About Transferring Results between Abaqus Analyses

Abaqus provides the capability to import a deformed mesh and its associated material state from Abaqus/Standard into Abaqus/Explicit and vice versa. This capability is particularly useful in manufacturing problems; for example, the entire sheet metal forming process (which requires an initial preloading, forming, and subsequent springback) can be analyzed. In this case the initial preloading can be simulated with Abaqus/Standard using a static procedure and the subsequent forming process can be simulated with Abaqus/Explicit. Finally, the springback analysis can be performed with Abaqus/Standard.

Abaqus also provides the capability to transfer desired results and model information from an Abaqus/Standard analysis to a new Abaqus/Standard analysis or from an Abaqus/Explicit analysis to a new Abaqus/Explicit analysis, where additional model definitions may be specified before the analysis is continued. For example, during an assembly process an analyst may first be interested in the local behavior of a particular component but later is concerned with the behavior of the assembled product. In this case the local behavior can first be analyzed in an Abaqus/Standard or Abaqus/Explicit analysis. Subsequently, the model information and results from this analysis can be transferred to a second Abaqus/Standard or Abaqus/Explicit analysis, where additional model definitions for the other components can be specified, and the behavior of the entire product can then be analyzed.

Finally, Abaqus provides the capability to transfer desired results and model information from multiple Abaqus/Standard analyses or multiple Abaqus/Explicit analyses to a new Abaqus/Explicit analysis, where additional model definitions can be specified before the analysis is continued. For example, during an assembly process an analyst may first be interested in the local behavior of a number of components but later is concerned with the behavior of the assembled product. In this case the local behavior of each component can first be analyzed individually in a series of Abaqus/Standard or Abaqus/Explicit analyses. Subsequently, the model information and results from these analyses can be transferred to a new Abaqus/Explicit analysis, where additional model definitions for the other components can be specified, and the behavior of the entire product can then be analyzed.

For this capability to work, the same maintenance release of Abaqus/Explicit and Abaqus/Standard must be run on computers that are binary compatible. You should only use the import capability within the same maintenance delivery of a general release.

This page discusses:

Saving the Analysis Results

The restart files from the original analysis contain the analysis results that are transferred from Abaqus/Standard or Abaqus/Explicit. Obtaining restart files is described in more detail in Writing Restart Files; brief summaries are provided below. By default, Abaqus/Standard does not write any restart information and Abaqus/Explicit writes results at the beginning and end of each step.

Saving Results from Abaqus/Standard

If the results are to be imported from an Abaqus/Standard analysis, the results from the original Abaqus/Standard job must be written to the restart (.res), analysis database (.mdl and .stt), part (.prt), and output database (.odb) files.

You can specify the increments at which restart information will be written. Restart information is always written at the end of a step in addition to the requested increments whenever you request restart data in Abaqus/Standard.

Saving Results from Abaqus/Explicit

If the results are to be imported from an Abaqus/Explicit analysis, the results from the original Abaqus/Explicit job must be written to the state (.abq) file at the time when transfer of the state of the deformed body is required. The state (.abq), restart (.res), analysis database (.mdl and .stt), package (.pac), part (.prt), and output database (.odb) files will be used for importing the results from Abaqus/Explicit.

You can specify whether the results are to be written at the exact time dictated by the specified time interval, n, during a step of an Abaqus/Explicit analysis or at the increment ending after the time dictated by the specified time interval. Results are always written at the end of a step, so it is not necessary to request results at the exact time intervals if results will be read only from the end of a step.

Specifying the Transfer of Model Data and Results

The import capability is used to transfer model data and results from one analysis to another. The following sections describe how to specify the import request. You can import element sets from models that are not defined as assemblies of part instances, or you can import part instances from models that are defined as assemblies of part instances.

Specifying the Transfer of Model Data and Results for Models That Are Not Defined as Assemblies of Part Instances

You can import element sets from a previous analysis to specify the transfer of model data and results for models that are not defined as assemblies of part instances. This import capability is illustrated in Springback of two-dimensional draw bending and Axisymmetric forming of a circular cup.

Each element set to be imported must have been defined in the original analysis. You can import any element set, including nested element sets and those with overlapping elements. An imported element set can also be a subset of another imported element set. The elements in these sets as well as the element set definitions are imported. Even though an element may be included in multiple imported elements sets, each element is imported only once in the import analysis. You cannot use element sets that are internal to the original analysis.

Repositioning Elements in the Model

You can reposition elements in the element sets from their original positions in the previous analysis to new positions in the import analysis. The new position is determined by a translation and/or rotation of the original position relative to the origin of the global coordinate system. The positioning data apply to all elements in the list of imported element sets. Element sets that require different positioning data need to be grouped separately during import.

Importing Model Data and Results of Element Sets Multiple Times

You can import model data and results of element sets from a previous analysis multiple times. You must define a new name and a new position for an element set that has been imported more than once. You specify the old element set name used in the previous analysis followed by the new element set name to be used in the import analysis. The old element set name must have been defined in the previous analysis. The use of internal sets is not supported.

New elements and nodes are generated with new element and node numbers for the renamed element sets. You specify element and node offsets; the new numbers are obtained by adding the offsets to the old numbers used in the previous analysis. It is your responsibility to select appropriate element and node offsets to preserve uniqueness of element and node numbering in the model.

The new position is determined as described in Repositioning Elements in the Model. To prevent multiple elements in the model from occupying identical positions, an old element set name must not appear more than once in the list of imported element sets for each import definition. Element sets that require renaming must be grouped separately during import from those that do not require renaming.

Importing Element Set, Node Set, and Surface Definitions One Time

All element set and node set definitions associated with the imported elements are imported by default. For models that are not defined as assemblies of part instances, you can also selectively import only specified element set or node set definitions. This capability provides a convenient way of selectively reusing the element or node sets defined in the original analysis. However, any members of such sets that do not belong to the imported elements are removed from the specified sets.

For example, suppose three element sets—SHELL3D, MEMB, and ALL—are defined in the original analysis. Element set ALL contains all of the elements in element sets SHELL3D and MEMB, as well as other elements. You choose to import only the element sets SHELL3D and MEMB (i.e., the elements in these sets as well as the element set definitions). In addition, you selectively import the element set definition ALL (but not the elements in this set). If element 100 belongs to element set ALL but not to either element set SHELL3D or element set MEMB, it will not be imported and will be removed from the list of elements belonging to element set ALL. The imported element set definitions are processed before any node or element definitions; therefore, even if element 100 is subsequently redefined in the import analysis, it will not belong to element set ALL (unless it is explicitly assigned to element set ALL in the import analysis).

Only node and element sets defined in the original or previous import analysis are available for importing. New sets defined during a restart run cannot be imported.

You can also selectively import surface definitions. Surfaces are not imported if they are defined with elements and nodes that are not imported. All surface definitions are imported automatically if you import surface definitions but do not specify the surfaces to import. For models that are not defined as assemblies of part instances, all surface definitions associated with the imported elements are imported by default in an Abaqus/Standard to Abaqus/Standard import analysis.

Importing Element Set, Node Set, and Surface Definitions Multiple Times

You can import element sets, node sets, and surfaces from a previous analysis multiple times. Element set, node set, and surface definitions associated with the imported elements are not imported by default, and you must define a new name for an element set, a node set, or a surface that has been imported more than once. You specify the old element set name, node set name, or surface name used in the previous analysis followed by the new element set name, node set name, or surface name to be used in the import analysis. The old name must have been defined in the previous analysis, and use of internal names is not supported.

New elements and nodes are generated with new element and node numbers for the renamed sets and surfaces using the offsets that you specified for import; the new numbers are obtained by adding the offsets to the old numbers used in the previous analysis.

Element sets, node sets, and surfaces that require renaming must be grouped separately during import from those that do not require renaming.

Importing Model Data and Results of Element Sets from Multiple Previous Analyses in an Abaqus/Explicit Analysis

You can import model data and results of element sets from multiple Abaqus/Standard analyses or multiple Abaqus/Explicit analyses to an Abaqus/Explicit analysis. However, you cannot import from a mix of Abaqus/Standard and Abaqus/Explicit analyses.

You must specify the name of each previous analysis in an import definition. When importing from multiple analyses, you cannot specify the previous analysis name using the oldjob option (see ).

New elements and nodes are generated with new element and node numbers for the renamed element sets. You specify element and node offsets; the new numbers are obtained by adding the offsets to the old numbers used in the previous analysis. It is your responsibility to select appropriate element and node offsets to preserve uniqueness of element and node numbering in the model.

The new position is determined as described in Repositioning Elements in the Model. To prevent multiple elements in the model from occupying identical positions, an old element set name must not appear more than once in the list of imported element sets for each import definition.

Element sets that require renaming must be grouped separately during import from those that do not require renaming.

Specifying the Transfer of Model Data and Results for Models That Are Defined as Assemblies of Part Instances

You can import part instances from a previous analysis to specify the transfer of model data and results for models that are defined as assemblies of part instances. If you import more than one part instance, all import parameters must be the same for each imported part instance. Each instance name that you specify must be the same as the instance name in the original analysis. Only sets that are defined within the imported instance will be imported. Surfaces defined within the imported instance are imported if you import surface definitions. Sets and surfaces defined at the assembly level must be redefined in the import analysis. New set and surface definitions can be added upon import. You cannot assign new sections, material orientations, normals, or beam orientations to the imported part instance.

Repositioning Part Instances in the Model

You can import a part instance and specify a new position for the part instance in the imported model. The new position is determined by a translation and/or rotation of the original position relative to the origin of the assembly (global) coordinate system.

Importing Part Instances in the Model Multiple Times

You can import a part instance from a previous analysis more than once. In each instance, you must define a new name and a new position for a part instance that has been imported more than once. You specify the old name of the part instance in the previous analysis and a new name for the part instance.

The new position is determined by a translation and/or rotation of the original position relative to the origin of the assembly (global) coordinate system. Sets defined within the part instance will be imported and repositioned. Surfaces defined within the imported instance are imported if you import surface definitions. Sets and surfaces defined at the assembly level must be redefined in the import analysis. New set and surface definitions can be added upon import. You cannot assign new sections, material orientations, normals, or beam orientations to the imported part instance. If you import more than one part instance, the part instances must be from the same output database (.odb) file and all import parameters must be the same for each imported part instance.

Importing Part Instances in the Model from Multiple Previous Analyses in an Abaqus/Explicit Analysis

For models defined as assemblies of part instances, you must specify the name of each previous analysis in an instance definition when importing from multiple previous analyses. In each instance you must define a new name and a new position for a part instance that has been imported more than once. You specify the old name of the part instance in the previous analysis and a new name for the part instance.

The new position is determined by a translation and/or rotation of the original position relative to the origin of the assembly (global) coordinate system. Sets defined within the part instance are imported and repositioned. Surfaces defined within the imported instance are imported if you import surface definitions. Sets and surfaces defined at the assembly level must be redefined in the import analysis. New set and surface definitions can be added upon import. You cannot assign new sections, material orientations, normals, or beam orientations to the imported part instance. If you import more than one part instance, all import parameters must be the same for each imported part instance.

Identifying the Analysis from Which the Data Will Be Obtained When Importing from a Single Previous Analysis

You must specify the name of the job from which the model and results data will be obtained.

Identifying the Individual Analysis from Which the Data Will Be Obtained When Importing from Multiple Previous Analyses

You must specify the name of the analysis from which the model data and results will be obtained.

Importing Model Data

Element property definitions of imported elements can be redefined only if the reference configuration is updated (see Updating the Reference Configuration) and the material state is not imported (see Importing the Material State). In this case the material orientation definitions (Orientations), hourglass stiffness but not hourglass control definitions, and transverse shear stiffness definitions (in the case of shell elements) of the imported elements can also be redefined.

For other reference configuration and material state combinations, the information required to define the section for each imported element will be imported from the original analysis. All material orientations will be transferred from the original analysis to the import analysis. Material orientations that are associated with imported elements cannot be redefined in the import analysis. However, orientation names that are not associated with any imported elements can be reused in the import analysis.

Transverse shear stiffness for imported shell elements cannot be redefined; the values will be transferred from the original analysis. Hourglass stiffness for the imported elements cannot be redefined in an Abaqus/Standard import analysis; the default values will be used. The section control definitions (kinematic formulation, order of accuracy in the element formulation, and hourglass control approach) to be used for imported elements cannot be redefined (see Transferring Results between Abaqus/Explicit and Abaqus/Standard for details).

Mass adjustment contributions (see Mass Adjustment) applied to an element set are always included when the element set is imported. There is no need to redefine these contributions in the import analysis unless different mass adjustment is required for the element set.

Nonstructural mass contributions (see Nonstructural Mass Definition) associated with an element set are not imported. These contributions need to be redefined in the import analysis if they are to be included in the model.

Only nodes associated with the imported elements are imported. New nodes can be defined in the import analysis.

Nodes or elements that use the same numbers as nodes or elements being imported can be defined provided that the reference configuration is updated, the material state is not imported, and the import is not done from an instance library. The new definitions will overwrite the imported definitions. If the reference configuration is not updated, new nodes or elements cannot use the imported node and element numbers irrespective of whether or not the material state is imported.

During results transfer from an Abaqus/Standard analysis to another Abaqus/Standard analysis or from an Abaqus/Explicit to another Abaqus/Explicit analysis, the coordinates of imported nodes can be modified from their imported values by respecifying the nodal definitions if the reference configuration is updated and the material state is not imported. This modification of the coordinates of imported nodes is not allowed during transfer of results from Abaqus/Explicit to Abaqus/Standard or vice versa.

Importing Model Data Defined by a Distribution

While transferring results from one Abaqus/Standard analysis to another Abaqus/Standard analysis, most element or material properties defined by a distribution (see Distribution Definition) are imported along with the elements. The only exceptions are spatially varying thicknesses and orientation angles defined on the layers of composite shells and solids; in this case Abaqus issues an error message during input file preprocessing.

While transferring results from an Abaqus/Explicit analysis to an Abaqus/Standard analysis, the only spatially varying element properties defined by a distribution that can be imported are shell thicknesses, shell offset, and section orientations for shell and solid elements. If any other element or material properties are defined with a distribution, Abaqus issues an error message during input file preprocessing.

While transferring results from an Abaqus/Standard analysis to an Abaqus/Explicit analysis or from an Abaqus/Explicit analysis to another Abaqus/Explicit analysis, the only spatially varying element properties defined by a distribution that can be imported are shell thicknesses, shell offset, section orientations for shell and solid elements, orientation angles defined for shell sections on the layers of composite shells, and section stiffness matrices specified directly for general shell sections. If any other element or material properties are defined with a distribution, Abaqus issues an error message during input file preprocessing. If an element set consists of elements whose properties are defined by one or more distributions, the element set cannot be imported more than once.

Section and material properties of imported elements can be redefined with distributions only if the reference configuration is updated (see Updating the Reference Configuration) and the material state is not imported (see Importing the Material State). In this case the material orientation definitions (Orientations), hourglass stiffness but not hourglass control definitions, and transverse shear stiffness definitions (in the case of shell elements) of the imported elements can also be redefined.

Importing Results from an Abaqus/Standard Analysis (Other than a Direct Cyclic Analysis)

If the results are imported from an Abaqus/Standard analysis, you can specify the step and increment in the restart file for which the results are to be imported. By default, the results written at the end of the analysis are imported.

Importing Results from an Abaqus/Standard Direct Cyclic Analysis

If the results are imported from a direct cyclic analysis, you can specify the step and iteration number in the restart file for which the results are to be imported. By default, the results written at the end of the analysis are imported.

Importing Results from an Abaqus/Explicit Analysis

If the results are imported from an Abaqus/Explicit analysis, you can specify the step and interval in the state file for which the results are to be imported. By default, the results written at the end of the analysis are imported.

Updating the Reference Configuration

Once the current model configuration of an Abaqus analysis is imported into Abaqus/Explicit or Abaqus/Standard, the analysis can be continued with or without updating the reference configuration to be the imported configuration. If the reference configuration is not updated to be the imported configuration, the displacements and strains are reported as total values relative to the original reference configuration and will, hence, be continuous. If the reference configuration is updated to be the imported configuration, displacements and strains reported in the import analysis are the total values relative to the updated reference configuration. This choice is useful if results need to be displayed relative to the imported configuration, such as may be desirable in springback analysis. The reference configuration cannot be updated if the imported analysis is geometrically linear.

The choice of whether or not to update the reference configuration can influence strain-free nodal adjustments associated with contact initialization in Abaqus/Standard. Strain-free adjustments can be used to resolve penetrations or gaps that exist in the reference configuration in Abaqus/Standard, so prior displacements are not considered by the strain-free adjustment algorithm upon import if the reference configuration is not updated. Strain-free nodal adjustments in Abaqus/Explicit are based on the current configuration rather than the reference configuration, so these adjustments are not sensitive to whether the reference configuration is updated in Abaqus/Explicit. Further details on strain-free adjustments are provided in Default Contact Initialization Method, Contact Initialization for General Contact in Abaqus/Standard, Contact Initialization for General Contact in Abaqus/Explicit, and Contact Initialization for Contact Pairs in Abaqus/Explicit.

If connector elements are imported, the configuration can be updated provided that the state is not imported.

When hyperelastic materials are imported, the configuration must be updated if the state is not imported.

Importing the Material State

You can specify whether or not the associated material state should be imported. If you choose to import the material state, the following are imported:

  • stresses;

  • equivalent plastic strains;

  • back stresses for the kinematic hardening models;

  • user-defined state variables;

  • damage-related state variables for the concrete damaged plasticity model;

  • damage-related state-variables for traction-separation response with cohesive elements;

  • damage-related state variables for ductile metals;

  • damage-related state variables for fiber-reinforced composites;

  • maximum deviatoric strain energy density during deformation history for Mullins effect;

  • internal strains and stresses for viscoelastic material models;

  • transformation strains and fraction of martensite for superelastic material models; and

  • connector state variables such as plastic strains, frictional slip, and damage state.

Thus, the state is imported correctly for further analysis only for the following:

  • linear elasticity,

  • Mises plasticity (including the kinematic hardening models),

  • extended Drucker-Prager plasticity,

  • crushable foam plasticity,

  • Mohr-Coulomb plasticity,

  • critical state (clay) plasticity,

  • cast iron plasticity,

  • concrete damaged plasticity,

  • Johnson-Cook plasticity,

  • hyperelasticity (including Mullins effect),

  • hyperfoam,

  • viscoelasticity,

  • superelasticity,

  • traction-separation response with damage for cohesive elements,

  • damage for ductile metals,

  • damage for fiber-reinforced composites,

  • connector behavior,

  • materials defined in user subroutines UMAT and VUMAT, and

  • materials defined using the parallel rheological framework for nonlinear viscoelastic-elastoplastic behavior.

For all other material models only stresses will be imported. No other state variables will be imported.

If the material behavior is defined in a user subroutine, you must ensure that the UMAT and VUMAT are consistent.

If connector elements are imported, the state can be imported provided that the configuration is not updated.

When hyperelastic materials are imported, the state must be imported if the configuration is not updated. In an import analysis where you specify that the reference configuration should not be updated and the material state should not be imported, the material state is imported for elements associated with hyperelastic materials and any initial conditions of the state specified for such elements are ignored.

Importing Rigid Bodies

A rigid body defined with an element set in the original analysis will be imported by default if all elements in the element set are imported; that is, if all of the rigid body elements belong to the imported element sets. The reference node of an imported rigid body is imported automatically, and you should not specify a new reference node for the imported rigid body. If the reference node of an imported rigid body is defined by a node set, the reference node set can be included in the imported node sets. If all elements belonging to a rigid body are imported multiple times, the rigid body and its reference node are imported the same number of times automatically. Multiple import of a rigid body with pin nodes or tie nodes assigned to the rigid body is not supported.

If a rigid body consists of a union of multiple element sets and these sets are imported multiple times, you must define a node set for the rigid body reference node. This node set must be imported to provide a unique node offset for the reference node.

A rigid body from an original analysis cannot be partially imported; that is, the full complement of rigid body elements must be imported. An assembly-level rigid body from the original analysis with parts and instances can be imported only if it refers to a reference node set defined at the part instance level in the original analysis. If the reference node is defined at the assembly level, the set and the rigid body cannot be imported.

Defining Constraints upon Import

Most constraints (such as multi-point constraints and surface-based tie constraints) are not imported from the original analysis and must be redefined in the import analysis. Using the reference configuration of the original analysis without update ensures identical reproduction of these constraints in the import analysis.

If a new constraint is defined in the import analysis, it is important to ensure that the constraint is not in violation either in the reference configuration or in the starting configuration of the import analysis. These two configurations are one and the same for newly introduced nodes. If a new constraint involves nodes of the original analysis, it is appropriate to update the reference configuration for the import analysis (see Updating the Reference Configuration for more information). In all import analyses, tie constraints are always defined with reference to the updated configuration.

In an Abaqus/Standard analysis with adaptive meshing and acoustic-to-structure tie constraints, the structural as well as the acoustic nodes may move from their initial positions.

Specifying a Tolerance for Shell Normals in the Updated Configuration

When the imported configuration is updated upon import, the mesh discretization may not satisfy the mesh geometry checks imposed in Abaqus/Explicit or Abaqus/Standard to evaluate whether or not a mesh is reasonable. In the case of highly warped shell elements it is possible that the normal at the center of the element that is calculated from the midsurface interpolation may differ from the normal that is interpolated from the rotated normals at the nodes. If the difference exceeds the tolerance specified, the analysis will terminate. This suggests that a fine mesh may be required to model areas of high curvature change to achieve a successful analysis.

The unit normal computed from the midsurface interpolation, n1, and that predicted by the interpolation of the rotated normals at the nodes, n2, must satisfy the condition:

1-ftol|n1n2|,

where you can specify the tolerance, ftol. If you do not specify a tolerance value, a default value of ftol = 0.1 is used.

Limitations for Import from Multiple Previous Analyses

The capability to import from multiple previous analyses has the following known limitations:

  • You can import only to an Abaqus/Explicit analysis.
  • The previous analyses must all be Abaqus/Explicit analyses or Abaqus/Standard analyses. A mix of Abaqus/Explicit and Abaqus/Standard analyses is not supported.

  • The use of either a part-instance model or a non-part-instance model but not both must be maintained in all previous analyses. A mix of previous analyses with and without instance definitions is not supported.

  • All previous analyses must be imported with the same settings for updating the reference configuration and for importing the material state.

  • All previous analysis models must have the same geometric dimension. A mix of two-dimensional, axisymmetric, and three-dimensional analyses is not supported.

  • All limitations that pertain to import from a single Abaqus/Explicit analysis or a single Abaqus/Standard analysis remain effective.