Importing a model from an output database

You can use an output database to import a model into Abaqus/CAE by selecting FileImportModel from the main menu bar.

The following functionality can be imported into a model from an output database:

  • Nodes and elements

  • Surfaces, node and element sets, and contact node sets

  • Materials and section definitions

  • Beam profiles

Although sections are imported, the assignment of a section to the appropriate element set is not imported. Similarly, the assignment of a beam profile to the appropriate beam section is not imported. When you submit an input file for analysis, Abaqus does not write some material definitions to the output database. As a result, if you import the output database into Abaqus/CAE, these materials will be missing from the model. If this occurs, you can import the model from the input file instead of from the output database.

Abaqus/CAE imports a part from an output database by reading the nodes and elements that define each part instance in the assembly. If the input file that created the output database was structured using parts and assemblies, each part instance imported from the output database appears as a separate part in Abaqus/CAE. In addition, the assembly appears in Abaqus/CAE along with each part instance. As a result, the model imported into Abaqus/CAE contains a part and a part instance corresponding to each part instance in the output database.

The nodes and elements that define a part instance in an output database have been translated and rotated to their position in the assembly. The resulting part that is imported into Abaqus/CAE has the same name as the original part instance in the output database, and its orientation reflects the orientation of the part instance in the output database. As a result, the orientation of the imported part may be different from the orientation of the part in the input file that created the output database.

If the input file that created the output database was not structured using parts and assemblies, Abaqus/CAE writes the mesh definition to the output database as a single part and a single part instance. If the single part in the output database includes an analytical rigid surface, the part that Abaqus/CAE tries to import will contain an invalid combination of deformable parts and analytical rigid parts. As a result the output database cannot be imported.