|
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
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) and Abaqus/Explicit uses a large-deformation formulation (that is, geometric nonlinearity is included). For
each step of an analysis, you can specify which formulation should be used; 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 (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.
Table 1. Valid initial conditions.
| Initial condition
|
Material state imported?
|
| Hardening
|
No
|
| Relative density
|
No
|
| Rotational velocity
|
Yes or No
|
| Solution-dependent state variables
|
No
|
| Stress
|
No
|
| Velocity
|
Yes or No
|
| Void ratio
|
No
|
Procedures
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 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.
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.
Achieving Static Equilibrium When Importing into Abaqus/Standard
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.
Once static equilibrium has been obtained, subsequent steps can be defined
using any analysis procedure that would normally follow a static analysis in
Abaqus.
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, 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)
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 a discussion of applying boundary conditions, see
Boundary Conditions.
Loads
Loads, including those applied for connector actuation, defined in the original analysis are not
imported. Loads might, 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) 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.
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 are reset to the
imported values; for example, the thermal strains are 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 is imported if the material state is imported.
Material Options
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.
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.
Mass Scaling
If mass scaling (Mass Scaling)
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.
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 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.
Elements
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 2.
Table 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, C3D8I, C3D8R, C3D8T, C3D8RT, C3D10, 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
|
| MASS, ROTARYI
|
| 1Connector elements can be imported from
Abaqus/Standard
to
Abaqus/Explicit;
but not vice versa.
|
When S3R shell elements are imported from
Abaqus/Explicit
into
Abaqus/Standard,
they are converted into degenerated S4R elements automatically. However, when S3R shell elements are imported from
Abaqus/Standard
into
Abaqus/Explicit,
they remain S3R elements. When C3D6 and C3D6T solid elements are imported from
Abaqus/Explicit
into
Abaqus/Standard,
the results at the single point integration are applied to both integration
points in
Abaqus/Standard
and the full integration is used automatically. However, when C3D6 and C3D6T solid elements are imported from
Abaqus/Standard
into
Abaqus/Explicit,
only the results at the first integration point are imported and are used in
the reduced integration. When quadrilateral and hexahedral acoustic finite
elements are imported between
Abaqus/Explicit
and
Abaqus/Standard,
they are converted to or from reduced-integration types, as required.
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)
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.
-
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 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.
-
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)
in
Abaqus/Standard
will not be imported into
Abaqus/Explicit.
-
Rigid surfaces will not be imported.
When importing results from an Abaqus/Standard analysis to an Abaqus/Explicit analysis, each element set specified can contain only compatible element types listed in
Table 3. Element types from different cells are not compatible and cannot be combined in the same
element set.
Table 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
|
| MASS, ROTARYI
|
Using Section Controls in an Import Analysis
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)
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 might 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.
Membrane and Shell Element Thickness Computation
The computations for membrane and shell element thicknesses are described
below.
Shell Elements Defined Using a General Shell Section
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.
Shell Elements Defined Using Shell Sections Integrated during Analysis and Membrane Elements
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.
Contact Angle Computation in SLIPRING-Type Connector Elements
The contact angle, ,
made by the belt wrapping around node b (see
Complex Connections) is
computed automatically in
Abaqus/Explicit,
ignoring the value specified within the
Abaqus/Standard
analysis.
Constraints
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
About Kinematic Constraints
for a discussion of the various types of kinematic constraints.
Interactions
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 might 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 might be different in Abaqus/Standard and Abaqus/Explicit. Examples of potential causes for differences include:
-
Abaqus/Standard typically uses a “pure main-secondary” approach, whereas Abaqus/Explicit typically uses a “balanced main-secondary” approach.
-
Depending on the contact formulations used,
Abaqus/Standard
and
Abaqus/Explicit
sometimes treat shell thicknesses and midsurface offsets differently.
Thus, when the contact conditions are defined in the import analysis, the contact state that
existed in the previous analysis might not be reproduced at the beginning of the import
analysis. This could lead to a redistribution of stresses and an analysis that differs from
what you desire. In some cases this problem can be mitigated by using nondefault options,
such as ignoring shell thicknesses in the contact calculations, to match behaviors in Abaqus/Standard and Abaqus/Explicit.
For a detailed description of the contact capabilities in
Abaqus
and the differences in the contact capabilities between
Abaqus/Standard
and
Abaqus/Explicit,
see
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. The output variables available
in
Abaqus/Standard
are listed in
Abaqus/Standard Output Variable Identifiers.
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
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 might 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.
Limitations
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 and dashpot 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)
must be defined in the original analysis.
-
Contact pair definitions and general contact definitions are not
imported. Analytical rigid surfaces 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,
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
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 might differ slightly at the point of import due to precision and
algorithmic differences between the two solvers across import. See Importing the Material State 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 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.
-
Element and contact pair removal/reactivation (Element and Contact Pair Removal and Reactivation)
cannot be used in the first step of an import analysis in
Abaqus/Standard.
It can be used in the subsequent steps.
-
For an Abaqus/Standard to Abaqus/Explicit import analysis in which elements in the Abaqus/Standard analysis were removed and reactivated in multiple steps (Element and Contact Pair Removal and Reactivation) and all elements are active for transfer at the
import step, some of the element states, such as strains, might not be transferred
correctly.
-
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)
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 (About ALE Adaptive Meshing)
was used in the previous
Abaqus/Explicit
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.
-
The first step after an import when the reference configuration 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).
This configuration difference is due to beam element formulation differences
between
Abaqus/Standard
and
Abaqus/Explicit.
Input File Template
Transferring Results between Abaqus/Explicit and Abaqus/Standard Using Models That Are Not Defined as Assemblies of Part Instances:
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
IMPORT SURFACE
Data lines to specify surface 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 Transferring Results between Abaqus/Standard and Abaqus/Explicit Using Models That Are Not Defined as Assemblies of Part Instances:
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
IMPORT SURFACE
Data lines to specify surface 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 Transferring Results between Abaqus/Explicit and Abaqus/Standard Using Models Defined as Assemblies of Part Instances:
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
IMPORT SURFACE
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
Transferring Results between Abaqus/Standard and Abaqus/Explicit Using Models Defined as Assemblies of Part Instances:
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
IMPORT SURFACE
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
|