RE: gEDA: gEDA and PCB

[t_porter@dingoblue.net.au]

On 26-Aug-2001 Magnus Danielson wrote:
> Dear All,
> 
> I've searched all of the kingdom and I can't find a good
> description
> of how to get myself to take a schematic and import all
> the necessary
> stuff into PCB and actually do a layout.
> 
>

Hi Magnus.

I use PCB all the time, and this is how I integrate gschem
and PCB.

1/ Create the schematic, and number all parts, note
the annotate.sh can do this nicely, and cut down the work
required.

2/ Create the netlist and I use 
"gnetlist -gPCB circuit.sch -o circuit.net"

I don't use the alternate method of gschem2pcb, because I
prefer to sellect the part footprint at pcb layout time,
instead of adding it to each and every schema part at
gschem time.

3/ Run up PCB, and load the circuit.net, then select the
parts and name them, if you do them in sequence, PCB will
auto increment the names, ie "r1,r2,r3" etc.

4/ Be aware that PCB will not allow nets that have pins
named as aplhabetical characters, such as "c" for colletor,
and the pins must be re named to "1,2,3" in the case of
a npn or pnp transistor. PCB will display "c,b,e" on the
pcb layout however. So go back to gschem and copy the
parts that need alteration and re name them, then change
the pin naming. So far I have changed the npn and pnp tran-
sistors and diode. When you have placed the components
check *carefully* until you are sure its all correct,
because in the case of the diode although the pins are
numbered "1,and 2" are they the right way around ?

Your ratsnest may be complete, and the pcb layout error free
but the diode *may* be backwards! The same applies to the
transistor pins, is the collector, really the collector
when you compare a real transistor to the payout ?

This is basically it!

Then you layout the board following the rats-nests until its
done, and at that point if there are no errors PCB will pop
up a lovely "Congrats you have finished and no errors"
window.

Having said all this, I have used many types of schema and
pcb packages over the years, and I just LOVE gschem and PCB.

But then I also love manual routing!

--
****                                                  ****
Kind Regards
Terry
--
****                                                  ****
   My Desktop is powered by GNU/Linux.