|
Comparison with the Restart Capability
Both the import and restart capabilities in
Abaqus/Standard
allow for the transfer of results and model information from one
Abaqus/Standard
analysis to another
Abaqus/Standard
analysis. However, the two capabilities have been designed for different
applications.
The restart capability allows a completed
Abaqus/Standard
analysis to be restarted and continued. The entire model and results from the
original analysis are transferred to the restart run, where additional analysis
steps can be defined. Not much new model data can be specified in the restarted
analysis; only model information such as new amplitude definitions, new node
sets, and new element sets are allowed. Detailed information on the restart
capability is given in
Restarting an Analysis.
The import capability also allows a completed
Abaqus/Standard
analysis to be continued. In addition, this capability allows for the analysis
to be continued with only desired components from the original analysis; the
entire model need not be transferred. New model data—such as elements, nodes,
surfaces, contact pairs, etc.—can be specified during the import analysis.
During the import analysis it is possible to choose whether only model
information from the previous analysis is to be transferred or if the results
associated with that model also are to be transferred.
For situations where the goal is to continue the original analysis with no
change to the model information, it is recommended that the restart capability
be used. For situations where the model information requires changes, or for
cases where you require control over the transfer of results, the import
capability should be used.
Specifying New Data in an Import 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/Standard
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/Standard uses a small-strain formulation (that is, geometric nonlinearity is ignored). For each
step of an analysis you can specify whether or not geometric nonlinearity should be
included; see Geometric Nonlinearity for details.
The default value for the formulation in an import analysis is the same as
the value at the time of import. Once the large-displacement formulation is
used during a given step in any analysis, it will remain active in all the
subsequent steps, whether or not the analysis is imported.
If the small-displacement formulation is used at the time of import, the
reference configuration cannot be updated.
Specifying Initial Conditions for Imported Elements and 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
|
Procedures
Results can be imported only from a general analysis step involving static
stress analysis, dynamic stress analysis, steady-state transport analysis,
coupled temperature-displacement analysis, or thermal-electrical-structural
analysis in
Abaqus/Standard.
Results transfer from linear perturbation procedures (General and Perturbation Procedures)
is not allowed.
Abaqus/Standard
offers several analysis procedures that can be used in an import analysis.
These procedures can be used to perform an eigenvalue analysis, static or
dynamic stress analysis, buckling analysis, etc. See
Solving Analysis Problems
for a discussion of the available procedures.
When results are transferred from an
Abaqus/Standard
dynamic analysis to another
Abaqus/Standard
analysis where the first step is a static procedure, the initial out-of-balance
forces must be removed gradually from the system. The removal of these forces
is performed automatically by
Abaqus/Standard
during the first static analysis step, as described below. If the first step in
the
Abaqus/Standard
analysis is not a static step (such as a dynamic step), the analysis proceeds
directly from the state imported from the previous
Abaqus/Standard
analysis.
Achieving Static Equilibrium When Importing from a Dynamic Analysis to a Static Analysis
When the current state of a deformed body in a dynamic analysis is imported
into a static analysis, the model will not initially be in static equilibrium.
Initial out-of-balance forces must be applied to the deformed body in dynamic
equilibrium to achieve static equilibrium. Both dynamic forces (inertia and
damping) and boundary interaction forces contribute to the initial
out-of-balance forces. The boundary forces are the result of interactions from
fixed boundary and contact conditions. Any changes in the boundary and contact
conditions will contribute to the initial out-of-balance forces.
In general, the instantaneous removal of the initial out-of-balance forces
in a static analysis will lead to convergence problems. Hence, these forces
need to be removed gradually until complete static equilibrium is achieved.
During this process of removing the out-of-balance forces, the body will deform
further and a redistribution of internal forces will occur, resulting in a new
stress state. (This is essentially what occurs during “springback,” when a
formed product is removed from the worktools.)
When the first step in the
Abaqus/Standard
import analysis is a static procedure, the following algorithm is used to
remove the initial out-of-balance forces automatically:
-
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.
Once static equilibrium has been obtained, subsequent steps can be defined
using any analysis procedure that would normally follow a static analysis.
When the first step is not a static analysis, no artificial stress state is
applied and the imported stresses are used in the internal force computations
for the element.
Boundary Conditions
Boundary conditions specified in the original analysis are not imported;
they must be redefined in the import analysis.
In some cases nonzero boundary conditions imposed in the original analysis
need to be maintained at the same values in the import analysis when the
imported configuration is not updated. In such cases you can prescribe a
constant (step function) amplitude variation for the analysis step (see
Prescribing Nondefault Amplitude Variations)
so that the newly applied boundary conditions are applied instantaneously and
held at that value for the duration of the step. Alternatively, you can refer
to an amplitude curve in the boundary condition definition (see
Amplitude Curves).
If boundary conditions in the original analysis are applied in a transformed
coordinate system (see
Transformed Coordinate Systems),
the same coordinate system should be defined and used in the import analysis.
For discussions on applying boundary conditions and multi-point constraints,
see
Boundary Conditions
and
About Kinematic Constraints.
Loads
Loads defined in the original analysis are not imported. Therefore, loads
may need to be redefined in the import analysis. There are no restrictions on
the loads that can be applied when results are imported from one analysis to
the other. In cases when the loads need to be maintained at the same values as
in the original analysis, you can prescribe a constant (step function)
amplitude variation for the analysis step (see
Prescribing Nondefault Amplitude Variations)
to apply the loads instantaneously at the start of the step and hold them for
the duration of the step. Alternatively, you can refer to an amplitude curve in
the load definition (see
Amplitude Curves).
If point loads in the original analysis are applied in a transformed coordinate
system (see
Transformed Coordinate Systems)
and the loads must be maintained in the import analysis, the load application
is simplified if the same coordinate system is defined and used in the import
analysis.
See
About Loads
for an overview of the loading types available in
Abaqus/Standard.
Predefined 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.
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 may sometimes be possible to
simplify the material definition. For example, if a Mises plasticity model was
used in the first
Abaqus/Standard
analysis and no further plastic yielding is expected in a subsequent
Abaqus/Standard
analysis, a linear elastic material can be used for the
Abaqus/Standard
analysis. However, if further nonlinear material behavior is expected, no
changes to the existing material definitions should be made. The history of the
state variables will not be maintained if the material models are not the same
in both the original analysis and the import analysis.
Elements
The import capability is available for thermal-electrical-structural
elements and a subset of the stress/displacement and coupled
temperature-displacement continuum, shell, membrane, truss, rigid, and surface
elements available in
Abaqus/Standard.
The complete list of supported elements is provided in
Table 2.
If elements that are removed (see
Element and Contact Pair Removal and Reactivation)
are imported, they become active in the import analysis and should be removed
in the first step of the import analysis.
Table 2. Element types that can be transferred from one
Abaqus/Standard
analysis to another.
| Element Type
|
Supported Elements
|
| Plane strain continuum
|
CPE3, CPE3H, CPE3T, CPE4, CPE4H, CPE4HT, CPE4I, CPE4IH, CPE4R, CPE4RHT, CPE4RT, CPE4T
|
| CPE6, CPE6H, CPE6M, CPE6MH, CPE6MHT, CPE6MT, CPE8, CPE8H, CPE8HT, CPE8R, CPE8RH, CPE8RHT, CPE8RT, CPE8T
|
| Plane stress continuum
|
CPS3, CPS3T, CPS4, CPS4I, CPS4R, CPS4T
|
| CPS6, CPS6M, CPS6MT, CPS8, CPS8R, CPS8RT, CPS8T
|
| Three-dimensional
continuum
|
C3D4,
C3D4H,
C3D4T,
C3D5,
C3D5H,
C3D6,
C3D6H,
C3D6T,
C3D8,
C3D8H,
C3D8HT,
C3D8I,
C3D8IH,
C3D8R,
C3D8RH,
C3D8RHT,
C3D8RT,
C3D8S,
C3D8HS,
C3D8T,
Q3D4,
Q3D6,
Q3D8,
Q3D8H,
Q3D8R,
Q3D8RH
|
| C3D10, C3D10H, C3D10HS, C3D10M, C3D10MH, C3D10MHT, C3D10MT, C3D15, C3D15H, C3D15V, C3D15VH, C3D20, C3D20H, C3D20HT, C3D20R, C3D20RHT, C3D20RT, C3D20T, C3D27, C3D27H, C3D27RH, Q3D10M, Q3D10MH, Q3D20, Q3D20H, Q3D20R, Q3D20RH
|
| Axisymmetric continuum
|
CAX3, CAX3H, CAX3T, CAX4, CAX4H, CAX4HT, CAX4I, CAX4IH, CAX4R, CAX4RH, CAX4RHT, CAX4RT, CAX4T
|
| CAX6, CAX6M, CAX6MH, CAX6MHT, CAX6MT, CAX8, CAX8H, CAX8HT, CAX8R, CAX8RH, CAX8RHT, CAX8RT, CAX8T
|
| Membrane
|
M3D3, M3D4R
|
| Two-dimensional rigid
|
R2D2
|
| Three-dimensional rigid
|
R3D3, R3D4
|
| Axisymmetric rigid
|
RAX2
|
| Three-dimensional shell
|
S4R, S3R, S4RT, S3RT, S4T, S3T
|
| Axisymmetric shell
|
SAX1
|
| Continuum shell
|
SC6R, SC8R, SC6RT, SC8RT
|
| Surface
|
SFM3D3, SFM3D4R
|
| Two-dimensional truss
|
T2D2, T2D2T
|
| Three-dimensional truss
|
T3D2, T3D2T
|
| Cohesive
|
COH2D4, COHAX4, COH3D6, COH3D8
|
| Inertial
|
MASS, ROTARYI
|
The following element types cannot be imported:
-
Acoustic elements
-
Axisymmetric-asymmetric continuum and shell elements
-
Beam elements
-
Connector elements
-
Coupled thermal-electrical elements
-
Diffusive heat transfer/mass diffusion elements and forced
convection/diffusion elements
-
Generalized plane strain elements
-
Gasket elements
-
Heat capacitance elements
-
Infinite elements
-
Piezoelectric elements
-
Special-purpose elements
-
Substructures
-
User-defined elements
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.
-
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
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
Most types of kinematic constraints specified in the original analysis are
not imported and must be defined again in the import analysis; however,
surface-based tie constraints are imported by default. See
About Kinematic Constraints
for a discussion of the various types of kinematic constraints.
Interactions
The various aspects of most surface-based mechanical contact definitions
(including the surface, contact pair, and contact property definitions) can be
imported. Thermal interactions, electrical interactions, and pore fluid surface
interactions cannot be imported. Certain types of mechanical contact
aspects—pressure, penetration loads, cohesive behavior, and debonded
surfaces—cannot be imported. The most commonly used mechanical contact
aspects—pressure-overclosure behavior, frictional behavior, and damping—can be
imported.
For models defined with element sets that are imported once, the ability to import
element-based and node-based surfaces is determined by whether or not the underlying
elements and nodes defining these surfaces are imported. If the underlying elements or nodes
of a surface are not imported, that surface will not be imported. Rigid surface definitions
are imported when the associated secondary surface is also imported. Contact pairs along
with the associated surface interaction definitions are imported provided that all the
secondary and main surfaces used in the original definition of the contact pair are also
imported. Other contact-related features (such as surface interaction, surface smoothing,
and clearance options) are also imported along with the contact pair definitions.
For models defined with part instances that are imported once, if the main and secondary
surfaces along with the contact pair and associated surface interaction are defined again in
the import analysis, the contact state associated with the contact pair is imported if the
material state is imported. Other contact-related features (such as surface smoothing and
clearance options) must be defined again if required.
For models defined with either element sets or part instances that are imported once or
multiple times, you can control the import of the contact pair definitions by importing the
main and secondary surfaces. When the main and secondary surfaces of a contact pair are
imported with the same repositioning, the contact pair along with the associated surface
interaction definitions are imported automatically. Other surface-dependent features (such
as surface smoothing and clearance options) are also generated along with the contact pair
definitions. The contact state associated with the generated contact pairs is imported if
the material state is imported.
Contact conditions modeled with contact elements will be ignored during the
transfer process.
The contact state associated with a stress/displacement analysis is imported
if the material state is imported. If the reference configuration is updated,
the accumulated contact strains will be set to zero. The contact state
associated with thermal, electrical, or pore fluid surface interactions is not
imported. The contact state associated with a crack propagation analysis is not
imported; initially bonded contact surface definitions are not transferred. If
a contact pair was inactive in the step from which the import was done due to
the use of contact pair removal (see
Removing and Reactivating Contact Pairs),
it must be deactivated again in the first step of the import analysis.
Additional contact information can be defined in the import analysis by
specifying new surfaces, contact pairs, and interactions. New contact pair
definitions can use the imported surface interaction definitions.
For a detailed description of the contact capabilities in
Abaqus/Standard,
refer to
About Contact Interactions.
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 have to be respecified. The output variables available in
Abaqus/Standard
are listed in
Abaqus/Standard Output Variable Identifiers.
The values of the following material point output variables will be
continuous in an import analysis when the material state is imported: stress,
equivalent plastic strain (PEEQ), and solution-dependent state variables (SDV) for
UMAT.
If the reference configuration is not updated, the displacements, strains,
whole element variables, section variables, and energy quantities will be
reported relative to the original configuration.
If the reference configuration is updated, displacements, strains, whole
element variables, section variables, and energy quantities will not be
continuous in an import analysis and will be reported relative to the updated
reference configuration.
Time and step number will not be continuous between the original and the
import analyses if the reference configuration is updated. Time and step number
will be continuous only if the reference configuration is not updated.
Limitations
The import capability has the following known limitations. Where applicable,
details are given in the relevant sections.
-
The same release of
Abaqus/Standard
must be run on computers that are binary compatible.
-
The capability is not available for fluid elements; infinite elements;
and spring, dashpot, and connector elements. See the discussion on
Elements
earlier in this section for further details.
-
Element sets and part instances cannot be imported more than once nor
can they be repositioned.
-
All elements and nodes must be included in at least one set in the
original analysis when importing part instances.
-
The contact state associated with thermal, electrical, and pore fluid
surface interactions is not imported; the contact state associated with crack
propagation is not imported.
-
General contact definitions are 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.
-
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 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.
-
When you import part instances individually from a previous analysis
that was defined as an assembly of part instances, reference nodes associated
with rigid body or coupling constraints defined on the imported instances will
not be available in the import analysis for load or boundary condition
application.
-
Pre-tension section definitions are not imported; they have to be
redefined in the import analysis.
-
Table collection definitions are not imported; they have to be redefined
in the import analysis.
-
The capability is not available for elements with composite solid
section definitions.
-
If the elements that are removed in the original analysis (see
Element and Contact Pair Removal and Reactivation)
are imported, they become active in the import analysis and should be removed
in the first step of the import analysis.
-
The symmetric model generation capability cannot be used in an import
analysis in
Abaqus/Standard.
-
An original analysis in which the symmetric model generation capability is employed
cannot be imported into a steady-state transport analysis.
-
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.
-
There may be a slight discontinuity during the transfer of state
variables for analyses using fully integrated, first-order continuum elements
if the elements are significantly deformed and the reference configuration is
updated.
-
Mesh-independent spot welds (see
Mesh-Independent Fasteners)
are not imported. However, the spot weld reference nodes are imported and can
be used to redefine spot welds in the import analysis. The locations of the
spot weld reference nodes and projection points are computed based upon the
reference configuration of the import analysis. Therefore, if the deformed
configuration of the imported model is significantly different from its
reference configuration, it is recommended that the reference configuration be
updated.
-
If the value of the friction coefficient is changed from the value given
in the model data of the original analysis, the changed value must be
respecified in the first step of the import analysis (see
Changing Friction Properties during an Abaqus/Standard Analysis).
-
The capability is not available if adaptive meshing (see
ALE Adaptive Meshing and Remapping in Abaqus/Standard)
is used in the original analysis.
-
Enriched features (see
Modeling Discontinuities as an Enriched Feature Using the Extended Finite Element Method)
are not imported.
-
Restart files from the original analysis are used in the analysis
preprocessor and in the
Abaqus/Standard
execution in the import analysis. When the import job is run in parallel on
computer clusters by using MPI-based
parallelization, these restart files are copied to each host machine. The
original job restart files are not decomposed to match the import analysis
parallel domain and may be large relative to the local disk space available on
the host machines. You can minimize this file size by requesting restart output
only for the increment from which import will occur.
-
During import from one general dynamic step to another general dynamic step, reaction
forces may experience jumps due to different time integrators or different time
integrator parameter settings between the steps.
Input File Template
Transferring Results Using Models That Are Not Defined as Assemblies of Part Instances:
First
Abaqus/Standard
analysis: HEADING
…
MATERIAL, NAME=mat1
ELASTIC
Data lines to define linear elasticity
PLASTIC
Data lines to define Mises plasticity
DENSITY
Data line to define the density of the material
…
BOUNDARY
Data lines to define boundary conditions
STEP, NLGEOM=YES
STATIC
…
RESTART, WRITE
END STEP Abaqus/Standard
import analysis: HEADING
IMPORT, STEP=step, INCREMENT=increment, STATE=YES, UPDATE=NO
Data lines to specify element sets to be imported
IMPORT ELSET
Data lines to specify element set definitions to be imported
IMPORT NSET
Data lines to specify node set definitions to be imported
**
*** Optionally define additional model information
**
BOUNDARY
Data lines to redefine boundary conditions
STEP, NLGEOM=YES
STATIC
…
END STEP Transferring Results Using Models Defined as Assemblies of Part Instances:
First
Abaqus/Standard
analysis: HEADING
PART, NAME=Part-1
Node, element, section, set, and surface definitions
END PART
ASSEMBLY, NAME=Assembly-1
INSTANCE, NAME=i1, PART=Part-1
<positioning data>
Additional set and surface definitions (optional)
END INSTANCE
Assembly level set and surface definitions
…
END ASSEMBLY
MATERIAL, NAME=mat1
ELASTIC
Data lines to define linear elasticity
PLASTIC
Data lines to define Mises plasticity
DENSITY
Data line to define the density of the material
…
BOUNDARY
Data lines to define boundary conditions
STEP
STATIC
…
RESTART, WRITE, FREQUENCY=n
END STEP Abaqus/Standard
import analysis: HEADING
Part definitions (optional)
ASSEMBLY, NAME=Assembly-1
INSTANCE, INSTANCE=i1, LIBRARY=oldjob-name
Additional set and surface definitions (optional)
IMPORT, STEP=step, INCREMENT=increment, STATE=YES, UPDATE=NO
END INSTANCE
Additional part instance definitions (optional)
Assembly level set and surface definitions
…
END ASSEMBLY
**
*** Optionally define additional model information
**
BOUNDARY
Data lines to define boundary conditions
STEP, NLGEOM=YES
STATIC
…
END STEP
|