The co-simulation technique is a capability for run-time coupling of Abaqus and another analysis program. An Abaqus analysis can be coupled to another Abaqus analysis or to a third-party analysis program to perform multiphysics simulations and multidomain (multimodel) coupling.
Abaqus provides built-in procedures to solve multiphysics simulations as described in “Multiphysics analyses” in “Solving analysis problems: overview,” Section 6.1.1. For multiphysics problems for which Abaqus does not provide a built-in solution procedure or where the solution procedure is limited in functionality, you can use the co-simulation technique to couple Abaqus with a third-party analysis program; for example, fluid-structure interaction (FSI) simulation in conjunction with computational fluid dynamics (CFD) analysis programs.
Co-simulation between Abaqus/Standard and Abaqus/Explicit illustrates 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.
Another application area is solving complex problems where the model is divided into multiple domains and different analysis programs are used to obtain solutions for each domain; for example, crash safety simulation performed in conjunction with the occupant simulation program MADYMO.
The Abaqus co-simulation technique:
can be used to solve complex fluid-structure interactions by coupling Abaqus with CFD analysis programs, including Abaqus/CFD analyses;
can be used to solve conjugate heat transfer problems by coupling Abaqus/Standard with CFD analysis programs, including Abaqus/CFD analyses;
can be used to solve complex analyses more effectively by coupling Abaqus/Standard to Abaqus/Explicit;
can be used for multiphysics simulations by coupling Abaqus with third-party analysis programs;
can be used to couple Abaqus with in-house codes using the SIMULIA Co-Simulation Engine or the multiphysics code coupling interface, MpCCI;
can be used for crash safety simulations by coupling Abaqus/Explicit with the occupant simulation program MADYMO;
is intended for advanced users with in-depth knowledge of Abaqus and the third-party analysis program;
allows for both unidirectional and bidirectional transfer of data;
can be used with Abaqus models having linear or nonlinear structural response; and
supports both steady-state and transient simulations.
In a co-simulation the interaction between the domains is through a common physical interface region over which data are exchanged in a synchronized manner between Abaqus and the coupled analysis program.
One domain may affect the response of another domain through one or more of the following:
the constitutive behavior, such as the yield stress defined as a function of temperature or stress defined as a function of other solution fields, such as thermal strains or the piezoelectric effect;
surface tractions/fluxes, such as a fluid exerting pressure on a structure;
body forces/fluxes, such as heat generation due to flow of current in a coupled thermal-electrical simulation;
contact forces, such as the forces due to contact between a vehicle and an occupant/pedestrian modeled as separate domains; and
kinematics, such as fluid in contact with a compliant structure where the interface motion affects the fluid flow.
Direct coupling using SIMULIA Co-Simulation methods.
Coupling using MpCCI, a third-party connectivity middleware.
SIMULIA Co-Simulation methods provide direct coupling between two Abaqus analyses or between Abaqus and third-party analysis programs, without any third-party communication tool. These methods are used for fluid-structure simulations, conjugate heat transfer, coupling Abaqus/Standard to Abaqus/Explicit for interaction between implicit dynamic and explicit dynamic domains, and coupling Abaqus to MADYMO for vehicle-occupant/pedestrian interaction.
You can perform complex fluid-structure interaction (FSI) problems by coupling Abaqus/Standard or Abaqus/Explicit to a computational fluid dynamics (CFD) analysis program. Abaqus/Standard and Abaqus/Explicit solve the structural domain, and the CFD analysis program solves the fluid domain. Abaqus/Standard and Abaqus/Explicit can be coupled with Abaqus/CFD as well as with several third-party CFD analysis programs.
For detailed information on coupling Abaqus/CFD to Abaqus/Standard or to Abaqus/Explicit, see “Preparing an Abaqus analysis for co-simulation,” Section 17.2.1, and “Abaqus/CFD to Abaqus/Standard or to Abaqus/Explicit co-simulation,” Section 17.3.2. For a complete list of qualified partner products, see www.simulia.com.
You can perform conjugate heat transfer problems involving fluids and structures by coupling Abaqus/Standard to a computational fluid dynamics (CFD) analysis program. Abaqus/Standard models heat transfer within the structure (see “Uncoupled heat transfer analysis,” Section 6.5.2, and “Fully coupled thermal-stress analysis,” Section 6.5.3), and the CFD analysis program solves the energy equation for the fluid flow surrounding the structure. Abaqus/Standard can be coupled with Abaqus/CFD as well as with several third-party CFD analysis programs.
For an example of Abaqus/CFD to Abaqus/Standard co-simulation, refer to “Conjugate heat transfer analysis of a component-mounted electronic circuit board,” Section 6.1.1 of the Abaqus Example Problems Manual. For detailed information on coupling Abaqus/CFD to Abaqus/Standard, see “Preparing an Abaqus analysis for co-simulation,” Section 17.2.1, and “Abaqus/CFD to Abaqus/Standard or to Abaqus/Explicit co-simulation,” Section 17.3.2. For a complete list of qualified partner products, see www.simulia.com.
In certain cases you can realize significant computational cost savings by partitioning a model and combining the Abaqus/Standard and Abaqus/Explicit solutions, such as
when the simulation is principally a candidate for Abaqus/Explicit, but where certain parts of the model can be idealized using substructures in Abaqus/Standard, or
when the simulation is principally a candidate for Abaqus/Standard, but where complex contact conditions would be handled more effectively by Abaqus/Explicit.
Crash safety simulation generally includes interaction between a vehicle and its occupant or a vehicle and a pedestrian. Abaqus/Explicit is used to model the vehicle, and MADYMO is used to model the occupant or the pedestrian.
In some cases the influence of the human response on the structural response of the vehicle is so small as to be negligible. In these cases only a part of the vehicle surrounding the human is used in a coupled analysis. The vehicle analysis is performed without the human, and the motion from a portion of the vehicle immediately surrounding the human is extracted as a submodel of the full vehicle response. The co-simulation technique is used to perform a coupled analysis with the human model and the vehicle submodel.
For an example of co-simulation with MADYMO, refer to “Rigid body dynamics with Abaqus/Explicit,” Section 1.3.7 of the Abaqus Benchmarks Manual. The coupling between Abaqus/Explicit and MADYMO is actively supported and tested by both SIMULIA and TNO MADYMO BV. For detailed information, refer to “Using coupling between Abaqus/Explicit and MADYMO in Abaqus” in the Dassault Systèmes Knowledge Base at www.3ds.com/support/knowledge-base or the SIMULIA Online Support System, which is accessible through the My Support page at www.simulia.com.
MpCCI, the multiphysics code coupling interface developed and distributed by the Fraunhofer-Institute for Algorithms and Scientific Computing (SCAI), provides an open system approach for general multidisciplinary simulations between Abaqus and any third-party analysis program that supports MpCCI. MpCCI provides a scalable communication infrastructure and mapping algorithms for multiple physics domains. In a co-simulation using MpCCI, Abaqus communicates in real time with the MpCCI coupling server to exchange fields with the third-party analysis program while each analysis advances its simulation time.
Coupling through MpCCI may occur between Abaqus and any third-party analysis program that supports the MpCCI interface. This includes in-house codes that have the MpCCI adapter embedded. SIMULIA actively supports and qualifies a link between Abaqus and FLUENT for fluid-structure interaction. For more information, refer to “Abaqus User's Guide for Fluid-Structure Interaction (FSI)” in the Dassault Systèmes Knowledge Base at www.3ds.com/support/knowledge-base or the SIMULIA Online Support System, which is accessible through the My Support page at www.simulia.com.
You will typically apply co-simulation techniques to problems where the most complex physics occurs within domains that are handled exclusively within an analysis program (e.g., Abaqus or a CFD analysis program). Due to the comparative numerical simplicity of the numerical techniques applied at the co-simulation interface, the physics controlling the interaction at the interface of the separate analysis domains (the strength of the physics coupling) must be relatively weak for the co-simulation technique to be applied effectively.
In a fluid-structure interaction (FSI) co-simulation the analysis domains are coupled in a staggered approach in a globally explicit manner; that is, the equations for each domain are solved separately, and loads and boundary conditions are exchanged at the common interface.
Similarly, in a crash safety simulation with the vehicle modeled in Abaqus/Explicit and the dummy modeled in MADYMO, the interaction of the domains is resolved by application of the forces resulting from the contact condition between the interface of the two domains.
The staggered approach is applicable to many problems that exhibit weak to moderate physics coupling. In cases where the coupling is sufficiently weak, the coupling may be required only in one direction (such as when a temperature field contributes to the structural response, but a reverse coupling provides no significant impact on the simulation results). The staggered approach may not be effective for problems that exhibit strong physics coupling.
Figure 17.1.1–1 illustrates the coupling strength with an analogy in the frequency domain. Consider a lumped parameter dynamic system with a coupling impedance directly related to a response frequency 
. In a staggered solution approach each domain is solved by temporarily ignoring the coupling terms represented by the gray spring and dashpot in Figure 17.1.1–1.
The strength of the physics coupling can generally be greater in the coupling of Abaqus/Standard to Abaqus/Explicit using the co-simulation technique. Through communication of “right-hand-side” and “left-hand-side” terms, Abaqus/Standard to Abaqus/Explicit co-simulation provides a robust interface solution across a wide range of problem parameters. In many cases you can choose to have Abaqus/Standard and Abaqus/Explicit each advance their solutions according to their own automatic time incrementation scheme without adversely affecting the interface solution stability.
For the latest support information and tips on running FSI simulations and crash safety simulations, see the Dassault Systèmes Knowledge Base at www.3ds.com/support/knowledge-base or the SIMULIA Online Support System, which is accessible through the My Support page at www.simulia.com.
