Contact our corporate or local offices directly.
Parent page: Schematic Objects
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.
Wires are available for placement in the Schematic Editor only, by:
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:
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:
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 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.
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:
nthvertex selected ready for editing.
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.
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.
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).
The following methods of non-graphical editing are available:
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 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:
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.
A 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.
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.
Contact our corporate or local offices directly.
Complete this form to request a free 15 day trial of Altium Designer: