Performing Design Updates to Your Captured Multi-board System in Altium Designer

To maintain synchronization between a multi-board schematic design and the child PCB projects it includes, the multi-board design supports the bidirectional exchange of pin/net data. Connectivity data can be imported into the multi-board design from child projects, and the multi-board design connectivity data may be passed back to the source PCB projects.

Importing from Child Projects

During the course of a multi-board design, it is likely that the source child projects will also be developed, and those changes need to be brought into (synchronized with) the multi-board design. This update process is achieved by re-importing the child design(s) into the multi-board design space via an Engineering Change Order (ECO). This exchange of pin/net data enables the connectivity data between the multi-board design and its constituent boards to be kept in sync.

Use the Design » Import From Child Projects command from the main menus or the design space's right-click menu to import changes from all child projects in the multi-board design, or the Design » Import From Selected Child Projects alternative to re-import the connection data for the project modules that are currently selected in the design space. These commands are also available from the right-click Design menu of a module graphic.

Any differences that are detected between the current multi-board design connectivity and the connection data in the child project(s), will be presented in the Engineering Change Order dialog. Use the ECO to validate and ultimately execute the required changes that will bring the child boards back into sync with the multi-board design.

If there are no differences, a comparator alert dialog will indicate such and, by implication, that no changes are required to maintain the multi-board design to child project synchronization.

The executed ECO will register any differences between the current multi-board design connectivity and the connection data that has been imported from the child project(s). This information is available in the Connection Manager dialog (Design » Connection Manager), which is also used to resolve or reject the updated connection data from the child project(s).

Updating Child Projects

The multi-board design connectivity data can be passed back to the source PCB projects through the child project Update feature (Design » Update Child Projects). To update an individual child project, select its associated module and choose the Design » Update Selected Child Projects command – both commands are also available on a module's right-click Design menu.

When the command is run, the design editor compares the connectivity data in the multi-board design with that in the child projects. Any differences that are detected will be listed as proposed changes in a following Engineering Change Order (ECO) dialog, or a comparator alert dialog will indicate that no differences have been encountered – and by implication, that no changes are required to maintain the multi-board design to child project synchronization.

In the example shown here, where the RS and RSW nets have been swapped on connector HDR1 in the LCD Board child project (M2 in the multi-board design), the ECO proposes a pin swap in the source project to synchronize the nets.

When the ECO is executed (after optional validation), the HDR1 connector pins in the LCD module child project are swapped.

Note that the Update Child Projects process would normally be performed after any conflicts have been resolved in the Connection Manager dialog, so as to synchronize the child projects to the correct state of the multi-board design.

Other detected and resolved changes, such as a mismatched net name are synchronized by a direct update to the target in the child project.