About transferring results between Abaqus analyses

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

Step module: OutputRestart Requests: enter n in the Frequency column for each step

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

Step module: OutputRestart Requests: enter n in the Number Interval column; click to check the Time Marks column for each step if you want the results written at the exact time intervals

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.

IMPORT
list of element sets that are to be imported

SHELL SECTION, MATERIAL=STEEL1, ELSET=BLANK1 .00082, 5 
SHELL SECTION, MATERIAL=STEEL2, ELSET=BLANK2 .00082, 5 
ELSET, ELSET=BLANK BLANK1, BLANK2

IMPORT BLANK

IMPORT
list of element sets that are to be imported and relocated
positioning data

IMPORT, RENAME, EOFFSET=element-offset, NOFFSET=node-offset
old_name_elem_set1, new_name_elem_set1
old_name_elem_set2, new_name_elem_set2
…
positioning data

IMPORT, UPDATE=NO ASSEMBLY_QUADRANT_1_LOWER,
  ASSEMBLY_QUADRANT_1_UPPER, 
  IMPORT, UPDATE=NO, RENAME, EOFFSET=80, NOFFSET=97
  ASSEMBLY_QUADRANT_1_LOWER, ASSEMBLY_QUADRANT_2_LOWER ASSEMBLY_QUADRANT_1_UPPER,
  ASSEMBLY_QUADRANT_2_UPPER 0., 0., 0., 0., 0., 0., 0., 0., 1.,
  90.,

IMPORT ELSET
IMPORT NSET

IMPORT ELSET, RENAME
IMPORT NSET, RENAME

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

Load module: Create Predefined Field: Step: Initial: choose Other for the Category and Initial State for the Types for Selected Step: select the instances to which the initial state should be assigned

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

INSTANCE, NAME=new instance-name, INSTANCE=old instance-name
positioning data
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 

Load module: Create Predefined Field: Step: Initial: choose Other for the Category and Initial State for the Types for Selected Step: Job name: output-database-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), 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 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.

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 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 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.

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

Load module: Create Predefined Field: Step: Initial: choose Other for the Category and Initial State for the Types for Selected Step: select instances: Step: select Specify: step and Frame: select Specify: 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

Load module: Create Predefined Field: Step: Initial: choose Other for the Category and Initial State for the Types for Selected Step: select instances: Step: select Specify: step and Frame: select Specify: 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

Load module: Create Predefined Field: Step: Initial: choose Other for the Category and Initial State for the Types for Selected Step: select instances: Step: select Specify: step and Frame: select Specify: 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, Controlling initial contact status in Abaqus/Standard, Controlling initial contact status for general contact in Abaqus/Explicit, and Adjusting initial surface positions and specifying initial clearances 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.

IMPORT, STEP=step, UPDATE=YES

IMPORT, STEP=step, UPDATE=NO

Load module: Create Predefined Field: Step: Initial: choose Other for the Category and Initial State for the Types for Selected Step: toggle Update reference configuration on or off

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.

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,

• 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.

IMPORT, STATE=YES

IMPORT, STATE=NO

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.

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 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 without updating the reference configuration, the acoustic elements at the interface may appear distorted when viewed in the undeformed plot mode in the Visualization module of Abaqus/CAE. This distortion appears because the reference configuration for the acoustic nodes is updated automatically while the configuration for the non-acoustic nodes is not. The deformed plot at time=0 displays the correct mesh.

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, ${\mathbf{n}}_{\mathbf{1}}$, and that predicted by the interpolation of the rotated normals at the nodes, ${\mathbf{n}}_{\mathbf{2}}$, must satisfy the condition:

where you can specify the tolerance, $f_{tol}$. If you do not specify a tolerance value, a default value of $f_{tol}$ = 0.1 is used.

IMPORT CONTROLS, NORMAL TOL=$f_{tol}$