UFR 2-13 Description
A fluid-structure interaction benchmark in turbulent flow (FSI-PfS-1a)
Introduction
A flexible structure exposed to a fluid flow is deformed and deflected owing to the fluid forces acting on its surface. These displacements influence the flow field resulting in a coupling process between the fluid and the structure shortly denoted fluid-structure interaction (FSI). Due to its manifold forms of appearance it is a topic of major interest in many fields of engineering. Based on enhanced numerical algorithms and increased computational resources numerical simulations have become an important and valuable tool for solving this kind of problem within the last decade. Today FSI simulations complement additional experimental investigations. A long-lasting vision of the computational engineer is to completely replace or at least strongly reduce expensive experimental investigations in the foreseeable future. However, to attain this goal validated and thus reliable simulation tools are required.
The long-term objective of the present research project is the coupled simulation of big lightweight structures such as thin membranes exposed to turbulent flows (outdoor tents, awnings...). To study these complex FSI problems, a multi-physics code framework was recently developed~\citep{fsi-les-2012}. In order to assure reliable numerical simulations of complex configurations, the whole FSI code needs to be validated at first on simpler test cases with trusted reference data. In~\cite{fsi-les-2012} the verification process of the code developed is detailed. The CFD and CSD solvers were at first checked separately and then, the coupling algorithm was considered in detail based on a laminar benchmark. A 3D turbulent test case was also taken into account to prove the applicability of the newly developed coupling scheme in the context of large-eddy simulations (LES). However, owing to missing reference data a full validation was not possible. The overall goal of the present paper is to present a turbulent FSI test case supported by experimental data and numerical predictions based on the multi-physics code developed. Thus, on the one hand the current FSI methodology involving LES and shell structures undergoing large deformations is validated. On the other hand, a new turbulent FSI benchmark configuration is defined, based on the specific insights into numerical flow simulation, computational structural analysis as well as coupling issues. Hence, the present study should provide a precisely described test case to the FSI community for the technically relevant case of turbulent flows interacting with flexible structures.
The present study is mainly related to two former investigation of Turek and Hron (2006,2010) and Gomes and Lienhart (2006, 2012) on vortex-induced fluid-structure interactions. The well-known 2D purely numerical laminar benchmarks of Turek and Hron (2006,2010) developed in a collaborative research effort on FSI (DFG Forschergruppe 493) consists of an elastic cantilever plate which is clamped behind a rigid circular cylinder. Three different test cases, named FSI1, FSI2 and FSI3 are provided, complemented by additional self-contained CFD and CSD test cases to check both solvers independently. These test cases were also used to validate the solvers applied in the present study (Breuer et al, 2012). In order to close the gap of complementary experimantel and numerical data, a nominally 2D laminar experimental case was provided by~\cite{gomes2006,gomes2013} and \cite{gomes2011b}. Here, a very thin metal sheet with an additional weight at the end is attached behind a rotating circular cylinder and mounted inside a channel filled with a mixture of polyglycol and water to reach a low Reynolds number in the laminar regime. Experimental data are provided for several inflow velocities and two different swiveling motions could be identified depending on the inflow velocity. Owing to the thin metal sheet and the rear mass the accurate prediction of this case is demanding. There are also turbulent FSI benchmarks involving 2D structures: in~\cite{stab-fsi-2008} a rigid plate with a single rotational degree of freedom was mounted into a water channel and experimentally studied by particle-image velocimetry (PIV). This study also presents the first comparison between experimental data and predicted results achieved by the present code for a turbulent FSI problem. As another turbulent experimental benchmark, the investigations of~\cite{gomes2010,gomes2013} and \cite{gomes2011b} have to be cited: the same geometry as in~\cite{gomes2006} was used, but this time with water as the working fluid leading to much higher Reynolds numbers within the turbulent regime. The resulting FSI test case was found to be very challenging from the numerical point of view. Indeed, the prediction of the deformation and motion of the very thin flexible structure requires two-dimensional finite-elements. On the other hand the discretization of the extra weight mounted at the end of the thin metal sheet calls for three-dimensional volume elements. Thus for a reasonable prediction of this test case both element types have to be used concurrently and have to be coupled adequately. Additionally, the rotational degree of freedom of the front cylinder complicates the structural simulation and the grid adaptation of the flow prediction.
Thus, in the present study a slightly different configuration is considered to provide in a first step a less ambitious test case for the comparison between predictions and measurements focusing the investigations more to the turbulent flow regime and its coupling to a less problematic structural model. For this purpose, a fixed cylinder with a thicker rubber tail and without a rear mass is used. This should open the computation of the proposed benchmark case to a broader spectrum of codes and facilitates its adoption in the community. Strong emphasis is put on a precise description of the experimental measurements, a comprehensive discussion of the modeling in the numerical simulation (for the single field solutions as well as for the coupled problem) and the processing of the respective data to guarantee a reliable reproduction of the proposed test case with various suitable methods.
Test case description
Description of the geometrical model and the test section
FSI-PfS-1a consists of a flexible thin structure with a distinct thickness clamped behind a fixed rigid non-rotating cylinder installed in a water channel (see Fig.~\ref{fig:rubber_plate_geom}). The cylinder has a diameter . It is positioned in the middle of the experimental test section with , whereas the test section denotes a central part of the entire water channel (see Fig.~\ref{fig:water_channel}). Its center is located at downstream of the inflow section. The test section has a length of , a height of and a width . The blocking ratio of the channel is about . The gravitational acceleration points in x-direction (see Fig.~\ref{fig:rubber_plate_geom}), i.e. in the experimental setup this section of the water channel is turned 90 degrees. The deformable structure used in the experiment behind the cylinder has a length and a width . Therefore, in the experiment there is a small gap of about between the side of the deformable structure and both lateral channel walls. The thickness of the plate is . This thickness is an averaged value. The material is natural rubber and thus it is difficult to produce a perfectly homogeneous 2 mm plate. The measurements show that the thickness of the plate is between 0.002 and 0.0022 m. All parameters of the geometrical configuration of the FSI-PfS-1a benchmark are summarized in Table~\ref{tab:geom_conf_bench}.
Description of the water channel
In order to validate numerical FSI simulations based on reliable experimental data, the special research unit on FSI~\citep{for493} designed and constructed a water channel (G\"ottingen type, see Fig.~\ref{fig:water_channel}) for corresponding experiments with a special concern regarding controllable and precise boundary and working conditions \citep{gomes2006, gomes2010, gomes2011b}. The channel (\mbox{$2.8~$m$~ \times~1.3~$m$~\times~0.5~$m}, fluid volume of $0.9~$m$^3$) has a rectangular flow path and includes several rectifiers and straighteners to guarantee a uniform inflow into the test section. To allow optical flow measurement systems like Particle-Image Velocimetry, the test section is optically accessible on three sides. It possesses the same geometry as the test section described in Section~\ref{sec:Description_model}. The structure is fixed on the backplate of the test section and additionally fixed in the front glass plate. With a 24~kW axial pump a water inflow of up to \mbox{$u_{\text{max}}=6$ m/s} is possible. To prevent asymmetries the gravity force is aligned with the x-axis in main flow direction.
Flow parameters
Several preliminary tests were performed to find the best working conditions in terms of maximum structure displacement, good reproducibility and measurable structure frequencies within the turbulent flow regime. Figure~\ref{fig:structure_lastpoint_peaks_ramp} depicts the measured extrema of the structure displacement versus the inlet velocity and Figure~\ref{fig:structure_lastpoint_frequency_St_ramp} gives the frequency and Strouhal number as a function of the inlet velocity. These data were achieved by measurements with the laser distance sensor explained in Section~\ref{sec:Laser_Sensor}. The entire diagrams are the result of a measurement campaign in which the inflow velocity was consecutively increased from 0 to . At an inflow velocity of the displacement are symmetrical, reasonably large and well reproducible. Based on the inflow velocity chosen and the cylinder diameter the Reynolds number of the experiment is equal to . Regarding the flow around the front cylinder, at this inflow velocity the flow is in the sub-critical regime. That means the boundary layers are still laminar, but transition to turbulence takes place in the free shear layers evolving from the separated boundary layers behind the apex of the cylinder. Except the boundary layers at the section walls the inflow was found to be nearly uniform (see Fig.~\ref{fig:water_channel_inflow}). The velocity components and are measured with two-component laser-Doppler velocimetry (LDV) along the y-axis in the middle of the measuring section at and . It can be assumed that the velocity component $\overline{w}$ shows a similar velocity profile as . Furthermore, a low inflow turbulence level of is measured. All experiments were performed with water under standard conditions at . The flow parameters are summarized to
Inflow velocity Flow density Flow dynamic viscosity
Material Parameters
Although the material shows a strong non-linear elastic behavior for large strains, the application of a linear elastic constitutive law would be favored, to enable the reproduction of this FSI benchmark by a variety of different computational analysis codes without the need of complex material laws. This assumption can be justified by the observation that in the FSI test case, a formulation for large deformations but small strains is applicable. Hence, the identification of the material parameters is done on the basis of the moderate strain expected and the St. Venant-Kirchhoff constitutive law is chosen as the simplest hyper-elastic material.
The density of the rubber material can be determined to be =1360 kg/m for a thickness of the plate h = 0.0021 m. This permits the accurate modeling of inertia effects of the structure and thus dynamic test cases can be used to calibrate the material constants. For the chosen material model, there are only two parameters to be defined: the Young's modulus E and the Poisson's ratio . In order to avoid complications in the needed element technology due to incompressibility, the material was realized to have a Poisson's ratio which reasonably differs from . Material tests of the manufacturer indicate that the Young's modulus is E=16 MPa and the Poisson's ratio is =0.48.
density =1360 kg/m, Young's modulus E=16 MPa, Poisson's ratio =0.48
Measuring Techniques
Experimental FSI investigations need to contain fluid and structure measurements for a full description of the coupling process. Under certain conditions, the same technique for both disciplines can be used. The measurements performed by \cite{gomes2006,gomes2010,gomes2013} used the same camera system for the simultaneous acquisition of the velocity fields and the structural deflections. This procedure works well for FSI cases involving laminar flows and 2D structure deflections. In the present case the structure deforms slightly three-dimensional with increased cycle-to-cycle variations caused by turbulent variations in the flow. The applied measuring techniques, especially the structural side, have to deal with those changed conditions especially the formation of shades. Furthermore, certain spatial and temporal resolutions as well as low measurement errors are requested. Due to the different deformation behavior a single camera setup for the structural measurements like in \cite{gomes2006,gomes2010,gomes2013} used was not practicable. Therefore, the velocity fields were captured by a 2D Particle-Image Velocimetry (PIV) setup and the structural deflections were measured with a laser triangulation technique. Both devices are presented in the next sections.
Particle-image velocimetry
A classic Particle-Image Velocimetry~\citep{adrian1991} setup depicted in Fig.~\ref{fig:piv} consists of a single camera obtaining two components of the fluid velocity on a planar surface illuminated by a laser light sheet. Particles introduced into the fluid are following the flow and reflecting the light during the passage of the light sheet. By taking two reflection fields in a short time interval t, the most-likely displacements of several particle groups on an equidistant grid are estimated by a cross-correlation technique or a particle-tracking algorithm. Based on a precise preliminary calibration, the displacements obtained and the time interval t chosen the velocity field can be calculated. To prevent shadows behind the flexible structure a second light sheet was used to illuminate the opposite side of the test section.
The phased-resolved PIV-measurements (PR-PIV) were carried out with a 4 Mega-pixel camera (TSI Powerview 4MP, charge-coupled device (CCD) chip) and a pulsed dual-head Neodym:YAG laser (Litron NanoPIV 200) with an energy of 200 mJ per laser pulse. The high energy of the laser allowed to use silver-coated hollow glass spheres (SHGS) with an average diameter of =10~µm and a density of = 1400 kg m as tracer particles. To prove the following behavior of these particles a Stokes number Sk=1.08 and a particle sedimentation velocity is calculated With this Stokes number and a particle sedimentation velocity which is much lower than the expected velocities in the experiments, an eminent following behavior is approved. The camera takes 12 bit pictures with a frequency of about 7.0 Hz and a resolution of 1695 x 1211 px with respect to the rectangular size of the test section. For one phase-resolved position (described in Section~\ref{sec:Generation_of_phase-resolved_data}) 60 to 80 measurements are taken. Preliminary studies with more and fewer measurements showed that this number of measurements represent a good compromise between accuracy and effort. The grid has a size of 150 x 138 cells and was calibrated with an average factor of 126 m/px}, covering a planar flow field of x/D = -2.36 to 7.26 and y/D = -3.47 to ~3.47 in the middle of the test section at z/D = 0. The time between the frame-straddled laser pulses was set to t=200 s. Laser and camera were controlled by a TSI synchronizer (TSI 610035) with 1 ns resolution. The processing of the phase-resolved fluid velocity fields involving the structure deflections is described in Section~\ref{sec:Generation_of_phase-resolved_data}.
Laser distance sensor
Non-contact structural measurements are often based on laser distance techniques. In the present benchmark case the flexible structure shows an oscillating frequency of about 7.1 Hz. With the requirement to perform more than 100 measurements per period, a time-resolved system was needed. Therefore, a laser triangulation was chosen because of the known geometric dependencies, the high data rates, the small measurement range and the resulting higher accuracy in comparison with other techniques such as laser phase-shifting or laser interferometry. The laser triangulation uses a laser beam which is focused onto the object. A CCD-chip located near the laser output detects the reflected light on the object surface. If the distance of the object from the sensor changes, also the angle changes and thus the position of its image on the CCD-chip. From this change in position the distance to the object is calculated by simple trigonometric functions and an internal length calibration adjusted to the applied measurement range. To study simultaneously more than one point on the structure, a multiple-point triangulation sensor was applied (Micro-Epsilon scanControl 2750, see Fig.~\ref{fig:sensor_alignment}). This sensor uses a matrix of CCD chips to detect the displacements on up to 640 points along a laser line reflected on the surface of the structure with a data rate of \mbox 800 profiles per second. The laser line was positioned in a horizontal (x/D = 3.2, see Fig.~\ref{fig:sensor_alignment}(a)) and in a vertical alignment(z/D = 0, see Fig.~\ref{fig:sensor_alignment}(b)) and has an accuracy of 40 µm}. Due to the different refraction indices of air, glass and water a custom calibration was performed to take the modified optical behavior of the emitted laser beams into account.
Numerical Simulation Methodology
The applied numerical method relies on an efficient partitioned coupling scheme developed for dynamic fluid-structure interaction problems in turbulent flows \citep{fsi-les-2012}. The fluid flow is predicted by an eddy-resolving scheme, i.e., the large-eddy simulation technique. FSI problems very often encounter instantaneous non-equilibrium flows with large-scale flow structures such as separation, reattachment and vortex shedding. For this kind of flows the LES technique is obviously the best choice~\citep{habil2002}. Based on a semi-implicit scheme the LES code is coupled with a code especially suited for the prediction of shells and membranes. Thus an appropriate tool for the time-resolved prediction of instantaneous turbulent flows around light, thin-walled structures results. Since all details of this methodology were recently published in \citet{fsi-les-2012}, in the following only a brief description is provided.
Computational fluid dynamics (CFD)
Within a FSI application the computational domain is no longer fixed but changes in time due to the fluid forces acting on the structure. This temporally varying domain is taken into account by the Arbitrary Lagrangian-Eulerian (ALE) formulation expressing the conservation equations for time-dependent volumes and surfaces. Here the filtered Navier-Stokes equations for an incompressible fluid are solved. Owing to the deformation of the grid, extra fluxes appear in the governing equations which are consistently determined considering the \emph{space conservation law (SCL)} \citep{demirdzic1988,demirdzic1990,lesoinne96}. The SCL is expressed by the swept volumes of the corresponding cell faces and assures that no space is lost during the movement of the grid lines. For this purpose the in-house code FASTEST-3D \citep{durstsch96,duscwe961} relying on a three-dimensional finite-volume scheme is used. The discretization is done on a curvilinear, block-structured body-fitted grid with collocated variable arrangement. A midpoint rule approximation of second-order accuracy is used for the discretization of the surface and volume integrals. Furthermore, the flow variables are linearly interpolated to the cell faces leading to a second-order accurate central scheme. In order to ensure the coupling of pressure and velocity fields on non-staggered grids, the momentum interpolation technique of \citet{rhie83} is used.
A predictor-corrector scheme (projection method) of second-order accuracy forms the kernel of the fluid solver. In the predictor step an explicit three substep low-storage Runge-Kutta scheme advances the momentum equation in time leading to intermediate velocities. These velocities do not satisfy mass conservation. Thus, in the following corrector step the mass conservation equation has to be fulfilled by solving a Poisson equation for the pressure-correction based on the incomplete LU decomposition method of \citet{stone68}. The corrector step is repeated (about 3 to 8 iterations) until a predefined convergence criterion ($\Delta\dot{m} < {\cal O}(10^{-9})$) is reached and the final velocities and the pressure of the new time step are obtained. In \cite{fsi-les-2012} it is explained that the original pressure-correction scheme applied for fixed grids has not to be changed concerning the mass conservation equation in the context of moving grids. Solely in the momentum equation the grid fluxes have to be taken into account as described above.
In LES the large scales in the turbulent flow field are resolved directly, whereas the non-resolvable small scales have to be taken into account by a subgrid-scale model. Here the well-known and most often used eddy-viscosity model, i.e., the \citet{smagorinsky} model is applied. The filter width is directly coupled to the volume of the computational cell and a Van Driest damping function ensures a reduction of the subgrid length near solid walls. Owing to minor influences of the subgrid-scale model at the moderate Reynolds number considered in this study, a dynamic procedure to determine the Smagorinsky parameter as suggested by \citet{germano} was omitted and instead a well established standard constant $C_s = 0.1$ is used.
Computational structural dynamics (CSD)
The dynamic equilibrium of the structure is described by the momentum equation given in a Lagrangian frame of reference. Large deformations, where geometrical non-linearities are not negligible, are allowed \citep{hojjat2010}. According to the preliminary considerations described in Section~\ref{sec:Structural_Tests}, a total Lagrangian formulation in terms of the second Piola-Kirchhoff stress tensor and the Green-Lagrange strain tensor which are linked by the St.\ Venant-Kirchhoff material law is used in the present study. For the solution of the governing equation the finite-element solver {Carat++}, which was developed with an emphasis on the prediction of shell or membrane behavior, is applied. {Carat++} is based on several finite-element types and advanced solution strategies for form finding and non-linear dynamic problems~\citep{wuechner2005,bletzinger2005,dieringer2012}. For the dynamic analysis, different time-integration schemes are available, e.g., the implicit generalized-$\alpha$ method \citep{chung93}. In the modeling of thin-walled structures, membrane or shell elements are applied for the discretization within the finite-element model. In the current case, the deformable solid is modeled with a 7-parameter shell element.
Coupling algorithm
To preserve the advantages of the highly adapted CSD and CFD codes and to realize an effective coupling algorithm, a partitioned but nevertheless strong coupling approach is chosen. Since LES typically requires small time steps to resolve the turbulent flow field, the coupling scheme relies on the explicit predictor-corrector scheme forming the kernel of the fluid solver.
Based on the velocity and pressure fields from the corrector step, the fluid forces resulting from the pressure and the viscous shear stresses at the interface between the fluid and the structure are computed. These forces are transferred by a grid-to-grid data interpolation to the CSD code Carat++ using a conservative interpolation scheme \citep{farhat98} implemented in the coupling interface CoMA \citep{coma}. Using the fluid forces provided via CoMA, the finite-element code Carat++ determines the stresses in the structure and the resulting displacements of the structure. This response of the structure is transferred back to the fluid solver via CoMA applying a bilinear interpolation which is a consistent scheme for four-node elements with bilinear shape functions.
For moderate and high density ratios between the fluid and the structure, e.g., a flexible structure in water, the added-mass effect by the surrounding fluid plays a dominant role. In this situation a strong coupling scheme taking the tight interaction between the fluid and the structure into account, is indispensable. In the coupling scheme developed in \citet{fsi-les-2012} this issue is taken into account by a FSI-subiteration loop which works as follows:
A new time step begins with an estimation of the displacement of the structure. For the estimation a linear extrapolation is applied taking the displacement values of two former time steps into account. According to these estimated boundary values, the entire computational grid has to be adapted as it is done in each FSI-subiteration loop. Then the predictor-corrector scheme of the next time step is carried out and the cycle of the FSI-subiteration loop is entered. After each FSI-subiteration first the FSI convergence is checked. Convergence is reached if the L$_2$ norm of the displacement differences between two FSI-subiterations normalized by the L$_2$ norm of the changes in the displacements between the current and the last time step drops below a predefined limit, e.g.\ $\varepsilon_{FSI} = 10^{-4}$ for the present study. Typically, convergence is not reached within the first step but requires a few FSI-subiterations (5 to 10). Therefore, the procedure has to be continued on the fluid side. Based on the displacements on the fluid-structure interface, which are underrelaxated by a constant factor $\omega$ during the transfer from the CFD to the CSD solver, the inner computational CFD grid is adjusted. The key point of the coupling procedure suggested in \citet{fsi-les-2012} is that subsequently only the corrector step of the predictor-corrector scheme is carried out again to obtain a new velocity and pressure field. Thus the clue is that the pressure is determined in such a manner that the mass conservation is finally satisfied. Furthermore, this extension of the predictor-corrector scheme assures that the pressure forces as the most relevant contribution to the added-mass effect, are successively updated until dynamic equilibrium is achieved. In conclusion, instabilities due to the added-mass effect known from loose coupling schemes are avoided and the explicit character of the time-stepping scheme beneficial for LES is still maintained.
The code coupling tool CoMA is based on the Message-Passing-Interface (MPI) and thus runs in parallel to the fluid and structure solver. The communication in-between the codes is performed via standard MPI commands. Since the parallelization in FASTEST-3D and Carat++ also relies on MPI, a hierarchical parallelization strategy with different levels of parallelism is achieved. According to the CPU-time requirements of the different subtasks, an appropriate number of processors can be assigned to the fluid and the structure part. Owing to the reduced structural models on the one side and the fully three-dimensional highly resolved fluid prediction on the other side, the predominant portion of the CPU-time is presently required for the CFD part. Additionally, the communication time between the codes via CoMA and within the CFD solver takes a non-negligible part of the computational resources.
Numerical CFD Setup
For the CFD prediction of the flow two different block-structured grids either for a subset of the entire channel ($w' / l = 1$) or for the full channel but without the gap between the flexible structure and the side walls ($w / l = 2.95$) are used (see Fig.~\ref{fig:Benchmark_FSI-PfS-1_full_and_subset_case}). In the first case the entire grid consists of about 13.5 million control volumes (CVs), whereas 72 equidistant CVs are applied in the spanwise direction. For the full geometry the grid possesses about 22.5 million CVs. In this case starting close to both channel walls the grid is stretched geometrically with a stretching factor $1.1$ applying in total 120 CVs with the first cell center positioned at a distance of $\Delta y / D = 1.7 \times 10^{-2}$.
Fig. xx X-Y cross-section of the grid used for the simulation (Note that only every fourth grid line in each direction is displayed here).
The gap between the elastic structure and the walls is not taken into
account in the numerical model and thus the width of the channel is
set to \mbox{$w$} instead of \mbox{$W$}. The stretching factors are kept below 1.1 with the first cell
center located at a distance of $\Delta y / D = 9 \times 10^{-4}$ from
the flexible structure. Based on the wall shear stresses on the
flexible structure the average $y^+$ values are predicted to be below
$0.8$, mostly even below $0.5$. Thus, the viscous sublayer on the
elastic structure and the cylinder is adequately resolved. Since the
boundary layers at the upper and lower channel walls are not
considered, no grid clustering is required here.
On the CFD side no-slip boundary conditions are applied at the rigid front cylinder and at the flexible structure. Since the resolution of the boundary layers at the channel walls would require the bulk of the CPU-time, the upper and lower channel walls are assumed to be slip walls. Thus the blocking effect of the walls is maintained without taking the boundary layers into account. At the inlet a constant streamwise velocity is set as inflow condition without adding any perturbations. The choice of zero turbulence level is based on the consideration that such small perturbations imposed at the inlet will generally not reach the cylinder due to the coarseness of the grid at the outer boundaries. Therefore, all inflow fluctuations will be highly damped. However, since the flow is assumed to be sub-critical, this disregard is insignificant. At the outlet a convective outflow boundary condition is favored allowing vortices to leave the integration domain without significant disturbances \citep{habil2002}. The convection velocity is set to \mbox{$u_\text{inflow}$}.
As mentioned above two different cases are considered (see Fig.~\ref{fig:Benchmark_FSI-PfS-1_full_and_subset_case}). In order to save CPU-time in the first case only a subset of the entire spanwise extension of the channel is taken into account. Thus the computational domain has a width of \mbox{$w'/l$ = 1} in z-direction and the flexible structure is a square in the x-z-plane. In this case a reasonable approximation already applied in \citet{fsi-les-2012} is to apply periodic boundary conditions in spanwise direction for both disciplines. For LES predictions periodic boundary conditions represent an often used measure in order to avoid the formulation of appropriate inflow and outflow boundary conditions. The approximation is valid as long as the turbulent flow is homogeneous in the specific direction and the width of the domain is sufficiently large. The latter can be proven by predicting two-point correlations, which have to drop towards zero within the half-width of the domain. The impact of periodic boundary conditions on the CSD predictions are discussed below.
For the full case with $w / l = 2.95$ periodic boundary conditions can no longer be used. Instead, for the fluid flow similar to the upper and lower walls also for the lateral boundaries slip walls are assumed since the full resolution of the boundary layers would be again too costly. Furthermore, the assumption of the slip wall is consistent with the disregard of the small gap between the flexible structure and the side walls discussed above.
Numerical CSD Setup
Motivated by the fact that in the case of LES frequently a domain modeling based on periodic boundary conditions at the lateral walls is used to reduce the CPU-time requirements, this special approach was also investigated for the FSI test case. The detailed discussion of this specific boundary modeling for the spanwise direction is given in Section~\ref{section:bc}. As a consequence, there are two different structure meshes used: For the CSD prediction of the case with a subset of the full channel the elastic structure is resolved by the use of $10 \times 10$ quadrilateral four-node 7-parameter shell elements. For the case discretizing the entire channel, 10 quadrilateral four-node shell elements are used in the main flow direction and 30 in the spanwise direction.
On the CSD side, the flexible shell is loaded on the top and bottom surface by the fluid forces, which are transferred from the fluid mesh to the structure mesh. These Neumann boundary conditions for the structure reflect the coupling conditions. Concerning the Dirichlet boundary conditions, the four edges need appropriate support modeling: on the upstream side at the rigid cylinder a clamped support is realized and all degrees of freedom are equal to zero. On the opposite downstream trailing-edge side, the rubber plate is free to move and all nodes have the full set of six degrees of freedom. The edges which are aligned to the main flow direction need different boundary condition modeling, depending on whether the subset or the full case is computed:
For the subset case due to the fluid-motivated periodic boundary conditions, periodicity for the structure is correspondingly assumed for consistency reasons. As it turns out later in Section~\ref{sec:Full_case_vs_Subset_case}, this assumption seems to hold for this specific benchmark configuration and its deformation pattern which has strong similarity with an oscillation in the first eigenmode of the plate. Hence, this modeling approach may be used for the efficient processing of parameter studies, e.g., to evaluate the sensitivity of the FSI simulations with respect to slight variations in model parameters shown in Section~\ref{sec:Sensitivity_study}. For this special type of support modeling, there are always two structure nodes on the lateral sides (one in a plane $z=-w/2$ and its twin in the other plane $z=+w/2$) which have the same load. These two nodes must have the same displacements in x- and y-direction and their rotations have to be identical. Moreover, the periodic boundary conditions imply that the z-displacement of the nodes on the sides are forced to be zero.
For the full case the presence of the walls in connection with the small gap implies that there is in fact no constraining effect on the structure, as long as no contact between the plate and the wall takes place. Out of precise observations in the lab, the possibility of contact may be disregarded. In principle, this configuration would lead to free-edge conditions like at the trailing edge. However, the simulation of the fluid with a moving mesh needs a well-defined mesh situation at the side walls which made it necessary to tightly connect the structure mesh to the walls (the detailed representation of the side edges within the fluid mesh is discarded due to computational costs and the resulting deformation sensitivity of the mesh in these regions). Also the displacement in z-direction of the structure nodes at the lateral boundaries is forced to be zero.
Coupling conditions
For the turbulent flow a time-step size of $\Delta t_{f} = 2 \times 10^{-5}$s ($\Delta t_{f}^{\ast} = 1.26 \times 10^{-3}$ in dimensionless form using $u_\text{inflow}$ and $D$ as reference quantities) is chosen and the same time-step size is applied for the structural solver based on the generalized-$\alpha$ method with the spectral radius $\varrho_\infty = 1.0$, i.e, the Newmark standard method. For the CFD part this time-step size corresponds to a CFL number in the order of unity. Furthermore, a constant underrelaxation factor of $\omega$ = $0.5$ is considered for the displacements and the loads are transferred without underrelaxation. In accordance with previous laminar and turbulent cases in \citet{fsi-les-2012} the FSI convergence criterion is set to $\varepsilon_{FSI} = 10^{-4}$ for the L$_2$ norm of the displacement differences. As estimated from previous cases \citep{fsi-les-2012} 5 to 10 FSI-subiterations are required to reach the convergence criterion.
After an initial phase in which the coupled system reaches a statistically steady state, each simulation is carried out for about 4~s real-time corresponding to about 27 swiveling cycles of the flexible structure.
For the coupled LES predictions the national supercomputer SuperMIG/SuperMUC was used applying either 82 or 140 processors for the CFD part of the reduced and full geometry, respectively. Additionally, one processor is required for the coupling code and one processor for the CSD code, respectively.
Generation of Phase-resolved Data
Each flow characteristic of a quasi-periodic FSI problem can be written as a function $f=\bar{f}+\tilde{f}+f'$, where $\bar{f}$ describes the global mean part, $\tilde{f}$ the quasi-periodic part and $f'$ a random turbulence-related part~\citep{reynolds72,cantwell83}. This splitting can also be written in the form $f = \left<f\right> + f'$, where $\left<f\right>$ is the phase-averaged part, i.e., the mean at constant phase. In order to be able to compare numerical results and experimental measurements, the irregular turbulent part $f'$ has to be averaged out. This measure is indispensable owing to the nature of turbulence which solely allows reasonable comparisons based on statistical data. Therefore, the present data are phase-averaged to obtain only the phase-resolved contribution $\left<f\right>$ of the problem, which can be seen as a representative and thus characteristic signal of the underlying FSI phenomenon.
The procedure to generate phase-resolved results is the same for the experiments and the simulations and is also similar to the one presented in \cite{gomes2006}. The technique can be split up into three steps:
- Reduce the 3D-problem to a 2D-problem - Due to the facts that in the present benchmark the structure deformation in spanwise direction is negligible and that the delivered experimental PIV-results are solely available in one x-y-plane, first the 3D-problem is reduced to a 2D-problem. For this purpose the flow field and the shell position in the CFD predictions are averaged in spanwise direction.
- Determine n reference positions for the FSI Problem - A representative signal of the FSI phenomenon is the history of the y-displacements of the shell extremity. Therefore, it is used as the trigger signal for this averaging method leading to phase-resolved data. Note that the averaged period of this signal is denoted $T$. At first, it has to be defined in how many sub-parts the main period of the FSI problem will be divided and so, how many reference positions have to be calculated (for example in the present work $n = 23$). Then, the margins of each period of the y-displacement curve are determined. In order to do that the intersections between the y-displacement curve and the zero crossings ($U_y = 0$) are looked for and used to limit the periods. Third, each period $T_i$ found is divided into $n$ equidistant sub-parts denoted $j$.
- Sort and average the data corresponding to each reference Position - The sub-part $j$ of the period $T_i$ corresponds to the sub-part $j$ of the period $T_{i+1}$ and so on. Each data set found in a sub-part $j$ will be averaged with the other sets found in the sub-parts $j$ of all other periods (see Fig.~\ref{fig:num_phase-resolved_method2_step2}). Finally, data sets of $n$ phase-averaged positions for the representative reference period are achieved.
The simulation data containing structure positions, pressure and velocity fields, are generated every 150 time steps. According to the frequency observed for the structure and the time-step size chosen about 50 data sets are obtained per swiveling period. With respect to the time interval predicted and the number of subparts chosen, the data for each subpart are averaged from about 50 data sets. A post-processing program is implemented based on the method described above. It does not require any special treatment and thus the aforementioned method to get the phase-resolved results is straightforward.
The current experimental setup consists of the multiple-point triangulation sensor described in Section~\ref{sec:Laser_Sensor} and the synchronizer of the PIV system. Each measurement pulse of the PIV system is detected in the data acquisition of the laser distance sensor, which measures the structure deflection continuously with 800 profiles per second. With this setup, contrary to \cite{gomes2006}, the periods are not detected during the acquisition but in the post-processing phase. After the run a specific software based on the described method mentioned above computes the reference structure motion period and sorts the PIV data to get the phase-averaged results.
Contributed by: Michael Breuer — Helmut-Schmidt Universität Hamburg
© copyright ERCOFTAC 2024