X-Authentication-Warning: delorie.com: mail set sender to geda-help-bounces using -f X-Recipient: geda-help AT delorie DOT com Subject: Re: [geda-help] Wire bridges in gschem? To: geda-help AT delorie DOT com References: <30c7dda0-4d20-55f8-708b-5d76e60f46cb AT zonnet DOT nl> From: moreno+geda-help AT mochima DOT com Message-ID: Date: Fri, 23 Mar 2018 10:26:12 -0400 User-Agent: Mozilla/5.0 (X11; Linux x86_64; rv:52.0) Gecko/20100101 Thunderbird/52.6.0 MIME-Version: 1.0 In-Reply-To: <30c7dda0-4d20-55f8-708b-5d76e60f46cb@zonnet.nl> Content-Type: text/plain; charset=utf-8; format=flowed Content-Language: en-US X-Added-Header: Content-Transfer-Encoding: 8bit X-MIME-Autoconverted: from quoted-printable to 8bit by delorie.com id w2NEQEfR024074 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 On 2018-03-23 09:00 AM, HansFong wrote: > Hello all, newbie gEda user here (also newbie in PCB-design). > > In PCB you can draw arbitrary lines and vias, which is handy if you > want to insert a single test pin (a physical pin you put on your PCB > to hook up a probe) in a line, or make a wire bridge (two vias with > nothing in between and an arbitrary distance in between them). Careful --- a via will not work if you're getting the PCB done with solder mask  (the solder mask covers vias). In PCB, you can get around this by just selecting the via and going to the menu Select --> Convert selection to element.  (I suspect that this is not what you want; I just thought I'd mention it) > So what is the proper way to make such things in gschem? > > 1) use connectors? The test-1 symbol already suggested is good at the schematic level, but unfortunately it does not have an associated footprint --- you could use JUMPER1; however, there doesn't seem to be one that does not place a hole.  I created my own, I called it Pad --- e.g., copy-n-paste the following into a file called Pad.fp in your footprints directory (e.g., $HOME/.gEDA/footprints): ---- BEGIN Pad.fp FILE ---- Element["" "" "" "" 78500 17000 0 0 0 100 ""] (     Pad[0 0 0 0 2mm 16mil 2.11mm "" "1" "edge2"] ) ---- END Pad.fp FILE ---- You can adjust the size --- 2mm is the diameter; 16mil is the clearance; 2.11mm is the diameter of the solder mask hole;  you can create multiple versions if you need to, for different sizes. > 2) use 0 ohm resistors? > > 3) ??? Already suggested, but I second that idea, which I've found myself using recently:  you can place vias and route a trace in a different layer (e.g., spare;  or even ground or signal2/3 if you're designing a two-layer board and are not using those extra layers).  Then, when sending off the Gerber files, just exclude the file for that extra layer.  The trick is:  PCB will know that the connection is made and will not report that there are missing rats. However, one detail --- see my comment above about the vias being covered by the solder mask;  if you use this trick, make sure to select the vias and convert them to elements! Cheers, Carlos --