Violations Associated with Connections when Validating a Design in Altium Designer

Default report mode:

Summary

This violation occurs when the name of the net associated with a connection on the Multi-board Schematic is not the same as the net associated with the corresponding pin of the connector on the child design project.

Notification

A notification is displayed in the Messages panel in the following format:

Net Name "<ConnectionNetName>" for connection "<ConnectionDesignator>" does not match with Net "<ConnectorPinNetName>" of "Pin <ConnectorDesignator-PinNumber>" in child project "Module <ModuleDesignator>(<ChildProjectName>)"

where:

• ConnectionNetName – is the name of the net (on the Multi-board Schematic) associated with the connection that connects from the indicated pin.
• ConnectionDesignator – is the designator of the connection.
• ConnectorPinNetName – is the name of the net associated with the indicated pin of the connector on the child design 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 the name of the net on the connector pin in one child project is different from that in the mated connector pin in another child project, i.e. the two boards being connected by a connection between the relevant parent modules on the Multi-board Schematic document.

Use the Connection Manager dialog to view the net names currently being used. The Net Name entry shows the name used for the connection on the Multi-board Schematic document. With the connection selected, this can also be seen visually in the Conflict Resolution area of the dialog. Where the connector pins have different nets associated with them in both child projects, the Net Name for the connection defaults to <FromPinNetName>/<ToPinNetName>. These net names are reflected in the Module Net fields for the From and To pins, respectively. Resolution can be in two ways:

• Use the Rename buttons in the Conflict Resolution area for both modules to quickly set the module net in each case to be the same as the net name for the connection. Then apply the changes and pass those changes back to the child projects using the Design » Update Child Projects command. The nets associated with the respective connector pins in those projects will be updated accordingly through use of an ECO.
• Change the naming for the net associated with the relevant connector pin in one of the child projects to be the same as that used for the connector pin in the other project. Then compile the child project and bring the change back to the Multi-board Schematic by using the Design » Import From Child Projects command. The net name for the connection will be updated accordingly through use of an ECO.

Default report mode:

Summary

This violation occurs when a connector pin represented in a module entry on the Multi-board Schematic is not connected to any net in the child design project referenced by that module.

Notification

A notification is displayed in the Messages panel in the following format:

"Pin <ConnectorDesignator-PinNumber>" is not connected in child project "Module <ModuleDesignator>(<ChildProjectName>)"

where:

• ConnectorDesignator-PinNumber is the designator of the connector component in the child design represented by the module's entry and the offending 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, and containing the connector whose indicated pin is not connected to a net.

Recommendation for Resolution

This violation can arise in a number of situations. Consider the following when resolving a violation of this type:

• If the pin of the referenced connector is not to be used within the design, tie it to the appropriate power line (e.g., GND).
• Ensure that any wiring to the connector pin is making electrical contact, i.e. the wire or bus connects to the pin's electrical hot spot.
• If the connector pin is intended to have a short wire and a net label, ensure that the net label exists and has been attached to the wire correctly.

Default report mode:

Summary

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

Notification

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 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.