In many engineering problems, we analyze how a fluid and a solid object affect each other. This study is called Fluid-Structure Interaction (FSI). It is a key concept in modern engineering that helps us understand the complex relationship between a fluid’s flow and a structure’s movement. In an FSI problem, the fluid applies pressure and forces that can cause the structure to move or change shape. Consequently, the structure’s movement changes the path of the fluid flow. This continuous interaction is also known as Fluid Solid Interaction.
A Fluid Structure interaction CFD simulation combines two fields of physics: fluid dynamics and structural mechanics. Instead of assuming that the solid walls are fixed, an FSI simulation calculates both the fluid flow and the structural response together. This approach is necessary when a structure is flexible enough that the forces from the fluid cause it to deform, bend, or vibrate in a significant way. For example, a standard CFD analysis is sufficient for water flowing in a rigid pipe. However, if the pipe is flexible and vibrates due to the flow, we must use a Fluid Structure interaction ANSYS simulation to get accurate results. This method is essential for designing everything from safe bridges that resist wind to efficient artificial heart valves. To see how these principles are put into practice, you can explore our detailed FSI tutorials.
Figure 1: Various applications of Fluid-Structure Interaction (FSI) simulation, from offshore structures and oil tankers to wind turbines and pump impellers.
FSI Modeling Approaches in ANSYS
When performing a Fluid-Structure Interaction ANSYS simulation, it is important to choose the correct modeling approach. ANSYS provides three main methods, each suited for different types of problems. The key is to select the approach that accurately captures the physics without being more complex than necessary. The main modeling approaches are Rigid Body FSI, One-Way FSI, and Two-Way FSI.
The simplest form is Rigid Body FSI. This approach is used when the solid structure moves within the fluid but does not change its shape or deform. The focus is only on the motion of the object. A great example of this is analyzing a floating boat on water. The boat moves up and down (heave) or tilts (pitch and roll) due to waves, but the boat’s hull itself is considered rigid. This is indeed a type of dynamic mesh 6DOF simulation, where the computational grid adapts to the body’s six degrees of freedom. For more information on this powerful technique, you can refer to our dynamic mesh 6DOF tutorials
Figure 2: Rigid Body FSI analysis of a floating boat using the 6DOF dynamic mesh method in ANSYS.
The next approach is One-Way FSI. We use this method when the fluid flow causes the structure to deform, but the deformation is very small and does not significantly affect the fluid flow. In this case, the fluid simulation is run first to calculate the pressure and thermal loads on the structure. Then, these loads are transferred one time to a structural solver to calculate the stress or deformation. The information only goes one way—from the fluid to the structure. This is a common and efficient approach for problems like analyzing stress on a building due to steady wind.
For problems with large structural changes that influence the fluid flow, we must use Two-Way FSI. This is the most complete and computationally intensive FSI simulation in ANSYS Fluent. In this method, the fluid and structural solvers constantly exchange information. The fluid forces deform the structure, and the new shape of the structure then changes the fluid flow. This cycle repeats at each time step, creating a fully coupled simulation. This method is essential for problems like a flag fluttering in the wind, the closing of an artificial heart valve, or the vibration of a flexible aircraft wing.
One-Way FSI Implementation
A One-Way FSI analysis, often called one-way coupling, is a powerful and efficient method for a wide range of engineering applications. The core principle is simple: the fluid flow applies loads to the structure, but the resulting structural deformation is considered too small to change the fluid flow behavior. This allows for a static data transfer of information from the fluid domain to the structural domain. Within the ANSYS ecosystem, there are two main workflows to achieve this: the highly flexible ANSYS Workbench approach and the specialized Intrinsic 1-way module within ANSYS Fluent.
The ANSYS Workbench Workflow
The most common and versatile method for a Fluid solid interaction Fluent simulation is by linking separate analysis systems in ANSYS Workbench. This workflow is powerful because it allows you to use the best features of both the CFD and the Finite Element Analysis (FEA) solvers. The process starts by performing a complete CFD analysis in Fluent to solve for the fluid dynamics. Once the fluid solution has converged, you have a detailed map of all the fluid-induced loads on the structure. These loads can be both thermal and structural, including:
- Pressure (Force Vector)
- Surface Temperature
- Volumetric Temperature
- Heat Transfer Coefficient (HTC)
- Heat Flux
Figure 3: Standard One-Way FSI workflow in ANSYS Workbench, linking Fluent results to ANSYS Mechanical.
The data transfer within Workbench is seamless. You can create a direct link from the Fluent Solution cell to the Mechanical Setup cell, which automatically imports the fluid loads. For more advanced cases, or if your load data comes from a different source, you can use the External Data module. This tool allows you to import load data from text files and apply it to your structural model. Once inside ANSYS Mechanical, you apply these imported fluid forces as boundary conditions to the relevant surfaces. The structural solver then calculates the final stress, strain, and deformation.
Figure 4: Using the External Data module in ANSYS for a One-Way FSI load transfer.
The Intrinsic 1-Way FSI Module in Fluent
For certain problems, ANSYS Fluent offers a more integrated approach: the Intrinsic 1-way module. This technique performs the Fluid-Structure Interaction analysis entirely within a single Fluent session. For this to work, your model must contain both fluid and solid cell zones that share a conformal mesh at their interface. Fluent solves the fluid dynamics first and then uses its built-in FEA solver to compute the structural deformation based on the fluid forces. This intrinsic solver primarily uses a Linear Elasticity model, which aligns perfectly with the small-deformation assumption of one-way FSI.
Figure 5: Enabling the intrinsic One-Way FSI using the Structural Model within ANSYS Fluent.
The primary options for the material model are:
- Linear Elasticity: This is the most common choice for one-way FSI. It assumes a linear relationship between the force applied and the resulting displacement. This model is appropriate only when the stress on the structure is expected to remain below the material’s yield strength, meaning it will return to its original shape.
- Nonlinear Elasticity: This more advanced model is used to simulate large deformations where the geometry changes significantly. It accounts for geometric nonlinearity, using models like the neo-Hookean hyper-elastic formulation. While it handles large displacements, the simulation is still considered “one-way” if these changes do not influence the fluid flow.
It is important to understand that this intrinsic structural model is configured and solved entirely inside the Fluent interface and is not compatible with the standard Workbench system-linking workflow. The choice between the Workbench and intrinsic methods depends on the complexity of the required structural analysis and the user’s preferred workflow.
* Note: A critical technical step in the Workbench workflow is transferring loads between two potentially different meshes. The surface mesh of the fluid model and the structural model rarely match perfectly. To solve this, ANSYS uses robust mapping and interpolation methods. These algorithms intelligently transfer the pressure and thermal data from the nodes of the fluid mesh to the nodes of the solid mesh, ensuring that the total force and energy are conserved. This accurate mapping is vital for a reliable structural analysis in any Fluid Structure interaction ANSYS simulation.
Two-Way FSI with System Coupling
When the interaction between the fluid and solid is strong enough that the structural deformation significantly alters the fluid flow, a high-fidelity Two-Way FSI simulation is necessary. This approach captures the continuous, dynamic feedback loop between the two physics. In the ANSYS ecosystem, this complex co-simulation is managed by the System Coupling module, a powerful orchestrator that controls the data exchange between ANSYS Fluent and ANSYS Mechanical.
Principle of Bidirectional Iterative Coupling
In an ideal world, the fluid and structural equations would be assembled into a single monolithic system and solved simultaneously. However, in practice, it is more effective to use a partitioned approach where specialized solvers for CFD and FEA “talk” to each other. This is precisely what System Coupling facilitates.
The simulation progresses through a continuous, iterative loop that ensures equilibrium is reached at every time step. This bidirectional data exchange is the core of the Fluid-Structure Interaction CFD analysis:
- Fluid Load Calculation: ANSYS Fluent solves the fluid dynamics equations for a single coupling iteration, calculating the pressure and viscous forces on the shared fluid-solid interface.
- Data Transfer (Forces): System Coupling receives the force data from Fluent and accurately maps it onto the mesh of the structural model in ANSYS Mechanical.
- Structural Deformation: ANSYS Mechanical solves for the structural response, calculating the resulting displacements and stresses based on the applied fluid loads.
- Data Transfer (Displacements): System Coupling receives the calculated nodal displacements from Mechanical and maps them back onto the fluid interface mesh in Fluent.
- Fluid Domain Update via Dynamic Mesh: This is a critical step. To account for the new structural position, ANSYS Fluent must physically update its mesh. This is handled by the Dynamic Mesh model, which deforms the fluid mesh to conform to the new boundary position received from System Coupling.
- Convergence Loop: With the updated mesh geometry, Fluent re-solves the fluid flow. This entire loop is called a coupling iteration and is repeated several times within a single time step until the exchanged data (forces and displacements) converges to a stable solution.
Figure 6: Bidirectional data exchange in a Two-Way FSI simulation managed by System Coupling.
The Dynamic Mesh capability in Fluent is the engine that makes Two-Way FSI possible. When System Coupling provides the new boundary positions from the structural analysis, the Dynamic Mesh model updates the fluid volume mesh accordingly. Without this, the fluid solver would be unaware of the structural changes.
The System Coupling option must be explicitly enabled on the moving wall boundaries within the Dynamic Mesh setup in Fluent. This tells Fluent that the motion for this specific zone will be dictated by the displacement data it receives from the coupling service.
Setting Up a Two-Way FSI in ANSYS Workbench
The entire workflow for a Fluid Structure interaction ANSYS co-simulation is managed visually and logically within the Workbench project schematic.
- Project Schematic Setup: The foundation of the analysis is built by dragging the required systems onto the project page: a Fluid Flow (Fluent) system and a Transient Structural system. A System Coupling system is then added, and the fluid and structural systems are linked to it. This creates the necessary connections for data exchange.
Figure 7: A typical Two-Way FSI project schematic in ANSYS Workbench, connecting the fluid and structural solvers through the System Coupling module.
2. Individual Physics Setup: Each solver must be configured with its own physics and must identify the FSI interface.
-
- In ANSYS Mechanical, you define the material properties, apply structural constraints (supports), and create a Named Selection for the surface that interacts with the fluid, identifying it as the “Fluid-Solid Interface”.
- In ANSYS Fluent, you set up the fluid properties and boundary conditions. Most importantly, you enable the Dynamic Mesh model and, for the corresponding “Fluid-Solid Interface” wall, you specify that its motion will be driven by System Coupling. It is a best practice to use the Double Precision solver in Fluent for FSI cases to maintain numerical accuracy.
3. System Coupling Configuration: The System Coupling interface is the master control for the entire co-simulation. Here you define:
-
- Data Transfers: You create the specific data transfers, for example, linking the Force variable from the Fluent interface to the Mechanical interface, and the Displacement variable from Mechanical back to Fluent.
- Analysis Controls: You set the total simulation End Time and the Step Size.
- Convergence Criteria: You define the number of Minimum and Maximum coupling iterations per time step and the convergence targets for the data transfers. The solution will proceed to the next time step only after these targets are met.
Understanding the Three Levels of Iteration
A transient FSI simulation in ANSYS Fluent is computationally intensive because it involves a nested hierarchy of three iteration levels.
Figure 8: The three levels of iterations in a transient Two-Way FSI simulation. The solver and coupling loops must converge for each individual time step.
- Time Steps: The outermost loop, advancing the simulation through physical time from start to finish.
- Coupling Iterations: The loop managed by System Coupling within each time step. It ensures the fluid and solid domains reach equilibrium before moving to the next time step.
- Solver Iterations: The innermost loops. These are the standard iterations performed by Fluent and Mechanical to solve their respective sets of non-linear equations within a single coupling iteration.
This robust, fully-coupled approach is the gold standard for accurately simulating complex FSI phenomena where the fluid-structure interaction is the dominant physical effect. The power of Two-Way FSI with System Coupling allows engineers to tackle some of the most challenging multiphysics problems across various industries. Check for more FSI tutorials provided by CFDLAND.
Figure 9: Applications of Two-Way FSI simulations, including (clockwise from top-left) aeroacoustics of a helical wind turbine, vibration of a column under wave loading, fuel sloshing in a tanker, and the biomechanics of the human eye.
Advanced FSI Configuration
Moving beyond the basic setup, mastering a Two-Way FSI simulation requires a deep understanding of the advanced configuration settings within each solver and the System Coupling module. This section covers the best practices, critical solver settings, and troubleshooting techniques that are essential for achieving a robust, accurate, and converged Fluid Structure interaction ANSYS simulation.
The System Coupling Control Center
The System Coupling interface is the central hub where you define the entire co-simulation procedure. While the individual physics are set up in Fluent and Mechanical, System Coupling controls how they interact. Key settings include:
- Analysis Type: Can be either transient or steady-state.
- Time Control: You define the total End Time and the Time Step Size. It is crucial to understand that these settings override any time step controls specified within ANSYS Fluent or Mechanical.
- Coupling Iterations: You set the Minimum and Maximum number of coupling iterations to be performed within each time step. The simulation will proceed to the next time step only after the data transfers have converged or the maximum iteration count is reached.
- Data Transfers: This is where you explicitly define the data being exchanged (e.g., Force from Fluent to Mechanical, Displacement from Mechanical to Fluent). You can also set convergence targets and relaxation factors for these transfers to stabilize the solution.
Figure 10: The System Coupling user interface, which acts as the central control panel for managing time steps, coupling iterations, and data transfers between the fluid and structural solvers.
Essential Solver Settings for Coupled Analysis
For a successful co-simulation, several settings within the individual solvers must be configured correctly.
- Solver Precision: It is a strong best practice to run the ANSYS Fluent solver in Double Precision for FSI cases. The high sensitivity of the fluid dynamics to small changes in boundary position makes the higher numerical precision essential for stability and accuracy.
- Understanding Force Transfer: The force transferred from Fluent is calculated based on the gauge pressure relative to a Reference Pressure. By default, this reference pressure is 0, so only gauge pressure and viscous forces are sent. For applications with significant ambient or operating pressures (e.g., a subsea pipe), you must adjust the Reference Pressure to transfer the correct absolute pressure load to the structural model. This is a common source of error in advanced FSI simulations.
- Solver Iterations per Coupling Step: The Max Iterations/Time Step setting in Fluent’s Run Calculation panel takes on a new meaning. It now defines the maximum number of CFD solver iterations performed for each coupling iteration, not for the entire time step.
Figure 11: Results of a pump FSI analysis, showing force transfer and resulting deformation in ANSYS Mechanical.
Conclusion
This guide has navigated the essential workflows for modeling Fluid-Structure Interaction within the ANSYS ecosystem. We have covered the spectrum from the efficient One-Way FSI approach for static load transfers to the high-fidelity Two-Way FSI method for fully dynamic, coupled problems. Understanding the roles of the System Coupling module, the necessity of the Dynamic Mesh model, and the best practices for solver configuration are the keys to achieving accurate and robust simulations. Mastering these tools empowers engineers to solve some of the most complex multiphysics challenges, from aerospace flutter to biomechanical flows.
For highly specialized or complex FSI simulations where expert guidance is needed, professional assistance can ensure optimal and timely results. You can order your tailored project to our CFD Experts here.