Working with Connections

Now reading version 22. For the latest, read: Working with Connections for version 24
Applies to Altium Designer version: 22

The connections established between modules in the schematic ultimately represent the connectivity between child project connectors, connector pins, and nets in the overall system design. The multi-board schematic editing environment provides comprehensive features that may be used to define, modify, check and update that connectivity as the overall product design is developed.

Connecting Child projects

To complete the process of creating and connecting Child Project Modules together, place a logical Connection between the Module Entries.

A range of connection types is available from the editor's Place menu or the Active Bar (at the top of the design space), including Direct Connection and Wire, which refer to connectors that plug together or are wired together, respectively. Click and drag the connection line between the Module Entry points to create the logical connectivity. Note that all elements in the system schematic editor, including Entry objects, can be dragged to a new location.

The following types of connections are available:

  • A Direct Connection is used whenever the connector on one board is to plug in directly to the connector on another board, without the use of a physical connection (wire, cable, or harness).
  • A Wire is a physical connection, providing a conduit for a single signal between two boards in a multi-board system, and whereby that wire is attached directly into a connector on each of those boards. Although placing a single wire on the document, in reality a series of wires will be used, in accordance with the number of signals/pins being connected between the connectors of the two boards.
  • A Cable is a physical connection, providing a conduit for net signals between two boards in a multi-board system, and whereby that cable plugs into a connector on each of those boards.
  • A Harness is a physical connection, providing a conduit for net signals between two boards in a multi-board system, and whereby that harness plugs into a connector on each of those boards.

Select a Connection graphic in the workspace to see its details, such as the included Nets and Pin connections, in the Properties panel.

Split Connections

In design situations where a child project connector serves more than one connected project, the source connector can be logically divided (in terms of pins/nets) using the multi-board schematic editor’s Split feature – in practice, one module is connected to two other modules.

An example of such a design would be where a single header plug on a PCB is intended to accommodate two smaller header sockets, which, in turn, connect to two other PCBs – the sectioned signals from a single (e.g., 20-pin) connection are distributed to a (e.g., 10-pin) connection one PCB and a (10-pin) connection on another PCB.

To split a connection, select the Module and then an Entry in the Properties panel. Select the button, and in the subsequent Split Entry dialog, check the listed pin Pin/Net combinations you want to separate (split off) to another Entry. Use the button to confirm the selections.

The editor will automatically create a new Module Entry for the separated Pins/Nets, which can then be connected to a different Module as required.

In the example shown, Entry HDR6 on Module M1 is intended to connect to both Module M2 (a panel LCD display) and Module M3 (a power supply board). The HDR6 Entry connections have been split to logically separate out three power Nets that will connect to HDR3 on power supply Module M3. This creates an additional HDR6 Entry on M1 (HDR6 [1-2,15]) that offers just the three power connections for M3, while the original HDR6 Entry is automatically reassigned to offer the remaining 17 connections, which ultimately connect to HDR1 on the LCD Module M2.

Select a Connection in the workspace to see its constituent Nets in the Properties panel. Here, one section of the (split) HDR6 Nets is connected to HDR3 through the wire connection W-PS, which represents the three power lines between the Main Board (M1) and Power Supply (M3). As shown in the image below, each virtual wire listed in the panel’s Connections area also includes its Entry name, Pin and Net at either end in the From and To columns.

Note that along with a connection's Designator, the wire name (#) and local Net name (Net) for each entry in the Connections list can be edited for convenience. These names are local to the Multi-board system design and do not affect the source Child Projects.

Edit Connections

The connections between Child Project Modules are not necessarily a pin-to-pin match, particularly when a connector is split in sections that are wired to different PCB Modules.

To edit or correct the Pin/Net matches between a Module interconnection, select the Connection in the workspace and then change the From/To assignments as required in the Properties panel’s Connections list entries.

Use the From or To drop-down list to select a new Net assignment, and therefore a different end-to-end signal relationship through that individual connection or wire, within the Module-to-Module connection.

Connection Manager

The overall connectivity in a Multi-board design, once established, is detailed in the Connection Manager dialog (Design » Connection Manager).

The upper region of the dialog lists all Net/Pin assignments grouped under their parent Connection Designators and type (Wire, Direct, etc.,), and includes their system design ID and Net Name, along with their From and To Pin/Net connections. Controls are available to quickly toggle the listing between showing all connections (Show Connections) and showing only changes that have been made (Show Changes Only). Use the dialog’s Show Mated Pins button to toggle the inclusion of details for literal Pin connections in the listing.

The Net information shown in the highlighted fields in the listing represents the proposed change.
Use the Clipboard button to quickly copy selected connection entries, including the headers (ID, Net Name, etc.,), for pasting into a text document or spreadsheet. Click the Report button to generate a report (*.xlsx) of the current connections.

The Connection Manager will highlight any connections that are considered as in Conflict, or in practice, any imported connection update that does not agree with the system design editor’s existing connectivity data map. Select a highlighted Net entry in the upper listing to see a graphic representation of the Conflict in the dialog's lower, Conflict Resolution region, and to access a range of button options that can be used to resolve it.

The Net information shown in the highlighted fields in the Connection Manager listing represents the proposed change. In the example case shown here, the Nets on HDR1 pins 4 and 5 in the Child Project (LCD Module) are in a different order – in fact, they have been swapped.

The Connection Manager will interpret this change and offer appropriate correction action buttons on the Conflict Resolution graphic. The options include:

  • Confirm – The Nets on Pins 4 and 5 for the HDR1 connector in Module M2 will be changed in the system design to match the updated assignments (as highlighted) in the dialog.
  • Revert – The current Net to Pin relationship for HDR1 in Module M2 will be retained. The proposed change is ignored by the system design. Note that the system design will then not match the net assignments in the child design(s).
  • Swap Pins – The Pin/Net assignments at the other end of the connection (at HDR6 on M1, the main board PCB) will be changed to maintain a correct Net relationship between the two Modules (M1 and M2).
  • Swap Wires - The virtual wires that connect between HDR1 on M2 and HDR6 on M1 will be changed (swapped in this case) to correct the Net connectivity conflict, and the connector Pin/Net assignments will not be changed. Here, wire W2 would then connect between Pin 4 on HDR6 and Pin 5 on HDR1, and W3 connect between Pins HDR6-5 and HDR1-4.
The Conflict Resolution options that are available will depend on the type of connection that is selected. The Swap Wires option, for example, will not be offered for a Direct Connection between Module Entries, where the PCBs are directly plugged together rather than wired together.

When a conflict resolution option has been selected, an affirmative answer in the following Confirmation dialog will cause the conflict resolution action to be applied to all conflicts of the same type.

The corrected Net assignments will be highlighted in green and also reflected in the dialog's lower connection graphic. Select the button to apply the updated assignments to the Multi-board system design.

Note that the Net Name values shown in the dialog are not changed when a Conflict is resolved since they represent the Net names in the local System Design. These names are automatically created when a connection is initially placed between Module Entries and may be changed at any time by editing that connection (or Wire, etc.,) in the Properties panel

Once the Conflict Resolution changes have been applied, they can be inspected in the Properties panel when the relevant connection is selected in the system design space.

In the Properties panel image shown below, the example conflict for the W-LCD connection was resolved using the Swap Wires option. This has effectively crossed over wires W2 and W3 so that the correct Net continuity is maintained, i.e the Reset and Read/Write Nets are matched between project Modules (LCD_RW# RSW and LCD_RS# RS, respectively).

Note

The features available depend on your level of Altium Designer Software Subscription.

Content