Placing off-page connectors

Off-page connectors provide connections between schematic pages within the same schematic folder. An off-page connector is connected by name to other off-page connectors within the same schematic folder.

Like-named off-page connectors in different schematic folders are not connected.
The Select Entire Net command is restricted to the active schematic page—it does not follow hierarchical blocks, hierarchical ports, or off-page connectors across schematic folders or schematic pages. For more information, see Tracing a net.
Remember that nets on a schematic page are electrically connected by name, by alias, or by connection to a named hierarchical port or off-page connector.
To connect an off-page connector to a bus, name the off-page connector with the same name and range as that of the bus. For example, to connect an off-page connector to a bus named ABC[0:3], name the off-page connector as ABC[0:3].

To connect schematic pages laterally (within the schematic folder)

From the Place menu, choose Off-Page Connector.
Select a symbol (standard or user-created), enter a name, and choose OK.
Place the symbol anywhere on the schematic page.
Repeat steps 1 through 3 for the other schematic pages (within the same schematic folder) that you wish to connect.
The size of a part or a symbol is limited to 32 by 32 inches.

To create a hierarchical port or off-page connector

Open the library that will hold the new symbol.
From the Design menu, choose New Symbol. The New Symbol Properties dialog box appears.
Enter a name and select off-page connector or hierarchical port as the symbol type, then click OK. The part editor opens with an empty part boundary box.
Use the graphics tools to create the symbol. The symbol dimensions expand automatically to accommodate the graphics.
From the File menu, choose Save. If you are creating the symbol in a new library that has not yet been saved, the Save As dialog box appears, giving you the opportunity to name the library file.

If you edit a library provided by OrCAD, it is important that you assign a new library name so that your changes are not overwritten when you upgrade or update your software.
When you save a project, Capture automatically creates a backup with a .DBK file extension. When you save a library, Capture automatically creates a backup with a .OBK file extension. If you save only a schematic page or a part, no backup is generated.