Altium NEXUS Documentation

Bundling Multiple Nets into Buses & Signal Harnesses in Altium NEXUS

Created: April 25, 2022 | Updated: April 25, 2022
All Contents

Parent page: Creating Circuit Connectivity in Your Schematics

A common challenge in a large design is keeping the nets manageable. Not only from the perspective of the designer creating the connectivity but also from the perspective of the reader that has to interpret and understand the schematic. This is particularly important when connecting between sheets as this is when both the designer and the reader can most easily get confused.

This can be helped by bundling nets into Buses or Signal Harnesses.

Working with Buses

Buses are used to bundle a series of sequential nets, for example, an address bus or a data bus. Their core requirement is that each net in the bus is named with a common base name, followed by a numeric identifier, as shown in the images below. For example, the nets Control1, Control2 and Control3 can be bundled into the bus Control[1..3]. Buses cannot be used to bundle an unrelated set of nets, such as the nets Enable, Read and Status, Signal Harnesses are used to do this, as explained below.

To create a valid bus, it must include all of these elements (as shown in the images below):

  • A Net Label on each of the individual nets
  • A Net Label on the Bus line
  • A Port named the same as the Bus if it is leaving this sheet

All of the elements shown in the image above must be included to create a valid Bus. Bus Entries only need to be used if you want to rip different bus elements from both sides of the Bus. All of the elements shown in the image above must be included to create a valid Bus. Bus Entries only need to be used if you want to rip different bus elements from both sides of the Bus.
All of the elements shown in the image above must be included to create a valid Bus. Bus Entries only need to be used if you want to rip different bus elements from both sides of the Bus.

Buses are not transferred to the PCB, instead, a Net Class can be created for each schematic Bus, or if required, for each Bus section. A bus section is created by specifying a bus which is actually a section of a larger bus, for example, from the bus D[15..0]. If this option is enabled then the PCB will include a Net Class for the entire bus, as well as each section that has been defined. Enable the required options in the Class Generation tab of the Options for Project dialog.

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

Summary

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

Availability

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

  • Choosing Place » Bus from the Schematic Editor main menus.
  • Clicking the Bus button () in the net wiring objects drop-down on the Active Bar located at the top of the design space. Click and hold an Active Bar button to access other related commands. Once a command has been used, it will become the topmost item on that section of the Active Bar.
  • Clicking the  button on the Wiring toolbar (View » Toolbars » Wiring to activate).
  • Right-clicking and choosing Place » Bus from the context menu.

Placement

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:

  1. Click or press Enter to anchor the starting point for the Bus.
  2. Position the cursor then 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.

Placement Modes

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.

During placement:

  • Press the Tab key to pause the placement and access the Bus mode of the Properties panel from where its line properties can be changed on-the-fly. Click the design space pause button overlay () to resume placement.
  • Press Shift+Spacebar to cycle through the three manual modes: 90°, 45° and Any Angle.
  • While in the 90°or 45° mode (known as true orthogonal modes), press Spacebar to cycle between the corner direction options. In these modes, the line segment attached to the cursor is a look ahead segment – the actual segment being placed precedes this look-ahead segment.
  • During placement, the current placement mode is displayed in the Status bar (at the very bottom of the design space). You can change modes at any time during Bus placement.

 45 degree mode

 90 degree mode

Press Shift+Spacebar to cycle through the different placement modes. Any angle modePress Shift+Spacebar to cycle through the different placement modes.

Attributes modified during placement (by using Tab to access the Properties panel) will become the default settings for further placement unless the Permanent option on the Schematic – Defaults 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.

Automatic Path Mode

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.

Placing a Bus segment in Auto Wire mode, as indicated by the dotted path line. When placed (right), the Bus path will automatically avoid obstacles.Placing a Bus segment in Auto Wire mode, as indicated by the dotted path line. When placed (right), the Bus path will automatically avoid obstacles.

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.

Electrical Snap

Along with its snap to grid feature, the schematic editor also supports snapping to available electrical connections. When an object that is 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 blue cross).

The electrical snap point is indicated by a blue cross.The electrical snap point is indicated by a blue cross.

Electrical Object Hotspot snapping is configurable in the General section of the Properties panel when in schematic Document Options mode.

Graphical Editing

The graphical editing method allows a placed Bus object to be selected directly in the design space and its size and/or shape graphically changed.

When a Bus object is selected, the following editing handles are available:

Selected Bus, ready for graphical editing.Selected Bus, ready for graphical editing.

  • Click and drag a non-handle point to reposition the entire Bus. When a Bus is not selected, click, hold and drag to reposition it.
  • Click and drag A to reposition the end points of the Bus.
  • Click and drag B to move a Bus vertex. The other vertices will remain anchored.
  • 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.Individual segment sub-selection.

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

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. Click the locked object to select it then disable the Locked property in the List panel or disable the Protect Locked Objects option to graphically edit the object.

Non-Graphical Editing

The following methods of non-graphical editing are available.

Editing via the Bus Dialog or Properties Panel

Panel page: Bus Properties

This method of editing uses the associated Bus dialog and Properties panel mode to modify the properties of a Bus object.

 The Bus dialog, on the left, and the Bus mode of the Properties panel on the right

After placement, the Bus dialog can be accessed by:

  • Double-clicking on the placed bus object.
  • Placing the cursor over the bus object, right-clicking then choosing Properties from the context menu.

During placement, the Bus mode of the Properties panel can be accessed by pressing the Tab key. Once the bus is placed, all options appear.

After placement, the Bus mode of the Properties panel can be accessed in one of the following ways:

  • If the Properties panel is already active, by selecting the bus object.
  • After selecting the bus object, select the Properties panel from the Panels button in the bottom right section of the design space, or by select View » Panels » Properties from the main menu.

The Bus properties can be accessed prior to entering placement mode from the Schematic – Defaults page of the Preferences dialog. This allows the default line properties for the Bus object to be changed, which will be applied when placing subsequent Buses.

Editing Multiple Objects

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.

Editing via a List Panel

Panel pages: SCH List, SCH Filter

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.

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].

    While <StartingNumericalIdentifer> can be greater than <EndingNumericalIdentifier>, using two net labels on the same bus with ordering that is not in the same direction (ascending or descending), the Mismatched bus label ordering violation will occur when validating the project. The default report mode of this violation type is Warning.

Autojunctions

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.

Bus Entries

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.

Use Bus entries when the nets need to be ripped from both sides of the Bus.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 is compiled, this would be expanded to D20, D21 .. D27, which can potentially cause net name conflicts.

Schematic Editor object properties are definable options that specify the visual style, content and behavior of the placed object. The property settings for each type of object are defined in two different ways:

  • Pre-placement settings – most Bus object properties, or those that can logically be pre-defined, are available as editable default settings on the Schematic - Defaults page of the Preferences dialog (accessed from the  button at the top-right of the design space). Select the object in the Primitive List to reveal its options on the right.

  • Post-placement settings – all Bus object properties are available for editing in the Bus dialog and the Properties panel when a placed Bus is selected in the design space.

 

If the Double Click Runs Interactive Properties option is disabled (default) on the Schematic - Graphical Editing page of the Preferences dialog, when the primitive is double-clicked or you right-click on a selected primitive then choose Properties, the dialog will open. When the Double Click Runs Interactive Properties option is enabled, the Properties panel will open. 
While the options are the same in the dialog and the panel, the order and placement of the options may differ slightly. 
In the below properties listing, options that are not available as default settings in the Preferences dialog are noted as "Properties panel only".

Properties

  • ​Width - use the drop-down to select the desired width. 

Vertices (Properties panel only)  

This region is used to modify the individual vertices of the currently selected region object. You can modify the locations of existing vertices, add new vertices or remove them as required. Bus connections between vertex points can be defined and support is also provided for exporting vertex information to and importing from a CSV-formatted file. 

  • Vertices Grid - lists all of the vertex points currently defined for the object in terms of:
    • Index - the assigned index of the vertex (non-editable).
    • X - the X (horizontal) coordinate for the vertex. Click to edit.
    • Y - the Y (vertical) coordinate for the vertex. Click to edit.
  • Add - click to add a new vertex point. The new vertex will be added below the currently focused vertex entry and will initially have the same X,Y coordinates as the focused entry. Click  to remove the currently selected vertex.

Bus Entries can be used to connect Wires to a Bus.Bus Entries can be used to connect Wires to a Bus.

Summary

A Bus Entry is an electrical design primitive that is used to connect a Wire to a Bus line. It has the ability to allow two different nets to connect to the same point on a Bus – if this was done using Wires, the two nets would short. If this capability is not required, bus entries do not need to be used.

Availability

Bus entries are available for placement in the Schematic Editor only by:

  • Choosing Place » Bus Entry from the main menus.
  • Clicking the Bus Entry button () in the net wiring objects drop-down on the Active Bar located at the top of the design space. Click and hold an Active Bar button to access other related commands. Once a command has been used, it will become the topmost item on that section of the Active Bar.
  • Clicking the  button on the Wiring toolbar (click View » Toolbars » Wiring to activate) .
  • Right-clicking then choosing Place » Bus Entry from the context menu.

Placement

After launching the command, the cursor will change to a cross-hair and you will enter Bus Entry placement mode.

  1. Click or press Enter to place a Bus Entry at the cursor position.
  2. Press Spacebar to rotate the Bus Entry counterclockwise (in increments of 90°) or press Shift+Spacebar to rotate clockwise.
  3. Press the X or Y keys while in placement mode to mirror the Bus Entry along the X-axis or Y-axis.
  4. Continue placing bus entries or right-click or press Esc to exit placement mode.

During placement, press the Tab key to pause the process and access the Bus Entry mode of the Properties panel from where its line properties can be changed on-the-fly. Click the design space pause button overlay () to resume placement.

Attributes modified during placement (via the Properties panel) will become the default settings for further placement unless the Permanent option on the Schematic – Defaults 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.

Graphical Editing

To move a Bus Entry, click and hold on it (the cursor will jump to the nearest electrical hotspot), then move it to the new location – connected Buses and Wires will remain attached. While moving the Bus Entry, use the X and Y keys to change the Bus Entry orientation on those axes.

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. Click the locked object to select it then disable the Locked property in the List panel or disable the Protect Locked Objects option to graphically edit the object.

Non-Graphical Editing

The following methods of non-graphical editing are available.

Editing via the Bus Entry Dialog or Properties Panel

Panel page: Bus Entry Properties

This method of editing uses the associated Bus Entry dialog and the Properties panel mode to modify the properties of a Bus Entry object.

The Bus Entry dialog, on the left, and the Bus Entry mode of the Properties panel on the right The Bus Entry dialog, on the left, and the Bus Entry mode of the Properties panel on the rightThe Bus Entry dialog, on the left, and the Bus Entry mode of the Properties panel on the right

After placement, the Bus Entry dialog can be accessed by:

  • Double-clicking on the placed bus entry object.
  • Placing the cursor over the bus entry object, right-clicking then choosing Properties from the context menu.

During placement, the Bus Entry mode of the Properties panel can be accessed by pressing the Tab key. Once the bus entry is placed, all options appear.

After placement, the Bus Entry mode of the Properties panel can be accessed in one of the following ways:

  • If the Properties panel is already active, by selecting the bus entry object.
  • After selecting the bus entry object, select the Properties panel from the Panels button in the bottom right section of the design space or by select View » Panels » Properties from the main menu.
The Bus Entry properties can be accessed prior to entering placement mode from the Schematic – Defaults page of the Preferences dialog. This allows the default line properties for the Bus Entry object to be changed, which will be applied when placing subsequent bus entries.

Editing Multiple Objects

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.

Editing via a List Panel

Panel pages: SCH List, SCH Filter

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.

Schematic Editor object properties are definable options that specify the visual style, content and behavior of the placed object. The property settings for each type of object are defined in two different ways:

  • Pre-placement settings – most Bus Entry object properties, or those that can logically be pre-defined, are available as editable default settings on the Schematic - Defaults page of the Preferences dialog (accessed from the  button at the top-right of the design space). Select the object in the Primitive List to reveal its options on the right.

  • Post-placement settings – all Bus Entry object properties are available for editing in the Bus Entry dialog and the Properties panel when a placed Bus Entry is selected in the design space.

           

If the Double Click Runs Interactive Properties option is disabled (default) on the Schematic - Graphical Editing page of the Preferences dialog, when the primitive is double-clicked or you right-click on a selected primitive then choose Properties, the dialog will open. When the Double Click Runs Interactive Properties option is enabled, the Properties panel will open. 
While the options are the same in the dialog and the panel, the order and placement of the options may differ slightly. 

Properties

  • Start (X/Y) 
    • X (first field) - the current X (horizontal) coordinate of the reference point of the object relative to the current design space origin. Edit to change the X position of the object. The value can be entered in either metric or imperial; include the units when entering a value whose units are not the current default. 
    • Y (second field) - The current Y (vertical) coordinate of the reference point of the object relative to the current origin. Edit to change the Y position of the object. The value can be entered in either metric or imperial; include the units when entering a value whose units are not the current default. 
  • End (X/Y) -
    • X (first field) - the current X (horizontal) coordinate of the reference point of the object relative to the current design space origin. Edit to change the X position of the object. The value can be entered in either metric or imperial; include the units when entering a value whose units are not the current default. 
    • Y (second field) - The current Y (vertical) coordinate of the reference point of the object relative to the current origin. Edit to change the Y position of the object. The value can be entered in either metric or imperial; include the units when entering a value whose units are not the current default. 
  • Size (X/Y) - the bus entry size.
  • Width - use the drop-down to select the desired width. 
  • Color - click the color box to select the desired color for the object.

Working with Signal Harnesses

Signal harnesses are highly flexible as they can be used to bundle any number of nets, buses and lower-level harnesses. As their name implies, they are analogous to a wiring harness, where any arrangement of wires can be bundled and routed through an electronic or electrical product. They are more complex to create and manage, but the reward is that they can greatly simplify the presentation of a schematic and enhance its readability.

Signal harnesses are used to bundle any combination of nets, buses, and lower-level signal harnesses.
Signal harnesses are used to bundle any combination of nets, buses, and lower-level signal harnesses.

The elements that make up a complete signal harness include:

  • Harness Connector - Think of a Harness Connector as a funnel, it gathers all of the signals that connect into this harness through the included Harness Entries. A key property of the Harness Connector is the Harness Type, this identifies the harness and is used to bind together the various elements that make up the signal harness, including the connected Ports / Sheet Entries.

    A placed Harness Connector A placed Harness Connector

    Summary

    A Harness Connector object is an electrical drawing primitive. It is essentially a container to group various signals together to form a Signal Harness including buses and wires. A Harness Connector is defined by the Harness Type.

    Availability

    Harness Connectors are available for placement in the Schematic Editor:

    • The following commands are available:
      • Click Place » Harness » Harness Connector from the main menus.
      • Click the Harness Connector button () in the graphic objects drop-down on the Active Bar located at the top of the design space. Click and hold an Active Bar button to access other related commands. Once a command has been used, it will become the topmost item on that section of the Active Bar.
      • Right-click in the design space then click Place » Harness » Harness Connector from the context menu.
      • Click the  button on the Wiring toolbar.
    A harness connector can also be defined textually in a Harness Definition File (*.Harness). Such a defined harness connector can be placed in the design using the Place » Harness » Predefined Harness Connector command from the main menus.
    Harness Definitions are automatically generated when a Harness Connector is constructed with Harness Entries. When the Harness Connector is modified, the corresponding Harness Definition is updated to reflect the modifications.
    The Harness Definition can be protected by manually locking the Harness Definition. This is achieved by typing Locked; before each Signal Harness Definition. This means that the Harness Definition will not be updated when the Harness Connector is modified and any new Harness Entries added to the schematics will not be added to the Harness Definition.
    If a Harness Definition is locked and a new Harness Entry is added to the graphical representation, the Conflicting Harness Definition violation will be displayed upon compilation.

    Placement

    After launching the command, the cursor will change to a cross-hair and you will enter Harness Connector placement mode. Placement is made by performing the following sequence of actions:

    1. Click or press Enter to anchor the tip of the Harness Connector.
    2. Move the cursor to adjust the size of the Harness Connector, then click or press Enter to anchor the corner and thereby complete placement of the Harness Connector.
    3. Continue to place other Harness Connectors or right-click or press Esc to exit placement mode.

    Additional actions that can be performed during placement while the harness connector is still floating on the cursor and before its tip is anchored are:

    • Press the Tab key to open the Harness Connector mode of the Properties panel from where properties for the harness connector can be changed on the fly.
    • Press the X or Y keys to mirror the harness connector along the X-axis or Y-axis respectively.

    While attributes can be modified during placement (Tab to open the Properties panel), keep in mind that these will become the default settings for further placement unless the Permanent option on the  Schematic – Defaults 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.

    Graphical Editing

    This method of editing allows you to select a placed harness connector object directly in the design space and change its size, shape or location graphically.

    When a harness connector object is selected, the following editing handles are available:

    A selected Harness Connector.

    • Click and drag A to resize the harness connector in the vertical and horizontal directions simultaneously.
    • Click and drag B to resize the harness connector in the vertical direction.
    • Click and drag C or anywhere on the harness connector away from editing handles to reposition it. While dragging, click the X or Y keys to mirror the harness connector along the X-axis or Y-axis.
    • The Harness Connector Type text for a harness connector object can be edited in-place by:
      1. Single-clicking the text to select it.
      2. Single-clicking again (or pressing Enter) to enter the in-place editing mode. Sufficient time between each click should be given to ensure the software does not interpret the two single-clicks as one double-click (which would open the Properties panel).
      3. To finish editing in-place text, press the Enter key or use the mouse to click away from the text.
    This feature is available only provided the Enable In-Place Editing option is enabled on the Schematic - General page of the Preferences dialog.
    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. Click the locked object to select it then disable the Locked property in the List panel or disable the Protect Locked Objects option to graphically edit the object. 

    Non-Graphical Editing

    The following methods of non-graphical editing are available.

    Editing via the Harness Connector Dialog or Properties Panel

    Panel page: Harness Connector Properties

    This method of editing uses the associated Harness Connector dialog and the Properties panel mode to modify the properties of a harness connector object.

     The Harness Connector dialog, on the left, and the Harness Connector mode of the Properties panel on the right

    After placement, the Harness Connector dialog can be accessed by:

    • Double-clicking on the placed harness connector object line.
    • Placing the cursor over the harness connector object line, right-clicking then choosing Properties from the context menu.

    During placement, the Harness Connector mode of the Properties panel can be accessed by pressing the Tab key. Once the harness connector is placed, all options appear.

    After placement, the Harness Connector mode of the Properties panel can be accessed in one of the following ways:

    • If the Properties panel is already active, by selecting the harness connector object.
    • After selecting the harness connector object, select the Properties panel from the Panels button in the bottom right section of the design space or select View » Panels » Properties from the main menu.

    The Harness Connector properties can be accessed prior to entering placement mode, from the Schematic - Defaults page of the Preferences dialog. This allows the default properties for the rectangle object to be changed, which will be applied when placing subsequent rectangles.
    If the Double Click Runs Interactive Properties option is disabled (default) on the Schematic - Graphical Editing page of the Preferences dialog, when the primitive is double-clicked or you right-click on a selected primitive then choose Properties, the dialog will open. When the Double Click Runs Interactive Properties option is enabled, the Properties panel will open. 
    While the options are the same in the dialog and the panel, the order and placement of the options may differ slightly. 

    Editing Multiple Objects

    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.

    Editing via a Panel

    Panel pages: SCH List, SCH Filter

    A List panel allows you 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 you to target and edit multiple design objects with greater accuracy and efficiency.

    Notes

    • By default, newly-placed Harness Connectors are given the Harness Type Harness.
    • The Harness Type can be hidden from view or moved to save space in your design. Click  in the Properties panel to hide the Harness Type.

    Schematic Editor object properties are definable options that specify the visual style, content and behavior of the placed object. The property settings for each type of object are defined in two different ways:

    • Pre-placement settings – most Harness Connector object properties, or those that can logically be pre-defined, are available as editable default settings on the Schematic - Defaults page of the Preferences dialog (accessed from the  button at the top-right of the design space). Select the object in the Primitive List to reveal its options on the right.

    • Post-placement settings – all Harness Connector object properties are available for editing in the Properties panel when a placed Harness Connector is selected in the design space.

                

    If the Double Click Runs Interactive Properties option is disabled (default) on the Schematic - Graphical Editing page of the Preferences dialog, when the primitive is double-clicked or you right-click on a selected primitive then choose Properties, the dialog will open. When the Double Click Runs Interactive Properties option is enabled, the Properties panel will open. 
    While the options are the same in the dialog and the panel, the order and placement of the options may differ slightly. 
    In the below properties listing, options that are not available as default settings in the Preferences dialog are noted as "Properties panel only".

    Location (Properties panel only) 

    • (X/Y)
      • X (first field) - the current X (horizontal) coordinate of the reference point of the object, relative to the current design space origin. Edit to change the X position of the object. The value can be entered in either metric or imperial; include the units when entering a value whose units are not the current default. 
      • Y (second field) - The current Y (vertical) coordinate of the reference point of the object, relative to the current origin. Edit to change the Y position of the object. The value can be entered in either metric or imperial; include the units when entering a value whose units are not the current default. 
    • Rotation - use the drop-down to select the rotation. 

    Properties

    • Harness Type - enter the name of the harness. Click the eye icon to show/hide harness name.
    • Bus Text Style - use the drop-down to select the style:
      • Full - select to show full identifiers of the connected buses in format <Name>[<StartingNumericalIdentifer>..<EndingNumericalIdentifier>] (for example, SW[0..7]).
      • Prefix - select to show only prefixes of connected buses in format <Name> (for example, SW).
    • Width - can be edited.
    • Height - can be edited.
    • Primary Position - can be edited.
    • Border - use the drop-down to select the default from the available choices.
    • Fill - click on the colored box to access a drop-down from which you can select the default color.

    Entries (Properties panel only)

    Use this region to manage the connector's associated harness entries.

    • Harness Entries Grid - the grid lists all of the harness entries currently defined for the harness connector.
    When a harness entry is physically connected to another signal harness (facilitating nested signal harnesses), it will automatically inherit that harness's type. 
    Standard multi-select techniques are supported (Ctrl+clickShift+click, click+drag). 
    • Add - click to add a new harness entry to the connector. The new entry will be added at the bottom of the list and given the default name of 0. Click  to delete the currently selected entry from the grid.
    • Font - click on the displayed font to change the font style in various ways.
  • Harness Entries - Each signal (net, bus or signal harness) that you want to be part of this signal harness, enters the Harness Connector through a Harness Entry. The Harness Entry includes a Harness Type property, this is only used when you are nesting signal harnesses - signifying that this Harness Entry has a lower-level signal harness connected to it.

    A placed Harness Entry
    A placed Harness Entry

    Summary

    A Harness Entry is an electrical design primitive that is placed within a Harness Connector. A Harness Entry is the connection point through which signals - through wires, buses, and other signal harnesses - are combined to form a higher-level Signal Harness. Signal Harnesses enable the logical grouping of different signals for increased flexibility and streamlined design.

    Availability

    Harness Entries are available for placement in the schematic editor only in the following ways:

    • Choose Place » Harness » Harness Entry from the main menus.
    • Click the  button on the Wiring toolbar.
    • Click the Harness Entry button () in the graphic objects drop-down on the Active Bar located at the top of the design space. (Click and hold an Active Bar button to access other related commands. Once a command has been used, it will become the top-most item on that section of the Active Bar.)
    • Right-click in the design space then choose Place » Harness » Harness Entry from the context menu.

    Harness entries can also be managed in the following non-graphical ways:

    • Added/edited/removed in the Entries region of the Harness Connector mode of the Properties panel. 
    • Added/edited/removed as part of the textual harness connector definition through a harness definition file (*.Harness). This defined harness connector can only be placed in the design using the Place » Harness » Predefined Harness Connector command from the main menus.
    Harness Definitions are automatically generated when a Harness Connector is constructed with harness entries. When the Harness Connector is modified, the corresponding Harness Definition is updated to reflect the modifications.
    The Harness Definition can be protected by manually locking the Harness Definition. This is achieved by typing Locked; before each Signal Harness Definition. This means that the Harness Definition will not be updated when the Harness Connector is modified; any new Harness Entries added to the schematics will not be added to the Harness Definition.
    If a Harness Definition is locked and a new Harness Entry is added to the graphical representation, the Conflicting Harness Definition violation will be displayed upon design validation.

    Placement

    After launching the command, the cursor will change to a cross-hair and you will enter harness entry placement mode. Placement is made by performing the following sequence of actions:

    1. Move the harness entry attached to the cursor over a placed harness connector on the sheet.
    2. Adjust the position of the harness entry in relation to the edge of the harness connector, opposite the connector's tip, then click or press Enter to anchor the harness entry and complete placement.
    3. Continue placing further harness entries or right-click or press Esc to exit placement mode.
    The coloring of the harness entry will aid in its correct placement. While outside of a harness connector, the entry will appear grayed out and you will be prevented from placing. When over a harness connector, the entry will revert to its true coloring, as defined by its color property indicating it can be placed at that location.

    While the harness entry is still floating on the cursor and while it is within the bounds of a harness connector, press the Tab key to pause the placement and access the Harness Entry mode of the Properties panel in which its properties can be changed on the fly. Click the design space pause button overlay () to resume placement.

    While attributes can be modified during placement (Tab to open the Properties panel), keep in mind that these will become the default settings for further placement unless the Permanent option on the Schematic - Defaults 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.

    Graphical Editing

    This method of editing allows you to select a placed harness entry object directly in the design space and change its location graphically.

    A selected Harness Entry
    A selected Harness Entry

    • Click and drag to reposition the harness entry vertically along the edge of its parent harness connector as required.
    • Hold Ctrl then click and drag the harness entry to move it from the current harness connector to another harness connector on the sheet. Once the harness entry has cleared the boundary of the source harness connector, the Ctrl key can be released.
    • Clicking and dragging the harness entry outside of the harness connector boundary will cause the harness connector to automatically resize to accommodate the entry's new location.
    • The name text for a harness entry object can be edited in-place by:
      1. Single-clicking the harness entry to select it.
      2. Single-clicking again (or pressing Enter) to enter the in-place editing mode. Sufficient time between each click should be given to ensure the software does not interpret the two single-clicks as one double-click.
      3. To finish editing in-place text, press Enter or use the mouse to click away from the harness entry.

        This feature is available only if the Enable In-Place Editing option is enabled on the Schematic - General page of the Preferences dialog.
    Multiple harness entries can be moved simultaneously. To do this, select all entries to be moved then click on one entry in the selection and drag the entire selection.
    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, that object cannot be selected or graphically edited. Click the locked object to select it then disable the Locked property in the List panel or disable the Protect Locked Objects option to graphically edit the object.

    Non-Graphical Editing

    The following methods of non-graphical editing are available.

    Editing via the Harness Entry Dialog or Properties Panel

    Properties page: Harness Entry Properties

    This method of editing uses the associated Harness Entry dialog and the Properties panel mode to modify the properties of a harness entry object.

    The Harness Entry dialog, on the left, and the Harness Entry mode of the Properties panel on the right The Harness Entry dialog, on the left, and the Harness Entry mode of the Properties panel on the right
    The Harness Entry dialog, on the left, and the Harness Entry mode of the Properties panel on the right

    After placement, the Harness Entry dialog can be accessed by:

    • Double-clicking on the placed harness entry object line.
    • Placing the cursor over the harness entry object line, right-clicking then choosing Properties from the context menu.

    During placement, the Harness Entry mode of the Properties panel can be accessed by pressing the Tab key. Once the harness entry is placed, all options appear.

    After placement, the Harness Entry mode of the Properties panel can be accessed in one of the following ways:

    • If the Properties panel is already active, by selecting the harness entry object.
    • After selecting the harness entry object, select the Properties panel from the Panels button in the bottom right section of the design space or select View » Panels » Properties from the main menu.
    If the Double Click Runs Interactive Properties option is disabled (default) on the Schematic - Graphical Editing page of the Preferences dialog, when the primitive is double-clicked or you right-click on a selected primitive then choose Properties, the dialog will open. When the Double Click Runs Interactive Properties option is enabled, the Properties panel will open. 
    While the options are the same in the dialog and the panel, the order and placement of the options may differ slightly.

    Editing via a List Panel

    Panel pages: SCH List, SCH Filter

    A List panel allows you 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 you to target and edit multiple design objects with greater accuracy and efficiency.

    Notes

    • A Harness Entry can be connected directly to a wire, a bus or a signal harness. The Harness Type field in the Harness Connector mode of the Properties panel is used when nesting signal harnesses. The field will auto-populate with the Harness Type of the connected signal harness.
    • If you need to negate (place a bar over the top of) a harness entry name, this can be done in two ways:
      • By including a backslash character after each character in the name (e.g., E\N\A\B\L\E\).
      • By enabling the Single '\' Negation option on the Schematic - Graphical Editing page of the Preferences dialog, then including one backslash character at the start of the name (e.g.,\ENABLE).

    Schematic Editor object properties are definable options that specify the visual style, content and behavior of the placed object. The property settings for each type of object are defined in two different ways:

    • Pre-placement settings – most Harness Entry object properties, or those that can logically be pre-defined, are available as editable default settings on the Schematic - Defaults page of the Preferences dialog (access from the  button at the top-right of the design space). Select the object in the Primitive List to reveal its options on the right.

    • Post-placement settings – all Harness Entry object properties are available for editing in the Harness Entry dialog and the Properties panel when a placed Harness Entry is selected in the design space.

    If the Double Click Runs Interactive Properties option is disabled (default) on the Schematic - Graphical Editing page of the Preferences dialog, when the primitive is double-clicked or you right-click on a selected primitive then choose Properties, the dialog will open. When the Double Click Runs Interactive Properties option is enabled, the Properties panel will open.
    While the options are the same in the dialog and the panel, the order and placement of the options may differ slightly.

    Properties

    • Harness Name – the name of the harness.
    • Harness Type – this field is used to specify a Harness Type for a particular signal harness system in the design. It is typically left blank when a wire or bus is connected to the harness entry, used only when another signal harness itself is connected. The Harness Type itself is defined either manually in the associated Harness Definition File, or as part of the properties of a Harness Connector. The associated drop-down lists all currently defined Harness Types detected across the source schematic documents of the active project.

      When the harness entry is physically connected to another signal harness (facilitating nested signal harnesses) it will automatically inherit that harness's type. The Harness Type field will populate with that harness's type, and become read-only.
    • Font – use the controls to select the font, font size, font color, and add any desired special characteristics to the font, such as bold, italics, and underlines.
  • Signal Harness line - The bus-like line that is placed to carry the signal harness across the sheet.

    A placed Signal Harness A placed Signal Harness

    Summary

    A Signal Harness is an electrical design primitive. It is an abstract connection that enables the logical grouping of different signals including buses, wires and other signal harnesses for increased flexibility and streamlined design. Signal Harnesses allow for the creation and manipulation of higher level abstract connections between sub-circuits in your PCB Projects. They allow for a more complex design within the same schematic design space, which increases the readability of designs and builds potential for reuse.

    Availability

    Signal harnesses are available for placement in the Schematic Editor in one of the following ways:

    • Choose Place » Harness » Signal Harness from the main menus.
    • Click the Signal Harness button () in the graphic objects drop-down on the Active Bar located at the top of the design space. (Click and hold an Active Bar button to access other related commands. Once a command has been used, it will become the top-most item on that section of the Active Bar.)
    • Right-click in the design space then choose Place » Harness » Signal Harness from the context menu.
    • Click the button on the Wiring toolbar.

    Placement

    After launching the command, the cursor will change to a cross-hair and you will enter signal harness placement mode. Placement is made by performing the following sequence of actions:

    1. Click or press Enter to anchor the starting point for the signal harness.
    2. Position the cursor then click or press Enter to anchor a series of vertex points that define the shape of the signal harness.
    3. After placing the final vertex point, right-click or press Esc to complete placement of the signal harness.
    4. Continue placing further signal harness objects or right-click or press Esc to exit placement mode.
    5. Use the Backspace or Delete keys to remove the last harness segment placed.

    Additional actions that can be performed during placement while the signal harness is still floating on the cursor and before its first corner is anchored are:

    • Press the Tab key to pause the placement and access the Signal Harness mode of the Properties panel from where its properties can be changed on the fly. Click the design space pause button overlay () to resume placement.

    Placement Modes

    When placing a signal harness there are three 'manual' placement modes, two of which have Start and End sub-modes. The mode specifies how corners are created when placing signal harnesses and the angles at which signal harnesses can be placed. During placement:

    • Press Shift+Spacebar to cycle through the 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 signal harness 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

    Press Shift+Spacebar to cycle through the different placement modes. Any angle mode Press Shift+Spacebar to cycle through the different placement modes.

    There is also an Auto Wire mode that 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 Signal Harness

    Schematics have a definable electrical grid that makes it easy to define electrical connections between objects. While placing a Signal Harness, when the Signal Harness falls within the electrical grid range of another electrical object, the cursor will snap to the fixed object and a Hot Spot (blue cross) will appear.

    Hot Spot (blue cross)Hot Spot (blue 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 in the General region of the Properties panel in Document Options mode (accessed when no objects are selected in the design space). 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.

    While attributes can be modified during placement (Tab to access the Properties panel), keep in mind that these will become the default settings for further placement unless the Permanent option on the Schematic - Defaults 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.

    Graphical Editing

    This method of editing allows you to select a placed signal harness object directly in the design space and change its size and/or shape graphically.

    When a signal harness object is selected, the following editing handles are available:

    A selected Signal Harness, ready for graphical editingA selected Signal Harness, ready for graphical editing

    • Click and drag A to reposition the end points of the signal harness.
    • Click and drag B to move a signal harness vertex. The end points will remain anchored.
    • Click and drag on a segment to grab that segment and reposition it. The end points and other vertices will remain anchored.
    • Right-click on a vertex point then choose the Edit Signal Harness Vertex n command to edit.
    • Click and hold on a vertex, then press Delete on the keyboard to remove that vertex.

    With the signal harness selected, click on a segment to individually select that segment. This harness 'sub-selection' is distinguished by the associated editing handles becoming red in color.

    Individual segment sub-selection Individual segment sub-selection

    The associated vertices for the segment can then be edited directly using the SCH List panel and any changes will appear immediately on the schematic.

    To move an entire signal harness, click and hold on the un-selected signal harness (or click and hold on the selected signal harness, away from vertices), 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. Click the locked object to select it then disable the Locked property in the List panel or disable the Protect Locked Objects option to graphically edit the object.

    Non-Graphical Editing

    The following methods of non-graphical editing are available.

    Editing via the Signal Harness Dialog or Properties Panel

    Properties page: Signal Harness Properties

    This method of editing uses the associated Signal Harness dialog and the Properties panel mode to modify the properties of a signal harness object.

     The Signal Harness dialog, on the left, and the Signal Harness mode of the Properties panel on the right

    After placement, the Signal Harness dialog can be accessed by:

    • Double-clicking on the placed signal harness object.
    • Placing the cursor over the signal harness object, right-click, then choose Properties from the context menu.

    During placement, the Signal Harness mode of the Properties panel can be accessed by pressing the Tab key. Once the signal harness is placed, all options appear.

    After placement, the Signal Harness mode of the Properties panel can be accessed in one of the following ways:

    • If the Properties panel is already active, by selecting the signal harness object.
    • After selecting the signal harness, select the Properties panel from the Panels button at the bottom right of the design space or select View » Panels » Properties from the main menu.
    If the Double Click Runs Interactive Properties option is disabled (default) on the Schematic - Graphical Editing page of the Preferences dialog, when the primitive is double-clicked or you right-click on a selected primitive then choose Properties, the dialog will open. When the Double Click Runs Interactive Properties option is enabled, the Properties panel will open.
    While the options are the same in the dialog and the panel, the order and placement of the options may differ slightly.
    The Signal Harness properties can be accessed prior to entering placement mode, from the Schematic - Defaults page of the Preferences dialog. This allows the default properties for the signal harness object to be changed, which will be applied when placing subsequent signal harnesses.

    Editing Multiple Objects

    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 SCH Filter or SCH List panel, a Properties panel field entry that is not shown as an asterisk (*) may be edited for all selected objects.

    Editing via a List Panel

    Panel pages: SCH List, SCH Filter

    A List panel allows you 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 you to target and edit multiple design objects with greater accuracy and efficiency.

    Autojunctions

    A T-junction in a signal harness 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 signal harness segment will be broken into two at the point where an autojunction is inserted. For example, when making a T-Junction, the perpendicular signal harness segment will be broken into two segments, one on each side of the junction. With this option disabled, the signal harness segment will remain unbroken at the junction.

    Working with Signal Harnesses

    The term Signal Harness is used to describe both the bus-like line that runs between a Harness Connector and a Harness Port and also the overall connectivity system created by these connected harness objects.

    The term Signal Harness is used to describe the bus-like line that runs between a Harness Connector and a Port, and also the harness connection system.The term Signal Harness is used to describe the bus-like line that runs between a Harness Connector and a Port, and also the harness connection system.

    Schematic Editor object properties are definable options that specify the visual style, content and behavior of the placed object. The property settings for each type of object are defined in two different ways:

    • Pre-placement settings – most Signal Harness object properties, or those that can logically be pre-defined, are available as editable default settings on the Schematic - Defaults page of the Preferences dialog (accessed from the  button at the top-right of the design space). Select the object in the Primitive List to reveal its options on the right.

    • Post-placement settings – all Signal Harness object properties are available for editing in the Signal Harness dialog and the Properties panel when a placed Signal Harness is selected in the design space.

                  

    If the Double Click Runs Interactive Properties option is disabled (default) on the Schematic - Graphical Editing page of the Preferences dialog, when the primitive is double-clicked or you right-click on a selected primitive then choose Properties, the dialog will open. When the Double Click Runs Interactive Properties option is enabled, the Properties panel will open. 
    While the options are the same in the dialog and the panel, the order and placement of the options may differ slightly. 

    In the below properties listing, options that are not available as default settings in the Preferences dialog are noted as "Properties panel only".

    Properties

    • Width - use the drop-down to select the default width from the available choices. Click on the color box to access a drop-down from which you can select the default color.

    Vertices (Properties panel only)

    • Grid - lists all of the vertex points currently defined for the object in terms of:
      • Index - the assigned index of the vertex (non-editable).
      • X - the X (horizontal) coordinate for the vertex. Click to edit.
      • Y - the Y (vertical) coordinate for the vertex. Click to edit.
    • Add - click to add a new vertex point. The new vertex will be added below the currently focused vertex entry and will initially have the same X, Y coordinates as the focused entry. Click  to remove the currently selected vertex.
  • Harness Type - A Harness Type is a set of Harness Entries. Each detected Harness Type is defined in a Harness Definition File, as described below. The Harness Type and its associated Harness Entries are essentially names of the containers that carry the nets, not the names of the nets themselves. To check the Harness Type value, hover the cursor over the object, for example, the Port, Sheet Entry, or Harness Connector.

    A Harness Connector Type
    A Harness Connector Type

    Summary

    A harness connector type is a child object of a harness connector. It is used to name the type of placed harness connector.

    Availability and Placement

    The harness connector type is automatically placed when the parent harness connector object is placed. It is not a design object that the user can directly place. When a harness type is initially placed, the harness connector type will appear as (*) until renamed.

    When you place a Harness Connector, you can specify the Harness Type by double-clicking on the Harness Connector object and populating the Harness Type field in the Properties panel or clicking directly on the Harness Connector Type field in the schematic design. By default, newly placed Harness Connectors are given the Harness Type Harness.
    The Harness Connector Type can be hidden from view or moved to save space in your design. Select the Harness Connector then open the SCH List panel and enable the Hide Harness Type option or double-click the Harness Connector Type object and disable the show/hide icon () option.

    Graphical Editing

    The harness connector type string can be edited graphically using what is known as in-place editing. To edit a harness connector type in-place, click once to select, pause for a second, then click a second time to enter edit mode. Once editing is complete, press Enter or click away from the string to exit in-place editing mode.

    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. Click the locked object to select it then disable the Locked property in the List panel or disable the Protect Locked Objects option to graphically edit the object.

    Non-Graphical Editing

    The following methods of non-graphical editing are available.

    Properties page: Harness Connector Type Properties

    This method of editing uses the associated Parameter dialog and the Properties panel mode to modify the properties of a harness entry object.

      The Parameter dialog, on the left, and the Parameter mode of the Properties panel on the right

    After placement, the Parameter dialog and the Parameter version of the Properties panel can be accessed by:

    • Double-clicking on the harness connector type name. When initially placed, the name will appear as * until renamed.
    • Placing the cursor over the harness connector type name, right-clicking then choosing Properties from the context menu.
    • If the Properties panel is already active, by selecting the harness connector type name.
    • After selecting the harness connector type object, select the Properties panel from the Panels button in the bottom right section of the design space or select View » Panels » Properties from the main menu.
    If the Double Click Runs Interactive Properties option is disabled (default) on the Schematic - Graphical Editing page of the Preferences dialog, when the primitive is double-clicked or you right-click on a selected primitive then choose Properties, the dialog will open. When the Double Click Runs Interactive Properties option is enabled, the Properties panel will open. 
    While the options are the same in the dialog and the panel, the order and placement of the options may differ slightly. 

    Editing via the Parameter Dialog or Properties Panel

    Panel page: Harness Connector Type Properties

    This method of editing uses the associated Parameter dialog and the Properties panel mode to modify the properties of a harness connector type object.

    The Parameter dialog, on the left, and the Parameter  mode of the Properties panel on the right The Parameter dialog, on the left, and the Parameter  mode of the Properties panel on the rightThe Parameter dialog, on the left, and the Parameter  mode of the Properties panel on the right

    After placement, the Parameter dialog can be accessed by:

    • Double-clicking on the placed harness connector type object line.
    • Placing the cursor over the harness connector type object line, right-clicking then choosing Properties from the context menu.

    During placement, the Parameter mode of the Properties panel can be accessed by pressing the Tab key. Once the harness connector is placed, all options appear.

    After placement, the Parameter mode of the Properties panel can be accessed in one of the following ways:

    • If the Properties panel is already active, by selecting the harness connector object.
    • After selecting the harness connector type object, select the Properties panel from the Panels button in the bottom right section of the design space or select View » Panels » Properties from the main menu.

    The Harness Connector properties can be accessed prior to entering placement mode, from the Schematic - Defaults page of the Preferences dialog. This allows the default properties for the rectangle object to be changed, which will be applied when placing subsequent rectangles.
    If the Double Click Runs Interactive Properties option is disabled (default) on the Schematic - Graphical Editing page of the Preferences dialog, when the primitive is double-clicked or you right-click on a selected primitive then choose Properties, the dialog will open. When the Double Click Runs Interactive Properties option is enabled, the Properties panel will open. 
    While the options are the same in the dialog and the panel, the order and placement of the options may differ slightly. 

    Editing via a List Panel

    Panel pages: SCH List, SCH Filter

    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.

    Schematic Editor object properties are definable options that specify the visual style, content and behavior of the placed object. The property settings for each type of object are defined in two different ways:

    • Pre-placement settings – most Harness Connector Type object properties, or those that can logically be pre-defined, are available as editable default settings on the Schematic - Defaults page of the Preferences dialog (access from the  button at the top-right of the design space). Select the object in the Primitive List to reveal its options on the right.

    • Post-placement settings – all Harness Connector Type object properties are available for editing in the Parameter dialog Properties panel when a Harness Connector Type is selected in the design space.

                  

    If the Double Click Runs Interactive Properties option is disabled (default) on the Schematic - Graphical Editing page of the Preferences dialog, when the primitive is double-clicked or you right-click on a selected primitive then choose Properties, the dialog will open. When the Double Click Runs Interactive Properties option is enabled, the Properties panel will open. 
    While the options are the same in the dialog and the panel, the order and placement of the options may differ slightly. 
    In the below properties listing, options that are not available as default settings in the Preferences dialog are noted as "Properties panel only".

    Location (Properties panel only)

    • (X/Y)
      • X (first field) - the current X (horizontal) coordinate of the reference point of the object, relative to the current design space origin. Edit to change the X position of the object. The value can be entered in either metric or imperial; include the units when entering a value whose units are not the current default. 
      • Y (second field) - The current Y (vertical) coordinate of the reference point of the object, relative to the current origin. Edit to change the Y position of the object. The value can be entered in either metric or imperial; include the units when entering a value whose units are not the current default. 
    • Rotation - use the drop-down to select the rotation. 

    Properties

    • Harness Connector - the harness connector associated with this object.
    • Name - displays the name.
    • Value - displays the actual filename text. Use the eye icon to show/hide the Value.​
    • Autoposition - check to enable auto-positioning, meaning that the text will remain in the chosen position as the component is moved and rotated.
    • Font - use the controls to configure the font, font size, color, and special settings such as bold and underlines.
    • Justification - select the desired justification of the text.
  • Harness Definition File - The software manages signal harnesses by recording the Harness Entries that are in each signal harness (Harness Type), in an ASCII Harness Definition File. The image below shows the syntax of a Harness Definition File, there is a line in the file for each Harness Type, which details the Harness Entries within that harness. A Harness Definition File is automatically created (and managed) for each schematic sheet that has Harness Connectors on it, you can find them in the \Settings folder in the project tree, as shown in the image below. If your design has had changes that impact the signal harnesses, the Harness Definition files are updated automatically. If a Harness Definition File is not present in the project folder, it is automatically re-created when the schematic sheet is opened (they can be deleted and will be automatically recreated if required).
  • Port + Sheet Entry - Like a Net or Bus, a Signal Harness can leave a sheet via a Port, and then connect to the higher level sheet through a matching Sheet Entry. Note that the software automatically changes the color of the Ports and Sheet Entries to show they are carrying a Signal Harness if the Sheet Entries and Ports use Harness Color option is enabled in the Schematic - Graphical Editing page of the Preferences dialog. Note also that the Port and Sheet Entry objects include a Harness Type property, this value is set automatically as you touch the Port to the Signal Harness line when you are placing the Port. For the Port on the schematic sheet where the Harness is defined (the Harness Connector is present) the Harness Type is automatically defined and is not editable. For a Port or Sheet Entry placed on a higher-level schematic sheet, it will be blank and editable, typically there is no need to manually set this. The assigned Harness Type can be checked at any time by hovering the cursor over the Port/Sheet Entry.

Harnesses definitions are stored in Harness Definition files, in the image above there are two signal harnesses defined: 1WB_Write_Read and JTAG.
Harnesses definitions are stored in Harness Definition files, in the image above there are two signal harnesses defined: 1WB_Write_Read and JTAG.

As mentioned, as well as a net or a bus, you can also wire a signal harness into a signal harness, creating what is referred to as nested signal harnesses. This situation is identified at the Harness Entry, which has its Harness Type property set to the value of the incoming signal harness.

As well as nets and buses, a signal harness can carry other signal harnesses.
As well as nets and buses, a signal harness can carry other signal harnesses.

In the previous image, the Stereo signal harness has been used twice. This is legitimate, as neither the signal harness nor the harness entries are used to identify the nets which that harness carries. You can re-use a signal harness anywhere in the design, use the Place » Harness » Predefined Harness Connector command to do this. The dialog includes options to include a Signal Harness line and a Port if required.

Existing signal harnesses can be re-used anywhere in the design, including on the same sheet to carry different nets.
Existing signal harnesses can be re-used anywhere in the design, including on the same sheet to carry different nets.

The elements that make up a signal harness are used by the design compiler to identify the nets that belong in that signal harness so that the individual logical connections carried between sheets can be resolved. Signal harness elements are not used to name the nets, this is done using the standard net naming methods already discussed.

This behavior can be overridden if required. The nets within a signal harness can be given a harness-level name, by placing a Net Label on the Signal Harness line. If this is done, then the original Net Label is no longer used, instead, the net is named based on the Net Label placed on the Signal Harness line + the Harness Entry, in the form:

  • System-defined net name = NetNameOnSignalHarness.HarnessEntryName

The JTAG signal harnesses have harness-level names defined by the presence of the Net Labels SOFT and HARD. The system-generated net names are shown in the image below.

The 1WD_Write_Read signal harness does not have a harness-level name, so its nets will retain the names from the Net Labels.
The JTAG signal harnesses have harness-level names defined by the presence of the Net Labels SOFT and HARD. The system-generated net names are shown in the image below.
The 1WD_Write_Read signal harness does not have a harness-level name, so its nets will retain the names from the Net Labels.

In the image above, each instance of the JTAG harness has a Net Label placed on the Signal Harness line, namely HARD and SOFT. Because this harness-level net name has been added, the net labels on the nets within these harnesses are just used to create the local connections within this sheet. The nets are automatically assigned a name using the naming syntax shown above, as can be seen in the image of the Navigator panel, below. 

Note the naming of the JTAG nets, derived from the harness Net Label and the Harness Entries.
Note the naming of the JTAG nets, derived from the harness Net Label and the Harness Entries.

PCB Net Classes can also be created for named signal harnesses, enable the option in the option in the Class Generation tab of the Project Options dialog. Net classes are only created for signal harnesses that are named by a Net Label.

An advantage of naming the nets in a signal harness by placing a Net Label on the Signal Harness line (as described in the previous section), is that it also allows you to work with signal harnesses without needing to include a Harness Connector and Harness Entries on the schematic sheet. Some designers prefer this approach as it results in a cleaner and simpler schematic, as shown in the image below, where the JTAG signal harness does not use a Harness Connector.

Note that this technique requires there to be at least one Harness Connector of that Harness Type somewhere in the design, or alternatively, the harness definition must be LOCKED in the Harness Definition file. This keyword prevents the software from removing it when the Harness Definition files are automatically updated. The syntax for locking a definition is shown in the image below.

Like signal harnesses that use Harness Connectors, a connector-free signal harness must be declared in one of the Harness Definition files for a schematic that it is used on.

Its declaration must include the LOCKED keyword, to ensure the software does not remove it or modify it.
Like signal harnesses that use Harness Connectors, a connector-free signal harness must be declared in one of the Harness Definition files for a schematic that it is used on.
Its declaration must include the LOCKED keyword, to ensure the software does not remove it or modify it.

Found an issue with this document? Highlight the area, then use Ctrl+Enter to report it.

Contact Us

Contact our corporate or local offices directly.

We're sorry to hear the article wasn't helpful to you.
Could you take a moment to tell us why?
200 characters remaining
You are reporting an issue with the following selected text
and/or image within the active document: