UFR 2-13 Test Case: Difference between revisions

From KBwiki
Jump to navigation Jump to search
Line 238: Line 238:
the positions of the vortices convected downstream are correctly
the positions of the vortices convected downstream are correctly
predicted.
predicted.
= 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
$\Delta y / D = 1.7 \times 10^{-2}$.
[[File:Benchmark_FSI-PfS-1_full_and_subset_case.jpg]]
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 =
= Generation of Phase-resolved Data =

Revision as of 08:14, 7 October 2013

A fluid-structure interaction benchmark in turbulent flow (FSI-PfS-1a)

Front Page

Description

Test Case Studies

Evaluation

Best Practice Advice

References

Comparison between numerical and experimental results

The investigations presented in Section~\ref{sec:Full_case_vs_Subset_case} based on slightly different material characteristics than defined in Section~\ref{sec:Material_parameters} have shown that the subset case permits a gain in CPU-time but nevertheless nearly identical results as the full case. Therefore, the numerical computation with the structural parameters defined in Section~\ref{sec:Material_parameters} ($E$ = 16 MPa, $h$ = 0.0021~m, $\rho_\text{rubber plate}$ = 1360 kg m$^{-3}$) is carried out for the subset case.

Two simulations are considered: one with the structural damping defined in Section~\ref{sec:validation_structure_model}, the other one without damping. These results are compared with the experimental data to check their accuracy. In order to quantitatively compare the experimental and numerical data, both are phase-averaged as explained in Section~\ref{sec:Generation_of_phase-resolved_data}. Similar to the numerical comparison presented in Section~\ref{sec:Full_case_vs_Subset_case} the displacement of the structure will be first analyzed and then the phase-resolved flow field is considered.

%-------------------------------------------------------------------- \subsubsection{Deflection of the structure}

\begin{figure}[!htbp] 

 \centering
 \includegraphics[width=0.9\linewidth,draft=\draftmode]
                 {FSI-PfS-1a_structure_phase_averaged_timephase}
                 \caption{\label{fig:swiveling_mode_FSI-PfS-1a}
                   Experimental structural results: Structure contour
                   for the reference period.}

\end{figure}

The structure contour of the phased-averaged experimental results for the reference period is depicted in Fig.~\ref{fig:swiveling_mode_FSI-PfS-1a}. Obviously, the diagram represents the first swiveling mode of the FSI phenomenon showing only one wave mode at the clamping. Figure~\ref{fig:comp_mean_period:a} depicts the experimental dimensionless raw signal obtained at a point located in the midplane at a distance of 9~mm from the shell extremity (see Fig.~\ref{fig:comp_full_subset:c}). Figure~\ref{fig:comp_mean_period:b} shows the numerical signal predicted without structural damping and Fig.~\ref{fig:comp_mean_period:c} the one computed with damping. Applying the phase-averaging process the mean phase of the FSI phenomenon for the experiment and for the simulations is generated. The outcome is presented in Fig.~\ref{fig:comp_mean_period:d} with the phase as the abscissa and the dimensionless displacement \mbox{$U_y^* = U_y / D$} as the ordinate. The amplitudes of the experimental signal varies more than in the predictions. Therefore, the maximal standard deviation of each point of the averaged phase is for the experiment bigger (0.083) than for the simulation (0.072 with and without damping). In order to check the reliability of the computed mean phase the coefficient of determination $R^2$ is computed: it is smaller for the mean experimental phase (0.9640) than for the mean simulation ones (0.9770 without damping and 0.9664 with damping). However, the values are close to unity, which is an indication that the averaged phases are representative for the signals. In Fig.~\ref{fig:comp_mean_period:d} the mean period calculated from the simulation without damping is quasi-antisymmetric with respect to \mbox{$U_y^* = 0$}. On the contrary the period derived from the experiment is not exactly antisymmetric with respect to the midpoint of the phase \mbox{$\phi = 

 \pi$}: the cross-over is not at the midpoint of the phase but

slightly deviates to the right. However, the absolute values of the minimum and maximum are nearly identical. As for the experimental phase, the simulation with damping generates a phase signal, which is not completely antisymmetric. In the experiment this weak asymmetry can be attributed to minor asymmetries in the setup or in the rubber material. The comparison in Fig.~\ref{fig:comp_mean_period:d} shows some differences in the extrema and a summary is presented in Table~\ref{tab:comparison_num_exp_damping}. Without structural damping the simulations produce extrema which are too large by about 10~\%. With structural damping the extrema are smaller, even smaller than in the experiment by about 6~\%. Thus, the structural damping also has a significant influence on the FSI predictions and can not be overlooked.

The frequency of the FSI phenomenon, i.e., the frequency of the y-displacements, is about \mbox{$f_{{FSI}_{\text{exp}}}=7.10\,$Hz} in the experimental investigations, which corresponds to a Strouhal number \mbox{$\text{St} \approx 0.11$}. In the numerical predictions without damping this frequency is \mbox{$f_{{FSI}_{\text{num}}}^{\text{no damping}}=7.08\,$Hz} and with damping \mbox{$f_{{FSI}_{\text{num}}}^{\text{damping}}=7.18\,$Hz}. This comparison shows an error of \mbox{$\epsilon_{f}=-0.25\,\%$} for the results without damping and \mbox{$\epsilon_{f}=1.15\,\%$} for the cases with damping. Nevertheless, the FSI frequency is also very well predicted in both cases. One can notice that the frequency of the coupled system slightly increases due to the structural damping. % \begin{table}[!htbp] 

 \centering
 \begin{tabular}{|l||c|c|c|c|c|c|c|}
   \hline
   Case                   & \multicolumn{7}{|c|}{Results} \\
   \hline
                          & St (Hz) & $f_{FSI}$ (\%) & Error & \mbox{$\left.U_{y}^*\right|_{max}$} & Error (\%) & \mbox{$\left.U_{y}^*\right|_{min}$} & Error \\
   \hline
   \hline
   Sim. (no damping)      & 0.1125 & 7.08   & -0.25   & 0.456             & 9.1  & -0.464            & -10.6 \\
  \hline
   Sim. (damping)         & 0.1140 & 7.18   & 1.15    & 0.396             & -5.32 & -0.395            & 6.02   \\
   \hline
   \hline
   Experiments            & 0.1128 & 7.10   & -       & 0.418             & -     & -0.420            & -     \\
   \hline
 \end{tabular}
 \caption{\label{tab:comparison_num_exp_damping} 
   Comparison between numerical results with and without structural 
      damping and the experiment.}

\end{table}

\begin{figure}[!htbp] 

 \centering
 \begin{minipage}{\linewidth}
   \centering
   \subfigure[\label{fig:comp_mean_period:a}
            Experimental raw signal: Dimensionless displacement.]{
     \includegraphics[width=0.45\linewidth,draft=\draftmode]{raw_signal_dispy_exp_real2}
   }\hspace{0.049\linewidth}
   \subfigure[\label{fig:comp_mean_period:b}Numerical raw signal (without damping): 
                    Dimensionless displacement.]{
     \includegraphics[width=0.45\linewidth,draft=\draftmode]{raw_signal_dispy_num}
   }
 \end{minipage}
 \begin{minipage}{\linewidth}
   \centering
   \subfigure[\label{fig:comp_mean_period:c}Numerical raw signal (with damping): 
                Dimensionless displacement.]{
     \includegraphics[width=0.45\linewidth,draft=\draftmode]{raw_signal_dispy_num_damping}
   }\hspace{0.049\linewidth}%
   \subfigure[\label{fig:comp_mean_period:d}Comparison of the averaged phase of the
   experimental and numerical data.]{
     \includegraphics[width=0.45\linewidth,draft=\draftmode]{comp_mean_period_damping}
   }
 \end{minipage}
 \caption{\label{fig:comp_mean_period}Comparison of experimental
   and numerical results; raw signals and averaged phases of a
   point located at 9 mm distance from the shell extremity.}

\end{figure}

%-------------------------------------------------------------------- \subsubsection{Phase-resolved flow field}

Owing to improved results in case of the structural damping, this case is chosen for the direct comparison with the measurements. The phase-averaging process delivers the phase-resolved flow fields. Four phase-averaged positions, which describe the most important phases of the FSI phenomenon, are chosen for the comparison: Fig.~\ref{fig:comparison_rubber_plate:1} shows the flexible structure reaching a maximal upward deflection at \mbox{$t \approx T / 

 4$}. Then, it deforms in the opposite direction and moves

downwards. At \mbox{$t \approx T / 2$} the shell is almost in its undeformed state (see Fig.~\ref{fig:comparison_rubber_plate:2}). Afterwards, the flexible structure reaches a maximal downward deformation at \mbox{$t \approx 3 

 T / 4$} as seen in Fig.~\ref{fig:comparison_rubber_plate:3}. At

\mbox{$t \approx T$} the period cycle is completed and the shell is near its initial state presented in Fig.~\ref{fig:comparison_rubber_plate:4}.

For each of the given phase-averaged positions, the experimental and numerical results (dimensionless streamwise and transverse velocity component) are plotted for comparison. Note that the shell in the experimental figures is shorter than in the simulation plots. Indeed, in the experiment it is not possible to get exactly the whole experimental structure, around 1 mm at the end of the structure is missing. As in Section~\ref{sec:Comparison_of_numerical_results} an additional figure shows the error between the simulation and the experiment for the velocity magnitude.

At \mbox{$t \approx T / 4$} (see Fig.~\ref{fig:comparison_rubber_plate:1}), when the structure is in its maximal upward deflection, the acceleration zone above the structure has reached its maximum. The acceleration area below the plate is growing. Both phenomena are correctly predicted in the simulations. The computed acceleration area above the structure is slightly overestimated. However the local error is mostly under 20 \%.

The separation points at the cylinder are found to be in close agreement between measurements and predictions. Accordingsly, also the location of the shear layers shows a good agreement between simulations and experiments. The shedding phenomenon behind the structure generates a turbulent wake, which is correctly reproduced by the computations. Owing to the phase-averaging procedure, as expected all small-scale structures are averaged out.

At \mbox{$t \approx T / 2$} (see Fig.~\ref{fig:comparison_rubber_plate:2}), the plate is near its undeformed state. The acceleration zone above the structure has shrunk in favor of the area below the plate. Regarding these areas the predictions show a very good agreement with the measurements (marginal local errors). The predicted wake directly behind the structure matches the measured one.

At \mbox{$t \approx 3 T / 4$} (see Fig.~\ref{fig:comparison_rubber_plate:3}), the downward deformation of the plate is maximal, the flow is the symmetrical to the flow observed at \mbox{$t \approx T / 4$} with respect to \mbox{y/D = 0}. Again the acceleration areas around the structure show a very good agreement with the measurements. Once more the wake is correctly predicted in the near-field of the structure.

At \mbox{$t \approx T$} (see Fig.~\ref{fig:comparison_rubber_plate:4}) the flow is symmetrical to the flow observed at \mbox{$t \approx T / 

 2$} with respect to \mbox{y/D = 0}. The computed acceleration area

above the structure is slightly overestimated, but the local error is under 20 \%. The wake is again correctly predicted except directly after the flexible structure.

For every position the local error is mostly under $20\,\%$. In the error plot the areas with a bigger local error are near the structure and in the shear layers. This can be explained by the fact that near the structure and in the shear layers the gradients of the flow quantities are large. Since the mesh used for the simulation is much finer than the PIV measurement grid, the accuracy of the numerical solution is much higher than the precision of the PIV measurements in these regions. Another reason is that the error expected by the PIV method is more important for low flow velocities. Close to the flexible structure and directly after its tail the flow velocity is small, which at least partially explains the deviations observed between the experimental and numerical results.

In summary, for every position the computed flow is in good agreement with the measured one. The shedding phenomenon behind the cylinder and the positions of the vortices convected downstream are correctly predicted.

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.

Test Case Study

Brief Description of the Study Test Case

This should:

  • Convey the general set up of the test-case configuration( e.g. airflow over a bump on the floor of a wind tunnel)
  • Describe the geometry, illustrated with a sketch
  • Specify the flow parameters which define the flow regime (e.g. Reynolds number, Rayleigh number, angle of incidence etc.)
  • Give the principal measured quantities (i.e. assessment quantities) by which the success or failure of CFD calculations are to be judged. These quantities should include global parameters but also the distributions of mean and turbulence quantities.


The description can be kept fairly short if a link can be made to a data base where details are given. For other cases a more detailed, fully self-contained description should be provided.

Test Case Experiments

Provide a brief description of the test facility, together with the measurement techniques used. Indicate what quantities were measured and where.

Discuss the quality of the data and the accuracy of the measurements. It is recognized that the depth and extent of this discussion is dependent upon the amount and quality of information provided in the source documents. However, it should seek to address:

  • How close is the flow to the target/design flow (e.g. if the flow is supposed to be two-dimensional, how well is this condition satisfied)?
  • Estimation of the accuracy of measured quantities arising from given measurement technique
  • Checks on global conservation of physically conserved quantities, momentum, energy etc.
  • Consistency in the measurements of different quantities.

Discuss how well conditions at boundaries of the flow such as inflow, outflow, walls, far fields, free surface are provided or could be reasonably estimated in order to facilitate CFD calculations

CFD Methods

Provide an overview of the methods used to analyze the test case. This should describe the codes employed together with the turbulence/physical models examined; the models need not be described in detail if good references are available but the treatment used at the walls should explained. Comment on how well the boundary conditions used replicate the conditions in the test rig, e.g. inflow conditions based on measured data at the rig measurement station or reconstructed based on well-defined estimates and assumptions.

Discuss the quality and accuracy of the CFD calculations. As before, it is recognized that the depth and extent of this discussion is dependent upon the amount and quality of information provided in the source documents. However the following points should be addressed:

  • What numerical procedures were used (discretisation scheme and solver)?
  • What grid resolution was used? Were grid sensitivity studies carried out?
  • Did any of the analyses check or demonstrate numerical accuracy?
  • Were sensitivity tests carried out to explore the effect of uncertainties in boundary conditions?
  • If separate calculations of the assessment parameters using the same physical model have been performed and reported, do they agree with one another?



Contributed by: Michael Breuer — Helmut-Schmidt Universität Hamburg

Front Page

Description

Test Case Studies

Evaluation

Best Practice Advice

References


© copyright ERCOFTAC 2024

Retrieved from "http://kbwiki.ercoftac.org/w/index.php?title=UFR_2-13_Test_Case&oldid=26677"