Working with a Net Label Object on a Schematic Sheet in Altium Designer

Parent page: Schematic Objects

Net labels identify and electrically connect different points in a schematic.

Summary

Electrical connectivity between schematic component pins can be created by placing a wire between those pins. This is called physical connectivity, as the pins are physically  connected with a wire. Connectivity can also be created logically by using suitable net identifiers, such as net labels. As well as providing a human-friendly identifier for a net, a net label allows you to connect points on a circuit without actually physically wiring them together.

Availability

Net labels are available for placement in the Schematic Editor only, by:

• Choosing Place » Net Label from the Schematic Editor main menu.
• Clicking the  button on the Wiring toolbar.

Placement

After launching the command, the cursor will change to a cross-hair and you will enter net label placement mode with a net label floating on the cursor:

• Press Tab to open the Net Label dialog, the Net property will be the active control in the dialog and the existing text selected ready for editing, simply type in the new net name and press Enter to close the dialog.
• If the net label requires rotation, press the Spacebar to rotate it in 90° steps. Press the X or Y keys to flip the net label along the X-axis or Y-axis respectively.
• Position the net label so that its bottom-left corner touches the object to which you want to assign it, then click or press Enter to place the net label.
• Continue placing further net labels, or right-click or press Esc to exit placement mode.

Considerations during placement:

• The electrical hotspot on a net label is the lower left corner, this corner must touch the wire, bus, or signal harness for a valid connection to be made.
• If the Net property of the net label is entered before it is placed and the value entered has a numeric ending, each subsequent net label will auto-increment this numeric value. This behavior is configured in the Auto-Increment During Placement options on the Schematic - General page of the Preferences dialog. For net labels only the Primary field applies, the Secondary field applies when the object has multiple fields, such as a Pin.

Graphical Editing

The net label can be edited graphically, using what is known as in-place editing. To edit a net label string in-place, click once to select, pause for a second, then click a second time to enter edit mode.

 Click once to select the string

 Pause, then click a second time to enter in-place edit mode.

 Here the string has been selected, ready to type in a replacement string.

The Net Label can be edited in-place.

Once editing is complete, press Enter or click away from the string to exit in-place editing mode.

Non-Graphical Editing

The following methods of non-graphical editing are available:

Via an Associated Properties Dialog

Dialog page: Net Label

This method of editing uses the Net Label dialog to modify the properties of a net label object.

The Net Label dialog.

The Net Label dialog can be accessed prior to entering placement mode, from the Schematic – Default Primitives page of the Preferences dialog. This allows the default properties for the net label object to be changed, which will be applied when placing subsequent net labels.

During placement, the dialog can be accessed by pressing the Tab key.

After placement, the dialog can be accessed in one of the following ways:

• Double-clicking on the placed net label object.
• Placing the cursor over the net label object, right-clicking and choosing Properties from the context menu.
• Using the Edit » Change command and clicking once over the placed net label object.

Via the SCH Inspector Panel

Panel pages: SCH Inspector, SCH Filter

The SCH Inspector panel enables the designer to interrogate and edit the properties of one or more design objects in the active document. Used in conjunction with appropriate filtering - by using the SCH Filter panel, or the Find Similar Objects dialog - the panel can be used to make changes to multiple objects of the same kind, from one convenient location.

Via the SCH List Panel

Panel pages: SCH List, SCH Filter

The SCH List panel allows the designer to display design objects from one or more documents in tabular format, enabling quick inspection and modification of object attributes. Used in conjunction with appropriate filtering - by using the SCH Filter panel, or the Find Similar Objects dialog - it enables the display of just those objects falling under the scope of the active filter – allowing the designer to target and edit multiple design objects with greater accuracy and efficiency.

Tips

1. Net labels create logical connectivity within a single schematic sheet, they do not create connectivity between schematic sheets. To do this, Ports must be used.
2. To negate (include a bar over the top of) a net label, use one of the following methods:
   1. Include a backslash character after each character in the net name (e.g. E\N\A\B\L\E).
   2. Enable the Single '\' Negation option on the Schematic - Graphical Editing page of the Preferences dialog, then include one backslash character at the start of the net name (e.g. \ENABLE).
3. When individual nets form a bus, there are specific requirements as to how they are named. For more information refer to the Bus page.
4. Net identifiers of different types do not automatically connect to one another even if they share the same name. For example a net label named AGND will not automatically connect to a power port named AGND, a wire must be placed to connect them.