Parent page: Schematic Objects
A Bus is a polyline object that represents a multi-wire connection and is an electrical design primitive.
Buses are available for placement in the Schematic Editor only by:
After launching the command, the cursor will change to a cross-hair indicating Bus placement mode. Placement is made by performing the following sequence of actions:
When placing a Bus there are three 'manual' placement modes, two of which have corner direction options. The modes specify how corners are created when placing buses and the angles at which buses can be placed.
The fourth available Bus placement mode is 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. When enabled during the Shift+Spacebar selection cycle, the mode is indicated by a thick dotted line from the segment vertex to the cursor.
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.
Along with its snap to grid feature, the schematic editor also supports snapping to available electrical connections. When an object being placed, such as a Bus, falls within a definable snap distance of a valid electrical connection, the cursor will jump to that electrical 'Hotspot' (shown as a red cross).
Electrical Object Hotspot snapping is configurable in the General section of the Properties panel when in schematic Document Options mode.
The graphical editing method allows a placed Bus object to be selected directly in the workspace and its size and/or shape graphically changed.
When a Bus object is selected, the following editing handles are available:
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 List panel, with any changes appearing immediately on the schematic.
The following methods of non-graphical editing are available:
Panel page: Bus Properties
This method of editing uses the associated Properties panel mode to modify the properties of a Bus object.
During placement, the Bus mode of the Properties panel can be accessed by pressing the Tab key. Note that the panel includes a Vertices tab, where you can edit the individual vertices of the currently selected Bus object –
Index 1 is the first placed vertex.
After placement, the Bus mode of the Properties panel can be accessed in one of the following ways:
The Properties panel supports multiple object editing, where the property settings that are identical in all currently selected objects may be modified. When multiples of the same object type are selected manually, via the Find Similar Objects dialog or through a Filter or List panel, a Properties panel field entry that is not shown as an asterisk (
*) may be edited for all selected objects.
A List panel displays design object types from one or more documents in tabular format, enabling quick inspection and modification of object attributes.
Used in conjunction with appropriate filtering – by selecting object types (using the panel's Include options), or 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. The properties for all the listed objects may then be edited directly in the List panel.
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 object. 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 on 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 that allows an individual net to be 'ripped' out of a Bus (Place » Bus Entry).
It also allows a net to be ripped out of a Bus in the same location as another individual net is 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, a standard Wire connection can 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.