Re: gEDA-user: Matching footprints with symbols

[Stefan Salewski <mail@xxxxxxxxxxxx>]

On Sat, 2010-04-17 at 01:48 +0200, Stefan Salewski wrote:
> On Sat, 2010-04-17 at 01:15 +0200, Armin Faltl wrote:
> 
> > use ;-)
> > 
> > Did anyone try my schematic posted in  
> > http://www.seul.org/pipermail/geda-user/2010-April/046716.html
> > - is the problem reproducable?
> > 
> 
> I missed your problem, sorry.
> 
> One remark: You used the minus sign "-" in your footprint names. This
> can give trouble in rare cases due to m4 macro expansion.
> 
> You may try renaming the footprint files, underscore character "_"
> should work fine.

OK, here are the results of closer inspection:

I put your files in directory armin:

stefan@AMD64X2 ~/armin $ ls -1
Hauptplatine_v1.pcb
Hauptplatine_v1.sch
cap_2.5-5x11-hor.fp
cap_3.5-8x11-hor.fp
capr_508.fp
coil_manual_R16.fp
gafrc
irf7413-2.sym
ltc1625-1.sym
project.txt
stefan@AMD64X2 ~/armin $


To make the symbols in this directory visible to gschem and friends we
need this line in gafrc file:
 
stefan@AMD64X2 ~/armin $ cat gafrc 

(component-library ".")

And we may need the "elements-dir ." to show gsch2pcb that we have
footprints in current directory. (Of course we should use dedicated
directories for symbols and footprints later...)

stefan@AMD64X2 ~/armin $ cat project.txt 
schematics Hauptplatine_v1.sch
output-name Hauptplatine_v1

elements-dir .

stefan@AMD64X2 ~/armin $ gsch2pcb project.txt 
=====================================================
gsch2pcb backend configuration:

   ----------------------------------------
   Variables which may be changed in gafrc:
   ----------------------------------------
   gsch2pcb:pcb-m4-command:    /usr/bin/m4
   gsch2pcb:pcb-m4-dir:        /usr/share/pcb/m4
   gsch2pcb:pcb-m4-confdir:    /etc/pcb
   gsch2pcb:pcb-m4-path:       /usr/share/pcb/m4  /etc/pcb
$HOME/.pcb  .
   gsch2pcb:m4-command-line:   /usr/bin/m4 -d  -I/usr/share/pcb/m4
-I/etc/pcb -I$HOME/.pcb -I. /usr/share/pcb/m4/common.m4 - >>
Hauptplatine_v1.new.pcb

   ---------------------------------------------------
   Variables which may be changed in the project file:
   ---------------------------------------------------
   gsch2pcb:use-m4:            yes

=====================================================
Using the m4 processor for pcb footprints
Rf: can't find PCB element for footprint RES-1016-630-240.fp
(value=4.7R)
So device Rf will not be in the layout.
R1: can't find PCB element for footprint RES-1016-630-240.fp
(value=3.92k_1%)
So device R1 will not be in the layout.
R2: can't find PCB element for footprint RES-1016-630-240.fp
(value=35.7k_1%)
So device R2 will not be in the layout.
C_Vcc: can't find PCB element for footprint
CAPPR-200P-500D-1100L-50d__Nichicon (value=4.7u)
So device C_Vcc will not be in the layout.
Db: can't find PCB element for footprint DO-41.fp (value=unknown)
So device Db will not be in the layout.

----------------------------------
Done processing.  Work performed:
5 file elements and 3 m4 elements added to Hauptplatine_v1.new.pcb.
5 elements could not be found.  So Hauptplatine_v1.new.pcb is
incomplete.

Next steps:
1.  Run pcb on your file Hauptplatine_v1.pcb.
2.  From within PCB, select "File -> Load layout data to paste buffer"
    and select Hauptplatine_v1.new.pcb to load the new footprints into
your existing layout.
3.  From within PCB, select "File -> Load netlist file" and select 
    Hauptplatine_v1.net to load the updated netlist.

4.  From within PCB, enter

           :ExecuteFile(Hauptplatine_v1.cmd)

    to update the pin names of all footprints.

stefan@AMD64X2 ~/armin $ 
stefan@AMD64X2 ~/armin $ locate -i RES-1016-630
stefan@AMD64X2 ~/armin $ 

Seems that footptints files are missing on my box, so it is difficult to
do further testing. Maybe this already helps.

You may try including this line "skip-m4" in your project.txt file to
ignore m4 files and problems with minus sign in footprint file names.
This works, because recent PCB program has copies of all old m4
footprints in newlib format. But it works not perfect, there is some
trouble with naming of footprint files. So it may be better to rename
your files, replacing the "-".

Best regards

Stefan Salewski
 




_______________________________________________
geda-user mailing list
geda-user@xxxxxxxxxxxxxx
http://www.seul.org/cgi-bin/mailman/listinfo/geda-user