9.2.4 Transferring results from one Abaqus/Explicit analysis to another
Products: Abaqus/Explicit Abaqus/CAE
References
Overview
Abaqus provides the capability to transfer desired results and model information from an Abaqus/Explicit analysis to a new Abaqus/Explicit 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/Explicit analysis. Subsequently, the model information and results from this analysis can be transferred to a second Abaqus/Explicit 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/Explicit 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/Explicit allow for the transfer of results and model information from one Abaqus/Explicit analysis to another Abaqus/Explicit analysis. However, the two capabilities have been designed for different applications.
The restart capability allows a completed Abaqus/Explicit 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/Explicit 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/Explicit 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/Explicit uses a large-strain formulation. 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 9.2.4–1 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.
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 temperature-displacement 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 |
| 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 )
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.
Input file template
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