What are Package Symbols

Package Symbols in PCB Editor have one, or more, Connect Pins, Pins with Pin Numbers. The Connect Pins in the Package Symbol have an exact match with the Pins defined in the Schematic Part in OrCAD Capture and are “what” get connected when routing the board. Some Package Symbols, typically connectors, may also have Mechanical Pins, Pins without Pin Numbers, that won’t be connected but are used to secure the component to the board.

Package Symbol requirements can be defined by a standard, IPC-7351, manufacturer’s data sheets, or specific manufacturing requirements. There are tools available, such as OrCAD Library Builder (additional product), that can assist with creating Package Symbols that meet the IPC-7351 standard. OrCAD Library Builder can also create STEP models for 3D representation. There are also some free sources, like Ultra-Librarian who also have a subscription service, that can assist in creating Package Symbols and others that provide calculators for standard Pin requirements and online Package Symbol resources.

Package Symbol Wizard

The Package Symbol Wizard can help to automate creation of some common Package Symbol types by creating the array of Pins from input parameters. Package Symbol types available from the Package Symbol Wizard are: DIP, through Pins along two sides; SOIC, surface mounted Pins along two sides; PLCC / QFP, surface mounted Pins on four sides; PGA / BGA, full, or partial, matrix of through hole, or surface mounted, Pins; TH Discrete, through Pin discrete component; SM Discrete, surface mounted Pin discrete component; SIP, single in line through hole, or surface mounted, Pins; ZIP, “zig-zag” through hole, or surface mounted, Pins. The selected Package Symbol type changes the parameters that the wizard prompts for. The wizard won’t cover every Package Symbol type but it may provide an efficient way to start a Package Symbol for subsequent editing.

Manually creating Package Symbols

Package Symbols can also be created manually. This can be to create specific Package Symbol details or, almost always, a requirement for creating connectors with keyed Pins.

Set the Units from Setup>Design Parameters, Design tab to match the units on the datasheet. The units used in the Package Symbol will be converted to match the units used in Board file when the Package Symbol is loaded into it.

The “area” occupied by the Package Symbol is defined with a Place Bound area, created on the subclass  Place_Bound_Top, or Place_Bound_Bottom, as required. This is called the “courtyard” in the IPC-7351 standard. A Max Height property can be assigned to the Place Bound area to define the Height of the Package Symbol above the surface of the board, this will be checked against any height restriction imposed by a Package Keepout area in the design. It is also possible to assign a Min Height property if there is space between the bottom of the component body and the board surface but this is rarely used with modern components. Assigning a Max Height property to a Place Bound in a Package Symbol will result in a “cube”, or “skyscraper”, view in the 3D canvas. A more realistic view can be obtained in the 3D canvas by mapping a STEP model to the Package Symbol. STEP models are readily available from mechanical CAD tools and internet sources like component manufacturer sites, distributor sites, and specialist CAD data sharing sites like http://3dcontentcentral.com and http://grabcad.com/. The default origin for STEP models is “body centre” so mapping between the origin in the STEP model and the mounting position for the Package Symbol is almost always required.

A Package Symbol requires, at least one, Ref Des “placeholder” defined from the available defaults in the Package Geometry Class: Silkscreen_Top, Assembly_Top or Display_Top (or _Bottom). The Text defined for the “placeholder” will be completely replaced by the Ref Des property imported from the netlist, the only purpose of the Text is to aid in locating a “default” position for the text. The Silkscreen Ref Des, if used, would conventionally be added outside of the body of the Package Symbol to be visible when the component is placed.

Saving Package Symbols

When the Package Symbol is saved a “dra” file of the name of the symbol is saved and the data is checked, if the checks pass, a “psm” file of the name of the symbol will also be saved. Typically, created Package Symbols would be saved to a “temporary” location and then checked before adding to any “master” library. Keep the “dra” and “psm” files together for any future editing.

All content Copyright 2022 Parallel Systems Ltd.