The ABAQUS co-simulation interface can be used to perform multidisciplinary analyses in which two or more distinct and coupled physical fields are modeled by different analysis codes. Data can be exchanged in a synchronized manner between the ABAQUS analysis products and third-party analysis tools supporting the Mesh-based Parallel Code-Coupling Interface, MpCCI.
Multidisciplinary problems involve two or more distinct physical subsystems that are coupled. One subsystem may affect the response of another subsystem 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; and
geometric changes, such as fluid in contact with a deforming structure.
The ABAQUS co-simulation interface:
is primarily intended for simulating FSI problems between ABAQUS and FLUENT;
can be used for multidisciplinary physical simulations between ABAQUS and any third-party analysis code supporting the MpCCI interface;
is intended for advanced users with in-depth knowledge of ABAQUS, the third-party code, and the functionality of the MpCCI; and
is suited for problems that exhibit weak to moderate physics coupling.
The fluid-structure interaction (FSI) concept covers a very broad scope of problems in which fluid flow and structural deformation interact and affect one another. The interaction can be mechanical, thermal, or both. FSI applications include hemodynamics in an artery, fluid flow in a pump, airflow over an aircraft wing, heat exchange in a radiator, heat transfer in turbine discs, fluid sloshing in a tank, and hydroplaning of a tire. The use of the co-simulation capability to perform an FSI simulation is illustrated in “Closure of an air-filled door seal,” Section 2.3.1 of the ABAQUS Example Problems Manual.
Figure 7.9.1–1 classifies FSI problems. The complexity of the simulation increases from left to right. At the uppermost level one can distinguish between rigid and flexible structural response problems. Rigid structural response problems are effectively handled by most CFD codes; thus, an ABAQUS co-simulation need be employed only for flexible structures.
In some cases the coupling strength (influence coefficient) in one direction may be so small as to be negligible (e.g., mechanical response influence on a fluid for a small-deformation analysis). These cases permit the use of a sequential “one-way” analysis, where loads are passed from one code to another code but not vice versa.
The ABAQUS co-simulation interface allows for both “one-way” and “two-way” transfer of loads. The structural response may be linear or nonlinear for material and geometric effects. Contact conditions can be included as long as the fluid topology remains constant. Both steady-state and transient simulations are supported. Further complexity arises if the physics are strongly coupled (see “Strength of physics coupling” below).
The ABAQUS co-simulation interface uses the Mesh-based Parallel Code Coupling Interface (MpCCI) middleware developed at the Fraunhofer Institute for Algorithms and Scientific Computing (Fraunhofer SCAI). MpCCI is a general code-coupling interface based on the Message Passing Interface (MPI). MpCCI allows ABAQUS to interface with any third-party analysis code that supports the MpCCI 3.0 interface.
The ABAQUS co-simulation interface uses a client-server architecture with the major software components illustrated in Figure 7.9.1–2. ABAQUS is linked to the MpCCI code plug-in for ABAQUS, which in turn is linked to an MpCCI client. This configuration is available with your normal ABAQUS release. Similarly, the third-party code is linked to an MpCCI code plug-in to the third-party code and to an MpCCI client. During a co-simulation, the clients (analysis codes) establish a connection with the MpCCI server. This connection is via a socket communication and can occur across the network between heterogeneous computer platforms. For example, ABAQUS could be running on a Windows system, the third-party code could be running on a UNIX system, and the MpCCI server on a Linux system. Alternatively, the MpCCI server and the clients can be run on the same workstation. The MpCCI server controls the client codes and handles the communication and data exchange. The MpCCI server also maps solution quantities from the sending mesh to the receiving mesh.
The Coupling Manager and MpCCI Graphical User Interface (GUI) obtain analysis-specific information from the analysis input files, query the user for coupling-specific information, write the MpCCI configuration file, and start the MpCCI server and client codes. An overview of the use of the MpCCI GUI can be found in “Executing the coupled analysis,” Section 7.9.4.
MpCCI introduces the concept of a coupling region, which enables MpCCI to couple analysis codes without knowledge of the codes' simulation algorithms (finite element method, finite volume method, etc.). Each code in a coupled simulation specifies its coupling region based on its own numerical mesh definitions and specifies the physical quantities (such as temperature, heat flux, pressure, displacements, etc.) it can send and/or receive. MpCCI computes the mesh neighborhoods between the coupled codes and interpolates solution quantities from the sender mesh onto the receiver mesh during the simulation. The meshes can be nonconforming, as illustrated in Figure 7.9.1–3.
MpCCI provides conservative and non-conservative mapping schemes to interpolate solution quantities. Conservative mapping schemes preserve the amount of a quantity entering or leaving a region during the interpolation and are necessary for flux quantities, such as heat flux, whose sum must be maintained across the region. Non-conservative interpolation schemes (such as bilinear interpolation for first-order quadrilaterals) are used for quantities that are functions of spatial coordinates and time, such as displacements or temperature, whose sum need not be strictly maintained across a region. The interpolation type is specified in the MpCCI configuration file and can be defined through the MpCCI GUI. Consult the MpCCI User’s Guide for details on the mapping schemes.
In an ABAQUS co-simulation the analysis domains are coupled in a loose manner; that is, the equations for each subdomain are solved separately, and loads and boundary conditions are exchanged only at the domain interface. In mathematical terms the interaction is through the “right-hand side” only, as depicted in Figure 7.9.1–4. The flow equations are solved by a CFD code, and the structural equilibrium equations and heat transfer equations are solved by ABAQUS. Only the right-hand sides at the interface are exchanged during the simulation. This approach is applicable to many problems that exhibit weak to moderate physics coupling.
This approach may not be effective for problems that exhibit strong physics coupling. In such cases it is best to solve the problem with a dedicated analysis code in which the solutions of all subdomains are combined into a single system and solved simultaneously (see Figure 7.9.1–5). Such solution approaches have their own numerical challenges and are not suited for a general-purpose analysis code such as ABAQUS.
Figure 7.9.1–6 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 loose coupled or “staggered” solution approach each subproblem is solved by temporarily ignoring the coupling terms represented by the gray spring and dashpot in Figure 7.9.1–6. When the response frequency and coupling impedance are low, a staggered approach will likely provide adequate solution accuracy and performance. However, when the response frequency is high, such that the coupling impedance is relatively large compared to the structure or fluid, you may encounter solution stability issues with a loose coupling approach. Performing a multidisciplinary analysis using the ABAQUS co-simulation interface involves the following steps:
Preparing the ABAQUS analysis and the third-party code for co-simulation (see “Preparing an ABAQUS analysis for co-simulation,” Section 7.9.2).
Directing the exchange process (see “Directing the exchange process,” Section 7.9.3).
Executing the coupled analysis (see “Executing the coupled analysis,” Section 7.9.4).
For general information about MpCCI, see http://www.scai.fraunhofer.de. For specific information about MpCCI and running coupled simulations, consult the MpCCI User's Guide.
For useful tips on running FSI simulations, check the ABAQUS Answers in the ABAQUS Online Support System (AOSS).
