You can use an ABAQUS input file to import a model into ABAQUS/CAE by selecting FileImportModel from the main menu bar. ABAQUS keywords that are imported from the input file are incorporated into a new model; for example, if the Young's modulus was imported from the *ELASTIC keyword, it will be available in the Property module. Keywords that are not supported are ignored during import. The input file does not have to be complete; for example, it may not contain any history data. Because an input file is unable to store all of the data from an ABAQUS/CAE model database, you should not use input files to archive model data.

The following functionality can be imported into a model from an ABAQUS input file:

See “Keyword support from the input file reader,” Section A.2, for a complete list of the keywords that are supported by the input file reader.

The import capability creates sets based on any *ELSET or *NSET keywords, as well as any ELSET or NSET parameters on other supported keywords. If the input file was written in terms of an assembly of part instances, ABAQUS/CAE preserves your intent when creating part and assembly sets. If a set was defined within a part (deformable or rigid), ABAQUS/CAE creates a part set. When you instance the part in the Assembly module, you can refer to the part set; however, the assembly-related modules provide only read-only access to part sets. If a set was defined within the assembly, ABAQUS/CAE creates an assembly set. For more information, see “How do part sets and assembly sets differ?,” Section 48.2.2.

In contrast, if the input file was not written in terms of an assembly of part instances, ABAQUS/CAE tries to minimize the number of sets created. In most cases, sets in the input file are imported as only assembly sets. However, if a section assignment refers to a set, ABAQUS/CAE imports the set as only a part set.

Element-based surfaces can be imported; however, ABAQUS/CAE imports a node-based surface as a set of nodes, not as a surface. As a result, an imported node-based surface appears in the Set manager and not in the Surface manager.

ABAQUS/CAE imports reactivated contact pairs only if the contact pairs were deactivated in the first analysis step.

When you analyze a submodel using ABAQUS/Standard or ABAQUS/Explicit, you provide the name of the output database or results file containing the global solution in the ABAQUS execution procedure; the file name does not appear in the input file. As a result, when you import an input file that analyzes a submodel, you must specify the name of the output database or results file containing the global solution that will drive the submodel. Select ModelEdit AttributesModel Name and enter the name of the file containing the global solution on the Submodel tabbed page.

Parts are imported from an input file in the form of an orphan mesh; an orphan mesh consists of node and element definitions along with the type of element assigned. The input file reader can import an orphan mesh containing most of the commonly used element types. However, the input file reader cannot import an orphan mesh containing the following element types:

The following element types can be imported, but their section properties are not yet supported: Pore pressure cohesive elements can be imported, but you cannot view them in the ABAQUS/CAE model. However, you can view pore pressure cohesive elements in the Visualization module after an analysis is complete.

You can use the Mesh module to change the element type assigned to an orphan mesh imported from an input file. In addition, you can use the Keywords Editor to include options that the input file reader does not support; for detailed instructions on using the Keywords Editor, see “Adding unsupported keywords to your ABAQUS/CAE model,” Section 9.9.1.