X-Authentication-Warning: delorie.com: mail set sender to geda-user-bounces using -f X-Recipient: geda-user AT delorie DOT com X-Google-DKIM-Signature: v=1; a=rsa-sha256; c=relaxed/relaxed; d=google.com; s=20120113; h=x-received:mime-version:x-originating-ip:in-reply-to:references :from:date:message-id:subject:to:content-type:x-gm-message-state; bh=hk9aXguvj9Dusk4IsnEQ2px6uXixjpeEu3SrO9JeO/Q=; b=XzKoJKnr2/pgVWjs5/Ar13Yct2wyKLajM8xeoHbuXlKwali7osQCaHszu0t2M/ABag 7gDsPTGwGmwSl/E89iO+6H9wXj/45hTIa/xswJJRU4XdV2Vt+ezbuCdTRrfGugfNjYAL ZrRU0clsupMiTWoSAfamLXuGqWSlqSgux+xqNRTSBjtCExz+FYHlMV50KsvTcRLYiQqS WgmCELYvjmYcY/F4euGkRLCo6wE8q390Qs+yOHxmudiUhYLTXPvwXH0TU5LUsxTyfsRb B6qN9HVHDykM95ZK7AujIOpWHiuuheZfOACWxSrrMNpLF/CSrcFQZ9AGSv3L2BQnsnMv ZHSQ== X-Received: by 10.58.133.81 with SMTP id pa17mr4079806veb.37.1367611080771; Fri, 03 May 2013 12:58:00 -0700 (PDT) MIME-Version: 1.0 X-Originating-IP: [2604:4280:1:c0de:204:acff:fea3:70be] In-Reply-To: <51841219.4010906@buffalo.edu> References: <5183F1E2 DOT 4000804 AT neurotica DOT com> <5183F419 DOT 3010800 AT estechnical DOT co DOT uk> <5183F787 DOT 8040007 AT neurotica DOT com> <5183FAA0 DOT 3030600 AT estechnical DOT co DOT uk> <51841219 DOT 4010906 AT buffalo DOT edu> From: Benjamin Bergman Date: Fri, 3 May 2013 14:57:30 -0500 Message-ID: Subject: Re: [geda-user] need advice about copper "keep out" areas To: geda-user AT delorie DOT com Content-Type: text/plain; charset=ISO-8859-1 X-Gm-Message-State: ALoCoQnKEWA+bj/DvKELhcQRLQVv8T57FR0X9cTgaVHy2pWrd+EZ3r45ChYyVteDQOYou8ONE7LT 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 That is an interesting technique, Steve. I'll have to keep that in mind. On my last board, I used one large rectangle for the copper pour and then used the hole tool to cut out the corners. I actually started with a large mounting hole, via, but didn't like the round pointy bits along the edge of the board, so I used the hole tool to cut those off. On Fri, May 3, 2013 at 2:38 PM, Stephen R. Besch wrote: > On 05/03/2013 01:57 PM, Ed Simmons wrote: >> >> On 03/05/13 18:44, Dave McGuire wrote: >>> >>> On 05/03/2013 01:30 PM, Ed Simmons wrote: >>>>> >>>>> ...for the lack of a better term. >>>>> >>>>> I would like to have the corners of a board not plated with copper, >>>>> such that the copper fill (which I normally do with one big polygon) >>>>> for >>>>> the ground plane is shaped like a big fat '+' character. >>>>> >>>>> Other than drawing a big fat '+' with polygons, does anyone have a >>>>> nice clean way to accomplish what I'm after? >>>>> >>>> Could this be done with a footprint containing pads (eg mounting or >>>> tooling holes in the corners) with clearance such that the copper stops >>>> where you wish? You could set the square flag to get the shape you're >>>> after. >>>> >>>> Hope that's useful... >>> >>> Oh, that's an interesting idea! I will explore that. Thank you! >>> >>> -Dave >>> >> I make a generic 1 pin symbol that refers to the footprint for a >> particular housing. Make sure you give the pads unique numbers or PCB will >> tell you to connect them together, this keeps things easy to manage in the >> schematics and PCB. >> >> Ed >> >> > I've tried all of the above techniques and they all work, but tend to be > limited to special cases. Multiple/Complex polygons work most of the time, > especially when the copper keep-out is at the board edge. However, in those > cases where there is a copper keep-out in the middle of the board, polygons > don't seem to work. I've recently used another technique which is ideal in > some cases, does not require composing a new footprint for every shape of > keep-out, and can be made completely general. I draw a free, closed trace > around the desired keep-out area. Rectangles will not cross this trace so > the area bounded by it will be copper free. This does leave a visible > "window frame" around the keep-out though. Sometimes this trace can be used > for connectivity as well. In any case, the Gap between the polygon and the > keep-out trace can be eliminated by drawing another trace in the gap. This > trace needs to partially overlap the Keep-Out trace. Then setting the join > flag on this second trace lets the polygon flood over the second trace, but > it still stops at the keep-out trace. One rather major limitation is that > other traces cannot cross the boundary either, so its not as useful in > crowded parts of the board unless you are willing to add a lot of > vias/jumpers or break the keep-out trace into enough segments - then trace > clearance will prevent copper fill getting past the trace. Another cool > thing about this technique is that you can drop another rectangle inside the > keep-out to make a separate, electrically independent copper pour. This is > useful for heat-sinks or sub-circuit power distributions or ground isolation > areas (e.g., separating analog circuitry from Digital circuitry). > > It is all a bit of a pain, but since PCB does not have an official Copper > Keep-Out, you do what you have to do and the more techniques the merrier. > > Steve Besch > > -- > fictio cedit veritati >