Select File
ImportModel from the main menu bar to import a model. You can import a model from the following:
Abaqus/CAE model database (*.cae)
Abaqus/CAE creates a copy of the model that you select in the current model database. Data other than model data, such as analysis jobs or custom user data that were created using the Abaqus Scripting Interface, are not copied to the current model database.
Abaqus input file (*.inp, *.pes)
Options and parameters in the input file are translated into objects recognized by the import capability, and Abaqus/CAE creates a new model. For a detailed list of the keywords supported by the import model capability, see “Keyword support from the input file reader,” Section A.2.
Most of the commonly used element types can be assigned to orphan elements. However, some element types cannot be imported from an input file. For a description of the input file reader and a full list of unsupported elements, see “Importing a model from an Abaqus input file,” Section 10.5.2.
The input file reader is not able to import models with a very large number (roughly 8000 or more) of steps.
Abaqus output database (*.odb)
Abaqus/CAE imports the nodes and elements defined in the output database along with the materials, sets, surfaces, section definitions, and beam profiles and creates a new model.
Nastran input file (*.bdf, *.dat, *.nas, *.nastran, *.blk, *.bulk)
Abaqus/CAE imports entities in the Nastran input file as a new model in the current model database. The Nastran-to-Abaqus conversion enables you to select the Abaqus elements to which you map Nastran elements, select a method for converting Nastran section data into Abaqus sections, use pre-integrated shell sections, scale mass/inertia values, convert Nastran subcases to Abaqus load cases in a linear perturbation step, and couple beam element offsets.
ANSYS input file (*.cdb)
Abaqus/CAE imports entities in the ANSYS input file as a new model in the current model database. The ANSYS-to-Abaqus conversion converts selected ANSYS entities to their equivalent entities in Abaqus and notes in a log file the entities that could not be translated.
To import a model:
From the main menu bar, select FileImportModel.
The Import Model dialog box appears.
Select the type of file from which to import the model.
Select Abaqus/CAE Database (file extension .cae) to import a model from an Abaqus/CAE database. For more information, see “Importing a model from an Abaqus/CAE model database,” Section 10.5.1.
Select Abaqus Input File (file extensions .inp and .pes) to import a model from an Abaqus input file. Abaqus/CAE imports the input file and creates a model using information from the supported options. Unsupported options and parameters are ignored. For more information, see “Importing a model from an Abaqus input file,” Section 10.5.2.
Select Abaqus Output Database (file extension .odb) to import a model from an output database. Abaqus/CAE imports the output database and creates a new model. For more information, see “Importing a model from an output database,” Section 10.5.3.
Select Nastran Input File (file extensions .bdf, .dat, .nas, .nastran, .blk, and .bulk) to import a model from a Nastran input file. Abaqus/CAE imports the Nastran data and creates a new model. For more information, see “Importing a model from a Nastran input file,” Section 10.5.4.
Select Ansys Input File (file extension .cdb) to import a model from an ANSYS input file. Abaqus/CAE imports the ANSYS data and creates a new Abaqus model. For more information, see “Importing a model from an ANSYS input file,” Section 10.5.5.
Select the file from which you want to import data, and click OK. For more information on specifying the file to open, see “Using file selection dialog boxes,” Section 3.2.10.
If you are importing a model from a model database file, the Import Model from Model Database dialog box appears. Complete the following additional steps:
Select the model that you want to copy from the selected model database.
If desired, rename the model as you import it into the current model database. By default, the copied model retains its original name.
If you want to copy objects between models immediately after you import the model, toggle on After export, show “Model->Copy Objects” dialog.
Click OK to close the Import Model from Model Database dialog box.
Abaqus/CAE imports the selected model into the current model database and, if you selected After export, show “Model->Copy Objects” dialog, Abaqus/CAE opens the Copy Objects dialog box. You can use this dialog box to select individual objects to copy between models in the current model database. For more information about selecting items in this dialog box, see “Copying objects between models,” Section 9.8.3.
If you are importing a model from an Abaqus input file or an output database file, Abaqus/CAE completes the import process by performing the following steps:
Creating the new model
Naming the model with the same name as the original input file or output database file
Making the imported model the current model
Displaying the imported model in the model list in the context bar
If you are importing a model from a Nastran input file, the Import Nastran Input File dialog box appears. Complete the following additional steps:
If desired, rename the model as you import it into Abaqus/CAE. By default, the imported model inherits the name of the Nastran input file.
From the Element Type Mapping options, choose the Abaqus element types to which you want to map the Nastran element types CBAR, CQUAD4, CHEXA(8), and CTETRA(10). For each Nastran element type, click 
, then select the Abaqus element type by toggling element controls from the dialog box that appears.
From the Section consolidation options, select the method you want to use to convert section or membrane data in the Nastran input file:
Select Preserve section IDs to create an Abaqus section corresponding to each Nastran PSHELL or PCOMP property ID and to create Abaqus discrete fields for shell or membrane thickness and material orientation data in Nastran.
Select Group by material ID to create a single Abaqus section for all elements referencing the same material and to create Abaqus discrete fields for shell thickness and material orientation data in Nastran.
Select None to create a separate shell or membrane section for each combination of orientation, offset, and/or thickness.
Toggle on Use pre-integrated shell sections to provide the section property data before the analysis. If this option is not selected, Abaqus calculates (integrates) the cross-sectional behavior from section integration points during the analysis.
Toggle on Apply mass/inertia scaling from PARAM, WTMASS to use the value on the Nastran data line PARAM, WTMASS, value as a multiplier for all density, mass, and rotary inertia values created in the Abaqus model.
Toggle on Convert subcases to load cases in a linear perturbation step to translate Nastran data lines that use the Nastran libraries SOL 101, SOL 108, or SOL 111 into Abaqus perturbation steps with load cases.
Toggle on Couple beam element offsets to translate beam element offsets in the Nastran data by creating new nodes at the offset locations, changing the beam connectivity to the new nodes, and rigidly coupling the new and original nodes. If this option is not selected, Abaqus translates beam element offsets to the centroid and shear center for the beam general section definition.
If you want to retain the Abaqus input file created during the translation process, toggle on Keep generated Abaqus input file.
Click OK to close the Import Nastran Input File dialog box.
Abaqus/CAE translates the Nastran data according to your specifications and imports the model into the current model database. If any errors arise during translation, you can display the translation log file in the Import Nastran Log dialog box, which enables you to browse the log file and search its contents for error messages.
