Fluid–structure interaction (FSI) is investigated in this study for vortex-induced vibration (VIV) of a flexible, backward skewed hydrofoil. An in-house finite element structural solver finite element analysis nonlinear (FEANL) is tightly coupled with the open-source computational fluid dynamics (CFD) library openfoam to simulate the interaction of a flexible hydrofoil with vortical flow structures shed from a large upstream rigid cylinder. To simulate the turbulent flow at a moderate computational cost, hybrid Reynolds-averaged Navier–Stokes–large eddy simulation (RANS–LES) is used. Simulations are first performed to investigate key modeling aspects that include the influence of CFD mesh resolution and topology (structured versus unstructured mesh), time-step size, and turbulence model (delayed-detached-eddy-simulation and $k−ω$ shear stress transport-scale adaptive simulation). Final FSI simulations are then performed and compared against experimental data acquired from the Penn State-ARL 12 in water tunnel at two flow conditions, 2.5 m/s and 3.0 m/s, corresponding to Reynolds numbers of 153,000 and 184,000 (based on the cylinder diameter), respectively. Comparisons of the hydrofoil tip-deflections, reaction forces, and velocity fields (contours and profiles) show reasonable agreement between the tightly coupled FSI simulations and experiments. The primary motivation of this study is to assess the capability of a tightly coupled FSI approach to model such a problem and to provide modeling guidance for future FSI simulations of rotating propellers in crashback (reverse propeller operation).

## Introduction

Fluid–structure interaction (FSI) has gained interest in many fields of engineering, e.g., offshore and inland civil structures, nano and mems devices, biomedical applications, and turbomachinery. In particular, in aerospace and marine applications, use of lightweight and composite materials has been increasing because of their advantages over metallics such as a long life time, higher strength, and reduced weight. However, when lightweight, flexible structures are subject to unsteady fluid flows, the interaction between the fluid and structure can be significant. The amplitude of structural vibration alters the nearby fluid flow and then the fluid response feeds back into the structural vibration. One of the motivations of this study is to improve the modeling capability for flow-induced vibration of rotating propellers in a crashback condition where the propeller operates in the reverse direction and creates a large, recirculating vortical flow. In some of the vortex-induced vibration (VIV) examples, structural vibrations can be as large as the structure’s dimensions [1,2]. Crashback is considered to be one of the most extreme operating conditions experienced by propellers [3,4].

In the past few decades, FSI modeling has been an active area of research with advances in high-performance computing and FSI modeling algorithms. However, the simultaneous analysis of structural dynamics and unsteady fluid flows at high Reynolds numbers (Re) of engineering interest is still challenging. In most cases, simulating a high Re turbulent flow itself requires an enormous amount of computing resources as discussed in Ref. [5], and adding FSI requires even more computing resources and time. Generally, for large, unsteady flow-induced structural deformations, a tightly coupled FSI approach is required in which structural and fluid governing equations are simultaneously satisfied, which can be accomplished by solving iteratively at each time-step until a specified tolerance is met [6]. A tightly coupled FSI approach typically requires far more computing resources than loosely coupled FSI (where the governing equations are not simultaneously satisfied) or computational fluid dynamics (CFD)-only simulations. Due to this difficulty, for example, in VIV research, many of the FSI simulations have used two-dimensional fluid domains [7,8].

Despite the vast amount of interest in FSI, there has not been much validation of FSI simulations for real-world engineering problems, especially where large amplitude structural vibration and high Re turbulent flows are present. This is mainly due to the high computational costs required for simulating a three-dimensional turbulent flow and its interaction with a flexible structure, as discussed in Ref. [9]. Due to this limitation, typical verification and validation practices in the field of FSI modeling have used two-dimensional CFD simulations that involve low Re, laminar flow. The FSI cases of Refs. [10,11] are such cases that model the vibration of a flexible structure induced by two-dimensional, laminar vortex shedding. These studies are widely accepted as “benchmark” FSI cases, which have been used by many investigators to verify their FSI approach.

On the experimental side of FSI, however, an experimental database for such laminar vortex-shedding types of flows is not extensive. This is because an ideal, two-dimensional flow is difficult to realize. However, a few notable experimental studies include [1215]. In particular, the experimental study of Derakhshandeh et al. [15] investigated the response of an elastically mounted airfoil under the influence of the wake of a circular cylinder in a water channel at a Reynolds number of 10,000 (based on cylinder diameter). The effects of various angles of attack and downstream positions of the airfoil were investigated. However, the numerical simulations were limited to a CFD-only simulation focused on predicting the shedding physics in the wake of the circular cylinder.

The overall aim of the present study is to provide one of the first comparisons of computational and experimental results for a high-Reynolds number, three-dimensional FSI case. Specifically, the vibration of a flexible, backward skewed hydrofoil in the wake of a circular cylinder at Reynolds numbers of 153,000 and 184,000 (based on cylinder diameter; see Fig. 1) is investigated. The backward skewed hydrofoil studied here experiences similar highly separated, vortical flow physics as a propeller experiences during crashback (reverse propeller operation) [3,4]. There are two objectives of this study: (1) simulate the fully coupled, time-dependent interaction of the flexible hydrofoil with turbulent vortex shedding using a tightly coupled FSI approach and (2) compare the simulated results with water tunnel experimental data. Given a reasonable comparison, the approach can then be applied in future work to simulate the more complex case of a rotating propeller in crashback.

## Computational Modeling Approach

The fluid is modeled as Newtonian and incompressible and the structure is modeled as an elastic and compressible material with a large deformation strain tensor. The turbulence modeling employed hybrid Reynolds-averaged Navier–Stokes–large-eddy simulation (RANS/LES) models: Delayed detached-eddy simulation (DDES) and $k−ω$ shear stress transport-scale adaptive simulation (SST–SAS) LES is a popular computational approach that resolves turbulent eddies down to the grid size. However, for wall-bounded simulations, the cost of LES increases tremendously compared to that without a wall. LES with wall-layer models [16] and hybrid RANS–LES [1719] allow simulations to be performed at a much more manageable computational cost.

For brevity, details of the fluid and structure mechanics governing equations are omitted here but can be found in Ref. [20]. The open-source finite-volume CFD library openfoam is used to solve the governing fluid dynamics equations. The structural dynamics are solved using an in-house finite element code FEANL developed by Campbell [14]. Specifically, the unsteady, incompressible flow equations were solved using a transient simple algorithm that permits large time-step sizes. This enables faster time marching at the expense of temporal accuracy. Fast time marching is useful especially in the cases where initial transients need to be passed quickly. To maintain stability, however, the algorithm often requires more pressure–velocity correction loops. The details of the transient simple algorithm in openfoam are described by Auvinen et al. [21].

The flow and structural solvers are coupled using a tightly coupled partitioned approach based on a fixed-point iteration as illustrated in Fig. 2. In this approach, the fluid and structure systems of equations are solved iteratively until a specified convergence tolerance is satisfied. The convergence criterion, ϵ, was set to a value between 0.001 and 0.01 based on previous validation studies [9]. For convergence, approximately 8–10 subiterations were required for the simulations reported herein (see Ref. [20] for more details).

Second-order accurate spatial and temporal discretization schemes were used in the CFD simulations. For the pressure–velocity coupling, the aforementioned transient simple solver was employed, where between 15 and 20 corrector loops were used to achieve iterative convergence at each time-step. A preconditioned conjugate gradient (PCG) solver with a geometric-algebraic multigrid (GAMG) preconditioner was used to solve the pressure equation, and a preconditioned bi-conjugate gradient (PBiCG) solver was used for the other solution matrices.

## Geometry and Computational Mesh

### Test Configuration.

The test configuration in the Penn State Applied Research Laboratory (ARL) 12 in water tunnel is shown in Fig. 1. A circular cylinder (60 mm diameter) is mounted in the test section inlet and a hydrofoil is positioned 3.42 cylinder diameters downstream in the turbulent wake of the cylinder. This induces moderate-amplitude structural vibrations of the hydrofoil due to shedding vortices from the upstream cylinder. In this test configuration, the vortex-shedding due to the upstream cylinder is dominant over the trailing-edge vortex shedding from the hydrofoil, which was confirmed in the water tunnel experiment by performing a test without an upstream cylinder [22]. Note that the hydrofoil is intentionally designed to have a backward-skewed shape with a −10 deg angle of attack to mimic propeller crashback conditions.

### Fluid.

The computational domain of the fluid is shown in Fig. 1. The domain comprises the water tunnel contraction, test section, and diffuser. On every surface in the domain, i.e., the cylinder, hydrofoil, and tunnel walls, a viscous sublayer-resolved grid was generated with a y+ value < 1 for the highest tunnel flow speed of approximately 5 m/s. See Ref. [23] for the definition of y+.

Unstructured and structured CFD meshes for the flow domain were generated using the commercial software pointwise. Varying mesh densities were generated for a mesh convergence study. The meshes used in this work are summarized in Table 1. All of the meshes have viscous sublayer resolution on the hydrofoil and cylinder, except the 3.9 M cell structured mesh where wall functions were used with y+ greater than 30. The 3.9 M cell mesh is considered to be too coarse for an LES or DES simulation given the range of Reynolds numbers of interest for this work. However, the coarse mesh was mainly used for testing purposes and to perform preliminary FSI simulations. More accurate FSI results are obtained using a much finer structured fluid mesh with 15 M cells. For additional details on the CFD mesh generation and resolution, see Ref. [20].

### Structure.

The hydrofoil is made of Inconel 718 and the load cell is made of berillium copper. The hydrofoil has a chord length of 50 mm and a span of 230 mm. The angle-of-attack of the hydrofoil is fixed at −10 deg. The first 115 mm of the span is straight, and then, from the midspan to the tip, the hydrofoil is swept forward (see Fig. 1). The hydrofoil cross section has a NACA 4408 profile. On the straight section of the fin span, the fin cross section is gradually reduced from a chord length of 50 mm to a minimum of 35 mm at about 57.5 mm from the hydrofoil base. This was done to induce larger deflections at the hydrofoil tip. More details of the hydrofoil can be found in Ref. [22].

Figure 3 shows the structural finite element (FE) model of the hydrofoil attached to the load cell. The FE model employs quadratic solid elements and has a high mesh density near the region where strain gages were placed in the experiment. A fixed boundary condition is applied to the root of the load cell (bottom-most surface in the figure). The first bending mode shape of the hydrofoil model is at 35.7 Hz in vacuo, which is slightly higher than the first resonance frequency at 32.7 Hz obtained from experimental modal testing in air. The in-water first resonance frequency of the hydrofoil FE model, which was obtained by performing a numerical pluck test in quiescent water (see Ref. [20] for additional information), is at 24.4 $Hz$ and the experimental value is 23.2 $Hz$. Based on how well the in-water fundamental resonance frequencies agree between the FE model and experimental data, the hydrofoil/load cell FE model with a fixed boundary condition appears to represent the physical boundary condition of the experiment reasonably well. It is important to note that the hydrofoil’s first in-water resonance frequency is relatively close to the vortex shedding frequency from the cylinder that varies between 10 and 16 Hz, depending on the flow speed in the water tunnel experiment. This range of frequencies (or flow speeds) was chosen in the water tunnel experiment to provide significant excitation but to be far enough away from the fundamental resonance frequency to avoid lock-in.

### Fluid Mesh Motion.

In the FSI simulation, the fluid mesh has to move in response to the structure’s motion. Therefore, FSI problems involve three components that must be solved: fluid dynamics, structural dynamics, and fluid mesh motion. Depending on the size of a fluid mesh, moving all of the fluid vertices in each simulation time-step can be costly. To reduce the computational overhead, only the fluid vertices in the vicinity of the hydrofoil defined by the region in Fig. 4 are taken into account, and mesh motion is solved using an overlay mesh motion approach developed by Campbell [14]. As shown in Fig. 4, the overlay model is located inside the test section and the bottom surface of the overlay model is aligned with the bottom surface of the fluid mesh. Below the water tunnel liner, the load cell is located outside of the fluid domain. Note that, in the water tunnel experiment, fluid enters into the load cell housing through a small gap, which is present to avoid any contact between the load cell and liner. The fluid in this gap was not modeled in the present study.

## High-Performance Computing

Most of the computations in this work were performed on the Spirit high-performance computing (HPC) system maintained by the U.S. Air Force Research Laboratory DoD Supercomputing Resource Center. Spirit has 4590 compute nodes, each with 16 Intel E5 Sandy Bridge cores and 32 GB of memory. All nodes are connected by FDR 14x Infiniband. An initial FSI simulation (3.9 M cells) was performed on the Lion-XF cluster maintained by Penn State’s Research Computing and Cyber-Infrastructure (RCC) department. Lion-XF has 184 nodes, each with Intel Xeon 3.06 GHz X5674 Westmere-EP processors and 48 GB of memory. All nodes are connected by a quad-data rate (QDR) Infiniband interconnect capable of throughput in excess of 32 GB/s. On the Spirit HPC system, for CFD-only and FSI computations, up to 800 cores were used, whereas the initial FSI simulation with the 3.9 M cell mesh was run on Lion-XF using 32 cores.

## Results and Discussion: Computational Fluid Dynamics

### Turbulence Model Comparison.

CFD-only simulations were performed using the unstructured coarse mesh (20 M cells) to evaluate the two different turbulence models: DDES and $k−ω$ SST–SAS. The performance of each turbulence model is compared based on the following metrics: fluid forces on the structure and resolved turbulence in the wake. The hydrofoil is modeled as rigid in these simulations which, therefore, do not take into account FSI effects. The tunnel flow speed in the test section is $UTunnel=2.5 m/s$, which is an intermediate flow speed among the flow speeds used in the water tunnel experiment. At this flow speed, the Reynolds numbers based on the cylinder diameter, D = 60 mm, and the hydrofoil chord length, $c=$ 50 mm, are approximately $ReD=$ 153,000 and $Rec=$ 128,000, respectively.

A qualitative comparison of the instantaneous flow fields is shown in Fig. 5, which demonstrates that the resolved turbulence in both the DDES and $k−ω$ SST–SAS simulations is comparable. Quantitatively, Fig. 6 shows the time histories of the forces on the cylinder (CD—drag coefficient and CL—lift coefficient) obtained from DDES and $k−ω$ SST–SAS. Figure 7 shows the time histories of the force predictions on the hydrofoil: Fx and Fy are the drag and lift forces on the hydrofoil, respectively.

The quantitative statistics of the force coefficients on the cylinder and the forces on the hydrofoil are summarized in Table 2. The shedding frequency is inferred from the lift force on the hydrofoil and the Strouhal number is based on the cylinder diameter. Based on published experimental data for vortex shedding from cylinders in an open environment, the Strouhal number at around $ReD$  = 153,000 varies between 0.17 (rough surface) and 0.27 (smooth surface) [24]. The Strouhal numbers predicted here, 0.314 from delayed-DES and 0.324 from $k−ω$ SST–SAS, are much higher than the values reported in Ref. [24]. However, the present case is not in an open environment, and there are significant blockage effects due to the close proximity of the tunnel walls. Further, considering the drag coefficient, CD, at Reynolds numbers ($ReD$) of about $1×105$ to $1×106$, the flow is in the critical regime and the drag coefficient can vary between 0.3 and 1.2 [25]. The predicted drag coefficients using DDES and $k−ω$ SST–SAS are within this range. Based on published open-environment data, the empirical lift coefficient is in the 0.1 range at these Reynolds numbers [26], which is close to the results predicted herein.

The two models show similar predictions of shedding frequency and drag on both the cylinder and hydrofoil. However, the RMS lift predictions on both the cylinder and hydrofoil are higher for DDES compared to $k−ω$ SST–SAS. This is also apparent from the force time histories shown in Fig. 7. Thus, for this case, the DDES model appears to better preserve the turbulent vortex shedding energy downstream of the cylinder. Because of this and the authors’ previous experience with simulating flow past a circular cylinder using DDES [9], the DDES model was chosen for the remaining CFD and FSI simulations.

### Mesh Convergence Study.

Figures 8 and 9 show visualizations of the instantaneous flow field for the different meshes using DDES. The inlet flow speed in the water tunnel test section is consistent in all of the cases, $UTunnel=2.5 m/s$. Qualitatively, small-scale flow structures are much better resolved by the structured meshes compared to the unstructured meshes as indicated by the presence of much smaller scale turbulent eddies in Fig. 9 compared with Fig. 8. Even in the 3.9 M cell structured mesh simulation, in which the mesh resolution is significantly coarser than the 20 M and 40 M cell unstructured meshes, turbulence in the wake appears to be better resolved.

The differences in the flow fields between structured and unstructured meshes become more obvious when the time-averaged flow fields are inspected, as shown in Figs. 10 and 11. Note that, although the duration of time-averaging, $ΔT$, varies between the cases, the time-averaging is long enough in each case to establish representative mean velocity fields for comparison between the cases. The extent of the wake velocity deficit downstream of the cylinder is much larger for the structured meshes compared with the unstructured meshes (Figs. 11 and 10, respectively). Inspecting the unstructured mesh wake velocity deficit in Fig. 10, it appears as though the wake prematurely dissipates relative to the structured meshes. This is due to the larger numerical dissipation inherent with the use of unstructured meshes and the finite volume method relative to structured meshes that are more orthogonal and aligned with the flow direction. As a result, we see that even the 3.9 M cell structured mesh appears to be less dissipative than the 40 M cell unstructured mesh.

Table 3 summarizes the results of the force predictions on the hydrofoil for the various mesh configurations evaluated. Note that the hydrodynamic force on the hydrofoil is very important, since this, in particular the RMS lift force, is what induces structural vibration in the FSI simulations. The mean drag force predictions from the 20 M and 40 M cell unstructured mesh cases are 5.36 N and 5.35 N, respectively, which are about three times higher than those of the 10 M and 15 M cell structured mesh cases. The hydrofoil force predictions for the unstructured and structured mesh cases vary because of the differences in the resolved velocity in the cylinder wake between the two mesh types. Specifically, because the cylinder wake is dissipated more quickly in the unstructured mesh cases, the mean drag and lift are higher due to a higher effective freestream velocity. Further, because the turbulent vortex shedding downstream of the cylinder is better resolved by the structured mesh, the RMS lift force is larger for the structured mesh cases. Note that, except for the 20 M cell unstructured mesh (which is the most dissipative case), there is little difference in the shedding frequency. Based on these results, subsequent CFD and FSI simulations employ the 15 M cell structured mesh.

### Time-Step Study.

For time-accurate hybrid RANS/LES or LES predictions, it is important to satisfy the Courant–Friedrichs–Lewy (CFL) condition, especially in the regions of high unsteadiness. The CFL number is the ratio of the distance that the flow (having a velocity magnitude V) is transported within a time-step, $Δt$, to the cell size, $Δx$, and is given by
$CFL=VΔtΔx$
(1)

If CFL is below one, the flow travels less than the cell size during $Δt$. Hence, for time-accurate simulations of small-scale unsteadiness, $CFL<1$ or smaller is desirable. As a general rule of thumb, it is recommended for large-eddy simulations to maintain a CFL around 0.5. In the previous section on mesh convergence (see Mesh Convergence Study section), all of the cases utilized a time-step size, $Δt=0.1 ms$, targeting a CFL of around 0.5 in the wake of the cylinder.

A time-step size of $Δt=0.1 ms$ used in the foregoing simulations for the comparison of turbulence models and mesh convergence is affordable for the CFD-only simulations. However, such small time-steps are prohibitive for FSI simulations. The tightly-coupled FSI algorithm employed in this work requires about 8–10 times longer computational times compared to a CFD-only simulation [9]. Because of this, larger time-steps are preferred for FSI simulations.

Table 4 shows the results of the CFD-only simulations using three different time-step sizes: 0.1 ms, 0.5 ms, and 1 ms. Using Richardson extrapolation [27], the temporal discretization error in the computed RMS lift force on the hydrofoil was estimated to quantify the influence of time-step size on the numerical accuracy of the solution (see Ref. [20] for details). The error estimates for RMS lift on the hydrofoil from the fine (0.1 ms) and medium (0.5 ms) time-step solutions are 0.30% and 5.16%, respectively. Therefore, although the simulation is not purely a “large-eddy simulation” in some regions of the flow where CFL > 1, using the medium time-step size (0.5 ms) significantly reduces the computational expense, thereby facilitating tightly coupled FSI, while still resolving the forces on the hydrofoil with reasonable accuracy.

In summary, the mesh convergence study demonstrated that the 15 M cell structured mesh yields relatively mesh-insensitive predictions of force on the hydrofoil. Using the 15 M cell structured mesh, the time-step study showed that reasonably accurate hydrofoil force predictions can be obtained using a time-step size of 0.5 ms. Accordingly, the 15 M cell structured CFD mesh and a time-step size of 0.5 ms were used in subsequent FSI simulations.

## Results and Discussion: Fluid–Structure Interaction Simulations

Fluid–structure interaction simulations were performed at two different flow speeds, 2.5 m/s and 3.0 m/s, which are within the range of flow speeds tested in the water tunnel, 2.5 m/s to 3.4 m/s [22]. At these flow speeds simulated, the Reynolds numbers based on the cylinder diameter are approximately 153,000 and 184,000, respectively. The Reynolds numbers based on the hydrofoil chord length are approximately 128,000 and 153,000, respectively.

Figure 12 shows contours of the predicted instantaneous velocity field in the tunnel for $UTunnel$  = 3.0 m/s along with contours of von Mises stress on the hydrofoil surface. In the contraction section of the tunnel (upstream of the cylinder), the flow accelerates as it approaches the cylinder. Downstream of the cylinder, the flow is characterized by unsteady vortex shedding, which buffets the hydrofoil and causes it to vibrate. The contours of von Mises stress show large values within the load cell and near the hydrofoil root.

The time-averaged velocity fields are shown in Fig. 13, which confirm the bulk tunnel flow speed in the test section for each simulation ($UTunnel=$ 2.5 m/s and 3.0 m/s). The flow fields are time-averaged for approximately 2.4 s of physical time. As shown by the velocity magnitude scale, the top panel of Fig. 13 indicates a maximum time-averaged velocity magnitude of 2.52 m/s and the bottom panel indicates a 3.00 m/s velocity magnitude, which are consistent with the desired flow speeds in the tunnel test section for the FSI simulations.

Figure 14 shows time-histories of the applied fluid force integrated over the hydrofoil (wetted) surface at $UTunnel$  = 2.5 m/s and 3.0 m/s. The lift force acts in the y-direction (cross-stream) and the drag force in the x-direction (streamwise). As shown by the time-histories, the applied fluid force is strongly periodic and shows a beating-like amplitude modulation that is typically seen in vortex-induced vibration [28]. As the tunnel flow speed increases from 2.5 m/s to 3.0 m/s, both the amplitude and shedding frequency of the applied fluid force increase significantly. At 2.5 m/s, the RMS lift force is 11.4 N, and at 3.0 m/s, the RMS lift force is 16.4 N. The flow shedding frequency, fs, is 14.43 Hz at 2.5 m/s and 19.01 Hz at 3.0 m/s. Based on these results, the shedding frequency increases by 32% and the RMS lift force by 44%, when the tunnel flow speed increases by 20%. Therefore, the shedding frequency roughly scales as expected, with flow speed to the first power, $fs∝U$, and the lift force scales with the flow speed to the second power, $L∝U2$.

Figure 15 shows time histories of the hydrofoil tip deflection at the two tunnel flow speeds. Note that the tip deflection is in the direction of lift. The hydrofoil chord length is 50 mm. The maximum deflection amplitude is about 8% of the chord length at 2.5 m/s and 12% of the chord length at 3.0 m/s. The hydrofoil is excited by the unsteady fluid force at the cylinder shedding frequency. As the tunnel flow speed increases from 2.5 m/s to 3.0 m/s, the amplitude of the tip deflection increases significantly in conjunction with the fluid lift force increase. Statistics of the deflection time histories are provided in Table 5.

Figure 16 shows the reaction force at the root of the hydrofoil as obtained by the load cell. Note that these reaction forces are similar to the lift and drag forces but differ due to the dynamic excitation of the hydrofoil. In the water tunnel experiment, the load cell is instrumented with strain gages to measure reaction forces. To compare with experimental data (see Comparisons with Experimental Data section), time histories of the reaction forces at the load cell are calculated from the FSI simulations at both tunnel flow speeds (2.5 m/s and 3.0 m/s).

Statistics of the computed time histories of the applied fluid force, tip deflection and reaction force are provided in Table 5. The statistics were calculated from the time histories acquired up to about 2.4 s of simulated physical time at $UTunnel=$ 2.5 m/s and about 2.5 s at $UTunnel$ = 3.0 m/s. As briefly discussed above, the shedding in the wake becomes more energetic as the flow speed increases. Hence, increasing the tunnel flow speed from 2.5 m/s to 3.0 m/s results in a larger tip deflection, applied force, and reaction force. It is important to note that the applied and reaction forces increase in a roughly consistent manner.

The frequencies of the applied lift, reaction lift and tip deflection are all consistent at each flow speed. Since the hydrofoil response is excited by vortex shedding from the upstream cylinder, it is expected that the frequencies of the reaction force and tip deflection should match the frequency content of the driving fluid force. At 2.5 m/s, the reaction force and tip deflection have strong content at 14.4 Hz, and at 3.0 m/s, they have strong content at 19.0 Hz. For comparison, the fundamental in-water resonance frequency of the hydrofoil from experimental modal testing is 23.2 Hz. Therefore, the ratios between the flow shedding frequency (driving frequency) and the fundamental in-water resonance frequency are 0.62 at 2.5 m/s and 0.82 at 3.0 m/s. The resonance and shedding frequencies are close enough to provide significant excitation, but far enough away to avoid lock-in.

## Comparisons With Experimental Data

The tightly coupled FSI calculations were conducted at tunnel flow speeds of 2.5 m/s and 3.0 m/s. However, in comparing with experimental data acquired in the water tunnel [22], the authors discovered that there is uncertainty in the flow speed measurements made in the experiments using static pressure probes (see Fig. 17). Unfortunately, the FSI simulations had completed and could not be rerun to exactly match the water tunnel flow speeds. Thus, we used CFD to develop correction factors between the measured and the actual bulk flow speed in the test section of the water tunnel during the experiments (see Ref. [20] for detailed discussion) and then selected the closest flow speeds for comparison with our FSI simulations. The flow speeds available for comparison, after correction factors were applied, are UTunnel = 1.86, 2.30, 2.56, 2.65, and 2.83 m/s for flow field measurements and UTunnel = 2.26 and 2.68 m/s for structural response measurements. In the following, comparisons of experimental and simulation results are made for similar, but not identical, run conditions to facilitate a qualitative and semiquantitative validation of the FSI simulations.

### Time-Averaged Flow Field.

In the water tunnel experiments [22], PIV was used to obtain instantaneous two-dimensional velocity field measurements at flow speeds of 1.86, 2.30, 2.56, 2.65, and 2.83 m/s. The PIV plane was located at z = 0.188 m (see Fig. 1 for coordinate system and origin) in the dashed box shown in the bottom panel of Fig. 17. Figure 18 shows contour plots of the time-averaged streamwise (x-direction) velocity field from the FSI simulation and PIV data. The x- and y-coordinates are scaled by the cylinder diameter, D, and the x-coordinate is offset by XC (center of the cylinder). Overall, the x-component mean velocity field in the FSI simulation shows relatively good agreement with the PIV data. The wake-deficit, where the streamwise velocity is close to zero downstream of the cylinder, is slightly under-predicted in the numerical results, but, otherwise agrees favorably with the PIV data.

Figure 19 shows contour plots of the RMS of the fluctuating velocity component in the cross-stream, or y, direction. Again, the FSI simulation and PIV data show favorable agreement, though the FSI simulation slightly under predicts the spatial extent of the region of large cross-stream velocity fluctuations in the cylinder wake. Note that the fluctuating component in the cross-stream direction is related to the vortex-induced vibration of the hydrofoil.

### Wake Velocity Profiles.

In the water tunnel experiment [22], laser Doppler velocimetry (LDV) was also used to acquire velocity profiles across the tunnel test section at various downstream locations. Figure 20 shows comparisons of the streamwise velocity profiles between the FSI simulation and LDV at distances of 1.3, 2, 2.7, and 3.3 diameters downstream of the cylinder center, XC. For comparison with LDV, the velocity profiles from the FSI simulation are normalized by UTunnel =  $3.0 m/s$. The normalized velocity profiles from LDV are the average results from all flow conditions: UTunnel = 1.86, 2.30, 2.56, 2.65, and 2.83 $m/s$. The profile shapes and velocity magnitudes agree relatively well at 1.3D, 2D, and 2.7D. At 3.3D downstream of the cylinder, however, the FSI simulation is seen to slightly under predict the wake deficit compared with the LDV data.

Figure 21 shows the fluctuating component of the cross-stream (y-direction) velocity at the same downstream locations. The cross-stream component is associated with the lift force that excites the hydrofoil vibration. Overall, the cross-stream fluctuating velocity profiles agree relatively well between the numerical results and experimental data.

### Hydrofoil Tip Displacement.

Figures 22 and 23 show the time histories of the tip displacement from the FSI simulations and the water tunnel experiments [22], respectively. The FSI simulations are performed at two tunnel flow speeds: UTunnel = 2.5 m/s and 3.0 m/s. In the water tunnel experiment, tip deflection data were acquired using a high-speed camera and laser vibrometer at various flow conditions. The two closest flow speeds that are selected from the experimental data for comparison are UTunnel = 2.26 m/s and 2.68 m/s. Although a rigorous comparison is difficult due to the difference in flow speeds between the FSI simulations and experiments, the results appear to be fairly consistent. As shown in Figs. 22 and 23, as the flow speed increases, the mean deflection, RMS deflection, and shedding frequency increase proportionally.

### Lift and Drag Forces.

In the water tunnel test [22], the lift and drag forces were measured using a load cell instrumented with strain gages, and data were acquired at various flow conditions. Figures 24 and 25 show the time histories of the computed and measured forces from the FSI simulations and experiments, respectively. Although the flow speeds are higher in the FSI simulation, the lift and drag forces from the FSI simulations are somewhat under-predicted. This may be due to numerical dissipation. From the mesh and time-step convergence studies, the “fine” structured mesh was chosen with a reasonably accurate time-step size. However, it may be that even the 15 M cell structured mesh does not sufficiently preserve the wake and shed vortices all the way downstream to the hydrofoil. Even so, the lift force predictions from the FSI simulations are in the same range as the experiments, which is reasonable given the complexity of the problem.

## Study Limitations

The primary limitation of this study is the lack of correspondence between the simulated and experimental flow speeds. Due to limitations in the experimental setup, there is uncertainty in the flow speed at which the experimental measurements were acquired. This precludes a rigorous quantitative comparison between the FSI simulations and experimental data at the same flow speed. Even so, to leverage the experimental data and permit a qualitative and semiquantitative comparison, experiments having the closest flow speeds to the FSI simulations were selected for comparison. Though not ideal, this study provides one of the first comparisons between computational simulations and experiments of a three-dimensional, high-Reynolds number FSI case. Overall, the FSI simulations and experiments compare reasonably well in a qualitative and semiquantitative fashion.

A secondary limitation of the present study is the inability to perform tightly coupled FSI simulations for an extended amount of physical time (more than approximately 2.5 s) to achieve complete statistical convergence of some flow quantities (e.g., cross-stream fluctuating velocity). The present FSI simulations were extremely computationally expensive. For example, a single FSI simulation using the 15 M cell structured mesh required approximately 500,000 central processing unit (CPU) hours to simulate 2.5 s of physical time (about 40 vortex shedding cycles). The 15 M cell FSI case employed about 800 CPU cores, and therefore, it took approximately 625 wall clock hours (26 days) to simulate 2.5 s of physical time. For comparison, the flow field measurements (PIV and LDV data) were time-averaged over several minutes. This practical constraint limited the number of FSI cycles over which time-averaging could be performed and may be the cause for some asymmetry in the fluctuating cross-stream velocity due to a lack of complete statistical convergence.

## Conclusions

Tightly coupled FSI simulations were performed to investigate the interaction of a hydrofoil and vortices shed from an upstream cylinder placed in the Penn State ARL 12 in water tunnel at Reynolds numbers of 153,000 and 184,000 (based on the cylinder diameter). First, two hybrid RANS–LES turbulence models, delayed-DES and $k−ω$ SST–SAS, were studied to evaluate their capabilities to simulate highly separated, bluff-body turbulent flows past a circular cylinder. CFD simulations were performed with 20 M and 40 M cell unstructured meshes, and 3.9 M, 10 M, and 15 M cell structured meshes. Based on the RMS lift force predictions, DDES CFD simulations appeared to better resolve the energy-containing vortices shed from the cylinder compared with $k−ω$ SST–SAS. Small-scale eddies in the wake were shown to be better resolved with the structured meshes than the unstructured meshes. In the subsequent FSI simulations, therefore, delayed-DES with a 15 M cell structured mesh was used.

Fluid–structure interaction simulations of a flexible hydrofoil were performed using an FSI solver that tightly couples the in-house finite element structural dynamics solver FEANL and openfoam. The results of FSI simulations at two flow speeds (2.5 m/s and 3.0 m/s) were compared against water tunnel experimental data at the closest flow speeds available. Despite some uncertainty in the experimental flow speeds and the need to correct experimental bulk flow speed estimates using CFD, overall the FSI simulations and experiments agree reasonably well. The tip deflection of the hydrofoil from the FSI simulations and experimental laser-vibrometer data show reasonable agreement in terms of mean and RMS displacements. The mean and RMS values of the reaction forces at the hydrofoil load cell show fair agreement between the FSI simulations and experiments, with some discrepancy that is likely attributable to numerical dissipation and the difficulty of completely resolving the turbulent wake, the entire distance between the upstream cylinder and the downstream hydrofoil.

In summary, despite some limitations, the comparisons presented herein demonstrate reasonable agreement between experiments and tightly coupled FSI simulations of three-dimensional turbulent vortex shedding from an upstream cylinder interacting with a flexible hydrofoil. For more accurate predictions of the hydrofoil deflection and lift/drag forces, FSI simulations using an even finer mesh and a smaller time-step size will be necessary.

## Acknowledgment

This work was funded by Naval Sea Systems Command (NAVSEA). The authors thank the following organizations for computing resources: Air Force Research Laboratory–DoD Supercomputing Resource Center (AFRL-DSRC) and the Research Computing Cyber-Infrastructure (RCC) at Penn State University.

## References

References
1.
Feng
,
C.
,
1968
, “
The Measurement of Vortex Induced Effects in Flow Past Stationary and Oscillating Circular and D-Section Cylinders
,”
Master's thesis
, University of British Columbia, Vancouver, BC, Canada.
2.
Gabbai
,
R.
, and
Benaroya
,
H.
,
2005
, “
An Overview of Modeling and Experiments of Vortex-Induced Vibration of Circular Cylinders
,”
J. Sound Vib.
,
282
(
3
), pp.
575
616
.
3.
Jessup
,
S.
,
Fry
,
D.
, and
Donnelly
,
M.
,
2006
, “
Unsteady Propeller Performance in Crashback Conditions With and Without a Duct
,”
26th Symposium on Naval Hydrodynamics
, Rome, Italy, Sept. 17–22.
4.
Vyšohlíd
,
M.
, and
Mahesh
,
K.
,
2006
, “
Large Eddy Simulation of Crashback in Marine Propellers
,”
26th Symposium on Naval Hydrodynamics
, Rome, Italy, Sept. 17–22, Vol.
9
, pp.
237
261
.
5.
Spalart
,
P. R.
,
Jou
,
W.-H.
,
Strelets
,
M.
, and
Almiaras
,
S. R.
,
1997
, “
Comments on the Feasibility of LES for Wings and on a Hybrid RANS–LES Approach
,” 1st
AFOSR
International Conference on DNS/LES, Ruston, LA, Aug. 4–8, pp. 137–147.
6.
Campbell
,
R.
, and
Paterson
,
E.
,
2011
, “
Fluid–Structure Interaction Analysis of Flexible Turbomachinery
,”
J. Fluids Struct.
,
27
(
8
), pp.
1376
1391
.
7.
Wanderley
,
J. B.
,
Souza
,
G. H.
,
Sphaier
,
S. H.
, and
Levi
,
C.
,
2008
, “
Vortex-Induced Vibration of an Elastically Mounted Circular Cylinder Using an Upwind TVD Two-Dimensional Numerical Scheme
,”
Ocean Eng.
,
35
(
14
), pp.
1533
1544
.
8.
Zhao
,
M.
,
Cheng
,
L.
, and
An
,
H.
,
2012
, “
Numerical Investigation of Vortex-Induced Vibration of a Circular Cylinder in Transverse Direction in Oscillatory Flow
,”
Ocean Eng.
,
41
, pp.
39
52
.
9.
Lee
,
A. H.
,
Campbell
,
R. L.
, and
Hambric
,
S. A.
,
2014
, “
Coupled Delayed-Detached-Eddy Simulation and Structural Vibration of a Self-Oscillating Cylinder Due to Vortex-Shedding
,”
J. Fluids Struct.
,
48
, pp.
216
234
.
10.
Turek
,
S.
, and
Hron
,
J.
,
2006
, “
Proposal for Numerical Benchmarking of Fluid-Structure Interaction Between an Elastic Object and Laminar Incompressible Flow
,”
Lecture Notes in Computational Science and Engineering
, Vol.
53
, Springer, Berlin, p.
371
.
11.
Dettmer
,
W.
, and
Perić
,
D.
,
2006
, “
A Computational Framework for Fluid–Structure Interaction: Finite Element Formulation and Applications
,”
Comput. Methods Appl. Mech. Eng.
,
195
(
41
), pp.
5754
5779
.
12.
Andrinopoulos
,
N.
,
2009
, “
Development of a Test Facility for Experimental Investigation of Fluid-Structure Interaction
,”
Licentiate thesis
, Department of Energy Technology, Division of Heat and Power Technology, Royal Institute of Technology, Stockholm, Sweden.
13.
Lienhart
,
H.
, and
Gomes
,
J. P.
,
2006
, “
Experimental Study on a Two-Dimensional Fluid-Structure Interaction Reference Test Case
,”
European Conference on Computational Fluid Dynamics
(
ECCOMAS CFD
), Delft University of Technology, Egmond aan Zee, The Netherlands, Sept. 5–8.
14.
Campbell
,
R. L.
,
2010
, “
Fluid–Structure Interaction and Inverse Design Simulations for Flexible Turbomachinery
,”
Ph.D. thesis
, The Pennsylvania State University, State College, PA.
15.
Derakhshandeh
,
J.
,
Arjomandi
,
M.
,
Dally
,
B.
, and
Cazzolato
,
B.
,
2016
, “
Flow-Induced Vibration of an Elastically Mounted Airfoil Under the Influence of the Wake of a Circular Cylinder
,”
Exp. Therm. Fluid Sci.
,
74
, pp.
58
72
.
16.
Piomelli
,
U.
, and
Balaras
,
E.
,
2002
, “
Wall-Layer Models for Large-Eddy Simulations
,”
Annu. Rev. Fluid Mech.
,
34
(
1
), pp.
349
374
.
17.
Spalart
,
P. R.
,
Deck
,
S.
,
Shur
,
M.
,
Squires
,
K.
,
Strelets
,
M. K.
, and
Travin
,
A.
,
2006
, “
A New Version of Detached-Eddy Simulation, Resistant to Ambiguous Grid Densities
,”
Theor. Comput. Fluid Dyn.
,
20
(
3
), pp.
181
195
.
18.
Menter
,
F. R.
,
Kuntz
,
M.
, and
Bender
,
R.
,
2003
, “
A Scale-Adaptive Simulation Model Using Two-Equation Models
,”
AIAA
Paper No. 2005-1095.
19.
Menter
,
F.
, and
Egorov
,
Y.
,
2005
, “
A Scale Adaptive Simulation Model for Turbulent Flow Prediction
,”
AIAA
Paper No. 2003-767.
20.
Lee
,
A. H.
,
2015
, “
Fluid-Structure Interaction of Large Amplitude Structure Vibrations and Moderately High Reynolds Number Turbulent Flows
,”
Ph.D. thesis
, The Pennsylvania State University, State College, PA.
21.
Auvinen
,
M.
,
Ala-Juusela
,
J.
,
Pedersen
,
N.
, and
Siikonen
,
T.
,
2010
, “
Time-Accurate Turbomachinery Simulations With Open-Source CFD; Flow Analysis of a Single-Channel Pump With OpenFOAM
,”
Fifth European Conference on Computational Fluid Dynamics
(
ECCOMAS CFD
), Lisbon, Portugal, June 14–17.
22.
Elbing
,
B. R.
,
Young
,
S. D.
,
Campbell
,
R. L.
,
Jonson
,
M. L.
,
Craven
,
B. A.
,
Kunz
,
R. F.
, and
Koudela
,
K. L.
,
2014
, “
Hybrid Multi-Material Rotor (HMMR) Phase 2: A Low-Frequency, High Amplitude Hydrodynamic Fluid-Structure-Interaction Experiment
,” Pennsylvania State University, State College, PA, ARL Technical Report No. TR 13-004.
23.
Kundu
,
P.
,
Cohen
,
L.
, and
Dowling
,
D.
,
2012
,
Fluid Mechanics
, 5th ed.,
, Cambridge, MA.
24.
Blevins
,
R. D.
,
1977
,
Flow-Induced Vibration
, Vol.
1
,
Van Nostrand Reinhold
,
New York
, p.
377
.
25.
Zdravkovich
,
M.
,
1997
,
Flow Around Circular Cylinders, Volume 1: Fundamentals
,
Oxford University Press
,
Oxford, UK
, p.
185
.
26.
Norberg
,
C.
,
2003
, “
Fluctuating Lift on a Circular Cylinder: Review and New Measurements
,”
J. Fluids Struct.
,
17
(
1
), pp.
57
96
.
27.
Roache
,
P. J.
,
1998
,
Verification and Validation in Computational Science and Engineering
,
Hermosa
,
Albuquerque, NM
.
28.
Travin
,
A.
,
Shur
,
M.
,
Strelets
,
M.
, and
Spalart
,
P.
,
2000
, “
Detached-Eddy Simulations Past a Circular Cylinder
,”
Flow, Turbul. Combust.
,
63
(
1
), pp.
293
313
.