Power and ground symbols

When you place a part that has power and ground pins, the power and ground pins of the part are automatically connected to like-named global power and ground nets of the schematic folder. This happens because, when you place the part, the power and ground pins of the part are assigned a net name that is the same as the pin name. If you need to isolate one power or ground pin from the others, you can assign it a unique net name.
Power and ground pins are invisible and global by default. This means that they are connected, on a project -wide basis, to all pins, power objects, and nets of the same name.
If you need to isolate a power or ground net, do one of the following:

make the pin visible and connect it to another net or power object
display the invisible power pin and connect it to a net or power object

For information on making power pins visible and on displaying invisible power pins, see Making power pins visible.

To place power or ground symbols

From the Place menu, choose Power
OR
Ground.
The Place Power or Place Ground dialog box appears.
In the Place Power dialog box, select a power symbol and click OK.
OR
In the Place Ground dialog box, select a ground symbol and click OK.
Use the mouse to move the symbol to the appropriate location and click. The symbol appears in the selection color.
Select the selection tool, or press Esc, to dismiss the power or ground tool.
Click an area where there are no parts or objects to deselect the symbol.

To place DC ground (‘0’) symbols in your PSpice designs, see Placing PSpice ground 0 symbols for PSpice simulations.

Shortcut

Tool palette:

To rotate power or ground symbols

Select the symbol.
From the Edit menu, choose the Rotate command. The symbol rotates 90 degrees counterclockwise.
Repeat step 2 as necessary.
Click an area where there are no parts or objects to deselect the symbol.

To create a power or ground symbol

Open the library that is to hold the new symbol, and select the library in the project manager.
From the Design menu, choose the New Symbol command. The New Symbol dialog box appears.
Enter a name and select Power 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 part boundary box dimensions change to accommodate the graphic elements.

To isolate a power net to a schematic folder

Place a power symbol and attach it to a hierarchical port.

To isolate a power net to a schematic page

Place a power symbol and attach it to an off-page connector.
When Capture resolves net name conflicts, the name of the off-page connector takes precedence over the name of the power object, and the scope of the off-page connector is limited to the schematic folder. All pins on the same page that are connected by name or by wire to the power symbol are connected to the isolated power net.
For example, say you want to isolate your analog and digital grounds and then connect them at one point when you make a printed circuit board. You place your analog circuitry on a separate schematic folder. On each page in the analog schematic folder, you place a ground symbol with the name GND. This implicitly connects all the pins named GND to ground. Then you connect that power symbol to an off-page connector named AGND. To connect AGND to the digital ground (GND), you can create a part whose footprint is a strip of copper with two pads, GND and AGND.