김경종
18 KiB
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 9.2.4–1 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 |
Boundary conditions
Boundary conditions (including connector motion) 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, including those applied for connector actuation, 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/Explicit.
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.
Connector elements
When connector elements are imported, any associated connector behavior definitions are imported by default. The imported connector behavior definitions can be modified only if the state is not imported.
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/Explicit analysis and no further plastic yielding is expected in a subsequent Abaqus/Explicit analysis, a linear elastic material can be used for the subsequent Abaqus/Explicit 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 a subset of the stress/displacement and coupled temperaturedisplacement continuum, shell, membrane, truss, connector, rigid, and surface elements available in Abaqus/Explicit. The complete list of supported elements is provided in Table 9.2.4–2. 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 9.2.4–2 Element types that can be transferred from one Abaqus/Explicit analysis to another.
| Element Type | Supported Elements |
| Plane strain continuum | CPE3, CPE4R, CPE4RT, CPE6M, CPE6MT, CPE3T |
| Plane stress continuum | CPS3, CPS4R, CPS4RT, CPS6M, CPS6MT, CPS3T |
| Three-dimensional continuum | C3D4, C3D4T, C3D6, C3D6T, C3D8R, C3D8RT, C3D10M, C3D10MT, C3D8, C3D8T, C3D8I |
| Axisymmetric continuum | CAX3, CAX4R, CAX3T, CAX4RT, CAX6M, CAX6MT |
| Membrane | M3D3, M3D4 M3D4R |
| Two-dimensional rigid | R2D2 |
| Three-dimensional rigid | R3D3, R3D4 |
| Axisymmetric rigid | RAX2 |
| Three-dimensional shell | S4R, S3R, S3, S4, S4RS, S4RSW, S3RS, S3T, S3RT, S4T, S4RT |
| Element Type | Supported Elements |
| Continuum shell elements | SC6R, SC8R, SC6RT, SC8RT |
| Axisymmetric shell | SAX1 |
| Surface | SFM3D3, SFM3D4R |
| Two-dimensional truss | T2D2 |
| Three-dimensional truss | T3D2 |
| Two-dimensional beam | B21, B22 |
| Three-dimensional beam | B31, B32 |
| Connector elements | CONN2D2, CONN3D2 |
| Cohesive | COH2D4, COHAX4, COH3D6, COH3D8 |
| Infinite elements | CINPS4, CINPE4, CINAX4, CIN3D8, ACIN2D2, ACIN3D3, ACINAX2 |
| Acoustic elements | AC2D3, AC2D4R, AC3D4, AC3D6, ACAX3, ACAX4R, AC3D8R |
| Inertial elements | MASS, ROTARYI |
The following element types cannot be imported:
• Heat capacitance elements
• Eulerian elements (EC3D8R and EC3D8RT)
• Particle elements (PC3D )
In addition, the following restrictions apply to the import capability:
• Rebars defined using rebar layers (“Defining reinforcement,” Section 2.2.3) are imported provided the underlying elements are also imported. Rebar reinforcements defined using the embedded element technique (“Embedded elements,” Section 35.4.1) are imported if the host and embedded elements used in this definition are also imported. Rebars defined as an element property (“Defining rebar as an element property,” Section 2.2.4) cannot be imported.
• If connector elements are imported, the configuration can be updated provided that the state is not imported and the state can be imported provided that the configuration is not updated.
• A rigid body containing both deformable and rigid elements cannot be imported. A rigid body that includes rigid elements is imported when the element set used to define the rigid body is specified for import. A rigid body that includes deformable elements is imported when the element set used to define the rigid body is specified for import. The imported rigid body definition is overwritten if it is respecified using the same element set. When the model is defined in terms of an assembly of part instances, the reference node of an imported rigid body must belong to an imported instance.
• When a rigid body is imported, any associated data such as pin node sets and tie node sets are part of the imported definition. However, these sets as imported contain only those nodes that are connected to the imported elements.
Constraints
Kinematic constraints (including multi-point constraints and surface-based tie constraints) specified in the original analysis are not imported and must be defined again in the import analysis. See “Kinematic constraints: overview,” Section 35.1.1, for a discussion of the various types of kinematic constraints.
Interactions
For general contact, the contact state is imported if general contact is defined in both analyses. Contact states are not imported for elements contained in element sets that are imported more than once.
For contact defined by contact pairs, contact definitions specified in the original analysis and the contact state are not imported. Contact can be defined again in the import analysis by specifying the surfaces and contact pairs.
Additional contact information can be defined in the import analysis by specifying new surfaces, contact pairs, and interactions.
For a detailed description of the contact capabilities in Abaqus/Explicit, refer to “Contact interaction analysis: overview,” Section 36.1.1.
Output
Output can be requested for an import analysis in the same way as for an analysis in which the results are not imported. Output requests in the original analysis are not transferred to the import analysis; output requests in the import analysis have to be respecified. The output variables available in Abaqus/Explicit are listed in “Abaqus/Explicit output variable identifiers,” Section 4.2.2.
The values of the following material point output variables will be continuous in an import analysis when the material state is imported: stress, equivalent plastic strain (PEEQ), and solution-dependent state variables (SDV) for VUMAT. Similarly, for a connector behavior, the plastic relative displacement (CUP), kinematic hardening shift force (CALPHAF), overall damage (CDMG), damage initiation criteria (CDIF, CDIM, CDIP), friction accumulated slip (CASU), and connector status (CSLST, CFAILST) will be continuous.
If the reference configuration is not updated, the displacements, strains, whole element variables, section variables, and energy quantities will be reported relative to the original configuration.
If the reference configuration is updated, displacements, strains, whole element variables, section variables, and energy quantities will not be continuous in an import analysis and will be reported relative to the updated reference configuration.
Time and step number will not be continuous between the original and the import analyses if the reference configuration is updated. Time and step number will be continuous only if the reference configuration is not updated.
Limitations
The import capability has the following known limitations. Where applicable, details are given in the relevant sections.
• The same release of Abaqus/Explicit must be run on computers that are binary compatible.
• The capability is not available for spring and dashpot elements. See the discussion on “Elements” earlier in this section for further details.
• If connector elements are imported, the configuration can be updated provided that the state is not imported and the state can be imported provided that the configuration is not updated.
• Surfaces are not imported.
• All elements and nodes must be included in at least one set in the original analysis when importing part instances.
• The rigid body must be redefined if the element set containing the assigned elements is imported more than once.
• Embedded elements must be redefined if the host element set is imported more than once in an Abaqus/Explicit import analysis.
• The contact state for contact pairs is not imported.
• If the material state is imported, only stresses will be imported for material models other than those defined by linear elasticity, hyperelasticity, hyperfoam, viscoelasticity, Mises plasticity, and damage for cohesive elements. See “Importing the material state” in “Transferring results between Abaqus analyses: overview,” Section 9.2.1, for details. For a connector behavior, the plastic displacements, the frictional slip, and the damage state are imported and the connector forces are recomputed. See “Importing the material state” in “Transferring results between Abaqus analyses: overview,” Section 9.2.1, for details.
• Loads, boundary conditions, multi-point constraints, equations, and surface-based tie constraints are not imported.
• Kinematic and distributing coupling constraints are not imported. In addition, the reference node of a coupling constraint will not be imported unless the reference node is part of another element definition that is imported.
• The results file, restart file, or output database file generated during the import analysis is not appended to the results file, restart file, or output database file of the original analysis.
• Mesh-independent spot welds (see “Mesh-independent fasteners,” Section 35.3.4) and tie constraints (see “Mesh tie constraints,” Section 35.3.1) are not imported. These constraints can be redefined in the import analysis and are formed using the reference configuration of the import model. If the reference configuration is updated, the redefined constraints may not match the old constraints exactly due to the differences in geometry. If new constraints are defined and the reference configuration of the import model is not updated, they may not initially be in compliance if the nodes involved in the constraint have nonzero displacements. This may cause numerical difficulty and potential abort of the import analysis. In this case it is recommended that you update the reference configuration upon import.
Transferring results using models that are not defined as assemblies of part instances:
First Abaqus/Explicit 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
*DYNAMIC, EXPLICIT
...
*RESTART, WRITE, NUMBER INTERVAL=n
*END STEP
Abaqus/Explicit import analysis:
*HEADING
*IMPORT, STEP=step, INTERVAL=interval, 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 define additional model information
**
*BOUNDARY
Data lines to redefine boundary conditions
*STEP
*DYNAMIC, EXPLICIT
...
*END STEP
Transferring results using models defined as assemblies of part instances:
First 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/Explicit import 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 define additional model information
**
*BOUNDARY
Data lines to define boundary conditions
*STEP
*DYNAMIC, EXPLICIT
...
*END STEP