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.

*RESTART, WRITE, FREQUENCY=n

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 (.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.

*RESTART, WRITE, NUMBER INTERVAL=n, TIME MARKS=NO

*RESTART, WRITE, NUMBER INTERVAL=n, TIME MARKS=YES

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,” Section 1.5.1 of the Abaqus Example Problems Manual, and “Axisymmetric forming of a circular cup,” Section 1.3.7 of the Abaqus Example Problems Manual.

*IMPORT
list of element sets that are to be imported

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, 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. 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. Sets defined at the assembly level must be redefined in the import analysis. New set definitions and surface definitions can be added upon import. You cannot assign new sections, material orientations, normals, or beam orientations to the imported part instance.

*INSTANCE, INSTANCE=instance-name
 Additional set and surface definitions (optional)
*IMPORT
*END INSTANCE

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

abaqus job=job-name oldjob=oldjob-name

*INSTANCE, LIBRARY=oldjob-name 

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,” Section 2.2.5), 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. Material orientations cannot be redefined in the import analysis; orientation names cannot be reused in the import analysis. For imported elements, the material orientations will be transferred from the original 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,” Section 9.2.2, for details).

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.

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,” Section 2.8.1) 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 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, 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 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.

*IMPORT, STEP=step, INCREMENT=increment

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.

*IMPORT, STEP=step, ITERATION=iteration

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.

*IMPORT, STEP=step, INTERVAL=interval

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” in “Controlling initial contact status in Abaqus/Standard,” Section 34.2.4; “Controlling initial contact status in Abaqus/Standard,” Section 34.2.4; “Controlling initial contact status for general contact in Abaqus/Explicit,” Section 34.4.4; and “Adjusting initial surface positions and specifying initial clearances for contact pairs in Abaqus/Explicit,” Section 34.5.4.

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

*IMPORT, STEP=step, UPDATE=YES

*IMPORT, STEP=step, UPDATE=NO

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; and

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

• 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,

• hyperelasticity (including Mullins effect),

• hyperfoam,

• viscoelasticity,

• traction-separation response with damage for cohesive elements,

• damage for ductile metals,

• damage for fiber-reinforced composites,

• connector behavior, and

• materials defined in user subroutines UMAT and VUMAT.

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.

*IMPORT, STATE=YES

*IMPORT, STATE=NO

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. For constraints such as surface-based ties it is appropriate to redefine these constraints in the original reference configuration. This ensures identical constraint data are regenerated in the import analysis. 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. When such acoustic and structure meshes are imported from Abaqus/Standard into Abaqus/Explicit and the tie constraint is redefined, the acoustic elements at the interface may appear distorted when viewed in the undeformed plot mode in the Visualization module of Abaqus/CAE (the deformed plot at time=0 displays the correct mesh). To regenerate constraints in the original configuration, specify that the reference configuration should not be updated to the imported configuration. If a new constraint is defined in the import analysis, it is appropriate to generate the constraint data based on the current configuration. See “Updating the reference configuration” above for more information.

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.

*IMPORT ELSET
*IMPORT NSET

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, , and that predicted by the interpolation of the rotated normals at the nodes, , must satisfy the condition:

*IMPORT CONTROLS, NORMAL TOL=