X-Authentication-Warning: delorie.com: mail set sender to geda-user-bounces using -f X-Recipient: geda-user AT delorie DOT com Message-ID: <51841219.4010906@buffalo.edu> Date: Fri, 03 May 2013 15:38:01 -0400 From: "Stephen R. Besch" User-Agent: Mozilla/5.0 (X11; Linux x86_64; rv:17.0) Gecko/20130329 Thunderbird/17.0.5 MIME-Version: 1.0 To: geda-user AT delorie DOT com Subject: Re: [geda-user] need advice about copper "keep out" areas 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> In-Reply-To: <5183FAA0.3030600@estechnical.co.uk> Content-Type: text/plain; charset=ISO-8859-1; format=flowed Content-Transfer-Encoding: 7bit X-PM-EL-Spam-Prob: X: 10% Reply-To: geda-user AT delorie DOT com 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