Re: gEDA-user: pcb question : ground plane

[9000 VAX <vax9000@xxxxxxxxx>]

On 5/18/05, Bernhard Kraemer <Bernhard.Kramer@xxxxxxxxxxxxxxxxx> wrote:
> Stuart Brorson a écrit :
> 
> >>Hello,
> >>
> >>I encountered another problem for which google couldn't give me an
> >>answer. I'd like to establish a ground plane in gEDA-pcb. With Protel,
> >>for example, I know that I have to draw a polygon over all my circuit,
> >>having checked a box "connect polygon to gnd" somewhere. I have tried
> >>similar with pcb and discovered that this overlays the polygon over all
> >>traces. That means that all traces are going to be interconnected.
> >>
> >>Hence my question: How do I establish a ground plane in gEDA pcb?
> >>
> >>
> >
> >Establishing a GND plane is a little different than you might think.
> >Here are the steps which have worked for me:
> >
> >1.  Set the layer where you want the plane "active".
> >2.  Draw your plane area using the polygon or rectangle tool.  PCB
> >    will automatically clear the plane away from all pins and vias in
> >    your design.
> >3.  For each pin or via which is attached to GND, use the "thrm"
> >    (thermal) tool and click on the pin or via.  This will place
> >    a thermal at the GND pin/via and make the GND connection.
> >4.  If you need a positive plane on an outside layer, do this:
> >    While still on the GND plane layer, draw a line inside the GND
> >    plane somewhere clear of other components.  This signals the
> >    Gerber generator to generate a positive plane layer.  Otherwise,
> >    PCB will generate a negative plane, which is apparently standards-
> >    compliant, but is not desired by many el-cheapo board houses.
> >
> >Caveats:
> >
> >*  If you mistakenly place a thermal somewhere where it doesn't belog,
> >   the DRC checker won't find it -- at least in my experience.  Am I
> >   doing something wrong?  Indeed, the whole mechanism of telling PCB
> >   that a plane is connected to a net is mysterious to me.  Can
> >   anybody enlighten us as to how to do this correctly?
> >*  The algorithm which does the auto-clear of plane around holes &
> >   vias can leave little scraps of unconnected metal laying around.
> >   You need to scan visually for those.  Note that you can't just
> >   delete the individual scraps because the program thinks that they
> >   are attached to the larger plane.  You generally have to draw your
> >   polygon to avoid creating little scraps in the first place.
> >   Yes, this is a misfeature.
> >
> >Have fun,
> >
> >Stuart
> >
> >
> Thank you for your answer, Stuart. But I'm still having problems. This
> is how I proceed:
> 
> 1) The plane where I want my ground plane to be active is the solder
> layer. So I choose "solder" as active layer and then ...
> 2) ... I draw a polygon or a rectangle covering the zone where I want
> may gound plane to appear.  It is true that the plane clears away from
> alle pins and vias in my design. But it doesn't clear away from my lines
> connecting these vias and pins! Which means, all my lines are shorted.
> 
> What could I do now?

First, you can draw your ground plane on the GND-sldr layer. It is
easier to handle this way.
Second, place your mouse on each of the solder layer lines (traces,
tracks...) and press 'j' once. By doing this, the solder layer lines
will clear solder layer planes. (or, alternatively, use a text editor
to edit the .pcb file directy. I did this and it is much faster. Just
be careful and back up your file before doing this)

vax, 9000

> 
> Yours,
> 
>  Bernhard
> 
>