Non-Creo models and components that you open in Creo behave like native Creo models. For example, if you try to open a non-Creo model when a model by the same file name and extension but a different location is already open in Creo, the model that is open in session is considered.

After you assemble the non-Creo part and assembly models as components of Creo assemblies, you can perform most component-level and assembly tasks in Creo.

You can right-click a non-Creo model on the Model Tree and click Information > Reference Viewer or click Tools > Reference Viewer and view the model information in the Reference Viewer.

The File > Save > Save a Copy command saves the non-Creo models as Creo models.

You can use the batch processing capability of Creo Distributed Batch to perform various assembly tasks such as export Creo assemblies with non-Creo components to the supported formats of IGES and STEP. The Task Type Definition (TTD) files of Creo Distributed Batch can batch process the tasks of the Creo assemblies even when the file names of the non-Creo components extend up to 80 characters, contain special characters, and have unique file extensions.

You can use the non-Creo models as drawing models. You can select Autodesk Inventor, CATIA, SolidWorks, and NX part and assembly models in the File Open dialog box and add them to new or existing drawings.

You can use the Replace command to substitute instances of the non-Creo components in the family tables. You can also replace by interchange or with a related model, such as replace a SolidWorks component model with a CATIA model. You can type the names of the non-Creo components in the family table cells. After you include the non-Creo components in the family tables and save the family tables, you can verify the family tables for the component names and file extensions. You cannot, however, create family tables for the non-Creo models or perform family table operations on the non-Creo models.

You can handle regeneration failures in a multi-CAD environment just as you handle them in a session of Creo. When model references fail, you can regenerate the multi-CAD assemblies in Creo just as you regenerate native Creo models. If the non-Creo components of Creo assemblies are missing, you can click Model > Regenerate > Regeneration Manager and regenerate the assemblies with the non-Creo content in the Resolve or the No Resolve mode. In the Resolve mode, you can use the Quick Fix option on the RESOLVE FEAT menu and the Find Component option on the QUICK FIX menu to browse and locate the missing component in the File Open dialog box.

In the default No Resolve mode, you can right-click the missing non-Creo component on the Model Tree and use the Retrieve Missing Component option on the shortcut menu to browse and locate the missing component in the File Open dialog box. You cannot delete the missing non-Creo components in the Resolve mode.

You can run Creo ModelCHECK on the non-Creo models and components in the Interactive and Regenerate modes. The Creo ModelCHECK report is generated for the non-Creo models and components and displayed in the Creo browser.