Mail Archives: geda-user/2013/05/03/15:47:05
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
- Raw text -