Parent page: Schematic Objects
A bus is an electrical design primitive. It is a polyline object that represents a multi-wire connection.
Buses 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 bus placement mode. Placement is made by performing the following sequence of actions:
When placing a bus there are 3 'manual' placement modes, 2 of which have Start and End sub-modes. The mode specifies how corners are created when placing buses and the angles at which buses 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 bus, when the bus 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 bus object directly in the workspace and change its size and/or shape, graphically.
When a bus object is selected, the following editing handles are available:
nthvertex selected ready for editing.
With the bus selected, click on a segment to individually select that segment. This bus '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.
The following methods of non-graphical editing are available:
Dialog page: Bus
This method of editing uses the Bus dialog to modify the properties of a Bus object.
The Bus 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 bus object to be changed, which will be applied when placing subsequent buses.
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:
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.
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.
A bus is used to bundle any number of nets. To do this, the following conditions must be met:
Address[7..0], or LED[1..8].
A T-junction in a bus is automatically connected by a junction (Compiler-Generated Juntion). If the Break Wires At Autojunctions option is enabled, on the Schematic - General page of the Preferences dialog, an existing bus segment will be broken into two at the point where an autojunction is inserted. For example, when making a T-Junction, the perpendicular bus segment will be broken into two segments, one each side of the junction. With this option disabled, the bus segment will remain unbroken at the junction.
A bus entry is a short, diagonal section of wire. A bus entry has a single function to perform, to allow an individual net to be ripped out of a bus at the same location another individual net is also ripped out of the bus, as shown in the image below. If a bus entry was not used in this situation, the two individual nets would connect together, creating a short-circuit. If it is not necessary to rip two individual nets from the same location on a bus, they do not have to be used.
Valid students can get their very own 6-month Altium Designer Student License for FREE! Just fill out the form below to request your Student License today.