Search In: Doc:Documentation: NEXUS Client
Altium DesignerAltium 365Altium MCAD CoDesignerAltium On-Prem Enterprise ServerAltium CircuitMakerAltium CircuitStudioCompany DashboardAltium Infrastructure Server
Ver: Version: 4
43.23.13.02.12.01.11.0
Close
Suche Search on Documentation

WorkspaceManager_Err-UnresolvedConflictUnresolved Conflict_AD

Created: August 03, 2021 | Updated: August 03, 2021 | Applies to version: 4

This document is no longer available beyond version 4. Information can now be found here: Unresolved Conflict for version 5

Nexus message

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 category: Violations Associated with Connections

Default report mode:

Summary

This violation occurs when a conflict exists in the connectivity between two connected boards in the system.

Compiler violations associated with Multi-board Design projects are only presented after running an Electrical Rules Check from the project's Multi-board Schematic document (*.MbsDoc). Do this by choosing the Design » Run ERC command from the main menus.

Notification

If compiler errors and warnings are enabled for display on the schematic (enabled on the Schematic - Compiler page of the  Preferences dialog), an offending object will display a colored squiggle beneath it. Hovering over the object will display a pop-up hint that summarizes the violation. 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>)"

where:

  • OldModuleNetName - is the name of the net associated to 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 to 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.
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 Direction 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 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.

Tip

  • Object hints will only appear provided the Enable Connectivity Insight option is enabled on the System - Design Insight page of the Preferences dialog. Use the controls associated with the Object Hints entry in the Connectivity Insight Options region of the page to determine the launch style for such hints (Mouse Hover and/or Alt+Double Click). 
If you find an issue, select the text/image and pressCtrl + Enterto send us your feedback.
Content