Structural-to-Structural Co-Simulation

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.

Refer to Dynamic impact of a scooter with a bump for an example of Abaqus/Standard to Abaqus/Explicit co-simulation.

This page discusses:

Coupling in Abaqus/Standard and Abaqus/Explicit Co-Simulation
Identifying the Co-Simulation Interface Region
Enhanced Subcycling Method for Interface Calculations
Original Subcycling Method for Interface Calculations
Lockstep Method for Interface Calculations
Creating a Configuration File
Executing the Coupled Analysis
Limitations

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:

You can use the following Abaqus/Explicit analysis procedure:

Explicit Dynamic Analysis

Identifying the Co-Simulation Interface Region

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).

<?xml version="1.0" encoding="utf-8"?>
<CoupledMultiphysicsSimulation>
   <template_std_xpl_subcycleEnhanced rotation="true or false">
      <Standard_Job>standard_job_name</Standard_Job>
      <Explicit_Job>explicit_job_name</Explicit_Job>
      <Explicit_Interface>region_name</Explicit_Interface>
      <duration>duration_value</duration>
   </template_std_xpl_subcycleEnhanced>
</CoupledMultiphysicsSimulation>

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.

Executing the Coupled Analysis

You execute the co-simulation from the command line, as described in Executing a Co-Simulation.

Diagnostics Information

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.

Limitations

The following limitations apply to Abaqus/Standard to Abaqus/Explicit co-simulation in addition to the limitations discussed in Preparing an Abaqus Analysis for Co-Simulation.

General Limitations

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.