Products: Abaqus/Standard Abaqus/CAE
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.
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.
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 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 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.
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.
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.
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 thermal-electrical-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.
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.
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 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 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.
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.
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.
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.
The material model must be redefined in the import analysis if changes to material damping are required.
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.
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 | |
| Three-dimensional continuum | C3D4, C3D4H, C3D4T, C3D6, C3D6H, C3D6T, C3D8, C3D8H, C3D8HT, C3D8I, C3D8IH, C3D8R, C3D8RH, C3D8RHT, C3D8RT, C3D8S, C3D8HS, C3D8T, Q3D4, Q3D6, Q3D8, Q3D8H, Q3D8R, Q3D8RH |
| C3D10, C3D10H, C3D10HS, C3D10M, C3D10MH, C3D10MHT, C3D10MT, C3D15, C3D15H, C3D15V, C3D15VH, C3D20, C3D20H, C3D20HT, C3D20R, C3D20RHT, C3D20RT, C3D20T, C3D27, C3D27H, C3D27RH, Q3D10M, Q3D10MH, Q3D20, Q3D20H, Q3D20R, Q3D20RH | |
| Axisymmetric continuum | CAX3, CAX3H, CAX3T, CAX4, CAX4H, CAX4HT, CAX4I, CAX4IH, CAX4R, CAX4RH, CAX4RHT, CAX4RT, CAX4T |
| CAX6, CAX6M, CAX6MH, CAX6MHT, CAX6MT, CAX8, CAX8H, CAX8HT, CAX8R, CAX8RH, CAX8RHT, CAX8RT, CAX8T | |
| Membrane | M3D3, M3D4R |
| Two-dimensional rigid | R2D2 |
| Three-dimensional rigid | R3D3, R3D4 |
| Axisymmetric rigid | RAX2 |
| Three-dimensional shell | S4R, S3R, S4RT, S3RT, S4T, S3T |
| Axisymmetric shell | SAX1 |
| Continuum shell | SC6RT, SC8RT |
| Surface | SFM3D3, SFM3D4R |
| Two-dimensional truss | T2D2, T2D2T |
| Three-dimensional truss | T3D2, T3D2T |
| Cohesive | COH2D4, COHAX4, COH3D6, COH3D8 |
| Inertial | MASS, ROTARYI |
The following element types cannot be imported:
Acoustic elements
Axisymmetric-asymmetric continuum and shell elements
Beam elements
Connector elements
Coupled thermal-electrical elements
Diffusive heat transfer/mass diffusion elements and forced convection/diffusion elements
Generalized plane strain elements
Gasket elements
Heat capacitance elements
Infinite elements
Piezoelectric elements
Special-purpose elements
Substructures
User-defined elements
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.
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.
Most types of kinematic constraints specified in the original analysis are not imported and must be defined again in the import analysis; however, surface-based tie constraints are imported by default. See “Kinematic constraints: overview,” Section 35.1.1, for a discussion of the various types of kinematic constraints.
The various aspects of most surface-based mechanical contact definitions (including the surface, contact pair, and contact property definitions) can be imported. Thermal interactions, electrical interactions, and pore fluid surface interactions cannot be imported. Certain types of mechanical contact aspects—pressure, penetration loads, and debonded surfaces—cannot be imported. The most commonly used mechanical contact aspects—pressure-overclosure behavior, frictional behavior, and damping—can be imported.
The ability to import element-based and node-based surfaces is determined by whether or not the underlying elements and nodes defining these surfaces are imported. If the underlying elements or nodes of a surface are not imported, that surface will not be imported. If only some of the underlying nodes or elements used in the original definition of the surface are imported, only that part of the surface corresponding to the imported elements will be imported. Rigid surface definitions are imported when the associated slave surface is also imported. Contact pair definitions are imported provided that all the slave and master surfaces used in the original definition of the contact pair are also imported.
Contact conditions modeled with contact elements will be ignored during the transfer process.
The contact state associated with a stress/displacement analysis is imported if the material state is imported. If the reference configuration is updated, the accumulated contact strains will be set to zero. The contact state associated with thermal, electrical, or pore fluid surface interactions is not imported. The contact state associated with a crack propagation analysis is not imported; initially bonded contact surface definitions are not transferred. If a contact pair was inactive in the step from which the import was done due to the use of contact pair removal (see “Removing and reactivating contact pairs” in “Defining contact pairs in Abaqus/Standard,” Section 36.3.1), it must be deactivated again in the first step of the import analysis.
Additional contact information can be defined in the import analysis by specifying new surfaces, contact pairs, and interactions. New contact pair definitions can use the imported surface interaction definitions.
For a detailed description of the contact capabilities in Abaqus/Standard, refer to “Contact interaction analysis: overview,” Section 36.1.1.
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/Standard are listed in “Abaqus/Standard output variable identifiers,” Section 4.2.1.
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 UMAT.
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.
The import capability has the following known limitations. Where applicable, details are given in the relevant sections.
The same release of Abaqus/Standard must be run on computers that are binary compatible.
The capability is not available for fluid elements; infinite elements; and spring, dashpot, and connector elements. See the discussion on “Elements” earlier in this section for further details.
Surfaces are not imported when the model is defined as an assembly of part instances.
All elements and nodes must be included in at least one set in the original analysis when importing part instances.
The contact state associated with thermal, electrical, and pore fluid surface interactions is not imported; the contact state associated with crack propagation is not imported.
General contact definitions are 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.
Loads, boundary conditions, multi-point constraints, and equations 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.
When you import part instances individually from a previous analysis that was defined as an assembly of part instances, reference nodes associated with rigid body or coupling constraints defined on the imported instances will not be available in the import analysis for load or boundary condition application.
Pre-tension section definitions are not imported; they have to be redefined in the import analysis.
The capability is not available for elements with composite solid section definitions.
If the elements that are removed in the original analysis (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.
The symmetric model generation capability cannot be used in an import analysis in Abaqus/Standard.
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.
There may be a slight discontinuity during the transfer of state variables for analyses using fully integrated, first-order continuum elements if the elements are significantly deformed and the reference configuration is updated.
Mesh-independent spot welds (see “Mesh-independent fasteners,” Section 35.3.4) are not imported. However, the spot weld reference nodes are imported and can be used to redefine spot welds in the import analysis. The locations of the spot weld reference nodes and projection points are computed based upon the reference configuration of the import analysis. Therefore, if the deformed configuration of the imported model is significantly different from its reference configuration, it is recommended that the reference configuration be updated.
If the value of the friction coefficient is changed from the value given in the model data of the original analysis, the changed value must be respecified in the first step of the import analysis (see “Changing friction properties during an Abaqus/Standard analysis” in “Frictional behavior,” Section 37.1.5).
The capability is not available if adaptive meshing (see “ALE adaptive meshing and remapping in Abaqus/Standard,” Section 12.2.7) is used in the original analysis.
Enriched features (see “Modeling discontinuities as an enriched feature using the extended finite element method,” Section 10.7.1) are not imported.
Restart files from the original analysis are used in the analysis preprocessor and in the Abaqus/Standard execution in the import analysis. When the import job is run in parallel on computer clusters by using MPI-based parallelization, these restart files are copied to each host machine. The original job restart files are not decomposed to match the import analysis parallel domain and may be large relative to the local disk space available on the host machines. You can minimize this file size by requesting restart output only for the increment from which import will occur.
First 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, NLGEOM=YES *STATIC … *RESTART, WRITE *END STEP
Abaqus/Standard import 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 define additional model information ** *BOUNDARY Data lines to redefine boundary conditions *STEP, NLGEOM=YES *STATIC … *END STEP
First 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/Standard 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, INCREMENT=increment, 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, NLGEOM=YES *STATIC … *END STEP