Altium Designer Documentation

Wire

Modified by Susan Riege on Apr 11, 2017

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, by:

  • Choosing Place » Wire from the Schematic Editor main menus.
  • Clicking the  button on the Wiring toolbar.

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 and 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.

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.

Placement Modes

When placing a wire there are 3 'manual' placement modes, 2 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

Press Shift+Spacebar to cycle through the different placement modes.

There is also an Auto Wire mode, which can be used to route quickly from the previous segment end, to the point where the cursor is clicked, using the Point to Point Router. The path of the route will be the most efficient possible, while avoiding existing placed objects on the sheet. Press Tab while in this mode to configure applicable options in the Point to Point Router Options dialog.

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.

Hot Spot (red cross).

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 Sheet Options tab of the Document Options dialog (Design » Document Options). It is recommended that you set the electrical grid to be slightly smaller than the current snap grid, or it becomes 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:

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 and 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.
To move an entire wire, click and hold on the un-selected wire, then move to the new location.
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.

Additonal Information About Dragging

  • 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 Inspector or SCH List panel, with any changes appearing immediately on the schematic.

You can also perform surgeon-like 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).

Considering a T-junction, which is formed of three wire segments and a junction, removal of one wire segment will result in the removal of the junction. The remaining two wire segments will simply be merged to form a single segment.

Delete selected track segments, including attached autojunctions where applicable, with a press of the Delete key.

A wire segment can also be removed through use of the Break Wire feature, with the Cutting Length option set to Snap To Segment.

Non-Graphical Editing

The following methods of non-graphical editing are available:

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.

The Wire 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 wire object to be changed, which will be applied when placing subsequent wires.

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 Wire object.
  • Placing the cursor over the Wire object, right-clicking and choosing Properties from the context menu.
  • Using the Edit » Change command and clicking once over the placed wire object.
The Wire dialog includes a Vertices tab, where you can edit the individual vertices of the currently selected wire object.

Via an Inspector Panel

Panel pages: SCH Inspector, SCHLIB Inspector, SCH Filter, SCHLIB Filter

An 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 applicable 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 a List Panel

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

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 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 the designer 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.

English
If you'd like to comment on the content on this page, use the Ctrl+Enter keyboard shortcut to send us your feedback. To include a section of the page in your comment (a typo, missing/wrong info, or incorrect imagery), highlight the text (max. 200 chars) and/or image first. Please restrict your feedback to documentation issues - for technical assistance refer to the Altium Forums.

Contact Us

Contact our corporate or local offices directly.

You are reporting an issue with the following selected text and/or image within the active document:
Request Free Trial

Complete this form to request a free 15 day trial of Altium Designer: