Altium NEXUS Documentation


Created: June 7, 2017 | Updated: May 6, 2020
Now reading version 3.2. For the latest, read: PlaceNetLabel for version 5
Applies to altium-nexus versions: 1.0, 1.1, 2.0, 2.1, 3.0, 3.1, 3.2 and 4
This documentation page references Altium NEXUS/NEXUS Client (part of the deployed NEXUS solution), which has been discontinued. All your PCB design, data management and collaboration needs can now be delivered by Altium Designer (with Altium Designer Enterprise Subscription) and a connected Altium 365 Workspace. Check out the FAQs page for more information.

Parent page: Schematic Commands

The following pre-packaged resource, derived from this base command, is available:

Applied Parameters: None


This command is used to place a Net Label object onto the active document. 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.

For detailed information about this object type, see Net Label.


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

  • Choosing Place » Net Label from the Schematic Editor main menu.
  • Locating and using the Net Label command () on the Active Bar.
If the command has been recently used from the Active Bar, it will become the active/visible button. Where other commands are available, this is indicated by a triangle at the bottom-right corner of the button. Click and hold on the active button to access a menu of all associated commands for that grouping.
  • Clicking the  button on the Wiring toolbar.
  • Right-clicking in the workspace and choosing Place » Net Label from the context menu.


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 the Tab key to access the Properties panel, from where properties for the net label can be changed on-the-fly, including the Net Name. Pressing Tab pauses placement, allowing you to interact with the panel (or other area of the software) directly. To resume, click the pause symbol that appears over the workspace.
  • 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 Name 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.


  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.
  5. For information on how a placed net label object can be modified graphically, directly in the workspace, see Graphical Editing.
  6. While attributes can be modified during placement (Tab to bring up the Properties panel), bear in mind that these will become the default settings for further placement unless the Permanent option on the Schematic - Defaults page of the Preferences dialog is enabled. If this option is enabled, the default properties of all object types are locked and are not changed if you edit an object's properties during placement. If this option is disabled, any changes you make to a particular object during placement (by pressing the Tab key while the object is floating on the cursor before placement to open the Properties panel) are used to update the default properties for that particular object type.


Found an issue with this document? Highlight the area, then use Ctrl+Enter to report it.

Contact Us

Contact our corporate or local offices directly.

We're sorry to hear the article wasn't helpful to you.
Could you take a moment to tell us why?
200 characters remaining
You are reporting an issue with the following selected text
and/or image within the active document: