|
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, 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.
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
|