Electronics Forum / CAD / January 2006

The 050 is the pin pitch in mils, .001 inches.  The 8 means it has 8
pads for an 8 pin part.  WG is the width of the gull-wing leads; be sure
to find a foot print with a larger number here than the TI spec sheet
shows for the maximum width of the part.  L is the length of the molded
body of the part; this really only affects the silk-screen, place
outline, etc. of the foot print, so be sure to use foot print with the
same or larger length than the actual part.  Note that similar packages
from different vendors can have different dimensions.  Foot prints that
have their basic dimensions specified in mm instead of inches, usually
have an "m" in the numbers.

You will be advised by others, and I would second that advice, to learn
to make your own foot prints, or at least to check the Orcad supplied
foot prints carefully against the vendors recommended layout.  It is not
that hard.  Foot prints are made in the Library Manager of the Layout
package.

I am not sure about CaptureCIS 10.5, I use CaptureCIS 7.2, but the
Capture package needs to know how to find the footprint libraries
(separate from the schematic symbol libraries) in order to display the
foot print when selecting parts from the database.  This was/is done by
creating a layout.ini file with the Layout package that contains all the
foot print libraries you want to use, and then copying the layout.ini
file from the Layout installation directory to the Capture installation
directory.

The pads in the foot print need to extend farther than the maximum
spread of the leads.

I am not familiar with that part, so I don't know if it has a standard
8-pin opamp pinout, but you can use any library symbol that looks good
to you and that contains numbered pins for every pin you want connected
on the layout.  The only information transfered from the schematic
symbol to the layout is the pin numbering information that is used to
create the netlist.  The netlist is what transfers information about the
schematic to Layout.  It makes no difference what the name of the symbol
is, so long as the pin numbers match the functions, AND there is a foot
print available that matches the pin numbers to the right physical pins
on the package (SOT-23 and TO-92 packages, amongst others, are often
numbered in conflicting ways by various vendors, so be careful about
this).  If you don't like the look of the available symbol, and there is
no standard available, make your own.  I rarely use any Orcad supplied
symbols, except for simple things like standard gates and op-amps.

Note that there is other information in the netlist for each part, such
as the name of the footprint to be loaded (but which can be overridden
once the design is in layout), the "value" of the part, the reference
designator, etc.