 5 - 8.  The component 
> has an exposed pad that goes across the pins 5 - 8.  How can I do the 
> symbol net="netname":"pin" so that pins 5-8 and the exposed pad (pin 9) 
> are all connected?

First, you'd have to decide how to represent this as a package.  To 
gEDA/gaf (the "schematics part" of gEDA), a package is some abstract unit 
which is connected via "pins" (there is no distinction between pins and 
pads here) to other packages.  The most straightforward way would be to 
draw a footprint in PCB, and then treat each pin and pad as an individual 
schematic "pin".

Next, you'd have to decide which of these pins you want to see in your 
schematic, how many symbols you want to use, and how the pins should be 
distributed to the symbols.  For example, you could create one symbol with 
N pins; or you could create one symbol for pins 1–3 and one symbol for all 
remaining pins; or you could create N symbols each containing one pin 
(which would be an incredibly tedious, but still valid way to represent 
the package--just make sure to set an identical refdes= attribute on each 
component).  Instead of adding a pin object to the symbol (which makes the 
pin visible in the schematic), you could also add a net= attribute to the 
symbol or component which basically acts as one or more "invisible pins".

Please keep in mind that the schematic, and therefore the netlist, only 
represents what *should* be connected, not what *is* connected.  If the 
pins/pads are internally connected and it is only necessary to connect one 
of them, then treat them as one pin with one pinnumber, as far as gEDA/gaf 
is concerned.  If they all need to be connected individually, treat them 
as individual pins and connect them on the schematic, either by visually 
shorting a number of pins, or by using a net= attribute.

--8323329-1082386632-1531861008=:2555--