OrCAD Libraries can contain a mixture of one, or more, Schematic Parts and / or one, or more, Symbols. Parts and Symbols may be copied from the supplied libraries to form user libraries. Using the provided libraries “as is” for anything more than initial testing may not be reliable since the contents of the provided libraries may be updated.

Use File>New>Library to create a new Library and then, before adding any Schematic Parts, or Symbols, save the new Library to a known filename in a known location. Also don’t save any user data into the product installation directories since this may be overwritten if the installation is updated, or deleted it the installation is removed.

In the Part and Symbol editor, the “Place” toolbar gets reduced to placing Pin, Pin Array and graphical objects.

Schematic Parts in an OrCAD Schematic Part library comprise of a Package, the entire component and associated properties, like the PCB Footprint, and Parts, which are the graphical elements and associated properties. A simple part may have one Package and one Part but more complex, “split”, Packages will have multiple Parts. Schematic Parts can be split into multiple sections because it makes them more convenient to place, like splitting connector pins into sections, separating resistor packs into resistors, or splitting multiple function packages into individual functions.

Schematic Parts are created with a “Normal View” by default but there is the option to create a “Convert View”, basically a different set of graphics for the same Schematic Part.

Package Properties include: the Name of the part; the Part Reference Prefix; the Number of sections, and whether the sections should be identified with Alphabetic or Numeric.

Pin Properties include: Pin Name; Pin Number; Type; Pin Shape and  Pin Group. Pin Name and Pin Number are both used for the PCB Editor netlist, Pin Type is used by the Electrical Rule Checking; Pin Shape is the graphical appearance – Line occupies three large grids and Short occupies one large grid; Pin Group is used to enable pin swapping in PCB Editor.

For PCB Editor, any unused Pins on the PCB Footprint need to accounted for in the Schematic Part, there is an NC property which takes a comma separated list of Pin Numbers if all of the Pins are not added to the graphics for the part.

All content Copyright 2022 Parallel Systems Ltd.