Working with an Off Sheet Connector Object on a Schematic Sheet in Altium Designer | Altium Designer 17.1 User Manual

Using Altium Documentation

Created: July 27, 2015 | Updated: November 27, 2017

Now reading version 17.1. For the latest, read: Off Sheet Connector for version 21

Applies to Altium Designer versions: 15.1, 16.0, 16.1, 17.0 and 17.1

Contents

Summary
Availability
Placement
Graphical Editing
Non-Graphical Editing

All Contents

Parent page: Schematic Objects

Off Sheet Connectors are used to create connections between schematic sheets.

Summary

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.

Availability

Off sheet connectors are available for placement in the Schematic Editor only, by choosing Place » Off Sheet Connector from the main menus.

Placement

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.

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.

Graphical Editing

The off sheet connector can be edited graphically, using what is known as in-place editing. To edit an off sheet connector 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 Off Sheet Connector can be edited in-place.

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

This feature is only available provided the Enable In-Place Editing option is enabled, on the Schematic – General page of the Preferences dialog.

If attempting to graphically modify an object that has its Locked property enabled, a dialog will appear asking for confirmation to proceed with the edit. If the Protect Locked Objects option is enabled on the Schematic – Graphical Editing page of the Preferences dialog, and the Locked option for that design object is enabled as well, then that object cannot be selected or graphically edited. Double click on the locked object directly and disable the Locked property or disable the Protect Locked Objects option, to graphically edit the object.

Off sheet connectors do not have independent font properties, they use the Document Font properties (also referred to as the System Font) of the schematic sheet they are placed on. Double-click in the sheet border to edit the Document Options, including the font.

Non-Graphical Editing

The following methods of non-graphical editing are available:

Via an Associated Properties Dialog

Dialog page: Off Sheet Connector

This method of editing uses the Off Sheet Connector dialog to modify the properties of an off sheet connector object.

The Off Sheet Connector dialog.

The Off Sheet Connector 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 off sheet connector object to be changed, which will be applied when placing subsequent off sheet connectors.

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 off sheet connector object.
Placing the cursor over the off sheet connector object, right-clicking and choosing Properties from the context menu.
Using the Edit » Change command and clicking once over the placed off sheet connector 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.