Working with Connections on a Multi-board Schematic in Altium NEXUS

This documentation page references Altium NEXUS/NEXUS Client (part of the deployed NEXUS solution), which has been discontinued. All your PCB design, data management and collaboration needs can now be delivered by Altium Designer and a connected Altium 365 Workspace. Check out the FAQs page for more information.


Parent page: Capturing the Logical System Design

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 workspace), 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.

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).

This 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. Use the dialog’s option to include details of the literal Pin connections in the listing.

The dialog’s lower Conflict Resolution area will indicate any connection conflicts between the current Multi-board system design and source (child) projects during a design update, as outlined below.