Parent page: Schematic Objects

A Bus is a polyline object that is used, in conjunction with other objects, to define the connection of multiple nets.


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 clicking Home | Circuit Elements |  from the main menus.


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:

  1. Click or press Enter to anchor the starting point for the bus.
  2. Position the cursor and click or press Enter to anchor a series of vertex points that define the shape of the bus.
  3. After placing the final vertex point, right-click or press Esc to complete placement of the bus.
  4. Continue placing further bus objects, or right-click or press Esc to exit placement mode.
  5. Use the Backspace or Delete keys to remove the last bus segment placed. If you do remove segments in this way, you must click to place a final segment, otherwise right-clicking will place the bus as it was, with all deleted segments reinstated.

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.

Placement Modes

When placing a bus there are 3 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:

  • 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 bus 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.

Graphical Editing

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:

Selected Bus, ready for graphical editing.

  • Click and drag A to reposition the end points of the bus.
  • Click and drag B to move a bus vertex. The end points will remain anchored.
  • Click and drag on a bus 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 Bus Vertex n command to access the Vertices tab of the Bus dialog, with the entry for the nth vertex selected ready for editing.
  • Click and hold on a bus 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.

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.

Individual segment sub-selection.

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

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

An object that has its Locked property enabled cannot be selected or graphically edited. Double click on the locked object directly and disable the Locked property, to graphically edit the object.

Non-Graphical Editing

The following methods of non-graphical editing are available:

Via an Associated Properties Dialog

Dialog page: Bus

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

Edit the properties of the Bus in the Bus dialog.

The dialog can be accessed during placement by pressing the Tab key.

After placement, the dialog can be accessed in one of the following ways:

  • Double-clicking on the placed Bus object.
  • Placing the cursor over the Bus object, right-clicking and choosing Properties from the context menu.
The Bus dialog includes a Vertices tab, where you can edit the individual vertices of the currently selected bus object.

Via the SCH Inspector Panel

Panel page: SCH Inspector

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 the Find Similar Objects dialog, the panel can be used to make changes to multiple objects of the same kind, from one convenient location.

Understanding Bus Connectivity

A bus is used to bundle any number of nets. To do this, the following conditions must be met:

  • Each individual net must be identified by a net label.
  • The individual nets must be named using the standard naming pattern <Name><NumericalIdentifer1>, <Name><NumericalIdentifer2>, for example Address0, Address1, ..., Address n.
  • The bus that the individual nets join must be identified by a net label, in the format <Name>[<StartingNumericalIdentifer>..<EndingNumericalIdentifier>], for example Address[7..0], or LED[1..8].


A T-junction in a bus is automatically connected by a junction.

Bus Entries

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.

Use bus entries when the nets need to be ripped from both sides of the bus.

It is recommended that net labels in a bus only contain alpha characters. For example, if you named the bus D2[0..7], when the design was compiled this would be expanded to D20, D21 .. D27 which can potentially cause net name conflicts.


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