Missing Component Models

Parent category: Violations Associated with Components

Default report mode:

Summary

This violation occurs when compiling an Integrated Library Package (*.LibPkg) and a linked model for a component in the source schematic library could not be found.

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. When the linked model is a footprint model, simulation model or PCB3D model, the message a notification is also displayed in the Messages panel in one of the following formats:

<ComponentName>: Could not find <ModelName> - when the model search scope is Any.

<ComponentName>: Could not find <ModelName> in <LibraryName> - when the model search scope is Library Name.

<ComponentName>: Could not find <ModelName> in <Path> - when the model search scope is Library Path.

where:

• ComponentName is the name of the component in the source schematic library.
• ModelName is the name of the 2D/3D Component, PCB3D, or simulation model, that is linked to the source component and which could not be found.
• LibraryName is the name of the library file specified to contain the linked model.
• Path is the absolute path to a library file specified to contain the linked model.

When the linked model is a signal integrity model, the message is displayed in the Messages panel in the following format:

<ComponentName>: Could not find 'GenericEntity'in <Path>

where:

• ComponentName is the name of the component in the source schematic library.
• Path is the absolute path to a library/model

Recommendation for Resolution

When the problem is a linked footprint, simulation or PCB3D model

This issue is typically caused by one of the following scenarios:

• The model name is incorrectly specified when defining the model link.
• The linked model does not reside in the specified library file.
• The library file containing the linked model has been moved or deleted.

The first port of call in resolving this violation is the associated setup dialog for the model type you are linking to - the PCB Model dialog, the Sim Model dialog, or the PCB3D Model Libraries dialog. In each case, check and ensure:

• The name of the model to which you are linking is correct and
• The correct option is used to locate the library/model file in which that model resides.

The format of the displayed error message depends on the search scope you have enabled when locating the model, and can be of great help when tracking down the problem with the model link:

• If the model could not be found in a specified path (search scope: Library Path), ensure that the library/model file you have specified actually exists at that location and also check the library/model file to see if the model with the specified name exists within.
• If the model could not be found in a specified library/model file (search scope: Library Name), ensure that the library/model file has been added to the Available Libraries list (Project Libraries, Installed Libraries, Project Search Paths). Also check to make sure the library/model file contains the model with the same name specified in the link.
• If the model could simply not be found (search scope: Any), ensure that a library/model file - containing a model with the same name as that specified in the link - has been added to the Available Libraries list.

When the problem is a linked signal integrity model

Typically caused when the type of signal integrity model (e.g. diode, IC) is not specified, this is resolved in the associated setup dialog for signal integrity models. The easiest way to access this is through the Component Properties dialog where both the signal integrity model type and pin models can be specified. Check that you are using the correct model(s) in the Models region of the Component Properties dialog and amend if necessary. The Add and Edit buttons can be used to create a new model or modify the existing user models without the need for having to edit them directly. You can then launch the Signal Integrity Model dialog by double-clicking on the entry for Signal Integrity Type, where the Update Ibis File button allows pins models to be imported from an Ibis model file.