ProductsAbaqus/StandardAbaqus/CAE Comparison with the restart capabilityBoth 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. 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 analysisAdditional 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 definitionsNew 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). 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 transformationNodal transformations (Transformed coordinate systems) 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 analysisBy 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 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 nodesInitial conditions can be specified on the imported elements or nodes only under certain conditions. Table 1 lists the initial conditions that are allowed depending on whether or not the material state is imported (see Importing the material state). 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.
ProceduresResults 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 perturbation procedures) 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 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 analysisWhen 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:
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 conditionsBoundary 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) 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). If boundary conditions in the original analysis are applied in a transformed coordinate system (see Transformed coordinate systems), 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 and About Kinematic Constraints. LoadsLoads 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) 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). If point loads in the original analysis are applied in a transformed coordinate system (see Transformed coordinate systems) 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 About loads for an overview of the loading types available in Abaqus/Standard. Predefined fieldsTemperatures, 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 optionsAll 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 materialsWhen 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 dampingThe material model must be redefined in the import analysis if changes to material damping are required. Changes to material definitionsWhen 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. ElementsThe 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 2. If elements that are removed (see Element and contact pair removal and reactivation) are imported, they become active in the import analysis and should be removed in the first step of the import analysis.
The following element types cannot be imported:
In addition, the following restrictions apply to the import capability:
ConstraintsMost 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 About Kinematic Constraints for a discussion of the various types of kinematic constraints. InteractionsThe 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, cohesive behavior, 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), 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 About contact interactions. OutputOutput 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. 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. LimitationsThe import capability has the following known limitations. Where applicable, details are given in the relevant sections.
Input file templateTransferring results using models that are not defined as assemblies of part instances: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 Transferring results using models defined as assemblies of part instances: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 |