김경종
20 KiB
Data lines to redefine boundary conditions
*STEP, NLGEOM=YES
*STATIC
...
*END STEP
Transferring results between Abaqus/Standard and Abaqus/Explicit using models that are not defined as assemblies of part instances:
Abaqus/Standard analysis:
*HEADING
...
*MATERIAL, NAME=mat1
*ELASTIC
Data lines to define linear elasticity
*PLASTIC
Data lines to define Mises plasticity
*DENSITY
Data line to define the density of the material
...
*BOUNDARY
Data lines to define boundary conditions
*STEP
*STATIC
...
*RESTART, WRITE, FREQUENCY=n
*END STEP
Abaqus/Explicit analysis:
*HEADING
*IMPORT, STEP=step, INCREMENT=increment, STATE=YES, UPDATE=NO
Data lines to specify element sets to be imported
*IMPORT ELSET
Data lines to specify element set definitions to be imported
*IMPORT NSET
Data lines to specify node set definitions to be imported
**
*** Optionally redefine the material block
**
*MATERIAL, NAME=mat1
*ELASTIC
Data lines to redefine linear elasticity
*PLASTIC
Data lines to redefine Mises plasticity
...
*BOUNDARY
Data lines to redefine boundary conditions
*STEP
*DYNAMIC, EXPLICIT
...
*END STEP
Transferring results between Abaqus/Explicit and Abaqus/Standard using models defined as assemblies of part instances:
Abaqus/Explicit analysis:
*HEADING
*PART, NAME=Part-1
Node, element, section, set, and surface definitions
*END PART
*ASSEMBLY, NAME=Assembly-1
*INSTANCE, NAME=i1, PART=Part-1
<positioning data>
Additional set and surface definitions (optional)
*END INSTANCE
Assembly level set and surface definitions
...
*END ASSEMBLY
*MATERIAL, NAME=mat1
*ELASTIC
Data lines to define linear elasticity
*PLASTIC
Data lines to define Mises plasticity
*DENSITY
Data line to define the density of the material
...
*BOUNDARY
Data lines to define boundary conditions
*STEP
*DYNAMIC, EXPLICIT
...
*RESTART, WRITE, NUMBER INTERVAL=n
*END STEP
Abaqus/Standard analysis:
*HEADING
Part definitions (optional)
*ASSEMBLY, NAME=Assembly-1
*INSTANCE, INSTANCE=i1, LIBRARY=oldjob-name
Additional set and surface definitions (optional)
*IMPORT, STEP=step, INTERVAL=interval, STATE=YES, UPDATE=NO
*END INSTANCE
Additional part instance definitions (optional)
Assembly level set and surface definitions
...
*END ASSEMBLY
**
*** Optionally redefine the material block
**
*MATERIAL, NAME=mat1
*ELASTIC
Data lines to define linear elasticity
*PLASTIC
Data lines to define Mises plasticity
*DENSITY
Data line to define the density of the material
...
*BOUNDARY
Data lines to define boundary conditions
*STEP, NLGEOM=YES
*STATIC
...
*END STEP
Transferring results between Abaqus/Standard and Abaqus/Explicit using models defined as assemblies of part instances:
Abaqus/Standard analysis:
*HEADING
*PART, NAME=Part-1
Node, element, section, set, and surface definitions
*END PART
*ASSEMBLY, NAME=Assembly-1
*INSTANCE, NAME=i1, PART=Part-1
<positioning data>
Additional set and surface definitions (optional)
*END INSTANCE
Assembly level set and surface definitions
...
*END ASSEMBLY
*MATERIAL, NAME=mat1
*ELASTIC
Data lines to define linear elasticity
*PLASTIC
Data lines to define Mises plasticity
*DENSITY
Data line to define the density of the material
...
*BOUNDARY
Data lines to define boundary conditions
*STEP
*STATIC
...
*RESTART, WRITE, FREQUENCY=n
*END STEP
Abaqus/Explicit analysis:
*HEADING
Part definitions (optional)
*ASSEMBLY, NAME=Assembly-1
*INSTANCE, INSTANCE=i1, LIBRARY=oldjob-name
Additional set and surface definitions (optional)
*IMPORT, STEP=step, INCREMENT=increment, STATE=YES, UPDATE=NO
*END INSTANCE
Additional part instance definitions (optional)
Assembly level set and surface definitions
*END ASSEMBLY
**
*** Optionally redefine the material block
**
*MATERIAL, NAME=mat1
*ELASTIC
Data lines to redefine linear elasticity
*PLASTIC
Data lines to redefine Mises plasticity
...
*BOUNDARY
Data lines to redefine boundary conditions
*STEP
*DYNAMIC, EXPLICIT
...
*END STEP
9.2.3 TRANSFERRING RESULTS FROM ONE Abaqus/Standard ANALYSIS TO ANOTHER
Products: Abaqus/Standard 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 transfer desired results and model information from an Abaqus/Standard analysis to a new Abaqus/Standard 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 analysis. Subsequently, the model information and results from this analysis can be transferred to a second Abaqus/Standard 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 release of 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.
Comparison with the restart capability
Both the import and restart capabilities in Abaqus/Standard allow for the transfer of results and model information from one Abaqus/Standard analysis to another Abaqus/Standard analysis. However, the two capabilities have been designed for different applications.
The restart capability allows a completed Abaqus/Standard analysis to be restarted and continued. The entire model and results from the original analysis are transferred to the restart run, where additional analysis steps can be defined. Not much new model data can be specified in the restarted analysis; only model information such as new amplitude definitions, new node sets, and new element sets are allowed. Detailed information on the restart capability is given in “Restarting an analysis,” Section 9.1.1.
The import capability also allows a completed Abaqus/Standard analysis to be continued. In addition, this capability allows for the analysis to be continued with only desired components from the
original analysis; the entire model need not be transferred. New model data—such as elements, nodes, surfaces, contact pairs, etc.—can be specified during the import analysis. During the import analysis it is possible to choose whether only model information from the previous analysis is to be transferred or if the results associated with that model also are to be transferred.
For situations where the goal is to continue the original analysis with no change to the model information, it is recommended that the restart capability be used. For situations where the model information requires changes, or for cases where you require control over the transfer of results, the import capability should be used.
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/Standard 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). For each step of an analysis you can specify whether or not geometric nonlinearity should be included; 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 can be specified on the imported elements or nodes only under certain conditions. Table 9.2.3–1 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, with one exception: for initial temperature or field variable conditions, the reference configuration must be updated.
Table 9.2.3–1 Valid initial conditions.
| Initial condition | Material state imported? |
| Field variable | No |
| Hardening | No |
| Relative density | No |
| Rotational velocity | Yes or No |
| Solution-dependent state variables | No |
| Stress | No |
| Temperature | No |
| Velocity | Yes or No |
| Void ratio | No |
Procedures
Results can be imported only from a general analysis step involving static stress analysis, dynamic stress analysis, steady-state transport analysis, coupled temperature-displacement analysis, or thermalelectrical-structural 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.
When results are transferred from an Abaqus/Standard dynamic analysis to another Abaqus/Standard analysis where the first step is a static procedure, the initial out-of-balance forces must 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 previous Abaqus/Standard analysis.
Achieving static equilibrium when importing from a dynamic analysis to a static analysis
When the current state of a deformed body in a 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 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.
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 specified in the original analysis are not imported; they must be redefined 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 discussions on applying boundary conditions and multi-point constraints, see “Boundary conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.3.1, and “Kinematic constraints: overview,” Section 35.1.1.
Loads
Loads defined in the original analysis are not imported. Therefore, loads may 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/Standard.
Predefined fields
Temperatures, whether they are prescribed or are degrees of freedom (as in a coupled thermal-stress analysis), and field variables at nodes are imported if the material state is imported.
If the reference configuration is updated and the material state is imported, the initial conditions for temperatures and field variables at the imported nodes will be reset to the imported values; for example, the thermal strains will now be measured relative to the imported temperatures. If the reference configuration is updated but the material state is not imported, the initial conditions are reset to zero. In this case you can respecify the initial conditions on the imported nodes.
If the temperature is a state variable (as in an adiabatic analysis where temperature is an integration point quantity), it will be imported if the material state is imported.
Material options
All material property definitions and orientations associated with imported elements are imported by default. Material properties can be changed by respecifying the material property definitions with the same material name. In this case all relevant material properties must be redefined since the old definitions that were imported by default will be overwritten. Material orientations associated with imported elements can be changed only if the reference configuration is updated and the material state is not imported; the material orientations associated with imported elements cannot be redefined for other combinations of the reference configuration and material state.
Hyperelastic materials
When hyperelastic materials are imported, the state must be imported if the configuration is not updated; if the state is not imported, the configuration must be updated.
Material damping
The material model must be redefined in the import analysis if changes to material damping are required.
Changes to material definitions
When material definitions are changed, care must be taken to ensure that a consistent material state is maintained. It may sometimes be possible to simplify the material definition. For example, if a Mises plasticity model was used in the first Abaqus/Standard analysis and no further plastic yielding is expected in a subsequent Abaqus/Standard analysis, a linear elastic material can be used for the Abaqus/Standard analysis. However, if further nonlinear material behavior is expected, no changes to the existing material definitions should be made. The history of the state variables will not be maintained if the material models are not the same in both the original analysis and the import analysis.
Elements
The import capability is available for thermal-electrical-structural elements and a subset of the stress/displacement and coupled temperature-displacement continuum, shell, membrane, truss, rigid, and surface elements available in Abaqus/Standard. The complete list of supported elements is provided in Table 9.2.3–2. If elements that are removed (see “Element and contact pair removal and reactivation,” Section 11.2.1) are imported, they become active in the import analysis and should be removed in the first step of the import analysis.
Table 9.2.3–2 Element types that can be transferred from one Abaqus/Standard analysis to another.
| Element Type | Supported Elements |
| Plane strain continuum | CPE3, CPE3H, CPE3T, CPE4, CPE4H, CPE4HT, CPE4I, CPE4IH, CPE4R, CPE4RHT, CPE4RT, CPE4T |
| CPE6, CPE6H, CPE6M, CPE6MH, CPE6MHT, CPE6MT, CPE8, CPE8H, CPE8HT, CPE8R, CPE8RH, CPE8RHT, CPE8RT, CPE8T | |
| Plane stress continuum | CPS3, CPS3T, CPS4, CPS4I, CPS4R, CPS4T |
| CPS6, CPS6M, CPS6MT, CPS8, CPS8R, CPS8RT, CPS8T |