Preparing an
Abaqus
analysis for co-simulation involves the following:
identifying an
Abaqus
analysis step for co-simulation analysis;
identifying the co-simulation interface regions in the
Abaqus
model; and
identifying the fields exchanged during the co-simulation.
This section provides an overview of preparing an Abaqus analysis for a co-simulation. The discussion in this section is general and may not apply
to every product pairing.Co-Simulation between Abaqus Solvers provides setup, execution,
and limitation details for co-simulation between Abaqus solvers. For co-simulation between Abaqus and third-party analysis programs, consult the appropriate User’s Guide.
Identifying an Abaqus Step for Co-Simulation Analysis
The co-simulation event need not begin at the start of the first step in an
Abaqus
analysis. However, it does need to start with the beginning of an analysis step
and end within that analysis step. Hence, you need to define the step durations
in
Abaqus
such that the start of the co-simulation event falls at the beginning of an
Abaqus
analysis step and to define that particular step so that the co-simulation
event ends by the end of that step. Regular loads and boundary conditions for
the
Abaqus
model are specified as usual.
Communication with the coupled analysis is initiated as the co-simulation event begins and is
terminated when the co-simulation event time is reached. Abaqus may terminate the co-simulation event when the end of the analysis step is reached before
the co-simulation event time or when the analysis cannot proceed any further; for example,
because of convergence problems. In such a case, a warning message is issued to all clients,
and the co-simulation is terminated.
Co-simulation is supported by the following
Abaqus
procedures:
Identifying the Analysis Program Communicating with Abaqus during the Co-Simulation
You can couple
Abaqus
with another
Abaqus
analysis or
Abaqus
with certain third-party analysis programs using the
SIMULIA Co-Simulation Engine.
For details on coupling with third-party analysis programs, see the respective
User's Guides.
Identifying the Co-Simulation Interface Region
Interaction between two
Abaqus
models or between an
Abaqus
model and a third-party analysis model takes place through a common interface
region referred to as the co-simulation interface region. The co-simulation
interface region may be a set of discrete points, a surface region, or a volume
region. You must be consistent in your interface region definition; if you
define a surface co-simulation region in one analysis, then you must define a
surface co-simulation region in the other analysis. Furthermore, these
co-simulation regions need to be co-located and have the same region
boundaries.
Interacting through Discrete Points
Interaction can occur through a set of discrete points where only nodal
position information without element topology information (e.g., tributary
area) defines the co-simulation interface region. In this case the spatial
mapping is limited to point-to-point mapping, and you must ensure that there
are matching nodes between the models.
In
Abaqus
you can use a node set or a node-based surface to define a co-simulation
interface region consisting of discrete points.
Interacting through a Surface
Interaction between distinct domains occurs through a common interface
surface. For example, when a fluid interacts with a solid without penetrating
it, the fluid-solid interface is defined through a surface. In this case both
nodal position and element topology information define the co-simulation
interface, and appropriate spatial mapping between dissimilar surface meshes is
performed to conservatively map fields.
Interacting through a Volume
Interaction between overlapping domains occurs through a volume. In this
case both nodal position and element topology information define the
co-simulation region, and appropriate spatial mapping between dissimilar volume
meshes is performed to conservatively map fields.
The interface region is defined by an element set.
Identifying the Fields Exchanged across a Co-Simulation Interface
The coupling of the domain models can be through loads and/or boundary
conditions prescribed at the co-simulation interface. In addition, mass, rotary
inertia, and heat capacitance terms can also be exchanged. Based on the physics
and the interaction type and its enforcement, you must specify the fields that
are imported and/or exported in an
Abaqus
analysis during the co-simulation.
The co-simulation interface can consist of a group of discrete points
(nodes), a surface region, or a volume region. Not all fields can be exchanged
across all region types.
This section provides a general overview of all fields available in
Abaqus.
For detailed information on the fields exchanged between two
Abaqus
solvers, see
Structural-to-Structural Co-Simulation.
For detailed information on fields exchanged by
Abaqus
and a third-party analysis program, see the respective User’s Guides.
Procedures Involving Mechanical Degrees of Freedom
Table 1
lists the fields that can be exchanged for procedures supporting mechanical
degrees of freedom (degrees of freedom 1–6), their associated field
identifiers, the supported co-simulation interface region types, and which
Abaqus
solvers support import and export of the field values.
Table 1. Exchanging fields for procedures supporting mechanical degrees of
freedom.
Field ID
Fields
Interface Type1
Abaqus
Solver2
Units
Import
Export
UT or U
Displacement
P, S, V
S, E
S, E
L
VT or V
Velocity (transient procedures)
P, S, V
S, E
S, E
AT or A
Acceleration (transient procedures)
P, S, V
S
S, E
UR
Rotations
P, S
S, E
S, E
radians
VR
Angular velocity (transient procedures)
P, S
S, E
S, E
radians
AR
Angular acceleration (transient procedures)
P, S
S
S, E
radians
COORD
Current coordinates
P, S, V
S, E
CF
Concentrated forces
P, S, V
S, E
S, E
F
CM
Concentrated moments
P, S
S, E
S, E
PRESS
Pressure normal to element surface
S
S
1 P
(points), S (surface region), V (volume region)
2 S
(Abaqus/Standard), E (Abaqus/Explicit)
The following procedures support co-simulation using mechanical degrees of
freedom:
Displacements (field IDUT or U) for
the translational degrees of freedom can be exported by
Abaqus/Standard
and
Abaqus/Explicit.
Displacements can be imported by
Abaqus/Standard
and
Abaqus/Explicit.
When imported, displacements are ramped from the values of the previous
exchange time point to those of the next target time point. In an implicit
dynamic analysis, velocity and acceleration must be imported when importing
displacement. The displacements are in the global coordinate system.
Displacements are available for points, surface regions, and volume
regions in
Abaqus/Standard
and
Abaqus/Explicit.
Velocity and Acceleration
Velocity (field IDVT or V) and
acceleration (field IDAT or A) for
the translational degrees of freedom can be imported and exported by
Abaqus/Standard
for transient procedures and by
Abaqus/Explicit.
In an implicit dynamic analysis, when importing velocity or acceleration, all
three fields—displacement, velocity, and acceleration—must be imported.
Velocity and acceleration are in the global coordinate system.
Velocity and acceleration are available for points, surface regions, and
volume regions in
Abaqus/Standard
and
Abaqus/Explicit.
Rotations
Rotations (field IDUR) can be imported and exported by
Abaqus/Standard
and
Abaqus/Explicit.
In an implicit dynamic analysis, rotational velocity and rotational
acceleration must be imported when importing rotations. Rotations are in the
global coordinate system.
Rotations are available for points and surface regions.
Rotational Velocity and Rotational Acceleration
Rotational velocity (field IDVR) and rotational acceleration (field
IDAR) can be
imported and exported by
Abaqus/Standard
for transient procedures and by
Abaqus/Explicit.
In an implicit dynamic analysis, when importing rotational velocity or
rotational acceleration, all three fields—rotation, rotational velocity, and
rotational acceleration—must be imported. Rotational velocity and rotational
acceleration are in the global coordinate system.
Rotational velocity and rotational acceleration are available for points
and surface regions.
Current Coordinates
Current nodal coordinates (field IDCOORD) can be exported by
Abaqus/Standard
and
Abaqus/Explicit.
The coordinates are the current coordinates of the deformed structure whether
small- or large-displacement analysis is performed. In general, it is preferred
to export displacements (field IDUT or U)
rather than current coordinates when results are mapped between dissimilar
interface regions. In cases where the partner client does not retain the
original coordinates, it may be necessary to send current coordinate values
rather than displacements.
Current coordinates are available for points, surface regions, and volume
regions in
Abaqus/Standard
and
Abaqus/Explicit.
Concentrated Forces
Concentrated forces (field IDCF), if imported, are ramped from the values
of the previous exchange time point to those of the next target time point in
Abaqus/Standard
and are kept constant over the exchange interval in
Abaqus/Explicit.
The concentrated forces are in the global coordinate system.
When exporting concentrated forces,
Abaqus/Standard
transfers reaction forces at interface nodes that have prescribed
displacements. The reaction forces are exported in the global coordinate
system.
Concentrated forces are available for points, surface regions, and volume
regions in
Abaqus/Standard
and
Abaqus/Explicit.
Concentrated Moments
Concentrated moments (field IDCM), if imported, are ramped from the values
of the previous exchange time point to those of the next target time point in
Abaqus/Standard
and are kept constant over the exchange interval in
Abaqus/Explicit.
The concentrated moments are in the global coordinate system.
Concentrated moments are available for points and surface regions in
Abaqus/Standard
and
Abaqus/Explicit.
Normal Pressure
Normal pressure (field IDPRESS), supported for import by
Abaqus/Standard,
is the traction normal component to the surface. Pressure values are ramped
from the values of the previous exchange time point to those of the next target
time point when imported into
Abaqus/Standard.
In most cases it is preferred to import concentrated forces (field
IDCF) since
these contain both the normal and shear traction components. For membrane-like
structures it might be preferable to import pressures.
Procedures Involving Thermal Degrees of Freedom
Table 2
lists the thermal fields available for co-simulation exchange, their associated
field identifiers, the supported co-simulation interface region types, and
which
Abaqus
solvers support import and export of the field values.
Table 2. Exchanging fields for procedures supporting thermal degrees of
freedom.
Field ID
Fields
Interface Type1
Abaqus
Solver2
Units
Import
Export
NT
Temperature as a nodal degree of freedom
P, S, V
S, E
S, E
CFL
Concentrated heat flux at a node
P, S, V
S, E
HFL
Heat flux normal to element surface
S
S
CFILM
Concentrated (nodal) film property
P
S
FILM
Film properties (MpCCI
only)
S
S
TEMP
Temperature as a field imported at nodes and used at element integration points
P, S, V
S
1 P
(points), S (surface region), V (volume region)
2 S
(Abaqus/Standard), E (Abaqus/Explicit)
The following procedures support co-simulation using thermal degrees of
freedom:
Nodal temperature (field IDNT) can be imported and exported by
Abaqus/Standard
and
Abaqus/Explicit.
Temperature values are ramped from the values of the previous exchange time
point to those of the next target time point when imported into
Abaqus/Standard.
Temperature values can be exchanged either on the top surface
(SPOS) or the bottom surface
(SNEG) of structural elements. Temperatures
cannot be exchanged on double-sided surfaces. When exchanging temperatures on
both the top and bottom faces, define two different regions; one to exchange
temperature on the top face and the other to exchange temperature on the bottom
face. For volume regions, only degree of freedom
NT11 is used, and it should not be used for
exchanging temperature values over volumes discretized by nonthermal element
types.
Heat Flux
Use concentrated heat flux (field IDCFL) for heat entering at a node in
Abaqus/Standard
and
Abaqus/Explicit.
Concentrated heat flux is available for points, surface regions, and volume
regions.
Heat flux values can be exchanged either on the top surface
(SPOS) or the bottom surface
(SNEG) of structural elements. Heat flux
cannot be exchanged on double-sided surfaces. When exchanging heat flux on both
the top and bottom faces, define two different regions; one to exchange heat
flux on the top face and the other to exchange heat flux on the bottom face.
Use surface heat flux (field IDHFL) for a distributed heat flux entering the
surface in
Abaqus/Standard.
Distributed heat flux is available only for surface regions.
Film Properties
Use surface film properties (field IDFILM) or concentrated (nodal) film properties
(field IDCFILM) to model convection governed by
where q is the heat flux entering the surface, h is a
film coefficient, is the wall temperature, and is the fluid or ambient temperature. You should use concentrated film
properties only when coupling system models to three-dimensional models.
Both the film coefficient and fluid temperature are passed into
Abaqus/Standard
and are kept constant over the subsequent exchange interval. When the fluid and
wall temperatures coincide, an arbitrary small value for the heat transfer
coefficient is passed into
Abaqus.
To obtain reasonable film properties for the first exchange interval, you
should ensure that the wall temperatures are initialized properly in
Abaqus
and that you provide a good estimate for the initial fluid temperature.
Film properties are available only for surface regions in
Abaqus/Standard.
Procedures Involving Pore Fluid Pressure
Table 3
lists additional fields that can be exchanged for a coupled pore fluid
diffusion/stress analysis, their associated field identifiers, the supported
co-simulation interface region types, and which
Abaqus
solvers support import and export of the field values.
Table 3. Exchanging fields for a coupled pore fluid diffusion/stress
analysis.
Field ID
Fields
Interface Type1
Abaqus
Solver2
Units
Import
Export
POR
Pore fluid pressure at a node
P, S, V
S
S
CFF
Concentrated fluid flow at a node
P, S, V
S
RVF
Reaction fluid volume flux due to prescribed pressure
P, S, V
S
1 P
(points), S (surface region), V (volume region)
2 S
(Abaqus/Standard), E (Abaqus/Explicit)
The following procedure involving pore fluid pressure supports
co-simulation:
Nodal pore pressure (field IDPOR) can be imported and exported by
Abaqus/Standard
for points, surface regions, and volume regions.
Concentrated Fluid Flow
Fluid flow (field IDCFF) defines the seepage flow at a node.
Concentrated fluid flow can be imported by
Abaqus/Standard
for points, surface regions, and volume regions.
Reaction Fluid Volume Flow
Reaction fluid volume flux (field IDRVF) defines the rate at which fluid volume is
entering or leaving the model through the node to maintain the prescribed pore
pressure. Reaction fluid volume flux can be exported by
Abaqus/Standard
for points, surface regions, and volume regions.
Procedures Involving Electromagnetic Response
Table 4
lists additional fields that can be exchanged for an electromagnetic analysis,
their associated field identifiers, the supported co-simulation interface
region types, and which
Abaqus
solvers support import and export of the field values.
Table 4. Exchanging fields for a electromagnetic analysis.
Field ID
Fields
Interface Type1
Abaqus
Solver2
Units
Import
Export
EMJH
Joule heating flux due to flow of current
V
S
EMBF
Magnetic body force intensity vector due to flow of induced
current
V
S
1 P
(points), S (surface region), V (volume region)
2 S
(Abaqus/Standard), E (Abaqus/Explicit)
The following procedure involving electromagnetics supports co-simulation:
The Joule heating flux (field IDEMJH) can be exported by
Abaqus/Standard
for volume regions. It can be imported in a downstream heat transfer analysis
as concentrated nodal heat flux (field IDCFL).
Magnetic Body Force Intensity Vector
The magnetic body force intensity vector (field
IDEMBF) can
be exported by
Abaqus/Standard
for volume regions. It can be imported in a downstream stress analysis as
concentrated force (field IDCF).
Temperature and Independent Field Variables
Field variables are time-dependent, predefined fields that exist over the
spatial domain of the model (see
Predefined Fields).
Field variables in conjunction with the co-simulation technique extend the
possibilities of multiphysics by allowing material point dependencies on an
external field defined by another application.
Field variables must be numbered consecutively starting with one. Field
variables can be defined:
by entering the data directly,
by reading an
Abaqus
results file or output database file,
in an
Abaqus/Standard
user subroutine, and
through the co-simulation interface.
If field variables are defined by multiple methods,
Abaqus
processes them in the order defined above. Care needs be taken when field
variables are used with structural elements, such as membranes and shells. In
this case only the top or bottom face forming the interface region receives a
value.
Table 5
lists the temperature and independent field variables available for
co-simulation exchange, their associated field identifiers, the supported
co-simulation interface region types, and which
Abaqus
solvers support import and export of the field values.
Table 5. Exchanging temperature and independent field variables.
Field ID
Fields
Interface Type1
Abaqus
Solver2
Units
Import
Export
TEMP
Temperature as field variable
V
S
FV1
Field variable 1
V
S
FV2
Field variable 2
V
S
FV3
Field variable 3
V
S
1 P
(points), S (surface region), V (volume region)
2 S
(Abaqus/Standard), E (Abaqus/Explicit)
The following
Abaqus/Standard
procedures support import of temperature and independent field variables:
Temperature (field IDTEMP) can be imported by
Abaqus/Standard
for procedures that allow material properties to be defined as a function of an
external temperature field. When imported, temperature values are ramped from
the values of the previous exchange time point to those of the next target time
point. Use field IDNT instead of field
IDTEMP to
import temperature values for thermal procedures (procedures using degrees of
freedom 11, 12, etc.).
Independent Field Variables
Independent field variables (field IDs
FV1, FV2, and
FV3) can be imported by
Abaqus/Standard,
allowing material properties to be defined as a function of the external
fields. When imported, independent field variable values are ramped from the
values of the previous exchange time point to those of the next target time
point.
Miscellaneous Fields
Table 6
lists miscellaneous fields available for co-simulation exchange, their
associated field identifiers, the supported co-simulation interface region
types, and which
Abaqus
solvers support import and export of the field values.
Table 6. Exchanging miscellaneous fields.
Field ID
Fields
Interface Type1
Abaqus
Solver2
Units
Import
Export
MASS or LUMPEDMASS
Mass
P, S
S, E
S, E
M
RI
Rotary inertia
P, S
S
E
1 P
(points), S (surface region), V (volume region)
2 S
(Abaqus/Standard), E (Abaqus/Explicit)
Lumped Mass
Lumped mass values (field IDMASS or
LUMPEDMASS) at nodes can be exported and
imported by
Abaqus/Standard
and
Abaqus/Explicit.
Lumped mass is available for points and surface regions.
Rotary Inertia
Nodal (lumped) rotary inertia (field
IDRI) can be
imported by
Abaqus/Standard
and exported by
Abaqus/Explicit
over points or surface regions for models using structural elements.
Defining the Coupling and Rendezvousing Scheme
Different types of analyses have different time integration requirements
that will influence or dictate the frequency of interaction between the
analyses in a co-simulation to obtain an accurate and robust solution. For
example, consider the difference in time integration between an implicit and an
explicit dynamic analysis. Furthermore,
Abaqus/Standard
can adjust the increment sizes automatically to obtain an economical and
accurate solution for transient problems (see
Incrementation).
For example, consider a transient heat transfer analysis modeling a diffusive
process; here the analysis may use small time increments at the beginning of
the analysis where there is a high gradient in the solution and large time
increments toward the end of the analysis when steady state is reached.
The parameters that you use to control these co-simulation exchanges depend
on the co-simulation interface that you are using.
You define the co-simulation algorithm and related exchange parameters
in a co-simulation configuration file.
For structural-to-structural co-simulation using
Abaqus/Standard
and
Abaqus/Explicit,
you must also provide co-simulation controls parameters in the input file.
Using the SIMULIA Co-Simulation Engine Configuration File
The
SIMULIA Co-Simulation Engine
employs an independent software component, termed the “director,” which defines
all aspects of the interaction for co-simulation between analysis programs and
provides the necessary instructions to implement the coupling and rendezvousing
schemes. You provide the director with relevant parameters for your scheme
choices through the co-simulation configuration file.
The configuration file must be in Extensible Markup Language
(XML) format, which uses the file extension
xml. You can define a configuration file through a
predefined template, or you can create a fully elaborated form of the
configuration file.
Using predefined configuration templates
For the co-simulation analysis cases described in Co-Simulation between Abaqus Solvers, predefined templates
that define common coupling and rendezvousing schemes are available. To use one of the
predefined templates, you must create a configuration file with the structure shown below.
<?xml version="1.0" encoding="utf-8"?>
Required XML declaration line
<CoupledMultiphysicsSimulation>
Required XML root element; identifies file as describing a multiphysics simulation
<template_name>
<template_parameter_1>parameter_1_name</template_parameter_1>
<template_parameter_2>parameter_2_name</template_parameter_2>
<template_parameter_3>parameter_3_name</template_parameter_3>
</template_name>
Closure of the template element
</CoupledMultiphysicsSimulation>
Closure of the XML root element
At run time, the
SIMULIA Co-Simulation Engine
director applies your parameter settings to the template, creating an
elaborated configuration file that is then used in the co-simulation analysis.
An elaborated configuration file is defined as a configuration file that
provides all details of the configuration explicitly without referring to a
template.
In cases where predefined templates are not available (such as coupling with an in-house or
third-party code) or are insufficient (for example, you want to exchange more variables at
the co-simulation interface region or adjust mapping tolerances), you must create an
elaborated configuration file. For tips on working with elaborated configuration files,
see “Advanced Uses of the SIMULIA Co-Simulation Engine Configuration File” in the Dassault Systèmes Knowledge Base at . For
detailed information about the elaborated configuration file, see the SIMULIA Co-Simulation Engine Application Programing Interface (API) documentation.
Coupling and Rendezvousing Schemes for Elaborated Configuration Files
You define the co-simulation coupling and rendezvousing schemes in an
elaborated configuration file.
Coupling Scheme
The coupling scheme defines the sequence of exchanges between analysis
programs and whether a coupled simulation can be run in a serial, parallel, or
implicit iterative manner. When deciding on the coupling scheme, you should
consider solution stability issues as well as the utilization impact on your
computing resources
Parallel Explicit Coupling Scheme (Jacobi)
In a parallel explicit coupling scheme, both simulations are executed
concurrently, exchanging fields to update the respective solutions at the next
target time. The parallel coupling scheme may make more efficient use of
computing resources; however, it is considered less stable than the sequential
scheme and should be employed only for weakly coupled physics simulations using
small coupling steps. The co-simulation partner analysis must also specify a
Jacobi coupling algorithm.
In a sequential explicit coupling scheme, the simulations are executed in
sequential order. One analysis leads while the other analysis lags the
co-simulation. The co-simulation partner analysis must also specify a
Gauss-Seidel coupling algorithm.
The sequential explicit coupling scheme should be employed only for weakly
coupled physics simulations using small coupling steps.
Iterative Coupling Scheme
In an iterative coupling scheme, the simulations are executed in
sequential order. One analysis leads while the other analysis lags the
co-simulation. Multiple exchanges per coupling step are performed until
termination criteria are met.
The termination criteria depend on the analyses in the co-simulation; for
co-simulation between
Abaqus
and third-party analysis products, consult the appropriate User’s Guide.
Coupling Step Size
The coupling step is the period between two consecutive exchanges and
consequently defines the frequency of exchange between the analyses in a
co-simulation. The coupling step size is established at the beginning of each
coupling step and is used to compute the target time (the time when the next
synchronized exchange occurs).
The methods available in
Abaqus
for computing the coupling step size are described in the sections below. To
determine the methods available for a co-simulation partner analysis, consult
the appropriate third-party program documentation.
Constant Coupling Step Size
A constant user-defined coupling step size is the most basic method of
defining a coupling step size. Both analyses advance while exchanging data at
target points according to
where
is a value that defines the coupling step size to be used throughout the
coupled simulation,
is the target time, and
is the time at the start of the coupling step.
Minimum Coupling Step Size
This method selects the minimum of the coupling step sizes suggested by
each analysis.
Abaqus
always uses the next increment suggested by its automatic incrementation as its
suggested coupling step size.
Maximum Coupling Step Size
This method selects the maximum of the coupling step sizes suggested by
each analysis.
Abaqus
always uses the next increment suggested by its automatic incrementation as its
suggested coupling step size.
Importing the Coupling Step Size
Abaqus
can import a coupling step size suggested by the co-simulation partner
analysis.
Exporting the Coupling Step Size
Abaqus
can export a suggested coupling step size to the co-simulation partner
analysis.
Time Incrementation Scheme
Abaqus
may take multiple increments per coupling step, or you can force
Abaqus
to use a single increment per coupling step.
Typically,
Abaqus
may perform several increments (referred to as “subcycling”) during the
coupling step. During subcycling,
Abaqus/Standard
ramps the loads and boundary conditions (with the exception of film properties)
from the values at the end of the previous coupling step to the values at the
target time, while in
Abaqus/Explicit
the loads are applied at the start of the coupling step and kept constant over
the coupling step.
Subcycling allows
Abaqus
to use its own time incrementation to reach the target coupling time;
specifically, it allows
Abaqus
to cut back the increment size if there are nonlinear events that require the
increment size to be reduced.
In certain cases you may force
Abaqus
to use a time increment size dictated by the coupling step size (i.e., no
subcycling). This allows both solvers to use the same time incrementation and
avoid interpolation of quantities during the coupling step. When proceeding in
this “lockstep” manner,
Abaqus
will not be able to reduce the time increment to resolve nonlinear events and,
consequently, will terminate the simulation in cases where the nonlinear events
require that the increment size be reduced.
Model Dimension and Coordinate Systems
Two-dimensional and three-dimensional
Abaqus
models are fully supported. Axisymmetric
Abaqus
models are supported only for
Abaqus/Standard
to
Abaqus/Explicit
co-simulation. For co-simulations that do not support two-dimensional and
axisymmetric models, you can represent these models as a three-dimensional
slice of unit thickness (or wedge element) with the appropriate boundary
conditions applied.
Vector quantities are defined according to
Abaqus
conventions; the first component represents the quantity along the
x-axis, the second quantity represents the quantity along
the y-axis, and the third quantity represents the quantity
along the -axis
(for three-dimensional models). For axisymmetric models in
Abaqus
the axis of revolution is about the y-axis. These
conventions apply to both the exported and the imported vector quantities.
All exported vector quantities are expressed in the global coordinate system
of the
Abaqus
model, ignoring any transformation definitions. Similarly, the third-party
program must provide vector quantities that are imported into
Abaqus
in the global coordinate system of the
Abaqus
model.
The third-party analysis program may use different conventions, please refer
to the appropriate third-party program documentation for further modeling
details and/or limitations.
Unit System
Abaqus
does not require that the analysis be run with a particular unit system. In
general, the unit system used in creating the
Abaqus
model may not be the same as that used with the third-party program model. When
the two unit systems differ, the fields exchanged between the two programs must
go through a transformation of units. Refer to the appropriate third-party
program documentation for further modeling details.
Restarting a Co-Simulation
Field imported into
Abaqus/Standard
and
Abaqus/Explicit
are not saved to the
Abaqus
restart database. Thus, to restart a co-simulation, the coupled analysis must
send the fields at the start of the restart analysis. These fields must balance
the conjugate fields computed by the
Abaqus
analysis such that equilibrium is maintained. You must synchronize the restart
information written between the analyses to ensure that the simulation is
restarted at the same solution (step) time. For more information, see
Synchronizing Restart Information Written in a Co-Simulation.
Specifically, the solution time for the particular step/increment number from
which
Abaqus
is restarted must correspond to the coupled analysis solution.
Limitations
The following limitations apply:
The steps in the
Abaqus
model must be defined such that the co-simulation fits entirely within a single
Abaqus
step. Further, there can be only one co-simulation in the
Abaqus
job. You can use the restart capability to perform multiple co-simulations for
an analysis (see
Restarting an Analysis).
A co-simulation surface or volume defined over beam, pipe, and truss
elements or defined over the edges of three-dimensional elements cannot be used
as an interface region. You should use discrete points to transfer loads and
boundary conditions.
A co-simulation surface or volume defined over modified triangular
elements or modified tetrahedral elements cannot be used as an interface
region.
Quadratic coupled temperature-displacement elements cannot be used as an
interface region in a co-simulation using the coupled temperature-displacement
procedure.
When performing a co-simulation, output at specified time points may not
be satisfied at the requested times, depending on the synchronization
parameters.
There may be further limitations depending on the third-party analysis
program being used. For more information, refer to the appropriate third-party
program documentation.