X-Authentication-Warning:	delorie.com: mail set sender to geda-help-bounces using -f
X-Recipient:	geda-help AT delorie DOT com
Date:	Mon, 28 Aug 2017 13:34:34 +0200 (CEST)
X-X-Sender:	igor2 AT igor2priv
To:	"Graham S (graham DOT seale AT gmail DOT com) [via geda-help AT delorie DOT com]" <geda-help AT delorie DOT com>
X-Debug:	to=geda-help AT delorie DOT com from="gedah AT igor2 DOT repo DOT hu"
From:	gedah AT igor2 DOT repo DOT hu
Subject:	Re: [geda-help] Symbols for components with extra internally connected
	pins in the footprint
In-Reply-To:	<CAHsNvaB61cG5aYuoTO1HVeuDfq=hPfuZ667L0fhEPk6g+k1V_Q@mail.gmail.com>
Message-ID:	<alpine.DEB.2.00.1708281327350.27212@igor2priv>
References:	<CAHsNvaB61cG5aYuoTO1HVeuDfq=hPfuZ667L0fhEPk6g+k1V_Q AT mail DOT gmail DOT com>
User-Agent:	Alpine 2.00 (DEB 1167 2008-08-23)
MIME-Version:	1.0
Reply-To:	geda-help AT delorie DOT com
Errors-To:	nobody AT delorie DOT com
X-Mailing-List:	geda-help AT delorie DOT com
X-Unsubscribes-To:	listserv AT delorie DOT com

Hi Graham,

On Mon, 28 Aug 2017, Graham S (graham DOT seale AT gmail DOT com) [via geda-help AT delorie DOT com] wrote:

>Hi gEDA help
>
>How does one deal with the symbol for a component that has more physical
>pins than symbol pins, because internally some are strapped together? I have
>searched through the Wiki help for some time, looking for a clear example,
>but not yet seen how to do it.
>
>Some power semiconductors use extra pins, as do many relays.
>
>An example is a simple changeover switch relay where there are 8 pins
>altogether.
>Two of the pins can be for the coil, and given a slotdef=1. That part is
>easy.
>
>The remaining 6 pins, using slotdef=2, are arranged such that each internal
>element uses up 2 pins, strapped together internally.
>
>This is where I need to understand how, (or whether) a single gschem symbol
>pin can be actually served by more than one pin in the footprint, and know
>how to arrange pinseq. I have spent some time adding the attributes to the
>example, though I suspect my arrangement might be done better
>

I think there are three common use cases:

If it's "use whichever of the connected pins": make the footprint have the 
same pin number for all the internally connected pins; yes, this means a 
specific footprint for your symbol; whichever you connect in pcb, will be 
accepted as a  valid connection

If it's "make pcb understand the two pins are internally connected, 
without having he same pin numbers", as in you can connect one of them and 
then continue routing from the other, typical example is like a 1206 zero 
ohm resistor used as a "jump" wire: use pcb-rnd instead of pcb; pcb-rnd 
does understand such internal connections since 2013. It still requires a 
footprint crafted for the part, tho.

If it's "4 gnd pins on this microcontroller, all must be connected to 
gnd": the symbol needs to explicitly connect all four, by pin number, to 
ground; you can do this either by drawing a new symbol that has these 
graphically or using attribute wizardy. Attributes can be used on top of 
an existing footprint, and they can make graphically invisible connection 
from whichever specific pin to a named net. That's how the heavy-symbol 
versions of the 74xxx connect gnd and power, if you want to take a look 
at an example.

HTH,

Igor2

- Raw text -