# gschem2pcb README

    ------------------------------------------------------------------
    JM Routoure. routoure@greyc.ismra.fr
    17/01/2000

    I would like to thank Stefan Petersen for debuging the scheme program.

    -------------------------------------------------------------------

    This document describes how to install (section I) and use (section II) the
    gschem2pcb package. Section III describes some of the footprints
    available in pcb

    The purpose of this package is to interface gschem with pcb. It uses a scheme
    program and a script.

    Section I : Installation.

    1. Untar the gschem2pcb.tar. You must obtain 3 files gschem2pcb.sh,
    GNET-PCBboard.scm and the README file.

    2. Move gschem2pcb.sh in a directory which is in your PATH (/usr/local/bin for
    instance ). Be sure that gschem2pcb.sh can be executed (chmod 755 gschem2pcb.sh)

    3. Move GNET-PCBboard.scm in the share directory of your gEDA distribution.
    Normally, it should be /usr/local/share/gEDA/scheme.

    4. Modify the common.m4 file of the pcb program (should be found in
    /usr/X11R6/lib/X11/pcb/m4/) like this : the include keywords at the end of the
    file  must be replace by

    include(/usr/X11R6/lib/X11/pcb/m4/connector.inc)
    include(/usr/X11R6/lib/X11/pcb/m4/dil.inc)
    include(/usr/X11R6/lib/X11/pcb/m4/misc.inc)
    include(/usr/X11R6/lib/X11/pcb/m4/plcc.inc)
    include(/usr/X11R6/lib/X11/pcb/m4/to.inc)
    include(/usr/X11R6/lib/X11/pcb/m4/qfp.inc)

    5. Edit the ~/.gEDA/gschemrc file and be sure that the following line exists :
    (attribute-name "footprint")

    6. Be sure that grep, sed and gawk are installed. That's all..

    Section II : using gschem2pcb.

    1. With gschem, create a schematic. All the device you want to have in pcb must
    have a Uref attribute. The footprint that you want to use in pcb are indicated
    by the footprint attribute (see section III for the description of the footprint
    in pcb)

    Be careful that the attributes Uref, name, value and device must not contain
    space char.
    --------------------------------------------------------

    2. Save your work (ultralownoise.sch for instance -ambitious design!) and type in a shell

    	gschem2pcb.sh ultralownoise.sch.

    note : the gschem file must end by .sch

    Error messages will appear if some space characters are found in the
    attributes Uref, name, value and device and if the name of the footprint was not
    found. Warning, pcb files are created even if errors occur!

    - if  ultralownoise.pcb does not exist, it will be created. A netlist file
    ultralownoise.net will also be created. In pcb, load the pcb (load layout). All
    the footprints will appears at the top-left corner of the windows. Load the
    netlist (load netlist file) and type the key "w". Place the footprints and type
    "o" to optimize the rastnet. See the pcb documentation for details.

    - if  ultralownoise.pcb exists, a ultralownoise.new.pcb file should be
    created. It should contain only the new device that have been added in the
    schematic since the last save of the ultralownoise.pcb file. Use "load layout
    data to paste buffer" to include the new footprints in the pcb file. The nestlist
    file is also updated so read it again.

    Section III. Description of the name of the footprint in pcb.
    pcb uses macro to define the footprints. For DIL packages, for instance, 2
    arguments are used to indicate the number of pins and the width in mil of the
    footprint. In gschem the footprint attribute of a 300 mil width and 8 pins DIL
    is:
    DIL 8 300.
    Warning, for that attribute, you have to included the space char!

    In the following. I describe the footprint attribute that are to be used in
    gschem for the footprint avalaible in pcb. N stands
    for the number of pins, W the width in mil, L the length in mil and D the
    diameter in mil
    CONNECTOR ROWS COLS	# single connector
    DIN41_651LAY N		# DIN 41.651 laying
    DIN41_651STAND N	# DIN 41.651 standing
    SUBD_LAY_BASE N		# SUB-D connector laying
    SUBD_MALE_LAY_BASE N 	# SUB-D connector male laying
    SUBD_FEMALE_LAY_BASE N 	# SUB-D connector female laying
    DIL N W			# dual-inline standard
    D N			# dual inline with W=244
    DW N			# dual inline with W=419
    SD N			# SD (ZIP)
    MULTIWATT15		# 15 pins multiwatt footprint
    R025			# standard 1/4W resistor !now attributes
    SIL N			# SIL
    CSIL			# SIL package with a common pin
    QFP132			# QFP132 flat pack
    LED D			# standing LED
    DIODE_LAY L		# laying diode
    AXIAL_LAY L		# standard axial footprint
    CRYSTAL W		# crystal package
    OSC			# a can oscillator
    ISA8			# 8 bit ISA Slot card
    OVEN_OSC		# ovenized-oscillator package
    RADIAL_CAN W		# a radial capcitor package
    PLCC N			# pllc
    PLCC N add		# pllc with additionnal border add
    QFP N add		# qfp 	with additionnal border add
    No additional parameters for the to footprints
    TO3_90
    TO3_45
    TO5
    TO92
    TO126
    TO126LAY-WIDE
    TO126STAND-WIDE
    TO220
    TO220LAY-WIDE
    TO220STAND
    TO220STAND-WIDE