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]" 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: Message-ID: References: User-Agent: Alpine 2.00 (DEB 1167 2008-08-23) MIME-Version: 1.0 Content-Type: TEXT/PLAIN; charset=US-ASCII; format=flowed 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 Precedence: bulk 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