Working with a Wire Object on a Schematic Sheet in Altium Designer

Parent page: Schematic Objects

Wires are used to create electrical connectivity in a schematic.

Summary

A wire is a polyline electrical design primitive that is used to form electrical connections between points on a schematic. It is analogous to a physical wire.

Availability

Wires are available for placement in the Schematic Editor only in the following ways:

• Choose Place » Wire from the main menus.
• Click the Wire button () in the drop-down on the Active Bar located at the top of the workspace. (Click and hold an Active Bar button to access other related commands. Once a command has been used, it will become the topmost item on that section of the Active Bar).
• Click the  button on the Wiring toolbar.
• Right-click in the workspace then choose the Place » Wire command from the context menu.​

Placement

After launching the command, the cursor will change to a cross-hair and you will enter wire placement mode. Placement is made by performing the following sequence of actions:

1. Click or press Enter to anchor the starting point for the wire.
2. Position the cursor then click or press Enter to anchor a series of vertex points that define the shape of the wire.
3. After placing the final vertex point, right-click or press Esc to complete placement of the wire.
4. Continue placing further wire objects or right-click or press Esc to exit placement mode.
5. Use the Backspace or Delete keys to remove the last wire segment placed.

Placement Modes

When placing a wire, there are three 'manual' placement modes, two of which have Start and End sub-modes. The mode specifies how corners are created when placing wires and the angles at which wires can be placed. During placement:

• Press Shift+Spacebar to cycle through the 90 Degree, 45 Degree and Any Angle modes.
• While in the 90 Degree or 45 Degree mode (known as true orthogonal modes), press Spacebar to cycle between the Start and End sub-modes.
• During placement, the current placement mode is displayed in the Status bar. You can change modes at any time during wire placement.
• In modes other than Any Angle, the line segment attached to the cursor is a look-ahead segment. The segment you are actually placing precedes this look-ahead segment.

 45 degree mode

 90 degree mode

 Any angle mode

Guided Wiring

Schematics have a definable electrical grid that makes it easy to define electrical connections between objects. As you are placing a wire, when the wire falls within the electrical grid range of another electrical object, the cursor will snap to the fixed object and a Hot Spot (red cross) will appear.

The Hot Spot guides you to where a valid connection can be made and automatically snaps the cursor to electrical connection points.

The electrical grid can be defined on the General tab of the Properties panel in Document Options mode. It is recommended that you set the electrical grid to be slightly smaller than the current snap grid or it can become difficult to position electrical objects one snap grid apart.

Graphical Editing

This method of editing allows you to select a placed wire object directly in the workspace and change its size and/or shape graphically.

When a wire object is selected, the following editing handles are available:

A selected Wire ready for graphical editing.

• Click and drag A to reposition the end points of the wire.
• Click and drag B to move a wire vertex. The end points will remain anchored.
• Click and drag on a wire segment to grab that segment and reposition it. The end points and other vertices will remain anchored.
• Right-click on a vertex point then choose the Edit Wire Vertex n command to access the Vertices tab of the Wire dialog with the entry for the nth vertex selected ready for editing.
• Click and hold on a wire segment then press Insert on the keyboard to add a vertex at that point.
• Click and hold on a vertex then press Delete on the keyboard to remove that vertex.

• When dragging objects connected by parallel wiring, stairs are created to minimize the creation of auto-junctions.
• While dragging, hotspots are used to provide visual indication of where auto-junctions are going to be created.
• Unnecessary/redundant auto-junctions are removed after dragging has ceased.

INDICATION OF NEW AUTO-JUNCTION CREATION

Depending on the affected wiring, performing a drag operation may result in the creation of auto-junctions at new locations. To provide visual feedback on where these new junction instances will be, hotspots are used. Enable the use of these hotspots and their color for wires and buses in the Auto-Junctions region on the Schematic - Compiler page of the Preferences dialog.

Selecting and Removing

With the wire selected, click on a segment to individually select that segment. This wire 'sub-selection' is distinguished by the associated editing handles becoming red in color.

Individual segment sub-selection.

The associated vertices for the segment can then be edited directly using the SCH List panel panel with any changes appearing immediately on the schematic.

You also can perform removal of selected wire segments with the tap of the Delete key. You can delete multiple segments across different wires - ensure that each is selected (Shift+click twice on each subsequent segment to include it in the overall segment selection). Auto-junctions are also accounted for - allowing you to remove a segment of a wire up to that junction only (and including that junction if only two other wire segments would otherwise remain connected to it).

Non-Graphical Editing

The following methods of non-graphical editing are available:

Via the Properties Panel

Properties page: Wire Properties

The properties of a Wire can be edited in the PCB editor's Properties panel, which allows editing of all item(s) currently selected in the workspace.

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

To access the properties of a placed Wire:

• Double-click on the Wire.
• Right-click on the Wire then select Properties from the context menu.
• If the Properties panel is already active, click once on the Wire to select it.

Via an Associated Properties Dialog

Dialog page: Wire

This method of editing uses the Wire dialog to modify the properties of a Wire object.

The Wire dialog can be accessed after placing a wire by right-clicking on a vertex point then choosing the Edit Wire Vertex n command.

Via a List Panel

Panel pages: SCH List, SCHLIB List, SCH Filter, SCHLIB Filter

A List panel allows you 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 applicable 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 you to target and edit multiple design objects with greater accuracy and efficiency.

Autojunctions

A T-junction in a wire is automatically connected by a junction (Compiler-Generated Junction). If the Break Wires At Autojunctions option is enabled on the Schematic - General page of the Preferences dialog, an existing wire segment will be broken into two at the point where an autojunction is inserted. For example, when making a T-Junction, the perpendicular wire segment will be broken into two segments, one on each side of the junction. With the Break Wires At Autojunctions option disabled, the wire segment will remain unbroken at the junction.