Altium Designer Documentation


Created: July 27, 2015 | Updated: April 11, 2017
Now reading version 17.1. For the latest, read: PlaceOffSheetConnector for version 21
Applies to Altium Designer versions: 15.1, 16.0, 16.1, 17.0 and 17.1

Parent page: Schematic Commands

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

Applied Parameters: OffSheetConnector=True


This command is used to place an Off Sheet Connector object onto the active document. An off sheet connector is an electrical design primitive. Off sheet connectors are used to connect nets across multiple schematic sheets that are descended from the same parent sheet symbol.

For detailed information about this object type, see Off Sheet Connector.


Off sheet connectors are available for placement in the Schematic Editor only, by:

  • Choosing Place » Off Sheet Connector from the main menus.
  • Right-clicking in the workspace and choosing Place » Off Sheet Connector from the context menu.


After launching the command, the cursor will change to a cross-hair and you will enter off sheet connector placement mode with an off sheet connector floating on the cursor:

  • Press Tab to open the Off Sheet Connector 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 name and press Enter to close the dialog.
  • If the off sheet connector requires rotation, press the Spacebar to rotate it in 90° steps. Press the X or Y keys to flip the off sheet connector along the X-axis or Y-axis respectively.
  • Position the off sheet connector so that its electrical hotspot (the end held by the cursor) touches the wire to which you want to connect it to, then click or press Enter to effect placement.
  • Continue placing further off sheet connectors, or right-click or press Esc to exit placement mode.
If the Net property of the off sheet connector is entered before it is placed and the value entered has a numeric ending, each subsequent off sheet connector 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 off sheet connectors only the Primary field applies, the Secondary field applies when the object has multiple fields, such as a Pin.


  1. It is important to remember that although there are times when an off sheet connector and a sub-divided sheet symbol can be useful, they do have limitations. They will not properly form automatic component classes and these need to be recreated manually in the PCB if you choose to use them.
  2. To successfully connect a particular net across two or more sheets, the off sheet connectors on each sheet must be assigned to the same net.
  3. Port Cross-References cannot be applied to off sheet connectors, therefore Ports should be used where possible.
  4. For information on how a placed off sheet connector object can be modified graphically, directly in the workspace, see Graphical Editing.
  5. While attributes can be modified during placement (Tab to bring up associated properties dialog), bear in mind that these will become the default settings for further placement unless the Permanent option on the Schematic – Default Primitives page of the Preferences dialog is enabled. When this option is enabled, changes made will affect only the object being placed and subsequent objects placed during the same placement session.


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: