Altium NEXUS Documentation

WorkspaceManager_Err-ComponentImplementationsWithInvalidPinMappingsComponent Implementations with Invalid Pin Mappings_AD

Created: August 3, 2021 | Updated: August 3, 2021
All Contents

Parent category: Violations Associated with Components

Default report mode:

Summary

This violation occurs when compiling an Integrated Library Package (*.LibPkg) and the pin mapping between the schematic component and the linked model is found to be invalid.

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 also displayed in the Messages panel in the following format:

ComponentName: Could not find port <ModelPinNumber> on model <ModelName> for pin <ComponentPinNumber> - PCB model related

ComponentName: Could not map port <ModelPinNumber> on model <ModelName> to a pin - simulation model related

where:

  • ComponentName is the name of the component in the source schematic library.
  • ModelPinNumber is the expected designator for the pin/pad that could not be found on the linked model.
  • ModelName is the name of the model that is linked to the component.
  • ComponentPinNumber is the designator of the pin on the source schematic component to which the erroneous pin of the model is mapped.

Recommendation for Resolution

Resolution involves accessing the mapping  between the schematic symbol and the target domain model. To do this, you'll first need to be viewing the properties for the applicable schematic library component. Double-click on the entry for the component in the Components list of the SCH Library panel to access the Properties panel, with the properties for that component loaded.

If the PCB model related error message is displayed, select the model in the Footprint section of the panel and click the  button underneath the list to access the PCB Model dialog. Once there, click on the Pin Map button to access the Model Map dialog. In the Component Pin Designator column, find the pin number flagged by the message (ComponentPinNumber). The violation arises because the corresponding entry in the Model Pin Designator column points to a pad designator that does not exist in the PCB model. Amend the entry as required. Typically there will be one-to-one mapping, with the designators on both sides the same.

If the simulation model related message is displayed, select the model in the Models section of the panel and click the  button underneath the list to access the Sim Model dialog. Once there, click on the Port Map tab. This violation will arise when the model pin is not correctly mapped to a pin of the schematic component. This can happen when the entry for the model pin has been set to a pin that is already mapped, or to Not Connected. Amend the entry as required.

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). 
Found an issue with this document? Highlight the area, then use Ctrl+Enter to report it.

Contact Us

Contact our corporate or local offices directly.

We're sorry to hear the article wasn't helpful to you.
Could you take a moment to tell us why?
200 characters remaining
You are reporting an issue with the following selected text
and/or image within the active document: