Importing a model from an Abaqus input file

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. Model component labels that differ only in case are not imported into Abaqus/CAE consistently; therefore, you should not use case to distinguish between model components of the same type. 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 topics are discussed:

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

  • Nodes and elements

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

  • Adaptive mesh controls

  • Material, section, and orientation definitions

  • Model and material descriptions

  • Interactions and interaction properties

  • Discrete fasteners (previously defined in Abaqus/CAE)

  • Loads and boundary conditions (in the global coordinate system)

  • Amplitudes

  • Procedures, output requests, and monitor variables


    Importing models with a very large number of attributes, such as steps or predefined fields, (on the order of 8000 or more) may take a significant amount of time.

See Will link to usi-kwb-inputreader,, for a complete list of the keywords that are supported by the input file reader. Not all keyword data lines are supported for import; Abaqus/CAE issues warning messages when unsupported entries are encountered. 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.

Importing parts

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

  • Tube support elements (ITS*)

  • User-defined elements (U*)

The following element types can be imported, but their section properties are not yet supported:

  • Distributing coupling elements (DCOUP*)

  • Drag chain elements (DRAG*)

  • Frame elements (FRAME*)

  • Gap contact stress/displacement elements (GAPCYL, GAPSPHER, and GAPUNI)

  • Interface elements (INTER*, ISL*, IRS*, ISP*, ITT*, and DINTER*)

  • Joint elements (JOINT*)

  • Line spring elements (LS*)

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 elements imported from an input file.

Importing sets and surfaces

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?.

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.

Importing descriptions

Model descriptions and material descriptions that appear as comment lines in input files are imported into Abaqus/CAE. The comment lines that immediately precede the header of the input file store the model description, which is available in the Edit Model Attributes dialog box upon import. The comment lines that immediately precede the material and material behavior definitions store the material descriptions, which are available in the Edit Material dialog box upon import.

The job description from the Edit Job dialog box appears as the data line for the header of the input file. If desired, you can modify this data line to include more details about the job; however, this data line is not imported into Abaqus/CAE.

Importing interactions, constraints, and fasteners

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

Abaqus/CAE imports multi-point constraints as MPC connector sections and wire features or as MPC constraints, depending on how the input file identifies the nodes involved.

A fully defined discrete fastener contains both an attachment line and a connector section assignment. In order to recreate these discrete fasteners as originally modeled in Abaqus/CAE upon import, Abaqus/CAE writes special comment lines to the input file when you submit a job for analysis. These special comment lines immediately precede the Abaqus keyword used to define the discrete fasteners, begin with **@ABQCAE, and are ignored by the Abaqus solvers.

Assembled fasteners and point-based (mesh-independent) fasteners cannot be imported from an input file.

Analyzing a submodel

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.