Default report mode:
This violation occurs when a conflict exists in the connectivity between two connected boards in the system.
A notification is displayed in the Messages panel in the following format:
Unresolved conflict exists: Net "<OldModuleNetName>" has been renamed to "<NewModuleNetName>" for "Pin <ConnectorDesignator-PinNumber>" in child project "Module <ModuleDesignator>(<ChildProjectName>)"
OldModuleNetName – is the name of the net associated with the indicated pin of the connector on the child design project, currently held in the Multi-board Schematic editor’s existing connectivity data map.
NewModuleNetName – is the name of the net now associated with the indicated pin of the connector on the child design project, after importing changes made to that child project.
ConnectorDesignator-PinNumber – is the designator of the connector component in the child design represented by the module's entry, and the pin of that connector.
ModuleDesignator – is the designator of the module on the Multi-board Schematic that is used to reference the child design project.
ChildProjectName – is the name, including extension, of the child project referenced by the module.
Recommendation for Resolution
This violation typically arises when a change has been made in relation to the connector in one child project, and when that change is imported back to the Multi-board Schematic document, it will break the existing connectivity defined between two connected boards. For example, the nets assigned to two pins of the connector might have been swapped in one child project, meaning that there is now a mismatch when following those pins through to another target board's connector.
Use the Connection Manager dialog to view unresolved conflicts. The Connection Manager dialog listing will highlight any connections that are considered as in Conflict, or in practice, any imported connection update that does not agree with the Multi-board Schematic editor’s existing connectivity data map. Click the Show Changes Only button to see just the conflicting pins/nets of the relevant connection(s). Select a highlighted Net entry in the list to see a graphic representation of the Conflict and to access a range of button options that can be used to resolve it. The options include:
- Confirm – the module nets on the pins for the connection in the Multi-board Schematic design document will be changed to match the updated assignments as shown in the dialog (the changes that were made in the child project).
- Revert – the current net to pin relationship for the connection in the Multi-board Schematic design document 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 will be changed to maintain a correct net relationship between the two modules that reference the connected boards.
- Swap Wires – the virtual wires that connect between the entries of the two modules (referencing the connected boards) will be changed (swapped) to correct the net connectivity conflict, and the connector pin/net assignments will not be changed.
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 Apply Changes button to apply the updated assignments to the Multi-board Schematic. If the resolution choice results in changes required to a child project, use the Design » Update Child Projects command to do this.