Saving the Analysis Results
The restart files from the original analysis contain the analysis results
that are transferred from
Abaqus/Standard
or
Abaqus/Explicit.
Obtaining restart files is described in more detail in
Writing Restart Files;
brief summaries are provided below. By default,
Abaqus/Standard
does not write any restart information and
Abaqus/Explicit
writes results at the beginning and end of each step.
Saving Results from Abaqus/Standard
If the results are to be imported from an
Abaqus/Standard
analysis, the results from the original
Abaqus/Standard
job must be written to the restart (.res), analysis
database (.mdl and
.stt ), part
(.prt ), and output database
(.odb ) files.
You can specify the increments at which restart information will be written.
Restart information is always written at the end of a step in addition to the
requested increments whenever you request restart data in
Abaqus/Standard.
Saving Results from Abaqus/Explicit
If the results are to be imported from an
Abaqus/Explicit
analysis, the results from the original
Abaqus/Explicit
job must be written to the state (.abq) file at the time
when transfer of the state of the deformed body is required. The state
(.abq), restart (.res), analysis
database (.mdl and .stt), package
(.pac), part (.prt), and output
database (.odb) files will be used for importing the
results from
Abaqus/Explicit.
You can specify whether the results are to be written at the exact time
dictated by the specified time interval, n, during a
step of an
Abaqus/Explicit
analysis or at the increment ending after the time dictated by the specified
time interval. Results are always written at the end of a step, so it is not
necessary to request results at the exact time intervals if results will be
read only from the end of a step.
Specifying the Transfer of Model Data and Results
The import capability is used to transfer model data and results from one analysis to
another. The following sections describe how to specify the import request. You can import
element sets from models that are not defined as assemblies of part instances, or you can
import part instances from models that are defined as assemblies of part instances.
Specifying the Transfer of Model Data and Results for Models That Are Not Defined as Assemblies of Part Instances
You can import element sets from a previous analysis to specify the transfer
of model data and results for models that are not defined as assemblies of part
instances. This import capability is illustrated in
Springback of two-dimensional draw bending
and
Axisymmetric forming of a circular cup.
Each element set to be imported must have been defined in the original
analysis. You can import any element set, including nested element sets and
those with overlapping elements. An imported element set can also be a subset
of another imported element set. The elements in these sets as well as the
element set definitions are imported. Even though an element may be included in
multiple imported elements sets, each element is imported only once in the
import analysis. You cannot use element sets that are internal to the original
analysis.
Specifying the Transfer of Model Data and Results for Models That Are Defined as Assemblies of Part Instances
You can import part instances from a previous analysis to specify the
transfer of model data and results for models that are defined as assemblies of
part instances. If you import more than one part instance, all import
parameters must be the same for each imported part instance. Each instance name
that you specify must be the same as the instance name in the original
analysis. Only sets that are defined within the imported instance will be
imported. Surfaces defined within the imported instance are imported if you
import surface definitions. Sets and surfaces defined at the assembly level
must be redefined in the import analysis. New set and surface definitions can
be added upon import. You cannot assign new sections, material orientations,
normals, or beam orientations to the imported part instance.
Identifying the Analysis from Which the Data Will Be Obtained When Importing from a Single Previous Analysis
You must specify the name of the job from which the model and results data
will be obtained.
Identifying the Individual Analysis from Which the Data Will Be Obtained When Importing from Multiple Previous Analyses
You must specify the name of the analysis from which the model data and
results will be obtained.
Importing Model Data
Element property definitions of imported elements can be redefined only if
the reference configuration is updated (see
Updating the Reference Configuration)
and the material state is not imported (see
Importing the Material State).
In this case the material orientation definitions (Orientations),
hourglass stiffness but not hourglass control definitions, and transverse shear
stiffness definitions (in the case of shell elements) of the imported elements
can also be redefined.
For other reference configuration and material state combinations, the information required to
define the section for each imported element will be imported from the original analysis.
All material orientations will be transferred from the original analysis to the import
analysis. Material orientations that are associated with imported elements cannot be
redefined in the import analysis. However, orientation names that are not associated with
any imported elements can be reused in the import analysis.
Transverse shear stiffness for imported shell elements cannot be redefined; the values
will be transferred from the original analysis. Hourglass stiffness for the imported
elements cannot be redefined in an Abaqus/Standard import analysis; the default values will be used. The section control definitions
(kinematic formulation, order of accuracy in the element formulation, and hourglass
control approach) to be used for imported elements cannot be redefined (see Transferring Results between Abaqus/Explicit and Abaqus/Standard for details).
Mass adjustment contributions (see
Mass Adjustment)
applied to an element set are always included when the element set is imported.
There is no need to redefine these contributions in the import analysis unless
different mass adjustment is required for the element set.
Nonstructural mass contributions (see
Nonstructural Mass Definition)
associated with an element set are not imported. These contributions need to be
redefined in the import analysis if they are to be included in the model.
Only nodes associated with the imported elements are imported. New nodes can
be defined in the import analysis.
Nodes or elements that use the same numbers as nodes or elements being
imported can be defined provided that the reference configuration is updated,
the material state is not imported, and the import is not done from an instance
library. The new definitions will overwrite the imported definitions. If the
reference configuration is not updated, new nodes or elements cannot use the
imported node and element numbers irrespective of whether or not the material
state is imported.
During results transfer from an
Abaqus/Standard
analysis to another
Abaqus/Standard
analysis or from an
Abaqus/Explicit
to another
Abaqus/Explicit
analysis, the coordinates of imported nodes can be modified from their imported
values by respecifying the nodal definitions if the reference configuration is
updated and the material state is not imported. This modification of the
coordinates of imported nodes is not allowed during transfer of results from
Abaqus/Explicit
to
Abaqus/Standard
or vice versa.
Importing Model Data Defined by a Distribution
While transferring results from one
Abaqus/Standard
analysis to another
Abaqus/Standard
analysis, most element or material properties defined by a distribution (see
Distribution Definition)
are imported along with the elements. The only exceptions are spatially varying
thicknesses and orientation angles defined on the layers of composite shells
and solids; in this case
Abaqus
issues an error message during input file preprocessing.
While transferring results from an
Abaqus/Explicit
analysis to an
Abaqus/Standard
analysis, the only spatially varying element properties defined by a
distribution that can be imported are shell thicknesses, shell offset, and
section orientations for shell and solid elements. If any other element or
material properties are defined with a distribution,
Abaqus
issues an error message during input file preprocessing.
While transferring results from an
Abaqus/Standard
analysis to an
Abaqus/Explicit
analysis or from an
Abaqus/Explicit
analysis to another
Abaqus/Explicit
analysis, the only spatially varying element properties defined by a
distribution that can be imported are shell thicknesses, shell offset, section
orientations for shell and solid elements, orientation angles defined for shell
sections on the layers of composite shells, and section stiffness matrices
specified directly for general shell sections. If any other element or material
properties are defined with a distribution,
Abaqus
issues an error message during input file preprocessing. If an element set
consists of elements whose properties are defined by one or more distributions,
the element set cannot be imported more than once.
Section and material properties of imported elements can be redefined with
distributions only if the reference configuration is updated (see
Updating the Reference Configuration)
and the material state is not imported (see
Importing the Material State).
In this case the material orientation definitions (Orientations),
hourglass stiffness but not hourglass control definitions, and transverse shear
stiffness definitions (in the case of shell elements) of the imported elements
can also be redefined.
Importing Results from an Abaqus/Standard Analysis (Other than a Direct Cyclic Analysis)
If the results are imported from an
Abaqus/Standard
analysis, you can specify the step and increment in the restart file for which
the results are to be imported. By default, the results written at the end of
the analysis are imported.
Importing Results from an Abaqus/Standard Direct Cyclic Analysis
If the results are imported from a direct cyclic analysis, you can specify
the step and iteration number in the restart file for which the results are to
be imported. By default, the results written at the end of the analysis are
imported.
Importing Results from an Abaqus/Explicit Analysis
If the results are imported from an
Abaqus/Explicit
analysis, you can specify the step and interval in the state file for which the
results are to be imported. By default, the results written at the end of the
analysis are imported.
Updating the Reference Configuration
Once the current model configuration of an
Abaqus
analysis is imported into
Abaqus/Explicit
or
Abaqus/Standard,
the analysis can be continued with or without updating the reference
configuration to be the imported configuration. If the reference configuration
is not updated to be the imported configuration, the displacements and strains
are reported as total values relative to the original reference configuration
and will, hence, be continuous. If the reference configuration is updated to be
the imported configuration, displacements and strains reported in the import
analysis are the total values relative to the updated reference configuration.
This choice is useful if results need to be displayed relative to the imported
configuration, such as may be desirable in springback analysis. The reference
configuration cannot be updated if the imported analysis is geometrically
linear.
The choice of whether or not to update the reference configuration can
influence strain-free nodal adjustments associated with contact initialization
in
Abaqus/Standard.
Strain-free adjustments can be used to resolve penetrations or gaps that exist
in the reference configuration in
Abaqus/Standard,
so prior displacements are not considered by the strain-free adjustment
algorithm upon import if the reference configuration is not updated.
Strain-free nodal adjustments in
Abaqus/Explicit
are based on the current configuration rather than the reference configuration,
so these adjustments are not sensitive to whether the reference configuration
is updated in
Abaqus/Explicit.
Further details on strain-free adjustments are provided in
Default Contact Initialization Method,
Contact Initialization for General Contact in Abaqus/Standard,
Contact Initialization for General Contact in Abaqus/Explicit,
and
Contact Initialization for Contact Pairs in Abaqus/Explicit.
If connector elements are imported, the configuration can be updated
provided that the state is not imported.
When hyperelastic materials are imported, the configuration must be updated
if the state is not imported.
Importing the Material State
You can specify whether or not the associated material state should be
imported. If you choose to import the material state, the following are
imported:
-
stresses;
-
equivalent plastic strains;
-
back stresses for the kinematic hardening models;
-
user-defined state variables;
-
damage-related state variables for the concrete damaged plasticity
model;
-
damage-related state-variables for traction-separation response with
cohesive elements;
-
damage-related state variables for ductile metals;
-
damage-related state variables for fiber-reinforced composites;
-
maximum deviatoric strain energy density during deformation history for
Mullins effect;
-
internal strains and stresses for viscoelastic material models;
-
transformation strains and fraction of martensite for superelastic
material models; and
-
connector state variables such as plastic strains, frictional slip, and
damage state.
Thus, the state is imported correctly for further analysis only for the
following:
-
linear elasticity,
-
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,
-
Johnson-Cook plasticity,
-
hyperelasticity (including Mullins effect),
-
hyperfoam,
-
viscoelasticity,
-
superelasticity,
-
traction-separation response with damage for cohesive elements,
-
damage for ductile metals,
-
damage for fiber-reinforced composites,
-
connector behavior,
-
materials defined in user subroutines
UMAT and
VUMAT, and
-
materials defined using the parallel rheological framework for nonlinear
viscoelastic-elastoplastic behavior.
For all other material models only stresses will be imported. No other state
variables will be imported.
If the material behavior is defined in a user subroutine, you must ensure
that the
UMAT and
VUMAT are consistent.
If connector elements are imported, the state can be imported provided that
the configuration is not updated.
When hyperelastic materials are imported, the state must be imported if the
configuration is not updated. In an import analysis where you specify that the
reference configuration should not be updated and the material state should not
be imported, the material state is imported for elements associated with
hyperelastic materials and any initial conditions of the state specified for
such elements are ignored.
Importing Rigid Bodies
A rigid body defined with an element set in the original analysis will be
imported by default if all elements in the element set are imported; that is,
if all of the rigid body elements belong to the imported element sets. The
reference node of an imported rigid body is imported automatically, and you
should not specify a new reference node for the imported rigid body. If the
reference node of an imported rigid body is defined by a node set, the
reference node set can be included in the imported node sets. If all elements
belonging to a rigid body are imported multiple times, the rigid body and its
reference node are imported the same number of times automatically. Multiple
import of a rigid body with pin nodes or tie nodes assigned to the rigid body
is not supported.
If a rigid body consists of a union of multiple element sets and these sets are imported
multiple times, you must define a node set for the rigid body reference node. This node
set must be imported to provide a unique node offset for the reference node.
A rigid body from an original analysis cannot be partially imported; that
is, the full complement of rigid body elements must be imported. An
assembly-level rigid body from the original analysis with parts and instances
can be imported only if it refers to a reference node set defined at the part
instance level in the original analysis. If the reference node is defined at
the assembly level, the set and the rigid body cannot be imported.
Defining Constraints upon Import
Most constraints (such as multi-point constraints and surface-based tie
constraints) are not imported from the original analysis and must be redefined
in the import analysis. Using the reference configuration of the original
analysis without update ensures identical reproduction of these constraints in
the import analysis.
If a new constraint is defined in the import analysis, it is important to ensure that the
constraint is not in violation either in the reference configuration or in the starting
configuration of the import analysis. These two configurations are one and the same for
newly introduced nodes. If a new constraint involves nodes of the original analysis, it is
appropriate to update the reference configuration for the import analysis (see Updating the Reference Configuration for more
information). In all import analyses, tie constraints are always defined with reference to
the updated configuration.
In an
Abaqus/Standard
analysis with adaptive meshing and acoustic-to-structure tie constraints, the
structural as well as the acoustic nodes may move from their initial positions.
Specifying a Tolerance for Shell Normals in the Updated Configuration
When the imported configuration is updated upon import, the mesh
discretization may not satisfy the mesh geometry checks imposed in
Abaqus/Explicit
or
Abaqus/Standard
to evaluate whether or not a mesh is reasonable. In the case of highly warped
shell elements it is possible that the normal at the center of the element that
is calculated from the midsurface interpolation may differ from the normal that
is interpolated from the rotated normals at the nodes. If the difference
exceeds the tolerance specified, the analysis will terminate. This suggests
that a fine mesh may be required to model areas of high curvature change to
achieve a successful analysis.
The unit normal computed from the midsurface interpolation,
, and that
predicted by the interpolation of the rotated normals at the nodes,
, must
satisfy the condition:
where you can specify the tolerance, .
If you do not specify a tolerance value, a default value of
= 0.1 is used.
Limitations for Import from Multiple Previous Analyses
The capability to import from multiple previous analyses has the following
known limitations:
- You can import only to an
Abaqus/Explicit
analysis.
-
The previous analyses must all be
Abaqus/Explicit
analyses or
Abaqus/Standard
analyses. A mix of
Abaqus/Explicit
and
Abaqus/Standard
analyses is not supported.
-
The use of either a part-instance model or a non-part-instance model
but not both must be maintained in all previous analyses. A mix of previous
analyses with and without instance definitions is not supported.
-
All previous analyses must be imported with the same settings for
updating the reference configuration and for importing the material state.
-
All previous analysis models must have the same geometric dimension. A
mix of two-dimensional, axisymmetric, and three-dimensional analyses is not
supported.
- All limitations that pertain to
import from a single
Abaqus/Explicit
analysis or a single
Abaqus/Standard
analysis remain effective.
|