Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE
“Transferring results between Abaqus analyses: overview,” Section 9.2.1
“Transferring results between Abaqus analyses,” Section 16.6 of the Abaqus/CAE User's Manual
Abaqus provides the capability to import a deformed mesh and its associated material state from Abaqus/Standard into Abaqus/Explicit and vice versa. In addition, new model information can be specified during the import analysis. This capability is useful for problems that involve several analysis stages. For example, in manufacturing processes the preloading can be analyzed using Abaqus/Standard and the subsequent forming operation can be simulated using Abaqus/Explicit. Finally, the springback of the material can be performed in Abaqus/Standard.
For this capability to work, the same release of Abaqus/Explicit and 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.
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 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) and Abaqus/Explicit uses a large-deformation formulation (i.e., geometric nonlinearity is included). For each step of an analysis you can specify which formulation should be used; see “Geometric nonlinearity” in “General and linear perturbation procedures,” Section 6.1.2, 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 (“Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 32.2.1) can be specified on the imported elements or nodes only under certain conditions. Table 9.2.2–1 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.
Results can be imported into Abaqus/Explicit only from a general analysis step involving static stress analysis, dynamic stress analysis, or steady-state transport analysis in Abaqus/Standard. Results transfer from linear perturbation procedures (“General and linear perturbation procedures,” Section 6.1.2) 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 “Procedures: overview,” Section 6.1.1, for a discussion of the available procedures.
For springback analysis of a formed component the first step in the Abaqus/Standard analysis usually consists of a static analysis procedure so that the initial out-of-balance forces can 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 Abaqus/Explicit analysis.
When the current state of a deformed body in an explicit 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 from the Abaqus/Explicit analysis to the Abaqus/Standard analysis 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, including any connector motion, specified in the original analysis are not imported. They must be defined again 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 “Procedures: overview,” Section 6.1.1) 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 32.1.2). 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 a discussion of applying boundary conditions, see “Boundary conditions in Abaqus/Standard and Abaqus/Explicit,” Section 32.3.1.
Loads, including those applied for connector actuation, defined in the original analysis are not imported. Loads may, therefore, 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 “Procedures: overview,” Section 6.1.1) 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 32.1.2). 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 32.4.1, for an overview of the loading types available in Abaqus.
The field variables at nodes are not imported. If the elements being imported are coupled temperature-displacement elements, the temperature is imported if the associated material state is imported. The temperature is also imported for an adiabatic analysis if the associated material state is imported. For all other cases the temperatures at nodes are not imported.
If the original analysis uses predefined temperature fields (“Predefined temperature” in “Predefined fields,” Section 32.6.1) to vary the temperatures at nodes, the import analysis will not be allowed to continue. If the original analysis uses predefined field variable definitions (“Predefined field variables” in “Predefined fields,” Section 32.6.1) to vary the field variables at nodes, the import analysis will be allowed to continue only if all the elements being imported are coupled temperature-displacement elements; however, the field variables are not imported. If the original analysis uses initial temperature (“Defining initial temperatures” in “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 32.2.1) and field variable (“Defining initial values of predefined field variables” in “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 32.2.1) conditions, the import analysis will be allowed to continue only if all the elements being imported are coupled temperature-displacement elements.
In addition, specification of initial conditions for temperatures and field variables is not allowed in an import analysis, unless all the elements being imported are coupled temperature-displacement elements. In this case initial conditions for temperatures and field variables can be specified on the imported nodes if the reference configuration is updated and the material state is not imported. Initial temperatures can be specified in the import analysis if it is an adiabatic analysis.
All material property definitions and the 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. 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 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.
If mass scaling (“Mass scaling,” Section 11.6.1) is used in Abaqus/Explicit, the scaled masses will not be transferred to the subsequent import analysis in Abaqus/Standard. The mass of the model for the Abaqus/Standard analysis will be based on either the imported or the redefined density definitions.
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 Abaqus/Explicit analysis and no further plastic yielding is expected in the Abaqus/Standard analysis (as is generally the case for springback simulations), 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 first-order continuum, modified triangular and tetrahedral elements, conventional shell, continuum shell, membrane, beam (both linear and quadratic), pipe (linear), truss, connector, rigid, and surface elements that are common to both Abaqus/Explicit and Abaqus/Standard, as defined in Table 9.2.2–2.
Table 9.2.2–2 Common element types that can be transferred between Abaqus/Explicit and Abaqus/Standard.
| Common element types |
|---|
| CPS3, CPS3T, CPS4R, CPS4RT, CPS6M, CPS6MT |
| CPE3, CPE3T, CPE4R, CPE4RT, CPE6M, CPE6MT |
| CAX3, CAX3T, CAX4R, CAX4RT, CAX6M, CAX6MT |
| C3D4, C3D4T, C3D6, C3D6T, C3D8, C3D8R, C3D8T, C3D8RT, C3D10M, C3D10MT |
| M3D3, M3D4, M3D4R |
| R2D2 |
| R3D3, R3D4 |
| RAX2 |
| S4, S4R, S3R, S4RT, S3RT |
| SC8R, SC8RT, SC6R, SC6RT |
| SAX1 |
| SFM3D3, SFM3D4R |
| T2D2 |
| T3D2 |
| B21, B22, PIPE21 |
| B31, B32, PIPE31 |
| CONN2D21, CONN3D21 |
| AC2D3, AC2D4R, AC2D4, ACIN2D2 |
| AC3D4, AC3D6, AC3D8R, AC3D8, ACIN3D3, ACIN3D4 |
| ACAX3, ACAX4R, ACAX4, ACINAX2 |
| COH2D4, COHAX4, COH3D6, COH3D8 |
| 1Connector elements can be imported from Abaqus/Standard to Abaqus/Explicit; but not vice versa. |
The following restrictions apply to the import capability:
Connector elements can be imported from Abaqus/Standard to Abaqus/Explicit but not vice versa. Further, 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.
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 33.4.1) 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.
Infinite elements and fluid elements cannot be imported.
Rigid elements for which the thickness is interpolated from the nodes in an Abaqus/Explicit analysis will not be imported into Abaqus/Standard.
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 into Abaqus/Explicit 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.
Failed elements in Abaqus/Explicit will not be imported into Abaqus/Standard.
Elements that are being removed or are inactive (see “Element and contact pair removal and reactivation,” Section 11.2.1) in Abaqus/Standard will not be imported into Abaqus/Explicit.
Rigid surfaces will not be imported.
When importing results from an Abaqus/Explicit analysis to an Abaqus/Standard analysis, each element set specified can contain only compatible element types listed in Table 9.2.2–3 and can contain at most three different element types.
Table 9.2.2–3 Compatible element types.
| ACINAX2, ACIN2D2, ACIN3D3, ACIN3D4 |
| CPE4R, CPE3, AC2D3, AC2D4 |
| CPS4R, CPS3 |
| CAX4R, CAX3, ACAX3, ACAX4 |
| AC3D4, AC3D6, AC3D8, C3D8, C3D8R, C3D4, C3D6 |
| M3D4R, M3D3, M3D4 |
| R3D3, R3D4 |
| S4R, S3R, SC6R, SC8R, S4 |
| SFM3D3, SFM3D4R |
| CAX6M, C3D10M |
| C3D8T, C3D4T, C3D6T |
| SC6RT, SC8RT, S4T, S4RT, S3T, S3RT |
When transferring results between Abaqus/Standard and Abaqus/Explicit, it is important that the hourglass forces are computed consistently. The enhanced hourglass control formulation (see “Enhanced hourglass control approach in Abaqus/Standard and Abaqus/Explicit” in “Section controls,” Section 26.1.4) is recommended for computing hourglass forces in the original as well as all subsequent import analyses.
Once section controls have been defined in the original analysis, they cannot be modified in any subsequent Abaqus/Standard or Abaqus/Explicit analysis. Therefore, if section controls are to be used in any one analysis in a series of import analyses, they must be specified in the very first analysis. The section controls specified for an element set in the original analysis will be used for the elements belonging to that element set in all subsequent import analyses.
Section controls other than the hourglass control formulation have appropriate defaults depending on the type of analysis and, generally, do not need to be changed. Nondefault values can be chosen subject to certain restrictions.
In an Abaqus/Standard analysis only the average strain kinematic formulation and second-order accurate element formulation are available; other kinematic formulations, element formulations, or section controls that are relevant only in an Abaqus/Explicit analysis can be specified in the Abaqus/Standard analysis. Such controls will be ignored in the Abaqus/Standard analysis but retained for the subsequent Abaqus/Explicit import analysis.
If a kinematic formulation other than average strain is used for solid elements in the Abaqus/Explicit analysis, the differences in the kinematic formulations may lead to errors in Abaqus/Standard if the elements are distorted or undergo large rotations.
Using the first-order accurate element formulation (default) in Abaqus/Explicit and the second-order accurate element formulation (the only available formulation) in Abaqus/Standard is not expected to cause significant errors, since the time increment size in Abaqus/Explicit is inherently small. One exception to this is when the Abaqus/Explicit analysis involves components undergoing several revolutions, in which case it is recommended that the second-order accurate element formulation be used in Abaqus/Explicit.
| Input File Usage: | Use the following options in the original analysis: |
*MEMBRANE SECTION, CONTROLS=name1, ELSET=elset1 *SHELL SECTION, CONTROLS=name2, ELSET=elset2 *SHELL GENERAL SECTION, CONTROLS=name3, ELSET=elset3 *SOLID SECTION, CONTROLS=name4, ELSET=elset4 Use options similar to the following one in the original analysis: *SECTION CONTROLS, NAME=name1 |
| Abaqus/CAE Usage: | Define section controls when you assign the element type in the original analysis: |
Mesh module: Mesh |
The computations for membrane and shell element thicknesses are described below.
For shells defined using a general shell section, the current thickness is computed based on the effective Poisson's ratio, which is 0.5 by default, in both Abaqus/Explicit and Abaqus/Standard.
| Input File Usage: | *SHELL GENERAL SECTION, POISSON= |
| Abaqus/CAE Usage: | Property module: homogeneous or composite shell section editor: Section integration: Before analysis: Advanced: Section Poisson's ratio |
For shells defined using shell sections integrated during analysis and for membranes in Abaqus/Standard, the current thickness is computed based on the effective Poisson's ratio, which is 0.5 by default. In Abaqus/Explicit, on the other hand, the computation of the thickness could be based either on the effective Poisson's ratio or the through-thickness strains, with the computation based on the through-thickness strains used by default.
If you do not specify a section Poisson's ratio for shell sections integrated during analysis or for membrane sections in an original Abaqus/Explicit or Abaqus/Standard analysis, the thickness computations in the original and all subsequent import analyses are carried out using the default methods. In other words, the thicknesses in all Abaqus/Standard analyses are computed using the default effective Poisson's ratio of 0.5, while the thicknesses in all Abaqus/Explicit analyses are computed using the through-thickness strains.
When the section Poisson's ratio is assigned a numerical value in an original Abaqus/Standard or Abaqus/Explicit analysis, the thickness computations in the original analysis and all subsequent import analyses are performed using the specified value for the effective Poisson's ratio.
| Input File Usage: | Use one of the following options: |
*SHELL SECTION, POISSON= *SHELL SECTION, POISSON=MATERIAL *MEMBRANE SECTION, POISSON= *MEMBRANE SECTION, POISSON=MATERIAL |
| Abaqus/CAE Usage: | Property module: Homogeneous or composite shell section editor: Section integration: During analysis: Advanced: Section Poisson's ratio Membrane section editor: Section Poisson's ratio |
The contact angle, 
, made by the belt wrapping around node b (see “Connection-type library,” Section 30.1.5) is computed automatically in Abaqus/Explicit, ignoring the value specified within the Abaqus/Standard analysis.
Most types of 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; however, embedded element constraints are imported by default. See “Kinematic constraints: overview,” Section 33.1.1, for a discussion of the various types of kinematic constraints.
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; however, you may not be able to use the exact contact definitions that were used in the original analysis because of differences in the contact capabilities between Abaqus/Standard and Abaqus/Explicit.
The contact constraint enforcement may be different in Abaqus/Standard and Abaqus/Explicit. Examples of potential causes for differences include:
Abaqus/Standard typically uses a “pure master-slave” approach, whereas Abaqus/Explicit typically uses a “balanced master-slave” approach.
Depending on the contact formulations used, Abaqus/Standard and Abaqus/Explicit sometimes treat shell thicknesses and midsurface offsets differently.
For a detailed description of the contact capabilities in Abaqus and the differences in the contact capabilities between Abaqus/Standard and Abaqus/Explicit, see “Contact interaction analysis: overview,” Section 34.1.1.
Output can be requested for an import analysis in the same way as for an analysis in which the results are not imported. The output variables available in Abaqus/Standard are listed in “Abaqus/Standard output variable identifiers,” Section 4.2.1. 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 UMAT and 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. Accelerations are recomputed at the start of an import analysis in Abaqus/Explicit and may be different from those obtained at the end of an Abaqus/Standard analysis. The differences in accelerations arise from the recalculation of the internal forces created by the imported stresses using the Abaqus/Explicit element formulation algorithms.
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/Explicit and Abaqus/Standard must be run on computers that are binary compatible.
The capability is not available for fluid elements; infinite elements; and spring, mass, dashpot, and rotary inertia elements. Connector elements can be imported from Abaqus/Standard to Abaqus/Explicit but not vice versa. 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.
All elements and nodes must be included in at least one set in the original analysis when importing part instances.
Node sets that are generated from existing element sets (see “Node definition,” Section 2.1.1) must be defined in the original analysis.
Surface definitions, contact pair definitions, and general contact definitions are not imported. Analytical rigid surfaces will not be imported.
If the material state is imported, only stresses will be imported for material models other than those defined by linear elasticity, hyperelasticity, Mullins effect, hyperfoam, viscoelasticity, Mises plasticity (including the kinematic hardening models), extended Drucker-Prager plasticity, crushable foam plasticity, Mohr-Coulomb plasticity, critical state (clay) plasticity, cast iron plasticity, concrete damaged plasticity, damage for cohesive elements, damage for ductile metals, or damage for fiber-reinforced composites. See “Importing the material state” in “Transferring results between Abaqus analyses: overview,” Section 9.2.1, for details.
If the state is imported for connector elements with behavior defined, the plastic displacements, the frictional slip, and the damage state are imported and the connector forces are recomputed. Some of the connector output variables, such as CU, are also recomputed on import. The recomputed variables may differ slightly at the point of import due to precision and algorithmic differences between the two solvers across import. See “Importing the material state” in “Transferring results between Abaqus analyses: overview,” Section 9.2.1, for details.
Temperatures and field variables at nodes are not imported. 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. See the discussion on “Predefined fields” 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.
Element and contact pair removal/reactivation (“Element and contact pair removal and reactivation,” Section 11.2.1) cannot be used in the first step of an import analysis in Abaqus/Standard. It can be used in the subsequent steps.
In a series of Abaqus/Standard and Abaqus/Explicit import analyses in the order Abaqus/Explicit(1) → Abaqus/Standard(1) → Abaqus/Explicit(2) →Abaqus/Standard(2), if elements in an element set are removed in the Abaqus/Standard(1) analysis, the subsequent Abaqus/Standard(2) import analysis does not recognize that this element set was removed in a previous analysis and fails with an error message stating that the element set is not found in the restart file. Such failures can be avoided by using flattened input files and requesting only the active element sets for import.
Section controls must be defined in the original analysis if any of a series of import analyses uses nondefault element formulations since section controls cannot be changed in an import analysis. See the discussion on “Using section controls in an import analysis” earlier in this section.
The symmetric model generation capability (“Symmetric model generation,” Section 10.4.1) 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.
An Abaqus/Standard import analysis where the reference configuration is not updated is not allowed if the adaptive meshing capability (“ALE adaptive meshing: overview,” Section 12.2.1) was used in the previous Abaqus/Explicit analysis.
Mesh-independent spot welds (see “Mesh-independent fasteners,” Section 33.3.4) and tie constraints (see “Mesh tie constraints,” Section 33.3.1) 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.
The first step after an import when the reference conference is updated should not be used to generate a substructure.
For beam structures that have acute curvatures and undergo large permanent changes in curvatures, slightly different equilibrated configurations will be seen when using import depending on whether or not the reference configuration is to be updated to the imported configuration (see “Updating the reference configuration” in “Transferring results between Abaqus analyses: overview,” Section 9.2.1). This configuration difference is due to beam element formulation differences between Abaqus/Standard and Abaqus/Explicit.
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/Standard 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 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, NLGEOM=YES *STATIC … *END STEP
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
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
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
