[Author Prev][Author Next][Thread Prev][Thread Next][Author Index][Thread Index]

gEDA-user: Re: Composite/negative layers in gerbers

Paul Kube wrote:

> 1.  Composite layers.  Not 100% clear to me what OLIMEX means by this, 
> but they might mean that a layer appears to be defined across more than 
> one file.  (Compare 
> http://ecommerce.pcbfabexpress.com/faq.jsp#faq080105_3)  So, remove the 
> %LNCUTS*% layer name parameter lines, which seem not to be needed, and 
> otherwise make all layer names be unique across the gerber files.  

This is a little shell script that postprocesses the gerbers so that
they are accepted by Basista. It does does what you suggest:

===============================================
#!/bin/bash
# A little, dirty script to deal with the complains of Basista.
#  -<(kmk)>- Mar2006

if [[ $1  == -? ]] || [[ $1 == -h ]] || [[ $1 == --help ]] ; then
        echo "usage: basista"
        echo "This script postprocesses geda output with sed. It assumes
that there is a set Gerber files in the current directory"
        exit
fi

# determine the name of the PCB
PCBNAME=`basename *_front.gbr _front.gbr`
echo PCB-Name: $PCBNAME

# Move output from previous runs of the script to /tmp
mv Bas_$PCBNAME*.gbr /tmp
mv Bas_$PCBNAME*.cnc /tmp
mv Bas_$PCBNAME.zip /tmp

# no need to prses the *.cnc files
ln -s $PCBNAME"_plated-drill.cnc" "Bas_"$PCBNAME"_Loecher_metallisiert.cnc"
ln -s $PCBNAME"_unplated-drill.cnc"
"Bas_"$PCBNAME"_Loecher_unmetallisiert.cnc"

# individualize the layer names
sed s/LNGROUP/LN_INFO/ \
                $PCBNAME"_fab.gbr" > "Bas_"$PCBNAME"_info.gbr"

sed     -e 's/LNGROUP/LN_TOP/' \
        -e '/\%LNTRACKS/d' \
        -e '/\%LNCUTS/d' \
                $PCBNAME"_front.gbr" > "Bas_"$PCBNAME"_top.gbr"

sed s/LNGROUP/LN_TOPMASK/ \
                $PCBNAME"_frontmask.gbr" > "Bas_"$PCBNAME"_top_mask.gbr"

sed -e 's/LNGROUP/LN_TOP_OVERLAY/' \
        -e '/\%LNTRACKS/d' \
        -e '/\%LNCUTS/d' \
                $PCBNAME"_frontsilk.gbr" > "Bas_"$PCBNAME"_top_overlay.gbr"

sed  -e 's/LNGROUP/LN_BOTTOM/'  \
         -e '/\%LNTRACKS/d' \
         -e '/\%LNCUTS/d' \
                $PCBNAME"_back.gbr" > "Bas_"$PCBNAME"_bottom.gbr"

 sed s/LNGROUP/LN_BOTTOMMASK/ \
                $PCBNAME"_backmask.gbr" > "Bas_"$PCBNAME"_bottom_mask.gbr"

  sed s/LNGROUP/LN_LINEOUT/ \
                $PCBNAME"_group8.gbr" > "Bas_"$PCBNAME"_lineout.gbr"

  # zip it into one single file
 zip "Bas_"$PCBNAME".zip" Bas*.gbr Bas*.cnc

echo "done."
==================================



-- 
Kai-Martin Knaak
kmk@xxxxxxxxxxxx
Blog: http://lilalaser.de/blog

Attachment: signature.asc
Description: OpenPGP digital signature