김경종
27 KiB
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).
Mass adjustment contributions (see “Adjust and/or redistribute mass of an element set,” Section 2.6.1) 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,” Section 2.7.1) 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,” 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.
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,” 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.
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.
Input File Usage: *IMPORT, STEP=step, INCREMENT=increment For models that are defined as assemblies of part instances, the *IMPORT option must appear within a part instance definition.
Abaqus/CAE Usage: In Abaqus/CAE you can import model data and results only from models that are defined as assemblies of part instances.
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
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.
Input File Usage: *IMPORT, STEP=step, ITERATION=iteration For models that are defined as assemblies of part instances, the *IMPORT option must appear within a part instance definition.
Abaqus/CAE Usage: In Abaqus/CAE you can import model data and results only from models that are defined as assemblies of part instances.
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
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.
Input File Usage: *IMPORT, STEP=step, INTERVAL=interval For models that are defined as assemblies of part instances, the *IMPORT option must appear within a part instance definition.
Abaqus/CAE Usage: In Abaqus/CAE you can import model data and results only from models that are defined as assemblies of part instances.
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
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” in “Controlling initial contact status in Abaqus/Standard,” Section 36.2.4; “Controlling initial contact status in Abaqus/Standard,” Section 36.2.4; “Controlling initial contact status for general contact in Abaqus/Explicit,” Section 36.4.4; and “Adjusting initial surface positions and specifying initial clearances for contact pairs in Abaqus/Explicit,” Section 36.5.4.
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.
Input File Usage:
Use the following option to specify that the reference configuration is to be updated to the imported configuration:
* \text { IMPORT }, \text { STEP } = \text { step }, \text { UPDATE } = \text { YES }
Use the following option to specify that the reference configuration should not be updated to the imported configuration:
* \text { IMPORT }, \text { STEP } = \text { step }, \text { UPDATE } = \text { NO }
For models that are defined as assemblies of part instances, the *IMPORT option must appear within a part instance definition.
Abaqus/CAE Usage: In Abaqus/CAE you can import model data and results only from models that are defined as assemblies of part instances.
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
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; 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.
Input File Usage: Use the following option to specify that the material state should be imported:
*IMPORT, STATE=YES
Use the following option to specify that the material state should not be imported:
*IMPORT, STATE=NO
For models that are defined as assemblies of part instances, the *IMPORT option must appear within a part instance definition.
Abaqus/CAE Usage: In Abaqus/CAE you can import model data and results only from models that are defined as assemblies of part instances. Abaqus/CAE always imports the material state. If you want to import only the deformed mesh, you can import an orphan mesh from a selected step and increment of an output database; see “What kinds of files can be imported and exported from Abaqus/CAE?,” Section 10.1.1 of the Abaqus/CAE User’s Guide.
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 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.
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, \mathbf { n _ { 1 } } , and that predicted by the interpolation of the rotated normals at the nodes, , must satisfy the condition:
1 - f _ {t o l} \leq | \mathbf {n _ {1}} \cdot \mathbf {n _ {2}} |,
where you can specify the tolerance, f _ { t o l } . If you do not specify a tolerance value, a default value of f _ { t o l } = 0.1 is used.
Input File Usage: If you update the reference configuration to be the imported configuration, you can specify a tolerance for error checking on shell normals:
* \text { IMPORT CONTROLS, NORMAL TOL } = f _ {t o l}
Abaqus/CAE Usage: The shell normal tolerance is not supported in Abaqus/CAE.
9.2.2 TRANSFERRING RESULTS BETWEEN Abaqus/Explicit AND Abaqus/Standard
Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE
References
• “Transferring results between Abaqus analyses: overview,” Section 9.2.1
• *IMPORT
• *IMPORT ELSET
• *IMPORT NSET
• *IMPORT CONTROLS
• *INSTANCE
• “Transferring results between Abaqus analyses,” Section 16.6 of the Abaqus/CAE User’s Guide
Overview
Abaqus provides the capability to import a deformed mesh and its associated material state from Abaqus/Standard into Abaqus/Explicit and vice versa. In addition, new model information can be specified during the import analysis. This capability is useful for problems that involve several analysis stages. For example, in manufacturing processes the preloading can be analyzed using Abaqus/Standard and the subsequent forming operation can be simulated using Abaqus/Explicit. Finally, the springback of the material can be performed in Abaqus/Standard.
For this capability to work, the same release of Abaqus/Explicit and Abaqus/Standard must be run on computers that are binary compatible.
Information about how to transfer results between Abaqus analyses is provided in “Transferring results between Abaqus analyses: overview,” Section 9.2.1.
Specifying new data in an import analysis
Additional model definitions such as new elements, nodes, surfaces, etc. can be defined during the import analysis. Initial conditions can also be specified during the import analysis.
New model definitions
New nodes, elements, and material properties can be added to the model in an import analysis once import has been specified. Nodal coordinates must be defined in the updated configuration, regardless of whether or not the reference configuration is updated on import (see “Updating the reference configuration” in “Transferring results between Abaqus analyses: overview,” Section 9.2.1). The usual Abaqus input can be used. Imported material definitions can be used with the new elements (which will need new section property definitions).
Nodal transformation
Nodal transformations (“Transformed coordinate systems,” Section 2.1.5) are not imported; transformations can be defined independently in the import analysis. Continuous displacements, velocities, etc. are obtained only if the nodal transformations in the import analysis are the same as those in the original analysis. Use of the same transformations is also recommended for nodes with boundary conditions or point loads defined in a local system.
Specifying geometric nonlinearity in an import analysis
By default, Abaqus/Standard uses a small-strain formulation (i.e., geometric nonlinearity is ignored) and Abaqus/Explicit uses a large-deformation formulation (i.e., geometric nonlinearity is included). For each step of an analysis you can specify which formulation should be used; see “Geometric nonlinearity” in “General and linear perturbation procedures,” Section 6.1.3, for details.
The default value for the formulation in an import analysis is the same as the value at the time of import. Once the large-displacement formulation is used during a given step in any analysis, it will remain active in all the subsequent steps, whether or not the analysis is imported.
If the small-displacement formulation is used at the time of import, the reference configuration cannot be updated.
Specifying initial conditions for imported elements and nodes
Initial conditions (“Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.2.1) can be specified on the imported elements or nodes only under certain conditions. Table 9.2.2–1 lists the initial conditions that are allowed depending on whether or not the material state is imported (see “Importing the material state” in “Transferring results between Abaqus analyses: overview,” Section 9.2.1). The reference configuration can be updated or not, as desired.
Table 9.2.2–1 Valid initial conditions.
| Initial condition | Material state imported? |
| Hardening | No |
| Relative density | No |
| Rotational velocity | Yes or No |
| Solution-dependent state variables | No |
| Stress | No |
| Velocity | Yes or No |
| Void ratio | No |
Procedures
Results can be imported into Abaqus/Explicit only from a general analysis step involving static stress analysis, dynamic stress analysis, or steady-state transport analysis in Abaqus/Standard. Results transfer from linear perturbation procedures (“General and linear perturbation procedures,” Section 6.1.3) is not allowed.
Abaqus/Standard offers several analysis procedures that can be used in an import analysis. These procedures can be used to perform an eigenvalue analysis, static or dynamic stress analysis, buckling analysis, etc. See “Solving analysis problems: overview,” Section 6.1.1, for a discussion of the available procedures.
For springback analysis of a formed component the first step in the Abaqus/Standard analysis usually consists of a static analysis procedure so that the initial out-of-balance forces can be removed gradually from the system. The removal of these forces is performed automatically by Abaqus/Standard during the first static analysis step, as described below. If the first step in the Abaqus/Standard analysis is not a static step (such as a dynamic step), the analysis proceeds directly from the state imported from the Abaqus/Explicit analysis.
Achieving static equilibrium when importing into Abaqus/Standard
When the current state of a deformed body in an explicit dynamic analysis is imported into a static analysis, the model will not initially be in static equilibrium. Initial out-of-balance forces must be applied to the deformed body in dynamic equilibrium to achieve static equilibrium. Both dynamic forces (inertia and damping) and boundary interaction forces contribute to the initial out-of-balance forces. The boundary forces are the result of interactions from fixed boundary and contact conditions. Any changes in the boundary and contact conditions from the Abaqus/Explicit analysis to the Abaqus/Standard analysis will contribute to the initial out-of-balance forces.
In general the instantaneous removal of the initial out-of-balance forces in a static analysis will lead to convergence problems. Hence, these forces need to be removed gradually until complete static equilibrium is achieved. During this process of removing the out-of-balance forces, the body will deform further and a redistribution of internal forces will occur, resulting in a new stress state. (This is essentially what occurs during “springback,” when a formed product is removed from the worktools.)
When the first step in the Abaqus/Standard import analysis is a static procedure, the following algorithm is used to remove the initial out-of-balance forces automatically:
- The imported stresses are defined at the start of the analysis as the initial stresses in the material.
- An additional set of artificial stresses is defined at each material point. These stresses are equal in magnitude to the imported stresses but are of opposite sign. The sum of the material point stresses and these artificial stresses, thus, creates zero internal forces at the beginning of the step.
- The internal artificial stresses are ramped off linearly in time during the first step. Thus, at the end of the step the artificial stresses have been removed completely and the remaining stresses in the material will be the residual stress state associated with static equilibrium.
Once static equilibrium has been obtained, subsequent steps can be defined using any analysis procedure that would normally follow a static analysis in Abaqus.
When the first step is not a static analysis, no artificial stress state is applied and the imported stresses are used in the internal force computations for the element.
Boundary conditions
Boundary conditions, including any connector motion, specified in the original analysis are not imported. They must be defined again in the import analysis. In some cases nonzero boundary conditions imposed in the original analysis need to be maintained at the same values in the import analysis when the imported configuration is not updated. In such cases you can prescribe a constant (step function) amplitude variation for the analysis step (see “Prescribing nondefault amplitude variations” in “Defining an analysis,” Section 6.1.2) so that the newly applied boundary conditions are applied instantaneously and held at that value for the duration of the step. Alternatively, you can refer to an amplitude curve in the boundary condition definition (see “Amplitude curves,” Section 34.1.2). If boundary conditions in the original analysis are applied in a transformed coordinate system (see “Transformed coordinate systems,” Section 2.1.5), the same coordinate system should be defined and used in the import analysis.
For a discussion of applying boundary conditions, see “Boundary conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.3.1.
Loads
Loads, including those applied for connector actuation, defined in the original analysis are not imported. Loads may, therefore, need to be redefined in the import analysis. There are no restrictions on the loads that can be applied when results are imported from one analysis to the other. In cases when the loads need to be maintained at the same values as in the original analysis, you can prescribe a constant (step function) amplitude variation for the analysis step (see “Prescribing nondefault amplitude variations” in “Defining an analysis,” Section 6.1.2) to apply the loads instantaneously at the start of the step and hold them for the duration of the step. Alternatively, you can refer to an amplitude curve in the load definition (see “Amplitude curves,” Section 34.1.2). If point loads in the original analysis are applied in a transformed coordinate system (see “Transformed coordinate systems,” Section 2.1.5) and the loads must be maintained in the import analysis, the load application is simplified if the same coordinate system is defined and used in the import analysis.
See “Applying loads: overview,” Section 34.4.1, for an overview of the loading types available in Abaqus.
Predefined fields
The field variables at nodes are not imported. If the elements being imported are coupled temperaturedisplacement elements, the temperature is imported if the associated material state is imported. The temperature is also imported for an adiabatic analysis if the associated material state is imported. For all other cases the temperatures at nodes are not imported.
If the original analysis uses predefined temperature fields (“Predefined temperature” in “Predefined fields,” Section 34.6.1) to vary the temperatures at nodes, the import analysis will not be allowed to continue. If the original analysis uses predefined field variable definitions (“Predefined field variables” in “Predefined fields,” Section 34.6.1) to vary the field variables at nodes, the import analysis will