Re: gEDA: gEDA and PCB

[Chris Ellec <cae@oco.net>]

Magnus Danielson wrote:
> 
> Dear All,
> 

> I basically want to actually do a layout now, and PCB seems to be the
> tool, until that distant day gPCB gets sufficiently usefull.
> 

The magic tool is gschem2pcb, a script that comes with gnetlist. It runs
gnetlist -g PCB and gnetlist -g PCBboard

If your schematic is toto.sch, then "gschem2pcb toto.sch" will generate
toto.pcb and toto.net.

In PCB, load toto.pcb then toto.net. When you save the pcb file from
pcb, it saves the netlist inside the pcb file, so there is only one file
after that. Give it a different name !

If you modify the schematics and run gschem2pcb again, it will create a
new file called toto.new.pcb with the new components, and write over the
toto.net. You can load the new.pcb on top of your existing pcb, so you
don't have to start all over, then reload the netlist.

That part is a little broken in that gschem2pcb doesn't always notice
your changes and sometimes generates an empty new.pcb. (it depends on
what was changed).

You can read the gschem2pcb script itself, there is a little description
at the beginning of the file.

Various people have posted m4 macros to generate layout that were not
supported, in case this happens to you. I made one for the smd resistors
for example, I have seen others for various connectors and so on.

On PCB, the problems I had were:
PCB 1.6.3 can not do vias through copper planes (fixed in 1.7.2)
PCB 1.7.2 can not generate gerber files with filled polygons

I need both features, so I'm kind of stuck right now.  (I am waiting for
Harry's response on that one).

But overall PCB is pretty good and I have had boards made on the outside
with it from the gerber files (4 layers) , and I make my own PCB from
the postscript output (2 layers).

Chris.