Co-simulation between two structural solvers (solvers exchanging
displacements and rotations and the conjugate fields' forces and moments) represents a very
strong physics coupling and requires special treatment at the co-simulation interface. Abaqus supports Abaqus/Standard to Abaqus/Explicit co-simulation and Abaqus to Simpack (a multibody dynamics solver) co-simulation by providing specialized interface handling.
Although you can perform a structural-to-structural co-simulation between two Abaqus/Standard analyses or between two Abaqus/Explicit analyses, it is not recommended due to the lack of proper handling at the interface.
Abaqus supports three interface handling methods: the enhanced subcycling method, the "original"
subcycling method, and the lockstep method. The enhanced subcycling method is the preferred
method, providing robust and accurate solutions in the most cost effective manner. This method
also allows constraints to be located on the co-simulation interface. The latter two methods
are documented for legacy purposes.
This section discusses analysis setup, execution,
and limitation details specific to Abaqus/Standard to Abaqus/Explicit co-simulation.
Coupling in Abaqus/Standard and Abaqus/Explicit Co-Simulation
Co-simulation between Abaqus/Standard and Abaqus/Explicit is a multiple domain analysis approach, where each Abaqus analysis operates on a complementary section of the model domain where it is expected to
provide the more computationally efficient solution. For example, Abaqus/Standard provides a more efficient solution for light and stiff components, while Abaqus/Explicit is more efficient for solving complex contact interactions. In addition, when a portion
of the Abaqus/Standard model is linear, you can use substructures to further reduce the computational cost .
You can use the following Abaqus/Standard analysis procedures:
The domains modeled in each Abaqus analysis are complementary, and the interaction between the models takes place through a
common interface region. You can specify an interface region using either node sets or
surfaces when coupling Abaqus/Standard to Abaqus/Explicit. However, you must be consistent in your region definition in Abaqus/Standard and Abaqus/Explicit. If you define a co-simulation region with a node set or node-based surface in one
analysis, you must use the same type of co-simulation region definition in the other
analysis. For node-based surfaces the nodes must be coincident because no topology
information is provided to conservatively map fields between the models. Likewise, if you
define a co-simulation region with an element-based surface in one analysis, you must define
your co-simulation region with an element-based surface in the other analysis.
You can have dissimilar meshes in regions shared in the Abaqus/Standard and Abaqus/Explicit model definitions. In some cases you can improve solution stability and accuracy by
ensuring that you have matching nodes at the interface (see Dissimilar Mesh-Related Limitations).
In the step definition, you declare a co-simulation step, define the interface region, and
specify the solution fields to exchange. When coupling Abaqus/Standard to Abaqus/Explicit, you can declare only a single interface region; if there are multiple regions, you must
combine them into a single region. The fields exchanged depend on the interface method and
whether or not rotational degrees of freedom are active at the interface.
Enhanced Subcycling Method for Interface Calculations
The enhanced subcycling method is the preferred method for coupling Abaqus/Standard to Abaqus/Explicit. This method ensures velocity compatibility at the interface, where calculations are
performed by an interface service; stiffness and mass properties of the underlying structure
are exchanged in the form of a dynamic interface operator providing robust and accurate
solutions for strongly coupled physics. Abaqus/Explicit subcycles (that is, takes one or more increments) per Abaqus/Standard increment to ensure a cost-effective solution of both domains. This method allows
constraints to exist on the co-simulation interface region. Table 1 and Table 2 provide descriptions of
fields exchanged and their causality (whether the field is imported or exported).
Table 1. Fields imported and exported by Abaqus/Standard for the enhanced subcycling method.
Field
Description
Causality
IFORCE
Interface force used by the interface service.
Import
IMOMENT
Interface moment used by the interface service when rotational degrees of
freedom are active.
Import
VT
Translational velocity.
Export
VR
Rotational velocity when rotational degrees of freedom are active.
Export
H
Dynamic interface operator used by the interface service; the dynamic operator
is constructed based on whether or not rotational degrees of freedom are
active.
Export
Table 2. Fields imported and exported by Abaqus/Explicit for the enhanced subcycling method.
Field
Description
Causality
VTINTRF
Translation velocity used by the interface service.
Import
VRINTFR
Rotational velocity used by the interface service when rotational degrees of
freedom are active.
Import
H
Dynamic interface operator used by the interface service; the dynamic operator
is constructed based on whether or not rotational degrees of freedom are
active.
Import
IFORCE
Interface force used by the interface service.
Export
IMOMENT
Interface moment used by the interface service when rotational degrees of
freedom are active.
Export
An interface solve is performed in Abaqus/Explicit for every Abaqus/Explicit increment. This solve can be costly because the interface matrix used for the interface
solve is dense, and its size scales with the number of interface nodes.
Original Subcycling Method for Interface Calculations
Similar to the enhanced subcycling method, the "original" subcycling method ensures
velocity compatibility at the interface and provides a robust and accurate solution for
strong coupled physics.
Table 3 and Table 4 provide descriptions of
fields exchanged and their causality. You must specify rotational fields even if they are
not active at the interface.
Table 3. Fields imported and exported by Abaqus/Standard for the original subcycle method.
Field
Description
Causality
VRINTRF
Rotational velocity used by the interface service.
Import
MASSINV
Inverse mass operator.
Import
RICUR
Rotary inertia.
Import
IFORCE
Interface force computed by the interface service.
Export
IMOMENT
Interface moment computed by the interface service.
Export
VT
Translation velocity used for initial conditions.
Export
VR
Rotational velocity used for initial conditions.
Export
VTINTRF
Translational velocity used by the interface service.
Import
Table 4. Fields imported and exported by Abaqus/Explicit for the original interface method.
Field
Description
Causality
IFORCE
Interface force computed by the interface service.
Import
IMOMENT
Interface moment computed by the interface service.
Import
VTINIT
Initial translational velocity.
Import
VRINIT
Initial rotational velocity.
Import
VT
Translational velocity.
Export
VR
Rotational velocity.
Export
MASS
Lumped mass.
Export
RICUR
Rotary inertia.
Export
An interface solve is performed in Abaqus/Standard for every Abaqus/Explicit increment. This solve can be costly for two reasons. First, the interface matrix used for
the interface solve is dense, and its size scales with the number of interface nodes.
Second, the interface matrix changes every Abaqus/Explicit increment, requiring factorization in Abaqus/Standard for every Abaqus/Explicit increment. You can reduce the impact of this cost by approximating the interface matrix
and factorizing it typically once for the duration of an Abaqus/Standard increment, rather than for eachAbaqus/Explicit increment. However, if the Abaqus/Explicit stable time increment changes significantly, the interface matrix is refactored for
stability reasons.
Factorizing the interface matrix every Abaqus/Explicit increment is the default. When the number of interface nodes is large, the cost of the
interface factorization is reduced using this approach. Only the interface matrix
factorization is performed once per Abaqus/Standard increment; the interface solve is performed every Abaqus/Explicit increment using this factorized interface matrix. Because this approach approximates the
interface matrix, it may slightly increase the drift in the displacement solution at the
co-simulation interface. The performance gain with this method depends on the number of
interface nodes, the subcycling ratio (which is the ratio between Abaqus/Standard and Abaqus/Explicit increments), and the size of the models. For models with greater than 100 interface nodes
and a subcycling ratio greater than 50, this method typically reduces the analysis time by a
factor between 1.2 and 3.0. The performance gain increases for larger subcycling ratios and
decreases for larger models.
You can also automate the selection of the fields for both Abaqus/Standard and Abaqus/Explicit models.
Lockstep Method for Interface Calculations
The time incrementation that you choose for coupling affects the solution computational
cost, accuracy, and stability. The enhanced subcycling method is frequently the more robust,
accurate, and cost effective method because Abaqus/Standard time increments, free of any forced co-simulation time incrementation constraints, are
commonly much longer than Abaqus/Explicit time increments. However, this subcycling method may be less cost effective when a large
portion of the nodes in the model are at the co-simulation interface. This is because
stabilization operations at the interface (a “free solve”) for each increment in the Abaqus/Explicit analysis is performed. These free-solve operations require an implicit solution of a
dense system of equations that scale with the number of interface nodes. In cases with a
large number of interface nodes, the computational cost of this interface solve can exceed
any cost savings seen due to subcycling. Therefore, for a model where a significant share of
the nodes are at the co-simulation interface, performance may be poorer with the subcycling
scheme. In such a case, you can use the lockstep method, where Abaqus/Standard is forced to use the time increment size of the Abaqus/Explicit analysis. This approach enforces displacement compatibility at the interface.
Table 5 and Table 6 provide descriptions of
the fields exchanged and their causality. You must specify rotational fields even if there
are no rotational degrees of freedom active at the interface.
Table 5. Fields imported and exported by Abaqus/Standard for the lockstep method.
Field
Description
Causality
CF
Concentrated force.
Import
CM
Concentrated moment.
Import
MASS
Lumped mass.
Import
RICUR
Rotary inertia.
Import
UTPRED
Predictor displacement.
Export
URPRED
Predictor rotation.
Export
VT
Translational velocity.
Export
VR
Rotational velocity.
Export
AT
Translational acceleration.
Export
AR
Rotational acceleration.
Export
Table 6. Fields imported and exported by Abaqus/Explicit for the lockstep method.
Field
Description
Causality
UTINIT
Initial displacements.
Import
URINIT
Initial rotations.
Import
VTINIT
Initial translational velocity.
Import
VRINIT
Initial rotational velocity.
Import
ATINIT
Initial translational acceleration.
Import
ARINIT
Initial rotational acceleration.
Import
UT
Displacement.
Import
UR
Rotation.
Import
CF
Concentrated forces.
Export
CM
Concentrated moments.
Export
MASS
Mass.
Export
RICUR
Rotary inertia.
Export
The selection of the fields for both Abaqus/Standard and Abaqus/Explicit models are automated.
Creating a Configuration File
You can use predefined templates to create a configuration file for the coupling schemes
described above. Table 7 describes the two predefined templates available for Abaqus/Standard to Abaqus/Explicit co-simulation and lists example configuration files that you can review.
Table 7. Templates for structural-to-structural co-simulation.
Enhanced subcycling method
Coupling scheme: Allow Abaqus/Explicit to subcycle. This is the recommended method.
template_std_xpl_subcycleEnhanced
Example file: exa_std_xpl_subcycleEnhanced.xml
Original subcycling method
Coupling scheme: Allow Abaqus/Explicit to subcycle.
template_std_xpl_subcycle
Example file: exa_std_xpl_subcycle.xml
Lockstep method
Coupling scheme: Abaqus/Standard and Abaqus/Explicit use a single increment per coupling step (lockstep).
template_std_xpl_lockstep
Example file: exa_std_xpl_lockstep.xml
To obtain an example configuration file, you can use the abaqus
fetch utility. For example, to obtain the example for Abaqus/Standard to Abaqus/Explicit subcycling, use the following command:
abaqus fetch job=GandC_contbeam_mixDofs
You can then modify the configuration by modifying the replaceable text (rotation degrees
of freedom active at interface, job names, Abaqus/Explicit interface region name and duration).
In certain cases you may need to use co-simulation configuration features that are not
described in the predefined templates. For example, you may want to change the dissimilar
mesh mapping search tolerances; these tolerances are available generally in the
configuration file but are not described in the predefined templates. For these cases, you
must create an elaborated configuration file; for more information, see Using Elaborated Configuration Files.
The Abaqus/Standard job provides detailed descriptions of co-simulation operations in the message
(.msg) file. For the subcycling scheme the status
(.sta) file provides summary information indicating when the
interface calculations followed by a re-solve of the increment are made, as shown in the
following example status file. The E suffix in the
attempt-count entry (column 3) indicates an increment performing interface calculations.
An increment without the E suffix indicates a re-solve of
the increment.
SUMMARY OF JOB INFORMATION:
STEP INC ATT SEVERE EQUIL TOTAL TOTAL STEP INC OF DOF IF
DISCON ITERS ITERS TIME/ TIME/LPF TIME/LPF MONITOR RIKS
ITERS FREQ
1 1 1E 0 1 1 0.000 0.000 0.001000
1 1 1 0 3 3 0.00100 0.00100 0.001000
1 2 1E 0 1 1 0.00100 0.00100 0.001000
1 2 1 0 3 3 0.00200 0.00200 0.001000
1 3 1E 0 1 1 0.00200 0.00200 0.001000
1 3 1 0 2 2 0.00300 0.00300 0.001000
1 4 1E 0 1 1 0.00300 0.00300 0.001000
1 4 1 0 3 3 0.00400 0.00400 0.001000
The
Abaqus/Explicit
job provides summary descriptions of co-simulation operations in the status
(.sta) file.
Displacement compatibility at the co-simulation interface is not maintained when you
choose either subcycling solution method. For these methods, velocity compatibility is
maintained, but you may see small amounts of displacement mismatch between Abaqus/Standard and Abaqus/Explicit as the simulation advances in time. This “drift” is more pronounced if severe
nonlinearity (such as plastic deformation) occurs at the co-simulation interface. You
can control this drift by adjusting Abaqus/Standard solution parameters so that the Abaqus/Standard increment size is reduced (for example, by limiting the maximum time increment size
or specifying a smaller half-increment residual tolerance for implicit dynamic
analyses).
Nodal transformations are not permitted on the co-simulation region
nodes.
The ALE technique may not be used in
elements attached to co-simulation region nodes.
Fully coupled temperature-displacement elements can be used, but no
temperature quantities are exchanged.
An
Abaqus/Standard
static stress analysis cannot be used with the lockstep time incrementation
scheme in
Abaqus/Standard
to
Abaqus/Explicit
co-simulation.
Only points and surface regions are allowed; coupling volume regions is
not supported.
Only a single region can be defined as the interface region; multiple
interface regions are not supported.
Dissimilar Mesh-Related Limitations
When your
Abaqus/Standard
and
Abaqus/Explicit
co-simulation region meshes differ, the following limitations apply:
Solution accuracy may be affected when your co-simulation region meshes
are not uniform in the presence or absence of rotational degrees of freedom;
for example, if a continuum element mesh is locally reinforced with beam or
shell elements at the co-simulation region interface.
In cases where the stress state near the co-simulation interface is
significant (approaching 1% or more) relative to the material stiffness, you
may observe appreciable irregular mesh distortion if the mesh density adjacent
to the co-simulation region differs greatly between the
Abaqus/Explicit
and
Abaqus/Standard
models. For example, this effect is common with large deformation of
hyperelastic materials. You can minimize this effect by choosing a similar or
finer mesh at the
Abaqus/Standard
co-simulation region when using the subcycling time integration scheme or by
choosing a similar or finer mesh at the
Abaqus/Explicit
co-simulation region when using the lockstep time integration scheme.
Abaqus/Standard Analysis Limitations
Abaqus/Standard
elements that have no equivalent degree-of-freedom counterpart in
Abaqus/Explicit
cannot be connected to co-simulation region nodes. These elements include
Axisymmetric elements with twist degrees of freedom (the
CGAX element family)
Axisymmetric solid elements with asymmetric deformation (the
CAXA element family)
Generalized plane strain elements (the
CPEG element family)
Coupled pore pressure-displacement elements
Heat transfer and thermal-electrical elements
Acoustic elements
Piezoelectric elements
The following specific limitations also apply:
A co-simulation region node cannot be a secondary node in a tie constraint, an
MPC constraint, or a kinematic coupling constraint.
Abaqus/Explicit Analysis Limitations
Stability and accuracy of the co-simulation solution may be adversely
affected when the following model features are defined at or near the
co-simulation region:
Connector elements connected to co-simulation region nodes.
Co-simulation region nodes that participate in a tie constraint, an
MPC constraint, or a kinematic coupling
constraint.
When using these features, you should compare the Abaqus/Standard and Abaqus/Explicit solutions (for example, compatibility of the displacement history) at the co-simulation
interface as an indicator of solution accuracy.