#  Rigid and Aeroelastic Analysis of Wind Induced Flow Behavior Around
Unscaled Tall Buildings using Numerical Techniques

V.A.U. De Alwisa* , P.H.T.D. Weerarathnea and K.K. Wijesundarab CONTACT V.A.U.
De Alwis<EMAIL_ADDRESS>aDepartment of Mechanical
Engineering, University of Peradeniya, Sri Lanka; bDepartment of Civil
Engineering, University of Peradeniya, Sri Lanka

###### Abstract

The study focuses on the wind loads acting on the standard Commonwealth
Advisory Aeronautical Council (CAARC) building model. Numerical modeling has
been used instead of employing wind tunnel experiments due to the requirement
of high physical space. This is mainly due to the superiority of CFD codes
included in turbulence models such as RANS and more precise LES. However, the
shortcoming arising through basing the result on numerical investigations is
compensated by direct comparison to experimental data available in the
literature. The study extends beyond the typical rigid building structure
giving account to the minor deformations resulting from the impact of the wind
force on an aeroelastic structure through coupled two-way fluid-structure
interaction while designing the building to have its natural fundamental
frequency of 0.2 Hz. An improved Smagorinsky-Lily model was used for all LES
models and the results were compared with available wind tunnel experimental
data. It was found that coupled LES analysis provided a better correlation to
wind tunnel data compared to rigid fluid domains with respect to pressure
distribution and wake formation despite the additional computation time taken.
However, all these readings were dependent on the boundary conditions which
need to be estimated concisely fur future use.

###### keywords:

CAARC Building, CFD, RANS, LES, Aeroelastic structure, Two-way FSI,
Smagorinsky-Lily

Hirt . (1978),Chen, Xu . (2020) Hirt . (1978) Hirt (1975) Hanson . (1982)
Hanson . (1986) Summers . (1986) Blocken . (2007) Yuan . (2014) Huang . (2007)
Koliyabandara . (2017) Mou . (2017) Koliyabandara . (2018) Dagnew . (2009)
Aboshosha . (2010) Akbay . (2018) Jansen . (1992) Chimakurthi . (1995) Chen,
Huang . (2020) Launder (1993) Tsuchiya . (1997)

##  1 Introduction

The popularity of tall buildings is growing due to the population growth and
the limited usable land in the major cities around the world. The geometrical
complexity and the maximum possible height of the buildings have already
reached a point where traditional methods for analyzing wind-induced responses
are obsolete due to the cost attached with it and the limited accuracy.
Moreover, Chen, Xu . (2020) concludes that conventional wind tunnel test
techniques (including HFBB, SMPSS and aeroelastic test techniques) and
advanced wind tunnel test techniques (including forced vibration test
techniques and hybrid aerodynamic-pressure/force balance test techniques) are
not fully capable of predicting wind-induced responses. As the height of the
building increases, it becomes more susceptible to wind loads. Therefore,
Computational Fluid Dynamics (CFD) provides a viable alternative for expensive
wind tunnel tests, at least in the preliminary design stage in the design to
determine wind-induced loads on high-rise buildings. But, even with the
modern-day computational power, it is impractical to obtain Direct Numerical
Solutions (DNS) to the Navier Stokes equations which represent the problem in
differential equations. As alternatives, Reynolds Averaged Navier Stokes
(RANS) and Large Eddy Simulation (LES) models are widely used for the
evaluation of wind effects on structures. RANS mainly relies on statistical
approaches that display a time-mean representation of the fluid flow. In
contrast, LES is a multi-scale computational modeling approach that offers a
more comprehensive way of capturing fluctuating turbulent flow by resolving
eddies formed due to turbulence. However, most of the studies available have
used the RANS approach instead of more accurate LES due to the high
computational power required for the latter.

Since the early 1980s, numerical studies of building aerodynamics have been
conducted. Hirt . (1978), one of the first papers dedicated to numerical
simulation of the wind action over bluff bodies, predicted that there are many
possibilities and considerable potential for achieving useful results in the
future due to hardware and software development of the computer resources. In
that particular study, a finite difference model is presented and applied to
some simple applications on bluff body aerodynamics through a solution
algorithm developed for transient fluid flows and presented in Hirt (1975).
There, the low numerical resolution of the grid in the vicinity of the bluff
bodies in basically every approximation method was highlighted as one of the
causes that contributes to the less accurate results.

The very beginning of investigating aerodynamics around buildings goes back to
1982. Hanson . (1982), Hanson . (1986) simulated wind flow around building
models with different configurations and compared to wind tunnel tests to
confirm the reliability by the means of experiments. The importance of using a
3D model instead of using 2D planes to evaluate the simulation is emphasized
in the above papers. Furthermore,Summers . (1986) discusses the inability to
accurately solve the wake region of the time-averaged flow around a bluff
surface-mounted obstacle in a boundary-layer wind tunnel. It is identified
that, with the approximate treatment of solid boundaries, simulations cannot
serve to accurately determine the structural loading of buildings. The
standard _k_ \- model was revised and a turbulence model was proposed by
Launder (1993) called the LK model. Murakami (1998) presented the further
developed MMK turbulence model addressing the issues of the LK model as
commented in Tsuchiya . (1997). In a more recent study, Koliyabandara . (2018)
compares 7 different turbulence models with available wind tunnel test data
and concludes that most of the turbulence models fail to accurately predict
pressure distribution of the leeward and side faces of the body due to the
flow separation. Therefore, the wind engineering community moved towards LES
to analyse wind loads and induced vibrations of building models due to complex
and unsteady turbulent flows, containing wake regions.

Murakami Mochida (1989), Murakami . (1990), Murakami (1993), Murakami (1997)
discuss turbulent modeling and applications of turbulence models to predict
the wind-induced vibration of building models. Murakami (1993) concludes that,
even though LES requires higher computational power, it provides higher
accuracy in results. The reason being, in LES, the time-dependent inflow
boundary is responsible for a more accurate representation of oncoming fluid
flow properties. Hence Dagnew . (2009) and Swaddiwudhipong Khan (2002)
recommended LES as a complementary tool for wind load evaluation. Huang .
(2007) performed a comprehensive analysis of the CAARC building model
employing numerical simulation where the building is considered as rigid and
aerodynamic coefficients and flow patterns around the building were predicted
through a CFD commercial software. Despite the fact that the dynamic
properties such as the natural fundamental frequency of the building are
discussed in the studies above, the coupled interaction of the building
configuration with the fluid domain is not taken into consideration.

So far, the Computational Wind Engineering (CWE) community has done a number
of numerical simulations based on wind effects over different building
configurations. While some of the numerical solutions of the above work focus
on problems such as interference effects between buildings (Summers . (1986)),
wind-driven environmental conditions and pedestrian comfort (Mochida Lun
(2008); Ramponi Blocken (2012) ; Stathopoulos Baskaran (1996); Yuan . (2014)),
others shed light on the wind interactions with structures (Huang . (2007);
Braun Awruch (2009); Koliyabandara . (2017); Mou . (2017); Chen, Huang .
(2020)). It is observed that the majority of the studies focus on numerical
analysis on rigid building models rather than aeroelastic building models.
Bathe Zhang (2004) suggests a developed scheme, which complies with
engineering practice for fluid-structure interaction problems and further
discusses the potential for an ideal scheme. Rugonyi Bathe (2001) employs
Lyapunov characteristic exponents to determine the long-term dynamic stability
of fluid-structure interaction systems, allowing them to distinguish between
chaotic and regular system behavior. Aboshosha . (2010) used Von Karman’s
spectrum and Davenport’s Coherency function to digitally create turbulent
velocity vectors, since LES in Ansys FLUENT package needed previous knowledge
of time-dependent velocity vectors of the atmospheric boundary layer. There,
the simulations were run to calculate the wind-induced response of tall
buildings that exhibit coupled modal behavior.

This study aims to counter most of the drawbacks that have not been addressed
in the previous studies described above so that to build a numerical
simulation that perfectly aligns with an experimental setup. The study
comprises several novelties. Mainly, the use of a partitioned coupling
approach between the building and wind domain has been the main aspect
highlighted in this study which has been barely touched in the literature in
the context of application for wind loads. Furthermore, even the studies
having the closest resemblance to the coupling code have not considered the
frequency modes of the original building which is taken into consideration in
this study. Moreover, an efficient block-based mesh method was introduced in
order to generate a finer mesh near the boundary region which gets coarser
when moving away from the building leading to optimized computational
performance. Furthermore, rather than using a scaled version of the actual
setup, the model was analyzed considering full-scale dimensions to avoid
inaccuracies that would cause by using different scaling theories. Finally, an
intra-study is conducted comparing three arbitrary simulation cases using the
same grid to compare the effect of turbulence and coupling methods for
pressure approximation.

For this purpose, three distinct analysis methods are used to analyze the
wind-induced response, along and across the CAARC building and the results are
compared with experimental data obtained at six research centers; The City
University (CU), University of Bristol (BU), Monash University (MU), National
Aeronautical Establishment (NAE), National Physical Laboratory (NPL), and
University of Western Ontario (UWO) (Melbourne, 1980), and also the
experimental readings obtained from Goliger and Milford (1988). The comparison
is focused to analyze the dependence of stiffness of the building, and the
dependence on whether the fluid flow analysis is RANS or LES has a significant
impact on the result. Initially, in Case 1 and Case 2, a comparison is drawn
between the dependence of different numerical models by comparing the results
generated for _k_ \- turbulence model and the Smagorinsky-Lilly subgrid-scale
model respectively for a rigid fluid model. Finally, the aeroelastic nature of
the building was also considered in Case 3 by implementing a two-way coupled
simulation setup between fluid and structural domains where the same
Smagorinsky-Lilly subgrid-scale model was used to estimate turbulence.

The RANS model, which is a way of resolving turbulent flows, solves time-
averaged Navier Stokes equations in a steady-state, whereas the LES model
predicts wind-driven reactions by filtering flow variables in order to resolve
large scales of motion and represent just the influence of small ones. The LES
model with the aeroelastic building configuration is expected to supersede the
LES model with the rigid building configuration since it emulates the natural
phenomena through two-way fluid-structure interactions.

##  2 Theory for turbulence models

###  2.1  K- model

According to Launder Sharma (1974), for low _Re_ formulation damping functions
are applied to the model coefficients in the turbulence equations. As by using
these model coefficients the mesh can be brought down to viscous sublayer (_y_
+$<$5), _k_ \- SST model is preferred for low _Re_ (Reynolds) number
applications. Therefore, in general the _k_ \- model is preferred for high
_Re_ number applications when the wall _y_ + is not within the buffer region
(5$<$_y_ +$<$30).

The _Re_ number for the flow in the fluid domain considered was measured at a
value of 1.36×104 and due to this _k_ \- model was used in this study as a
RANS turbulence model. Further, various literature have shown high accuracy
results for wind flows lying around these _Re_ number ranges once _k_ \- model
is used (Huang ., 2007). The theory associated with the standard _k_ \- model
is briefly described as follows. However, it is highly recommended to refer
FLUENT theory guide (Ansys, 2011).

The distinction between different RANS turbulent models is made with respect
to the Reynolds stress term in the Navier Stokes Equations customized for RANS
models as given in Equation 1.

$\frac{\partial(\rho U)}{\partial t}+\nabla\cdot(\rho UU)=-\nabla
p+\nabla.[\mu(\nabla U+(\nabla U)^{T})]+\rho
g-\nabla(\frac{2}{3}\mu(\nabla.U))-{\color[rgb]{1,0,0}\nabla.(\overline{\rho
U^{\prime}U^{\prime}}})$ (1)

All these symbols are used according to their standard definitions (Ansys,
2011). The Reynolds stress term is denoted by red and in order to evaluate
this commonly the Boussinesq hypothesis is used. The hypothesis can be stated
as in Equation 2.

$-\overline{\rho U^{\prime}U^{\prime}}=\mu_{t}(\nabla U+(\nabla
U)^{T})-\frac{2}{3}\rho kI-\frac{2}{3}(\nabla.U)I$ (2)

Here , _µ t_ denotes the eddy viscosity and _I_ is the standard symbol used
for turbulent intensity. It is obvious according to the equation that in order
to calculate the Reynolds stress term the eddy viscosity needs to be
estimated. Different methods have been used in the literature in order to
calculate this value.The most commonly used approach for eddy viscosity
formulation is by using transport equations for _k_ and terms and thus it
could be solved according to Equation 3.

$\mu_{t}=C_{\mu}\frac{\rho k^{2}}{\epsilon}$ (3)

The transport equation for _k_ is normally the same for all RNG, realizable
and standard _k_ \- models and it is written as in Equation 4.(The four terms
at the end are used for sources and sinks.)

$\frac{\partial(\rho\epsilon)}{\partial t}+\nabla.(\rho
Uk)=\nabla.[(\mu+\frac{\mu_{t}}{\sigma_{k}})\nabla
k]+P_{k}+P_{b}-\rho\epsilon+S_{k}$ (4)

However, this is not the same for the terms. The calculation for the term is
done according to the following Equation 5.

$\frac{\partial(\rho\epsilon)}{\partial t}+\nabla.(\rho
U\epsilon)=\nabla.[(\mu+\frac{\mu_{t}}{\sigma_{\epsilon}})\nabla\epsilon]+C_{1}\frac{\epsilon}{k}(P_{k}+C_{3}P_{b})-C_{2}\rho\frac{\epsilon^{2}}{k}+S_{\epsilon}$
(5)

Where _C 1_, _C 2_, _C 3_ denote the model coefficients for the turbulence and
their values vary between each of those models chosen among RNG, realizable
and _k_ \- models.The model coefficients used in the FLUENT code can be found
in Launder Sharma (1974). In each of these coefficients, separate damping
functions are included within to account for the damping that occurs in the
viscous sublayer. Due to this the _k_ \- model has the capability to solve the
turbulence dissipation upto the closest cell layer from the building wall
making the results accurate. Far away from the wall the damping function
approaches unity returning the high Reynolds number formulation of the _k_ \-
model. Since the results of _k_ \- models are much dependent on these
functions under low Reynolds number formulation, the model is generally
preferred for high _Re_ applications where separation and reattachment are not
abundant.

However, even if the turbulence dissipation is calculated accurately in order
to determine the forces, viscous shear stress should also be taken into
consideration. In order to estimate this correctly, wall functions are used in
FLUENT. The software uses two types of wall functions which are standard and
enhanced to calculate the viscosity. The use of the function depends on the
_y_ + values in the mesh region, and if the _y_ + does not lie between 5 and
30 the standard wall functions would be recommended. This is because the
linear estimate of viscosity falls in line with the viscosity predicted by
Direct numerical simulations except for the buffer region where they deviate
vastly from each other.

Upon generating the results for the RANS calculation, it was observed that the
minimum _y_ + recorded along the boundary of the building wall was 30, which
means none of the cells is within the buffer region and all of them would lie
in the log law region (_y_ +$>$30). However, it is said that the best practice
is to allocate the closest cells to the walls to the viscous sublayer due to
different inefficiencies in the log law model that occur when there are
adverse pressure gradients and strong curvature in the wall which is not seen
in the model discussed in the study. Furthermore, due to the high number of
elements that have already been established for this model it was impractical
to reduce the _y_ + further by decreasing the cell size based on the available
computational resources. Moreover, as an unscaled model was used and the
closest mesh block had a size of 0.25 m by employing an inflation layer to
reduce the _y_ + to the viscous sublayer would mean an abrupt increase in the
aspect ratio of those cells which would reduce the mesh quality and fail to
deliver the purpose expected by having a structured cartesian mesh.

###  2.2 Smagorinsky Lilly model

Similar to the RANS turbulence models, subgrid-scale models in FLUENT also use
the Boussinesq hypothesis to compute the subgrid-scale turbulent stresses
using an eddy viscosity approach. The equations used to calculate the subgrid-
scale turbulent stress and the strain tensor are shown in Equations 6 and 7
and all of them use the standard notations used in Ansys (2011).

$\tau_{sgs}=2\rho\upsilon_{sgs}S^{*}_{ij}-\frac{2}{3}k_{sgs}\delta_{ij}$ (6)

$S^{*}_{ij}=\frac{1}{2}(\frac{\partial U_{i}}{\partial x_{j}}+\frac{\partial
U_{j}}{\partial x_{i}}-\frac{\partial U_{k}}{3\partial x_{k}}\delta_{ij})$ (7)

All the subgrid-scale models available today differ by the turbulent viscosity
term in Equation 8. The original Smagorinsky-lilly model was developed in the
1960s and due to its defects in giving accurate predictions, FLUENT uses a
modified set of equations. The basic equations in developing the subgrid-scale
viscosity is given in Equation 8.

$\upsilon_{sgs}=l^{2}_{0}*\sqrt{2S_{ij}S_{ij}}$ (8)

Where $l_{0}$ is the subgrid length scale which is similar to the integral
length scale used in the RANS equations. Although the strain rate can be
calculated from resolved eddies, the subgrid length scale is difficult to be
determined directly. The original Smagorinsky Lilly model uses an estimation
of $C_{s}$Δ as the subgrid length scale where a value of 0.17 is used for the
Smagorinsky coefficient ($C_{s}$) and Δ gives the cell size. But this
coefficient is only accurate for a homogeneous isotropic turbulence scenario
and would be inaccurate if used for a flow near walls due to the
underprediction of shear. Furthermore, the original model would result in non-
trivial viscosity modeled near the wall regions making the whole fluid domain
filled with homogenous eddies. Due to this, a novel parameter called the
mixing length is introduced which is expressed as in Equation 9.

$l_{m}=\kappa y$ (9)

Where __is the Von Karman constant and _y_ is the distance from the wall. Due
to this the eddy size would decrease when moving towards the wall. As the
subgrid scale length scale cannot be greater than the mixing scale it could be
expressed as in Equation 10 (Ansys, 2011).

$L_{s}=min(\kappa d,C_{s}\Delta)$ (10)

Furthermore, deviating from the original model $C_{s}$ is also used as 0.1 in
FLUENT as it has been able to give accurate results for a wide range of
simulations. However, this model is also valid outside the buffer region and
different other adjustments such as the Van driest approximation have to be
used in order to create successful numerical results if _y_ + lies within the
buffer region.

##  3 Numerical Simulation Setup

###  3.1 Computational domain and mesh arrangement for fluid domain

For this study, the geometric model was selected according to standard full-
scale dimensions of CAARC building. The building was modeled as a 30 m×45
m×180 m cavity made in the fluid domain considered using the ANSYS Design
modeler modeling package. As for the first two cases out of the three, the
aeroelastic nature of the building is not taken into consideration; a mere
modeling of a cavity together with a static mesh is sufficient.

In deciding the dimensions of the fluid domain to be considered for the flow
around bluff bodies, special attention should be given to the obstacle effect
that arises due to inflow and outflow conditions (Murakami, 1998). This is
also to allow the boundary layer to develop fully so that the properties
within the vicinity of the building are captured efficiently. After
considering different sets of guidelines, the dimensions of the domain were
concluded to be as in Figure 1, where _H,Dx, Dy_ are building dimensions and
_H_ = 180 m, _Dx_ = 30 m and _Dy_ = 45 m.(Koliyabandara ., 2018).

(a) Side view of the fluid domain

(b) Top view of the fluid domain

Figure 1: Dimensions of the computational fluid domain

As the cavity is confined to the middle, the interference of the flow pattern
at the boundaries would hardly affect the results captured around the
building. Furthermore, both along-wind and across-wind pressure distributions
are captured in this analysis by plotting the results along the wall boundary
at four sides as shown in Figure 2. A parameter called (_x_ /_L_) is
introduced along the perimeter and consequently, the following values are
established in the corners of the building.

Figure 2: Plot of x/L along the faces of the building.

Although the computational domain seems to be straightforward, the generation
of the mesh seems to be intricated due to the compromise that has to be made
between accuracy and computational efficiency based on the available
resources. Besides, the mesh size has to be large enough so that the
computational memory is sufficient enough to solve the computational matrix
and should be small enough to capture the maximum amount of turbulent kinetic
energy. According to Summers . (1986), the grid should be fine enough to hold
a minimum of 80 percent of turbulent kinetic energy.

Furthermore, the traditional mesh methods account to have a structured grid
whenever it’s possible to capture the flow near bluff bodies. Also, it is
essential for the mesh to be body fitted since it is vital to capture the flow
patterns near the building wall accurately. Due to this, it is important to
create a grid of varying sizes such that it is much finer close to the
buildings. The lately introduced “Cutcell” assembly meshing algorithm in ANSYS
meshing became certainly an excellent candidate which satisfies most of these
requirements. Unlike using a patch conforming tetrahedral mesh arrangement
close to the building due to the capability of FLUENT code to hold both
structured and unstructured grids in its solver as in (Huang ., 2007) a
cartesian Cutcell method provides a way to use a structured mesh wherever
possible. This not only decreases the computational time by reducing the
number of nodes thereby reducing the degrees of freedom, but also takes part
in h-refinement as polyhedral elements are formed at hanging nodes between
structured elements of different sizes (Balafas, 2014) as shown in Figure 3.

Figure 3: Formation of polyhedral elements at hanging nodes in Cartesian mesh

As it is seen in the mesh arrangement in Figure 4, a smooth transition is
obtained between mesh domains of varying sizes with the combination of
triangular and polyhedral elements by using the “body of influence” option
available in ANSYS meshing. This also enables to keep the grid sizes smaller
close to the building and paves the way to use large mesh sizes far away from
the building. On the other hand, the use of such a method gives advantages
over multiple body meshing since a contact meshing is formed within contact
regions if traditional methods of assembly meshing are used. This would have
not only increased the node count but would have displayed discontinuing
streamlines due to the elements formed at the interface with negligible
thickness. Table 1 gives the element size in each mesh region and Figure 5
shows the division of these mesh blocks.

To decide on the grid sizes, as described earlier the percentage of the
kinetic energy-resolved by the mesh should be considered. As this study is
mainly focused on finding the pressure distribution around the building
accurately, the size was decided in such a way to solve the maximum amount of
turbulent kinetic energy near the mesh regions very close to the building
cavity. To calculate the lowest mesh size, initially, a parameter called the
integral length scale needs to be calculated as shown in Equation 11.

$l_{o}=\frac{k^{3/2}}{\epsilon}$ (11)

In this expression, turbulent kinetic energy solved by the mesh is denoted by
_k_ and the turbulent dissipation rate is denoted by . To hold at least 80
percent of the turbulent kinetic energy, the minimum grid length should be
less than at least ${1/5}^{th}$ of the integral length scale $l_{0}$.

The value of $l_{0}$ computed based on the turbulent kinetic energy and the
turbulence dissipation rate yielded a value of 3.72 m which gives a minimum
grid length of 0.74 m. However, the two blocks closest to the building cavity
are of mesh sizes 0.25 m and 0.5 m respectively which means that most of the
turbulent kinetic energy close to the building cavity is solved by the mesh
used for the Large-eddy simulation.

(a) Unzoomed view

(b) Zoomed view

Figure 4: Dimensions of the fluid domain Figure 5: Complete plan view
illustration of mesh blocks

Positions and the grid sizes of the mesh blocks  Distance from the building to
the mesh block surface (m) Mesh block Mesh size (m) From surface 1,2,3 From
surface 4 From surface 5 1 0.25 2.95 5 2.5 2 0.4 2.5 5 2.5 3 0.5 5 10 5 4 1 10
20 10 5 1.2 20 40 20 6 1.6 40 80 40 7 3.2 80 80 60

Also since wake formation is observed behind the building, the grid was
created in a way that finer mesh sizes dominate the rear side of the building
than at the front as shown in block sizes in Figure 5. Note that in addition
to the blocks shown, the global mesh size for the remaining domain surrounding
these blocks was set to 6.4 m.

The complete grid generated for the fluid domain consisted of 38 million
elements and the computations were performed in a workstation having 24 cores
and 128 GB of memory.

###  3.2 Boundary conditions

To draw out an effective comparison between experimental and simulation
results, it is mandatory to obtain a clear idea about the nature of the
boundary conditions used when conducting the experiment. Mainly, the inlet
boundary conditions should correlate to the wind conditions used in the wind
tunnel experiment to get maximum efficacy of the simulation.

Usually, two types of inlet profiles are used for boundary layer conditions.
One uses a power law exponent, whereas the other uses a function related to
logarithmic laws. Different studies have used these two at multiple occasions
depending on the preferences of the authors involved. In the study of Obasaju
(1992), a logarithmic law has been used to estimate the boundary layer, and
Huang . (2007) has used the power law exponent profile. In this study, the
power law exponent profile has been followed according to Equation 12 due to
the excellent comparison obtained in Huang . (2007) relative to experimental
readings of Melbourne (1980). and the corresponding plot for the profile is
shown in Figure 6.

$\frac{U}{U_{H}}=(\frac{Z}{Z_{H}})^{a}$ (12)

Figure 6:  Power-law exponent profile used at the velocity-inlet

The terminology used for this expression can be summarized as follows.

_U_ gives the wind velocity at the preferred height; $U_{H}$ gives the speed
of the wind at reference height. (maximum height of the domain); _Z_ denotes
the preferred height and $Z_{H}$ denotes the maximum height of the domain.
Finally ‘ _a_ ’ gives the power law exponent which has been estimated to be
0.28 in Melbourne (1980).

###  3.3 Computational domain and mesh arrangement for structural domain

The significance of this study is mainly to determine the effect generated by
the Aeroelastic nature of the building. The building structure was modelled as
a simple hollow cantilever beam of rectangular shell cross section fixed to
the ground. The thickness of the shell was determined such that the building
shows a fundamental natural frequency of 0.2 Hz according to Huang . (2007).

The shell structure was modelled using cladding as the material of Modulus of
Elasticity of 25 GPa. To further emulate the behavior of a building, a
combination of different mesh elements was used for the building structure.
The shell was modeled using standard shell 181 elements due to the advantages
it gives with respect to solution time, operational capacity, stability and
accuracy in contrast to the use of solid elements (İrsel, 2019). Moreover, 39
interior floors touching the four walls were created to enhance the structural
stability, which were also modeled using 4 node 6-DOF shell 181 elements.
Furthermore, columns were embedded in addition to the plates and the building
shell. The resulting structure showed rigidity to forces of the magnitude of
wind loads and the non-linear deformations which were present earlier were
eliminated. The dimensions of the building components were optimized such that
the concrete plates have a thickness of 0.85 m leading to a fundamental
frequency of 0.2 Hz obtained for the vibration. .

Consequently, it was observed that the mode shape for the fundamental
frequency of 0.2 Hz corresponded to the direction in which the deformation
acts once the wind load acts on the building surface and the modal frequencies
are given in Table 2.

Frequency modes  Mode Frequency(Hz) 1 0.20 2 0.26 3 0.92 4 1.05 5 1.10 6 1.17

##  4 Two-Way Fluid Structure Interaction

###  4.1 Overview

As far as two way fluid structure analysis is concerned, there could be two
approaches; either a monolithic approach or a partitioned approach (Akbay .,
2018) which is used more commonly. The ANSYS Workbench uses a partitioned
coupling framework that enables support for data mapping in shared memory and
distributed parallel processors which makes simulation times lower
(Chimakurthi ., 1995).

A brief description of the theoretical background relevant to this study is
provided in this section for ease of understanding. For more information it is
highly recommended to refer Ansys (2015). Two algorithms are usually used for
the data transfer between two different setups.

  1. 1.

Profile preserving algorithm - Used to transfer non-conserved quantities (eg-
displacement)

  2. 2.

Conservative profile preserving algorithm - Used to transfer conserved
quantities (eg- force)

Both these algorithms work under four sub algorithms.

####  4.1.1 Data Pre-processing

These algorithms are used in the initial stage to create supplemental data on
mesh locations which are required at mapping and interpolation stages.

####  4.1.2 Mapping

Mapping algorithms are also divided into two based on the type of data
transfer algorithm. Thus there exist Bucket surface and General Grid Interface
(GGI) algorithms that are dedicated to Profile preserving and Conservative
algorithms respectively.

The Bucket surface algorithm is employed to assign weights required for
displacement mapping in this study. Here the mapping takes place between the
nodes on the target side with mesh elements on the source side. Therefore the
initial step is to focus on dividing the mapping source mesh into an imaginary
structured grid; each grid section here is called a “Bucket”. As the system
coupling algorithm does not support interactions with 2D buckets, bucket grids
are generated only for a 3D grid. Subsequently, every node would be linked
with a generated bucket. To ensure proper linking takes place, a checking loop
is activated which traces all source elements to find target elements. This
isoparametric mapping takes place according to the nonlinear Equation 13 given
below.

${\hat{x}}=[N_{a}^{e}(\zeta)]\\{x_{a}^{e}\\}$ (13)

In this expression, acts as vector element local-coordinates which correspond
to global coordinates of the target node which is $\hat{x}$. Also, $N_{a}^{e}$
denotes the linear shape functions corresponding to the source element,
whereas $x_{a}^{e}$ denotes global coordinates of element local node $a$. This
mapping algorithm also includes tolerance levels when mapping between nodes
and elements and more details about these can be found on Jansen . (1992).

The General Grid Interface algorithm is used for force mapping functions in a
way such that element faces on both source and target sides are divided by the
number of nodes, and the resulting faces are converted into 2D quadrilaterals
which are eventually turned into “control surfaces”. The final weight
contributions for mapping are evaluated through an accumulation of these
control surface contributions. More details on this algorithm can be found on
Galpin (1995).

####  4.1.3 Interpolation

This is where target node values are provided with the aid of source data and
mapping weights are generated by the use of mapping algorithms. As given in
Equation 14 mapping weights are applied.

$\phi=\sum_{i=1}^{n}w_{i}\phi_{i}$ (14)

$\phi$ denotes the target node, thereby making $\phi_{i}$ the value at $i$ th
source node. $w_{i}$ denoted the associated weight. Value of $n$ depends on
the mapping algorithm used. Accordingly, for the bucket surface algorithm, $n$
implies the source element node number while for GGI mapping it denotes the
number of intersected areas on the control surface.

After this stage, Post processing algorithms are used on interpolated data to
increase the convergence. Two algorithms are usually used for this purpose
which could be a ramping or under-relaxation algorithm; both of which are
explained in Ansys (2015). Collection of all these algorithms would complete
the data transfer algorithm. After each iteration undergoes all the steps in
the data transfer algorithm, the root mean square is checked for data
transfers in both ways. This RMS value is calculated according to Equation 15
.

$RMS=\sqrt{\overline{(\hat{\Delta_{l}}})^{2}}$ (15)

In here, the parameter $\hat{\Delta_{l}}$ is the normalized data transfer
value which is itself calculated as in Equation 16.

$\hat{\Delta_{l}}=\frac{\Delta_{l}}{0.5\times((max|{\phi}|-min|{\phi}|)+\overline{|{\phi}|})}$
(16)

Where $\phi$ and $l$ denotes the values and locations of the data transfer
values respectively. This is the general data transfer code that is used in
the system- coupling database which is employed in this study. It should be
noted that these algorithms could be used only for triangular and
quadrilateral elements between two data exchanging surfaces. Although
polyhedral elements were used for this study, none of them were included
between mesh grid transitions, which led to the successful compatibility of
the algorithms to the grid generated.

###  4.2 Functioning of two way- FSI

Initially, individual solvers relevant to Structural and fluid setups are
modified to enable the coupling between the two domains. Thus, the building
model in the Structural solver is arranged in a way such that the building
floor is fixed to the ground and the building walls act as fluid system
couplings. Five couplings are formulated for the five walls and once the
simulation is initiated these walls transfer data with the fluid domain
according to Bucket surface and GGI algorithms . Moreover, in the fluid domain
setup, the entire mesh is set to a deformable dynamic mesh so that the grid
has the capability to keep contact with the fluid domain at each time step
involving structural deformation. Similar to the structural setup, the fluid
domain building walls are also set to “system coupling” regions so that the
solver identifies with what domains it needs to transfer data in the
structural setup.

Both these setups are centrally governed by the system coupling system and so
that the individual solvers of fluid analysis and structural analysis are
shared within this setup. Here, mainly data transfers are created such that
the forces on the fluid section are transferred towards the structural domain
according to GGI algorithm while in the same iteration displacement data from
the structural setup are shared with the fluid domain according to Bucket
surface algorithm. Thus this process repeats itself for each timestep until
every data transfer is converged leading this to a fairly time-consuming
process when compared to the rigid models. This iterative process is described
by the flow diagram in Figure 7.

Figure 7:  Flow diagram for the iterative scheme in Ansys system coupling

In addition to these data a coupled pressure solver and a second order
transient formulation were used for the solving process of the equations
involved. A time step of 0.1 s was able to achieve convergence for all time
steps and the setup was allowed to run for 150 time steps to get a stabilised
pressure variation along the building wall.

##  5 Results and Discussion

The results of the three cases : Rigid RANS model analysis, Rigid LES model
analysis and aeroelastic LES model analysis were taken adhering to the main
objective; which is to make a comparison between simulation models to find out
which gives the closest approximation to the experimental phenomena such that
costly experiments can be replaced by simulations in future at least for the
preliminary level of design. For this purpose, the results were mainly
compared with experimental results obtained from the Melbourne (1980) study at
2/3rd the height of the building and from Goliger Milford (1988) study at the
1/3rd height. A comparison is initially drawn with respect to the normalized
pressure variation (Equation 17) obtained around the building which would in
turn capture all three responses related to a study on wind loads.

$Normalized\,Pressure(P^{\prime})=\frac{p}{\frac{1}{2}\rho u^{2}_{H}}$ (17)

Where $P$ is the dynamic pressure observed around the building, $\rho$ is the
density of air and $u_{H}$ gives the velocity of the wind boundary layer at
the top of the building.

###  5.1 Case 1 – Rigid RANS model analysis

Results obtained for the normalized pressure coefficients at 2/3rd of the
height of the building were plotted against _x_ /_L_ as shown in Figure 8 and
compared them with results obtained from the NPL study of Melbourne (1980).
Only the NPL study has been used from Melbourne (1980) since it was done using
the closest boundary conditions to the present study and it has shown the
closest resemblance to simulation results in previous studies.(Huang ., 2007;
Braun Awruch, 2009)

Figure 8: Normalised pressure variation along the building wall at a height of
120 m for Case 1

Overall, it is clear that along most of the faces the normalized pressure has
been overpredicted to the results obtained from the Melbourne (1980) study. In
total, along the 4 faces, about 4 experimental readings from the Melbourne
(1980) study have been superimposed on the simulation curve obtained for the
RANS study. Although the results have been predicted very precisely in the
front face of the building, the rear side of the building has been unable to
exhibit accurate results. There is a substantial overprediction of. This is
probably because of the inability of RANS to correctly predict the wake
formation behind the building. This is most often the case of the RANS models
that happen due to eliminating fluctuations in turbulence due to averagings.
This can be more clearly seen by comparing the results at another building
height (60 m from the ground) as in Goliger Milford (1988). This study has
fewer experimental points and was done under two turbulent intensities and the
comparison with these results at 1/3rd the height of the building is shown in
Figure 9.

Figure 9: Normalized pressure variation along the building wall at a height of
60 m for Case 1

From Figure 9, it is clear that the _k_ \- model has the ability to predict
the pressure variation at the front face at multiple building heights.
However, within the vicinity of other faces the deviations from the
experimental results have been significant despite the correlation observed in
the shape of the curve. To obtain the reasoning behind this, further
investigation was carried out by looking at the eddy formation and turbulence
close to the building.

Thus, the plot for velocity streamlines and the pressure contours at the
sectional front and plan views are plotted in the same figure as shown in
Figure 10 (a) and (b), respectively.

(a) Sectional front view

(b) Sectional plan view at building height of 120 m

Figure 10: Velocity streamlines and pressure variation observed for Case 1

A very high positive pressure is obtained once the wind comes and strikes the
frontal face of the building thereby resulting in flow separation along
building edges. This results in a positive pressure region in front of the
building and also a recirculating region in the wake area which ultimately
results in a pressure difference creating a net force in the along-wind
direction. It is also clear that the flow separation in the frontal face
happens in two directions whereas most of the streamlines flow down along the
building converging into a single eddy and the flow striking very close to the
top of the building tends to separate towards the wake region forming a large
eddy at the top end of the building. It is further clear the streamline flow
observed in the plan view is very close to being symmetric and two clear large
eddies are formed. This is the main reason to observe a symmetric normalized
pressure variation and hence predicts the pressure at both sides of the
building to be equal, which is inaccurate in reality. However, even if the
details are lesser, this simulation run took only 1/10th of the computational
effort when compared to running the solution with subgrid-scale models.

###  5.2  Case 2 -Rigid LES model analysis

Figure 11 and Figure 12 show the pressure variation of the building at 120 m
and 60 m height respectively once a rigid model was simulated by using the
Smagorinsky SGS turbulence model.

Figure 11: Normalized pressure variation along the building wall at a height
of 120 m for Case 2 Figure 12: Normalized pressure variation along the
building wall at a height of 60 m for Case 2

In Figure 11, roughly 8 points from the simulation data have been successfully
superimposed to the experimental data for the NPL study suggesting better
correlation to the RANS model. At first glance, one would observe that as in
the RANS model the front face of the building shows great alignment with all
the experimental readings. Although, the dip in normalized pressure at the
first side of the building has been overestimated in the LES rigid model by a
fairly large margin, the pressure at the back wall has been predicted to a
high accuracy level in the LES analysis suggesting that the wake formation
behind the building has been captured to high precision. This is further
elaborated in the velocity streamline and pressure contour formation depicted
in Figure 13.

(a) Sectional front view

(b) Zoomed sectional front view

(c) Sectional plan view at building height of 120 m

Figure 13: Velocity streamlines and pressure variation observed for Case 1

Similar to the Case 1, Upon striking the building wall, air streamlines
separate into two directions such that eddies are formed close to the ground
from the streamlines that travel down. However, the contrasting behavior is
seen in flow separation at the top building edge as shown in Figure 13 (a).
Upon zooming into the building top it was observed that a large number of tiny
eddies are formed near wake separation suggesting a high percentage of
turbulence resolvement. Moreover, due to this high amount of small amplitude
vibrations could result at the top of the building which would not be captured
by a rigid building structure. The plan view in Figure 13 (c) also shows an
unsymmetric eddy distribution of various sizes amalgamating to form a more
complete wake region of lower pressure values.

###  5.3 Case 3– Aeroelastic LES model analysis

To plot the results of pressure variance when the building undergoes
deformation the usual approach of plotting the pressure along the building
wall line could not be used. This is because due to the aeroelastic nature the
position of the building would be different from the initial position and its
coordinates are unknown. Hence a plane was defined at a building height of 120
m and the pressure variation was plotted along the line (polyline) at which
this boundary intersects with the building. The normalized pressure variation
at 2/3rd of building height was obtained accordingly and plotted as in Figure
14.

Figure 14: Normalized pressure variation along the building wall at a height
of 120 m for Case 3 Figure 15: Normalized pressure variation along the
building wall at a height of 60 m for Case 3

In this variation, in Figure 14, it is clearly seen that the pressure
variation along the Z=120 line has been able to trace a high majority of
points for readings obtained for NPL in Melbourne (1980). Thus, in total, the
curve has been able to recreate 12 of 15 data points in the NPL experiments
conducted which supersedes the precision shown by Huang . (2007) and Braun
Awruch (2009) studies. Furthermore, the study of Goliger Milford (1988)
determined experimental pressure values predicted at the 1/3 rd of the
building height and it has also been used to determine the degree of accuracy
of this aeroelastic study as in Braun Awruch (2009) as in Figure 15.

According to Figure 15, the pressure variation in the front face lies midway
between the low turbulence and high turbulence experiments conducted by
Goliger and Milford (1988). This is similar to the pressure behavior at the
front face observed in Braun Awruch (2009) despite the small over-prediction
in Braun Awruch (2009). However, this may be due to the change in the
considered Reynolds number for that study and the present study. The almost
constant pressure approximation in the side face matches with the results
obtained in Braun Awruch (2009) where the simulation curve lies close to the
experimental data. However, the major difference in the two studies is within
the rear wall boundary of the building. As observed in Braun Awruch (2009) the
pressure variation at the rear side seem to deviate largely from the results
gained by Goliger Milford (1988), whereas this study has managed to show a
close approximation even to this wake region by the increased normalized
pressure midway when moving from one end to the other. Thus it is quite clear
that this study has the capability to predict the results within the vicinity
at multiple building heights with reasonable accuracy.

Similar to the velocity and pressure plots in the previous cases, the velocity
distribution streamlines and pressure contours were plotted as in Figure 16.
As expected the behaviors obtained closely resembled the observations made in
studying Case 2 with respect to the wake formation, wake separation and the
suction region. However, the eddy positions seem to be the only variable that
could be compared between the two as it is clear that the eddies have shown
different displacements which could have been due to the displacements that
occur in the fluid mesh as a result of the two-way coupling. Moreover, more
eddies are formed at the rear side of the building which is due to the added
flexibility of the building.

(a) Sectional front view

(b) Sectional plan view at building height of 120 m

Figure 16: Velocity streamlines and pressure variation observed for Case 3

####  5.3.1 Aeroelastic response

To study the aeroelastic nature the directional wind displacements of the
building are studied in along-wind and across-wind directions. Figure 17 shows
the variation in displacement of the top of the building (maximum
displacement) along the direction of wind propagation which corresponds to the
mode shape of the fundamental frequency. According to the variation it is
clear that the building vibrations are undergoing sinusoidal displacements
with time about a mean value of 4.5 mm with decreasing amplitude over time. As
structural damping is not incorporated into the building structure, the main
cause for this would be the aeroelastic damping caused in the fluid eddies.
The displacement observed is completely positive due to the net pressure force
acting on the building as a result of the difference in pressure at frontal
and rear faces.

Figure 17: Damped along-wind directional displacement of the building top

Furthermore, directional displacement was also considered in _y_ direction
(across-wind response) as shown in Figure 18.

Figure 18: Across-Wind directional displacement of the building top  Figure
19: Across-wind directional acceleration of the building top

The directional deformations do not approach zero according to the obtained
results. Furthermore as given in Figure 19 the acceleration of the building in
the _y_ direction tends to decrease initially but then tend to follow a
constant peak to peak variation suggesting an ever present fluctuating force
existing in the lateral direction. Thus a fluctuating across-wind response is
obtained that lies completely within the positive _y_ axis. This is mainly due
to the turbulence prediction that is given by the Smagorinsky model. As
unbalanced eddies are formed in the two sides a net force is produced towards
the lateral direction thus vibrating the building back and forth in addition
to the wind induced pressure along _y_ direction. The combined effect of these
forces in perpendicular directions would result even in moments that would
induce torsional vibrations to the building.

###  5.4 Comparison

This section in the paper is utilized to discuss the bottom line of the
findings taken from the three cases studied. Since only the NPL study in
Melbourne (1980) has boundary conditions which is closest to this study, the
discussion was carried out comparing the normalized pressure at building
heights of 120 m and 60 m respectively to the findings of NPL study. However,
the comparison at 1/3rd of the height of the building was done using only
Goliger Milford (1988) since much data is not available for this parameter.The
results from all the cases are plotted for comparison purposes for 120 m of
building height as in Figure 20.

Figure 20: Plot of Normalized pressure along the building perimeter for Case
1, 2 and 3 at building height of 120 m Figure 21:  Plot of Normalized pressure
along the building perimeter for Case 1, 2 and 3 at building height of 60 m

The three curves plotted in the same axes pave the way to obtain a comparison
with all three cases. In Figure 20, the least difference among the cases is
obtained on the front face of the building. This should obviously be the case
as such fluid impingement on a wall could only cause a change in pressures
which cause vibrations to the building. The behavior shown implies that at the
building front face _k_ \- model acting on a rigid building domain is accurate
enough to generate an accurate pressure prediction. However, when considering
the regions where wake generation is involved it is clearly seen that RANS
modeling on a rigid structure would not provide acceptable results. Due to the
bending nature that is instilled in the building the aeroelastic model shows
very minute deviations relative to the other two involved cases suggesting
that once there is a flexible two-way coupling data transfer is efficiently
transferred through two models.

A similar comparison result was seen in Figure 21 as well where the simulation
results are compared to experimental values obtained at 1/3rd of building
height. Here the _k_ \- model showed a large deviation to the side and rear
faces of the building, whereas the rigid model that incorporated an LES
turbulence model was not able to show an elevated pressure at the rear face
compared to the side faces.However, this was not the case for the coupled
analysis, as it has been able to match its pressure variation with
experimental results.

To further elaborate the accuracy of the cases discussed a quantitative
comparison is done for the percentage deviation of the simulation results from
NPL results at building height of 120 m as shown in Figure 22.

Figure 22: Plot of Normalized pressure along the building perimeter for Case
1, 2 and 3 at building height of 60 m

Figure 22 shows that percentage error in Case 1 has been below 30% in all the
faces except for the rear face where flow separation and wake formation
occurs. At the rear face, error percentages have increased even beyond 40%
showing its inability to predict the wake accurately. Case 2 has shown
acceptable results, except at the corners where the error percentages have
plunged even beyond 50%. In contrast to both these cases, percentage errors of
Case 3 have been less than 20% for almost all the experimental results and
have been significantly less at the corner points due to the building
flexibility. Overall, average percentage errors of the cases around the
building have mounted to 19.7%, 18.5%, 12.7% for Cases 1,2 and 3 respectively,
whereas, once the front face is excluded the percentages have been reported as
22.2%, 16.6%, and 12.5% respectively suggesting the superiority of the coupled
analysis.

Furthermore, important observations were made on behalf of the velocity
streamlines and wake formation due to the difference in pressure. All three
buildings tended to show flow separating in two directions upon striking the
building wall. However, discrepancies were looked upon with respect to the
wake formation and the vortice separation in the three cases. The RANS model
showed an incomplete wake formation behind the building filled with large
eddies. This portrayed the inability of the standard _k_ \- model to capture
the wake efficiently even when large Reynolds number flows are employed for
which the _k_ \- model with standard wall function is decided as the most
optimum method. In contrast, both Smagorinsky models were able to capture the
full effect of wake formation and the final two models differed only through
the eddy positions that resulted due to the structural displacement. To
discuss the accuracy of the current study further and to stretch its limits
beyond the scope of measuring the pressure at a single building height, the
pressure at 1/3rd building height was analyzed, and its results did not
deviate from the results as in any case in the literature. By the aeroelastic
analysis carried out it was verified that the displacements in along-wind
direction tend to dominate due to direct wind loads acting on the building,
but due to the aeroelastic damping of the wind the building tend to die out
its high amplitude vibrations to the mean value in the long term. More
importantly, displacements were also observed in the lateral directions where
forces would be borne due to the difference in eddy patterns; and convincingly
these displacements did not show a consistent damping behavior that would
result in a permanent acceleration in the lateral direction.

##  6 Conclusion

This work focused on creating an accurate numerical simulation setup for the
purpose of studying the wind flow around tall buildings, which has been
previously analyzed using various numerical and experimental techniques. Main
goal of the study was to devise the setup which would duplicate the same
results given by an experimental setup performed at identical conditions;
given that available computational resources are used at an optimum level.
Comparisons were drawn between different cases for the same CFD grid with
respect to the viscous model for fluid flow and nature of the structural
domain. An efficient mesh method was introduced with structured blocks having
various element sizes and which had tetrahedral, hexahedral mostly and
polyhedral elements at locations which had grid size transitions . When the
building model was considered to be aeroelastic, the structure was designed to
comprise of components with dimensions which would emulate the resonance
frequencies of the actual building. Furthermore, the standard system coupling
algorithms in FLUENT were used for the aeroelastic analysis as a partitioned
coupling method for the first time in a wind engineering application.
Important findings obtained from this research could be postulated as follows.

  * •

The pressure approximation around the building is highly dependent on the
nature of the velocity profile and the turbulent intensity profile used.
Therefore, always care should be taken to compare the simulation results with
experiment results obtained at similar boundary conditions to get a reliable
comparison.

  * •

The frontal face of the building would provide accurate pressure predictions
independent of the turbulence model and the nature of the structural domain.
At each of the cases the highest pressure was observed at the frontal face of
the building where the fluid flow separated into both upward and downward
directions. Therefore, to predict the forces acting on the frontal face
minimum computation resources could be used, while the $y$+ values stay
outside the buffer region.

  * •

A Reynolds Averaged method such as the _k_ \- model would not be able to
resolve a large percentage of the turbulent kinetic energy. The resulting flow
would create two large eddies which are symmetric along the central axis of
the building passing perpendicular to the sectional plan view. Thus this
symmetricity produces an even pressure distribution in the two shorter sides
of the building. Moreover, the normalized pressure distribution in faces other
than the frontal face could not show comparable agreement to experimental
results for the building heights discussed, especially at the rear face
suggesting RANS modeling would not capture the wake region accurately.

  * •

The use of the Smagorinsky- Lilly model resulted in a more complete wake
generation and thus consisted of eddies of much smaller sizes. Further, no
symmetricity was observed around any axes for eddy patterns and pressure
variations. A much better correlation was observed with experimental results
for the wake region suggesting the accuracy of the LES simulations. However,
small inaccuracies are caused due to the displacements that happen in the
structural domain which are not taken into account. However , a rigid LES
model is sufficient to extract results of a model which would not show
substantial structural displacements.

  * •

The coupled analysis could not show considerable changes in eddy patterns
relative to the rigid case as the deformations do not occur at a large scale.
However, when the pressure was observed it showed better correlation than the
rigid case and results almost overlapped with experimental results. Therefore
this method is suitable to fine tune the results obtained for a LES based
rigid model study to increase the accuracy. However, this comes at the expense
of additional computational time due to the check for convergence that happens
for each time step for the data transfer between the two domains.

  * •

If structural damping is not taken into consideration, a building under wind
load would show underdamped sinusoidal displacement in the along-wind
direction due to aeroelastic damping. When the wind acts perpendicular to the
front face there could not be a across-displacement due to wind load directly.
However, due to eddy formation and uneven pressure distribution a net force
would be created in the across-wind direction. This was proved to result in a
sinusoidal acceleration in the lateral direction.

In conclusion, the use of two -way fluid structure interaction is an excellent
method to obtain accurate results for wind loads acting on tall structures,
when there is sufficient computational power. However, still wind-tunnel tests
have an edge over numerical methods in terms of accuracy but both methods are
under constant development. This simulation setup could be further improved by
doing the study for various wind-incidence angles and also by considering the
interference effect caused by neighboring buildings. Also improvements could
be made with respect to data transfer and mapping algorithms, grid generation
and more reliable subgrid scale turbulence models.

## Acknowledgements

The authors sincerely acknowledge Department of Mechanical Engineering,
University of Moratuwa for providing software facilities for this study.

## References

  * Aboshosha . (2010) aboAboshosha, H., Alhefnawy, L., Fathelbab, F. Shamel, A.  2010\.  Wind Induced Vibrations of Tall Buildings Using CFD Wind induced vibrations of tall buildings using cfd.  The Fifth International Symposium on Computational Wind Engineering (CWE2010).
  * Akbay . (2018) akbayAkbay, M., Nobles, N., Zordan, V. Shinar, T.  2018\.  An Extended Partitioned Method for Conservative Solid-Fluid Coupling An extended partitioned method for conservative solid-fluid coupling.  374\.  https://doi.org/10.1145/3197517.3201345  10.1145/3197517.3201345
  * Ansys (2011) ansthAnsys, I.  2011\.  ANSYS FLUENT theory guide Ansys fluent theory guide.  Canonsburg, Pa794.
  * Ansys (2015) ansscAnsys, I.  2015\.  ANSYS System Coupling User’s Guide Ansys system coupling user’s guide.  Canonsburg, Pa.
  * Balafas (2014) balaBalafas, G.  2014\.  Polyhedral mesh generation for CFD-analysis of complex structures Polyhedral mesh generation for cfd-analysis of complex structures.  Diplomityö. Münchenin teknillinen yliopisto.
  * Bathe Zhang (2004) bathBathe, KJ. Zhang, H.  2004\.  Finite element developments for general fluid flows with structural interactions Finite element developments for general fluid flows with structural interactions.  International journal for numerical methods in engineering601213–232.
  * Blocken . (2007) blockenBlocken, B., Carmeliet, J. Stathopoulos, T.  2007\.  CFD evaluation of wind speed conditions in passages between parallel buildings—effect of wall-function roughness modifications for the atmospheric boundary layer flow Cfd evaluation of wind speed conditions in passages between parallel buildings—effect of wall-function roughness modifications for the atmospheric boundary layer flow.  Journal of Wind Engineering and Industrial Aerodynamics959-11941–962.
  * Braun Awruch (2009) braunBraun, AL. Awruch, AM.  2009\.  Aerodynamic and aeroelastic analyses on the CAARC standard tall building model using numerical simulation Aerodynamic and aeroelastic analyses on the caarc standard tall building model using numerical simulation.  Computers & Structures879-10564–581.
  * Chen, Huang . (2020) chenChen, Z., Huang, H., Tse, K., Xu, Y. Li, CY.  2020\.  Characteristics of unsteady aerodynamic forces on an aeroelastic prism: A comparative study Characteristics of unsteady aerodynamic forces on an aeroelastic prism: A comparative study.  Journal of Wind Engineering and Industrial Aerodynamics205104325.  https://doi.org/10.1016/j.jweia.2020.104325
  * Chen, Xu . (2020) zeng20Chen, Z., Xu, Y., Huang, H. Tse, KT.  2020\.  Wind tunnel measurement systems for unsteady aerodynamic forces on bluff bodies: review and new perspective Wind tunnel measurement systems for unsteady aerodynamic forces on bluff bodies: review and new perspective.  Sensors20164633.
  * Chimakurthi . (1995) chimaChimakurthi, S., Reuss, S., Tooley, M. Scampoli, S.  1995\.  ANSYS Workbench System Coupling: a state-of-the-art computational framework for analyzing multiphysics problems Ansys workbench system coupling: a state-of-the-art computational framework for analyzing multiphysics problems.
  * Dagnew . (2009) dagnewDagnew, AK., Bitsuamalk, GT. Merrick, R.  2009\.  Computational evaluation of wind pressures on tall buildings Computational evaluation of wind pressures on tall buildings.  11th American conference on Wind Engineering. San Juan, Puerto Rico. 11th american conference on wind engineering. san juan, puerto rico.
  * Galpin (1995) galpinGalpin, H., Broberg.  1995\.  Three Dimensional Navier Stokes Predictions of Steady State Rotor Three dimensional navier stokes predictions of steady state rotor.
  * Goliger Milford (1988) goliGoliger, A. Milford, R.  1988\.  Sensitivity of the CAARC standard building model to geometric scale and turbulence Sensitivity of the caarc standard building model to geometric scale and turbulence.  Journal of Wind Engineering and Industrial Aerodynamics311105–123.
  * Hanson . (1982) hans82Hanson, T., Smith, F., Summers, D. Wilson, C.  1982\.  Computer simulation of wind flow around buildings Computer simulation of wind flow around buildings.  Computer-Aided Design14127–31.
  * Hanson . (1986) hans86Hanson, T., Summers, D. Wilson, C.  1986\.  A three-dimensional simulation of wind flow around buildings A three-dimensional simulation of wind flow around buildings.  International journal for numerical methods in fluids63113–127.
  * Hirt (1975) hirt75Hirt, C.  1975\.  A numerical solution algorithm for transient fluid flow A numerical solution algorithm for transient fluid flow.  Los Alamos Scientific Laboratory Report.
  * Hirt . (1978) hirtHirt, C., Ramshaw, J. Stein, L.  1978\.  Numerical simulation of three-dimensional flow past bluff bodies Numerical simulation of three-dimensional flow past bluff bodies.  Computer Methods in Applied Mechanics and Engineering14193–124.
  * Huang . (2007) huangHuang, S., Li, Q. Xu, S.  2007\.  Numerical evaluation of wind effects on a tall steel building by CFD Numerical evaluation of wind effects on a tall steel building by cfd.  Journal of Constructional Steel Research635612–627.
  * İrsel (2019) irselİrsel, G.  2019\.  The effect of using shell and solid models in structural stress analysis The effect of using shell and solid models in structural stress analysis.  Vibroengineering PROCEDIA27115–120.
  * Jansen . (1992) jansenJansen, K., Shakib, F. Hughes, TJ.  1992\.  Fast projection algorithm for unstructured meshes Fast projection algorithm for unstructured meshes.
  * Koliyabandara . (2017) koli17Koliyabandara, S., Jayasundara, H. Wijesundara, K.  2017\.  ANALYSIS OF WIND LOADS ON AN IRREGULAR SHAPED TALL BUILDING USING NUMERICAL SIMULATION Analysis of wind loads on an irregular shaped tall building using numerical simulation.  ICSECM2017-456.
  * Koliyabandara . (2018) koli18Koliyabandara, S., Jayasundara, H. Wijesundara, K.  2018\.  Evaluation of Different Turbulence Models in Determining Wind Loads on Tall Buildings Evaluation of different turbulence models in determining wind loads on tall buildings.
  * Launder (1993) lau93Launder  1993\.  Modeling flow-induced oscillations in turbulent flow around a square cylinder Modeling flow-induced oscillations in turbulent flow around a square cylinder.  ASME Fluid Engineering conference 1993. Asme fluid engineering conference 1993.
  * Launder Sharma (1974) launderLaunder, BE. Sharma, BI.  1974\.  Application of the energy-dissipation model of turbulence to the calculation of flow near a spinning disc Application of the energy-dissipation model of turbulence to the calculation of flow near a spinning disc.  Letters in heat and mass transfer12131–137.
  * Melbourne (1980) melMelbourne, W.  1980\.  Comparison of measurements on the CAARC standard tall building model in simulated model wind flows Comparison of measurements on the caarc standard tall building model in simulated model wind flows.  Journal of Wind Engineering and Industrial Aerodynamics61-273–88.
  * Mochida Lun (2008) mochidaMochida, A. Lun, IY.  2008\.  Prediction of wind environment and thermal comfort at pedestrian level in urban area Prediction of wind environment and thermal comfort at pedestrian level in urban area.  Journal of wind engineering and industrial aerodynamics9610-111498–1527.
  * Mou . (2017) mouMou, B., He, BJ., Zhao, DX. Chau, Kw.  2017\.  Numerical simulation of the effects of building dimensional variation on wind pressure distribution Numerical simulation of the effects of building dimensional variation on wind pressure distribution.  Engineering Applications of Computational Fluid Mechanics111293–309.
  * Murakami (1993) mura93Murakami, S.  1993\.  Comparison of various turbulence models applied to a bluff body Comparison of various turbulence models applied to a bluff body.  Computational Wind Engineering 1 Computational wind engineering 1 ( 21–36).  Elsevier.
  * Murakami (1997) mura97Murakami, S.  1997\.  Current status and future trends in computational wind engineering Current status and future trends in computational wind engineering.  Journal of wind engineering and industrial aerodynamics673–34.
  * Murakami (1998) mura98Murakami, S.  1998\.  Overview of turbulence models applied in CWE–1997 Overview of turbulence models applied in cwe–1997.  Journal of Wind Engineering and Industrial Aerodynamics741–24.
  * Murakami Mochida (1989) mura89Murakami, S. Mochida, A.  1989\.  Three-dimensional numerical simulation of turbulent flow around buildings using the k- $\varepsilon$ turbulence model Three-dimensional numerical simulation of turbulent flow around buildings using the k- $\varepsilon$ turbulence model.  Building and Environment24151–64.
  * Murakami . (1990) mura90Murakami, S., Mochida, A. Hayashi, Y.  1990\.  Examining the - model by means of a wind tunnel test and large-eddy simulation of the turbulence structure around a cube Examining the - model by means of a wind tunnel test and large-eddy simulation of the turbulence structure around a cube.  Journal of wind engineering and Industrial Aerodynamics3587–100.
  * Obasaju (1992) obaObasaju, E.  1992\.  Measurement of forces and base overturning moments on the CAARC tall building model in a simulated atmospheric boundary layer Measurement of forces and base overturning moments on the caarc tall building model in a simulated atmospheric boundary layer.  Journal of Wind Engineering and Industrial Aerodynamics402103–126.
  * Ramponi Blocken (2012) ramponiRamponi, R. Blocken, B.  2012\.  CFD simulation of cross-ventilation for a generic isolated building: impact of computational parameters Cfd simulation of cross-ventilation for a generic isolated building: impact of computational parameters.  Building and environment5334–48.
  * Rugonyi Bathe (2001) rugoRugonyi, S. Bathe, KJ.  2001\.  On finite element analysis of fluid flows fully coupled with structural interactions On finite element analysis of fluid flows fully coupled with structural interactions.  CMES- Computer Modeling in Engineering and Sciences22195–212.
  * Stathopoulos Baskaran (1996) stathStathopoulos, T. Baskaran, B.  1996\.  Computer simulation of wind environmental conditions around buildings Computer simulation of wind environmental conditions around buildings.  Engineering structures1811876–885.
  * Summers . (1986) sum86Summers, D., Hanson, T. Wilson, C.  1986\.  Validation of a computer simulation of wind flow over a building model Validation of a computer simulation of wind flow over a building model.  Building and Environment21297–111.
  * Swaddiwudhipong Khan (2002) swadSwaddiwudhipong, S. Khan, M.  2002\.  Dynamic response of wind-excited building using CFD Dynamic response of wind-excited building using cfd.  Journal of sound and vibration2534735–754.
  * Tsuchiya . (1997) tsu97Tsuchiya, M., Murakami, S., Mochida, A., Kondo, K. Ishida, Y.  1997\.  Development of a new k- $\varepsilon$ model for flow and pressure fields around bluff body Development of a new k- $\varepsilon$ model for flow and pressure fields around bluff body.  Journal of Wind Engineering and Industrial Aerodynamics67169–182.
  * Yuan . (2014) yuanYuan, C., Ng, E. Norford, LK.  2014\.  Improving air quality in high-density cities by understanding the relationship between air pollutant dispersion and urban morphologies Improving air quality in high-density cities by understanding the relationship between air pollutant dispersion and urban morphologies.  Building and Environment71245–258.