Altium Designer Documentation

Bus

Modified on Apr 11, 2017

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.

Summary

A bus is an electrical design primitive. It is a polyline object that represents a multi-wire connection.

Availability

Buses are available for placement in the Schematic Editor only, by:

  • Choosing Place » Bus from the Schematic Editor main menus.
  • Clicking the  button on the Wiring toolbar.
  • Right-clicking and choosing Place » Bus from the context menu.

Placement

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.

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 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:

  • 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.

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 of a Bus

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.

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 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, or SCH List 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.

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.

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 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:

  • Double-clicking on the placed Bus object.
  • Placing the cursor over the Bus object, right-clicking and choosing Properties from the context menu.
  • Using the Edit » Change command and clicking once over the placed bus object.
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 pages: SCH Inspector, SCH Filter

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.

Via the SCH List Panel

Panel pages: SCH List, SCH Filter

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.

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].

Autojunctions

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.

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.

 

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: