Products
Abaqus/Explicit
Abaqus/CAE
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.
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). 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) 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 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 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.
Table 1. Valid initial conditions.
| Initial condition |
Material state imported |
| Field variable |
No |
| Hardening |
No |
| Relative density |
No |
| Rotational velocity |
Yes or No |
| Solution-dependent state variables |
No |
| Stress |
No |
| Temperature |
No |
| Velocity |
Yes or No |
| Void ratio |
No |
Boundary Conditions
Boundary conditions (including connector motion) specified in the original analysis are not
imported. They must be redefined in the import analysis.
In some cases nonzero boundary conditions imposed in the original analysis need to be
maintained at the same values in the import analysis when the imported configuration is not
updated. In such cases you can prescribe a constant (step function) amplitude variation for
the analysis step (see Prescribing Nondefault Amplitude Variations) 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 and About Kinematic Constraints.
Loads
Loads, including those applied for connector actuation, defined in the original analysis
are not imported. Therefore, loads might 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/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 might 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 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.
Table 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,
C3D4H,
C3D4T,
C3D5,
C3D6,
C3D6T,
C3D8R,
C3D8RT,
C3D10,C3D10T,
C3D10M,
C3D10MT,
C3D8,
C3D8T,
C3D8I |
| Axisymmetric continuum |
CAX3,
CAX4R,
CAX3T,
CAX4RT,
CAX6M,
CAX6MT |
| Membrane |
M3D3,
M3D4M3D4R
|
| 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 )
In addition, the following restrictions apply to the import capability:
-
Rebars defined using rebar layers (Defining Reinforcement) are imported
provided the underlying elements are also imported. Rebar reinforcements defined using
the embedded element technique (Embedded Elements) 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) 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 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 all the elements used to define the rigid body are included in
the element sets 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 About Kinematic Constraints for a discussion
of the various types of kinematic constraints.
Similarly, surface-based kinematic and distributing coupling constraints specified in the
original analysis are not imported and must be defined again in the import analysis. If
transfer of material state is specified for import, the displacements and rotations of the
reference nodes are transferred in the import analysis. This also applies to reference nodes
that do not belong to any imported elements. By transferring nodal results, the constraint
will be in initial equilibrium in the imported model.
Interactions
For general contact, the contact state is imported if general contact is defined in the
original and import analyses and if all underlying elements associated with a given contact
constraint are imported without repositioning or are repositioned using identical
translation and rotation.
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 About Contact Interactions.
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 must be respecified. The
output variables available in Abaqus/Explicit are listed in Abaqus/Explicit 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 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.
-
All elements and nodes must be included in at least one set in the original analysis
when importing part instances.
-
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 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 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 is not imported unless the reference node is
part of another element definition that is imported.
- Fluid cavity definitions are not imported. In addition, the reference node of a fluid
cavity is not 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) 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 might 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 might not initially be in
compliance if the nodes involved in the constraint have nonzero displacements. This
might cause numerical difficulty and potential exit of the import analysis. In this case
it is recommended that you update the reference configuration on 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
IMPORT SURFACE
Data lines to specify surface 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
IMPORT SURFACE
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
|