Computational Evaluation of Wind Pressures on Tall Buildings
Content
Computational evaluation of wind pressures on tall buildings
Agerneh K. Dagnew 1, Girma T. Bitsuamalk2, Ryan Merrick3
Research Assistant, Civil and Environmental Engineering department (CEE), International
Hurricane Research Center (IHRC), Florida International University (FIU), Miami, Florida,
USA, [email protected]
1
2
Assistant Professor of Wind/Structural Engineering, CEE, IHRC, FIU, Miami, Florida, USA
[email protected]
3
Senior Technical Coordinator, RWDI USA LLC, Miramar, Florida, USA,
[email protected]
ABSTRACT
At present, the wind engineering toolbox consists of wind-tunnel testing of scaled models, limited
full-scale testing, field measurements, and mechanical load/pressure testing. The evolution of
computational wind engineering (CWE) based on computational fluid dynamics (CFD)
principles are making the numerical evaluation of wind loads a potentially attractive
proposition. This is particularly true in light of the positive development trends in hardware and
software technology, as well as numerical modeling. The present study focuses on numerical
evaluation of wind pressures on tall buildings by using the Commonwealth Advisory
Aeronautical Council (CAARC) building model (Melbourne, 1980). The CARRC model has been
used extensively to study wind loading on tall buildings in wind tunnel studies and is usually
adopted for calibration of experimental techniques. Numerically obtained pressure coefficients
on the surface of CAARC building under different configurations of adjacent building are
compared with wind tunnel data collected at the RWDI USA LLC laboratory for the present
study and from literature. The present numerical simulation uses mostly Reynolds Averaged
Navier- Stokes equations (RANS) and Large Eddy Simulation (LES) for selected few cases.
KEY WORDS: Computational fluid dynamics, boundary layer wind tunnel, wind pressure, tall
building, RANS, LES
INTRODUCTION
Buildings, bridges, large span roof structures and other civil structures must be able to withstand
the external loads imposed by nature, at least to the extent that the disastrous damage of natural
force reduced to the acceptable limit (Irwin, 2007). Wind is one of the major forces responsible
for the catastrophic failure and loss of life. Therefore, accurate evaluation and prediction of wind
loads and proper mitigations are very important in reducing the adverse effects of wind in the
built environment. In addition to the mean and the background (due to turbulent fluctuations)
loads on rigid buildings, flexible structures will be subjected to resonant wind loads as well. The
primary source of the along-wind motion is the pressure fluctuations in the windward and
leeward faces due to the fluctuation in the approach flow and its interaction with the building.
Building codes and Standards usually provide loads along the wind direction for common shapes
1
in open and suburban terrain category perhaps with the exception of the AS-NZ 2002 code which
attempts to provide provisions in for the cross-wind direction as well. The cross-wind motion is
mainly caused by fluctuations in the separating shear layers. Torsional motion can be caused due
to imbalance in the instantaneous pressure distribution on each face of the building either due to
oblique wind directions, unsteadiness in the approaching flow, partial sheltering and interference
from surrounding buildings or due to own shape and dynamic structural properties. Studies
shows that for many high-rise buildings, the crosswind and torsional response may exceeds the
along wind response in terms of both limit state and serviceability requirements (Kareem, 1985).
Nevertheless, most existing standards, including ASCE07-05, only provides procedure for
evaluation of along-wind effects. For complex cases, the standards refer to physical model
testing in boundary layer wind tunnel (BLWT) facility.
The success of application of computational fluid dynamics (CFD) in aeronautical engineering is
very encouraging. Acknowledging the difference between streamlined and bluff body flows, the
use of computational fluid dynamics for predicting wind effects in the atmospheric boundary
layer appears very promising. This is particularly so considering the recent advances in hardware
and software technology, development of reliable sub-grid turbulence models and numerical
reproduction of inflow turbulence (Tamura 2008). At this stage of CWE application, however, a
systematic validation of CWE models through comparison with wind tunnel experiments shall
continue to enhance the confidence and warrant its use for practical applications.
Significant progress has been made in the application of CWE to evaluate wind loads on
buildings (e.g. Murakami and Mochida 1988; Selvam 1997; Stathopoulos 1997; Wright et al.
2003; Camarri et al. 2005; Tamura 2006; Tutar and Celik 2007; El-Okda et al. 2008; Tominaga
et al. 2008a; Cóstola et al. 2009 and others). Significant progress has also been made on the
evaluation of wind load modifications due to topographic elements (Bitsuamlak et al. 2004,
2006; Poggi and Katul 2007). Some countries have already established working groups to
investigate the practical applicability of CWE and develop recommendations for their use for
wind resistant design of actual buildings and for assessing pedestrian level winds, within the
framework of the Architectural Institute of Japan (AIJ) (Tamura et al. 2008, Tominaga et al.
2008b`) and the European cooperation in the field of scientific and technical (COST) research
(Franke et al. 2004). Further, AIJ provides methods for predicting wind loading on buildings by
the Reynolds Averaged Navier Stokes equations (RANS) and LES. Practical applications of
CWE are widespread in areas such as pedestrian level wind evaluation Chang (2006), Lam and
To (2006), Blocken and Carmeliet (2008), Yoshie et al. (2007), and Tablada et al. (2009), where
only the mean wind speeds are required for evaluating pedestrian comfort (Stathopoulos and Hu
2004). CWE applications for wind driven rain are reported by researchers such as Choi (2000),
and Blocken and Cameliet (2004). Some CFD wind flow studies for urban neighborhood
include Zhang et al. (2006), Huang et al. (2006), and Jiang et al. (2008). While most of studies
mentioned above focus on straight winds, studies by Lin and Savory (2006), and Hangan and
Kim (2008) focused on simulation of downburst. Other common uses of CWE, include
augmentation of experimental wind engineering research: Sengupta and Sarkar (2008)
augmented their microburst and tornado wind simulator facility with numerical simulation;
Merrick and Bitsuamlak (2008) used numerical simulation to facilitate selection of an artificial
surface roughness length to be applied on curved surfaced buildings during wind tunnel testing
as a means to compensate for High Reynolds number effects that is usually missing from low
wind speed tunnels.
2
The majority of numerical prediction of wind pressure loads on buildings devoted on the basic
cube shape, because of its geometrical simplicity yet representing the complex features of
building aerodynamics and availability of experimental data (Stathopoulos 2002; Nozawa and
Tamura 2002; Lim et al. 2009). These include full-scale low-rise building structures such as
Silsoe Cube (Wright and Easom 1999, 2003), Texas Tech University (Senthooran et al. 2004)
and Wall of Wind test building (Bitsuamlak et al. 2008). Some of the computational studies for
Tall Buildings include studies by Nozawa and Tamura (2002), Huang et al., (2007), Tominaga et
al., (2008), Tamura (2008) and Braun et al. (2009). Huang et al. (2007) and Braun et al. (2009)
focused on the aerodynamics of Commonwealth Advisory Aeronautical Council (CAARC)
building model and investigate the flow pattern and mean and rms pressure coefficient. CAARC
tall building is considered as one of the most extensively studied building model and popular in
wind tunnel researcher community as well (Wardlaw and Moss 1970 as referenced by Braun et
al. 2009; Melbourne 1980; Obasaju 1992). As a result, the present study also uses the CAARC
building model both for the numerical as well as boundary layer wind tunnel investigation thus
allowing a comparative study among different researcher results which is required perhaps at this
stage of CWE application for building aerodynamics. Different from previous CAARC studies in
literature which focuses on isolated building, the present study include experimental and
numerical aerodynamic analysis of CAAR building model under different orientation of adjacent
building conditions. While the numerical simulation uses Fluent 6.3 commercial software and
employs mostly RANS and LES (for limited case) turbulence models, the experimental part
include boundary layer wind tunnel experiments conducted at RWDI USA LLC, Miramar FL for
the present study.
Unlike flow around streamed line object, analysis of flow around sharp edged bluff-body
involves many difficulties as pointed out by Murakami (1998) and Stathopoulos (1997).
Intensive studies have been done on the suitability of various turbulence models (Murakami and
Mochida 1989; Murakami 1998; Castro and Graham 1999; Saha and Ferziger 1996, 1997).
RANS has been used in wind engineering application due to their simplicity in modeling and
reduced computational cost. Despite the computational cost, LES (large eddy simulation) is
believed to have reached the stage where analysis can be carried out within a reasonable
computational time for complicated turbulent flow around actual buildings and should be
considered as a complementary tool for wind loads evaluation (Tamura, 2008).
NUMERICAL MODEL
Based on a preliminary exploratory study on surface mounted cube, different turbulence models
from literature have been examined for their relative suitability for the present bluff body
application. Figure 1 shows comparison between numerically obtained pressure coefficients on
surface mounted cube by several researches with experimental results. As expected LES
provides superior results that agree well the experimental data obtained from wind tunnel and
full-scale tests. From RANS family of models the RNG k- provides relatively better result
compared to the standard k- model. In the present study RNG k- has been therefore opted due
to its relatively good agreement with BLWT compared to Standard k- and relatively lower
computational resource demand compared to LES. Only for comparison purpose LES has been
applied for Case 1A and Case 1B. Due to the chaotic nature of flow around bluff bodies, the
turbulence flows significantly affected by the presence of walls. The near-wall treatment has a
great impact on the result of the numerical simulation. Murakami et al. (1999) discussed the
difficulty in using no-slip boundary condition at solid walls for flows with high Reynolds
3
number, such as the present case. For such flow environment, Werner and Wengle (1991) wall
functions in the viscous sub layer (as provided by Fluent 6.3), which will reduce the use of
excessive fine meshes around the solid walls can be used. While for Case 1A, very fine meshes
are used in the near-wall region in attempt to resolve the low Reynolds number flow up to the
wall surface and Werner and Wengle (1991) wall functions are applied for Case 1B. Case 2 and
3 uses non-equilibrium wall functions as described in FLUENT user manual (2006).
1.5
Bitsuamlak et al., 2008 (K-e)
Wright and Easom, 2003 (K-e)
Wright and Easom, 2003 (RNG)
1
Wright and Easom, 2003 (NL)
Lim et al., 2009 (LES)
0.5
Wind tunnel (Holscher et al., 1998)
Wind tunnel (Richards et al., 2007)
Full Scale (Richards et al., 2007)
Cp
0
-0.5
-1
-1.5
-2
A
B
C
D
Figure 1 Comparison of mean pressure coefficients by several researchers using several turbulence models.
NUMERICAL AND WIND TUNNEL MODEL SETUPS
The geometrical modeling for the numerical simulation of CAARC building model mimics the
1:400 scale rigid model of the wind tunnel testing. The CAARC model has a rectangular
prismatic shape with dimensions 100 ft (x) by 150 ft (y) by 600 ft (z) height. The flow is
described in a Cartesian coordinate system (x, y, z), in which the x-axis is aligned with the
stream-wise direction, the z-axis is in the perpendicular direction and the y-axis is in the vertical
direction. The computational domain dimensions, boundary conditions and the wind tunnel
configurations and are given in Fig. 2. The driver (inlet), lateral and downstream boundaries are
extended laterally to minimize blockage issue on the aerodynamics of the test building. The
Reynolds number based on building height H and inflow velocity UH at z H is 3.8 x10 5 . Open
exposure velocity profile with power low exponent of 0.16 is used during the present BLWT test.
4
Table 1: Study cases
Case
Case 1A
Case 1B
Case 1C
Case 1D
Case 2A
Case 2B
Case 2C
Case 2D
Case 3A
Configuration
Velocity profile
Isolated
Isolated
Isolated
Isolated
full height adj. bldg upwind of CAARC
full height adj. bldg upwind of CAARC
full height adj. bldg downwind of CAARC
full height adj. bldg downwind of CAARC
half height adj. bldg upwind of CAARC
BLWT (Huang 2007)
BLWT (present)
ASCE (exposure B)
ASCE (exposure C)
ASCE (exposure B)
ASCE (exposure C)
ASCE (exposure B)
ASCE (exposure C)
ASCE (exposure B)
Scale
1:250
1:400
In the present study, three building configurations under four different flow fields have been
investigated. Table 1 describes all cases considered for the numerical simulation of CAARC
building model. Case 1 simulates wind effects on the isolated building without considering the
interference action of the surroundings. Case 2 simulates CAARC building with an adjacent
surrounding building having similar height with the test building placed upwind and downwind
of the study building. Case 3 simulates similar to Case 2 but the adjacent building has only half
height of the CAARC model.
The computational domain contains non uniform grid points and the grid stretching ratio for LES
simulation is less than 1.1 to avoid cut-off wave number between neighboring grids, see Fig. 3.
High mesh resolution is used in the low Reynolds viscous sub-layer zone. The inlet velocity
boundary condition comprising four different mean profiles as shown in Fig. 4 has been
simulated. For transient flow simulation generation of inflow turbulence for LES analysis (Case
1A), the velocity fluctuation is generated using spectral synthesizer available in Fluent. Free out
flow boundary conditions are imposed as the downstream of the computational domain. Wall
treatments as described in Numerical Model section are used at the building wall and the ground
surface. At the top and side boundaries are assumed to have zero velocity gradient and
symmetric boundary conditions are applied.
5
(a) Computational domain and boundary conditions: Case 1.
Isolated test
building
(b) Wind tunnel configurations.
6
(c) Computational domain: Case 3.
(d) Computational domain: Case 2.
Figure 2 Computational and wind tunnel set up.
Vertical section
Horizontal section
Figure 3 Typical grid used in the present study: Case 1A.
7
1.6
BLWT (Huang et aL., 2007)
BLWT (Present study)
1.4
ASC E (Exposure - C)
ASC E (Exposure - B)
Z(m) - Model scale
1.2
1
0.8
0.6
0.4
0.2
0
8
9
10
11
12
13
14
15
16
U(m/s)
Figure 4 Inflow boundary condition (velocity profiles) used in the present study.
RESULT AND DISCUSSIONS
For validation and comparison purposes, both standard and LES simulations have been used
for Case 1A and Case 1B. Measurements of mean pressure coefficients normalized by the
dynamic pressure at the building height are compared with the present BLWT data as well as
those obtained from literature. The mean pressure coefficients, Cp, on the upper windward,
sidewall and leeward faces are extracted for the isolated building case at 2/3H of the building as
shown in Fig. 5 for various inflow boundary conditions. As shown in Fig. 5, there is a good
agreement between the present LES as well as Braun’s (2009) and Huang’s (2007) numerical
simulation results of the current study with the experimental results on the windward face. The
agreement deteriorates slightly at the sidewalls and improves at the lee-ward wall. The standard
method over-predicts the pressure coefficient at the stagnation point and at flow separation
point.
8
1.5
Present study (ke - Case 1A )
Present study (LES - Case 1A)
Figure 2. Comparison of mean pressure
coefficient.
1
Present study (LES - Case 1B)
Braun et al., (2009)-numerical
Huang et al., (2007)-numerical
0.5
Wind tunnel (B LW T- P resent study)
Wind
tunnel
(Tong
Ji University)
Figure 3. Mean velocity contour at mid-vertical
and
2/3 H
horizontal
section.
Cp
0
-0.5
-1
-1.5
-2
0
0.5
1
1.5
2
2.5
3
3.5
4
X '/Dx
Figure 5 Measurements of mean pressure coefficients over the perimeter at Z/H =2/3: Velocity pressure
normalized by UH (12.7m/s)
Windward wall
Leeward wall
Figure 6 Contour plot of mean pressure distribution over the building walls (Case 1A)
9
Figure 6 shows mean-pressure contour pots of the windward and leeward face of configuration
Case 1A. The horseshoe vortex shape contour generated on the front wall agrees well with
Huang et al. (2007) and Braun et al. (2009) flow field investigation. To asses the effects of
inflow boundary conditions, the present work studies four different inflow conditions as outlined
in table 1. Where each of the categories varies in their velocity profile, turbulence intensity and
turbulence integral length scale. Figure 7 exhibits the comparison of mean pressure coefficients
obtained by numerical simulation with the wind tunnel data. Among all, there is reasonable
agreement between Case 1C and the experiment on the windward face. As expected there is
substantial increase in prediction of mean Cp by the numerical method.
1.5
Case 1B (RNG )
1
Case 1C (Exposure-B )(RNG)
Case 1D (Exposure-C)(RNG)
Wind Tunnel (P resent study)
Mean Cp
0.5
0
-0.5
-1
-1.5
-2
0
0.5
1
1.5
2
2.5
3
3.5
4
4.5
5
X'/Dx
Figure 7 Measurements of mean pressure coefficients over the perimeter at Z/H =2/3 (Case 1): Velocity
pressure normalized by UG (14.63 m/s)
Effect of adjacent building plays an important role on the aerodynamic response of buildings.
Each building site is unique and needs to be examined case by case. In the present study a
limited attempt was made to assess the effect of different adjacent building with different height,
Case 2 with same height as with the study building and Case 3 with half height. The numerical
as well as the wind tunnel test results, reveals the sheltering effect due to the presence of tall
structures upwind of the study building as shown in Fig. 8. Approximately a 150% reduction in
mean pressure coefficient has been observed relative to the isolated case. Figure 9 presents the
same case but when the adjacent building is placed in the leeward direction of the flow. In this
case the interference has no significant on the front wall pressure distribution but there is
10
0
0
1
2
3
4
5
-0 .2
-0 .4
-0 .6
M e an C p
-0 .8
W ind Tu nne l (P re se nt stud y)
-1
C a se 2 A (E xp o sure -B )(R NG )
-1 .2
C a se 2 B (E xp o sure -C )(RN G )
-1 .4
-1 .6
-1 .8
-2
X '/D x
Figure 8 Comparison of mean pressure coefficients over the perimeter at Z/H =2/3 (Case 2A & 2B): Velocity
pressure normalized by UG (14.63 m/s).
1.5
W ind tunne l (P re se nt stud y)
1
C a se 2 C (E xpo sure -B )
C a se 2 D (E xpo sure -C )
Me a n C p
0.5
0
-0.5
-1
-1.5
-2
0
0.5
1
1.5
2
2.5
3
3.5
4
4.5
5
X '/D x
Figure 9 Measurements of mean pressure coefficients over the perimeter at Z/H =2/3 (Case 2C & 2D):
Velocity pressure normalized by UG (14.63 m/s)
11
reduction in suction pressure coefficient. The presence of the half height adjacent building have
less significant impact on the mean pressure load compared to the effect of full height adjacent
building as can be expected.
1.5
Case 1B (BLWT - Present study)
Case 1B (Exposure - B)(RNG)
1
Case 2 (BLWT - Present study)
Case 2A (Exposure - B)(RNG)
Case 3 (BLWT - Present study)
0.5
Mean Cp
Case 3A (Exposure - B)(RNG)
0
-0.5
-1
-1.5
-2
0
0.5
1
1.5
2
2.5
3
3.5
4
4.5
5
X'/Dx
Figure 10 Comparison of mean pressure coefficients over the perimeter at Z/H =2/3: Surrounding
interference effects
Mean pressure contours on the building surface are shown in Figs 11a and 11b for Cases 2 and 3
respectively. Flow modification due to complex fluid structure interactions including the
adjacent buildings are also shown in Figs. 11c and 11d for Cases 2 and 3 respectively. Flow
separation points, down washes on windward walls, recirculation behind buildings that are
signature of tall buildings are clearly depicted in these figures. These capabilities of CFD
simulations are very useful in explaining aerodynamics phenomena among wind engineers and to
structural engineers and architects.
12
(a) Case 2
Mean pressure coefficients
(b) Case 3
(c) Velocity path lines: Case 2
(d) Velocity path lines: Case 3
Figure 11 Mean pressure coefficient and velocity path lines: Case 2& Case 3
13
CONCLUSIONS AND FUTURE WORKS
Several comparisons between CFD and experimental analysis have been discussed in order to
better understand the current state-of-the-art and assess the potential use of numerical wind load
predictions approaches for practical use. In the past, consistent efforts have been made to make
CFD a better tool for evaluation of wind loads. The application of CFD techniques to predict
wind load, on CAARC model and with different surrounding conditions reveals the suitability of
CFD tools for preliminary assessments and detail explanation of complex building aerodynamic
characteristics. Consistent to reports in literature, numerical data comparison with
measurements in boundary wind tunnel carried out in the present study suggests that an accurate
time-dependent analysis, such as LES analysis is very vital. Planned future studies include detail
LES analysis of buildings incorporating various orientation of surrounding effects.
ACKNOWLEDGMENT
The support from National Science Foundation (through NSF Career award to the second author)
is gratefully acknowledged.
REFERENCES
American Society of Civil Engineers, American National Standard: Minimum design loads for buildings
and other structures, ASCE 7-05.
AS/NZS 1170.2:2002, Australian/New Zealand Standard: Structural Design Actions Part 2: Wind Actions
Standards.
Bitsuamlak, G.T. (2006), “Application of computational wind engineering: A practical perspective”,
Third National Conference in wind Engineering, January 5-7, Kolkata, India.
Bitsuamlak, G.T., Dagnew, A.K., Gan Chowdhury, A. (2008), “Computational blockage and wind
simulator proximity effects assessment for a new full-scale testing facility”, 4th International
Conference”, Advances on Wind and Structures (AWAS08), Jeju, Korea.
Bitsuamlak, G.T., Stathopoulos, T., and Bédard, C. (2006), “Effect of upstream hills on design wind load:
a computational approach”, Wind and Structures. 9 (1), 37-58.
Bitsuamlak, G.T., Stathopoulos, T., Bédard, C. (2004), “Numerical evaluation of turbulent flows over
complex terrains: A review”, Journal of Aerospace Engineering, 17(4), 135-145.
Blocken, B. and Carmeliet, J., (2008), “Pedestrian wind conditions at outdoor platforms in a high-rise
apartment building: generic sub-configuration validation, wind comfort assessment and uncertainty
issues”, Wind and Structures. 11(1), 51-70.
Blocken, B., Carmeliet, J. (2004), “A Review of Wind-driven Rain Research in Building Science”, Jnl. of
Wind Eng. Ind. Aerod., 92(13), 1079-1130.
Braun, A.L. (2009), “Aerodynamic and aeroelastic analyses on the CAARC standard tall building model
using numerical simulation”, Computer and Structures 87. 564-581.
Camarri, S., Salvetti, M.V., Koobus B.,and Dervieux, A. (2005), “Hybrid RANS/LES simulations of a
bluff-body flow”, Wind and Structure, 8(6), 407–426.
14
Castro, I.P., Graham, J.G.R., (1999), “Computational wind engineering: the way ahead?”, Proc. Inst.
Civil Eng. Struct. Build. 134, 275–277.
Chang, C. (2006), “Computational fluid dynamics simulation of pedestrian wind in urban area with the
effects of tree”, Wind and Structures, 9(2), 147-158.
Choi ECC (2000), “Variation of Wind-driven Rain Intensity with Building Orientation”, Journal of
Architectural Engineering; 6, 122–130.
Cóstola, D., Blocken, B. and Hensen, J.L.M. (2009), “Overview of pressure coefficient data in building
energy simulation and airflow network programs”, Building and Environment, In press.
El-Okda, Y.M, Ragab, S.A., and Hajj, M.R. (2008) “Large-eddy simulation of flow over a surfacemounted prism using a high-order finite-difference scheme”, Jnl. of Wind Eng. Ind. Aerod., Vol. 96,
Issues 6-7, pp 900-912.
Franke, J., Hirsch, C. Jensen, A.G., Krus, H, W., Schatzmann, M., Westbury, P.S., Miles, S.D., Wisse, J.A.
and Wright, N.G. (2004), Recommendations on the Use of CFD in Wind Engineering. In van Beeck,
J.P.A.J., ed., Proceeding of the International Conference on Urban Wind Engineering and Building
Aerodynamics: COST Action C14- Impact of Wind and Storm on City Life and Built Environment. RohdeSaint-Genese: Von Karman Institute for Fluid Dynamics. C.1.1.-C.1.11.
Hangan, H. and Kim, J.D. (2008), “Swirl ratio effects on tornado vortices in relation to the Fujita scale”,
Wind and Structures, 11(4), 291-302.
Holscher, N., Niemann, H.J., 1998, “Towards quality assurance for wind tunnel tests: A comparative
testing program of the Windtechnologische Gesellschaft”, Jnl. of Wind Eng.Ind. Aerod., 74, 599-608.
Huang, H., Kato, S. and Ooka, R. (2006), “CFD analysis of ventilation efficiency around an elevated
highway using visitation frequency and purging flow rate”, Wind and Structures, 9(4), 297-313.
Huang, S., Q.S Li, and S. Xu. (2007), “Numerical evaluation of wind effects on a tall steel building by
CFD”. Journal of Constructional Steel Research 63, 612-627.
Irwin, P.A. (2008), “Bluff body aerodynamics in wind engineering”, Jnl. of Wind Eng. Ind. Aerodyn.96,
701–712.
Kareem ,A.(1985), “Lateral-torsional motion of tall buildings to wind loads”, Jnl. of Struct. Eng., ASCE
111 (11),(2479–2496.
Lam, K.M. and To, A.P. (2006), “Reliability of numerical computation of pedestrian-level wind
environment around a row of tall buildings”, Wind and Structures, 9(6), 473-492.
Lin, W. E. and Savory, E. (2006), “Large-scale quasi-steady modelling of a downburst outflow using a
slot jet”, Wind and Structures,9(6), 419-440.
Lim, C.H., Thomas, T.G., Castro, I.P. (2009), “Flow around a cube in a turbulent boundary layer: LES
and experiment”, Jnl. of Wind Eng. Ind. Aerod., In press
Merrick, R., and Bitsuamlak, G.T. (2008), "Control of flow around a circular cylinder by the use of
surface roughness", 4th International Conference”, Advances on Wind and Structures (AWAS08), Jeju,
Korea.
15
Melbourne, W.H. (1980), “Comparison of measurements of the CAARC standard tall building model in
simulated model wind flows”, Jnl. of Wind Eng. Ind. Aerodyn. 6:78–88.
Murakami, S., Mochida, A. (1989), “3-D numerical simulation of airflow around a cubic model by means
of the k-e model”, Jnl. of Wind Eng. Ind. Aerodyn.,Vol 31, 283-303.
Murakami, S. (1993), “Comparision of various turbulence models applied to a bluff body”, Jnl. of Wind
Eng. Ind. Aerodyn. 46-47, 21-36.
Murakami, S. (1998), “Overview of turbulence models applied in CWE”, Jnl. of Wind Eng. Ind. Aerodyn.
74-76, 1-24.
Murakami,S., 1997. Current status and future trends in computational wind engineering. Jnl. of Wind
Eng. Ind. Aerodyn. 67&68, 3-34.
Nozu, T., Tamura, T., Okuda, Y., Sanada, S. (2008), “LES of the flow around building wall pressures in
the center of Tokyo”, Jnl. of Wind Eng. Ind. Aerodyn.96, 1762-1773.
Nozawa, K., Tamura, T. (2002), “Large eddy simulation of the flow around a low-rise building immersed
in a rough-wall turbulent boundary layer”, Jnl. of Wind Eng. Ind. Aerodyn. 90, 1151–1162.
Obasaju, E.D. (1992), “Measurement of forces and base overturning moments on the CAARC tall
building model in a simulated atmospheric boundary layer”, Jnl. of Wind Eng. Ind. Aerodyn.40, 103-126.
Poggi, D. and Katul, G.G., 2007, “Turbulent flows on forested hilly terrain: the recirculation region”,
Quarterly Journal of the Royal Meterological Society, 133: 1027–1039.
Richards, P.J., Hoxey, R.P., Connell, B.D., Lander, D. P. (2007), “Wind-tunnel modelling of the Silsoe
Cube”, Jnl. of Wind Eng. Ind. Aerod., 95, 1384–1399.
Shah, K.B., Ferziger, J.H. (1996), “Large-eddy simulations of flow past a cubical obstacle”,
Thermosciences Division Report TF-70, Department of Mechanical Engineering, Stanford University.
Shah, K.B., Ferziger, J.H. (1997), “A fluid mechanician’s view of wind engineering: large-eddy
simulation of flow past a cubical obstacle”, Jnl. of Wind Eng. Ind. Aerodyn. 67&68, 211–224.
Senthooran,S., Lee, D. D., Parameswaran ,S. (2004),“A computational model to calculate the flowinduced pressure fluctuations on buildings. Jnl. of Wind Eng. Ind .Aerodyn. 92, 1131–1145
Selvam, S.P. (1997), “Computation of pressures on Texas Tech university building using large eddy
simulation”, Jnl. of Wind Eng. Ind. Aerod., 67&68, 647-657.
Sengupta, A., and Sarkar. (2008), “Experimental measurement and numerical simulation of an impinging
jet with application to thunderstorm microburst winds”, Jnl. of Wind Eng. Ind. Aerod., 96(3), 345-365.
Stathopoulos, T. (1997), “Computational wind engineering: Past achievements and future challenges”,
Jnl. of Wind Eng. Ind. Aerod., 67-68, 509-532.
Stathopoulos, T. Wu, H. (2004), “Using Computational Fluid Dynamics (CFD) for pedestrian winds”,
Proceedings of the 2004 Structures Congress, Nashville, TN.
16
Stathopoulos, T. (2002), “The numerical wind tunnel for industrial aerodynamics: Real or virtual in the
new millennium?”, Wind and Structures. Vol. 5, No. 2~4, 193-208.
Tablada,A., Troyera,F. D., Blocken, B., Carmeliet, J., Verschure, H .(2009), “On natural ventilation and
thermal comfort in compact urban environments – the Old Havana case”, Building and Environment, In
Press.
Tamura, T., Nozawa, K., and Kondo, K. (2008), “AIJ guide for numerical prediction of wind loads on
buildings”, Jnl. of Wind Eng. Ind. Aerod., 96, 1974–1984.
Tamura, T. (2006), “Towards practical use of LES in wind engineering”, The fourth international
symposium in Computational Wind Engineering (CWE2006), Yokohama, Japan.
Tamura, T. (2008), “Towards practical use of LES in wind engineering”, Jnl. of Wind Eng. And Ind.
Aerodyn. 96, 1451–1471.
Tominaga, T., Mochida, A., Murakami, S., Sawaki, S. (2008), “Comparison of various revised k–e
models and LES applied to flow around a high-rise building model with 1:1:2 shape placed within the
surface boundary layer”, Jnl. of Wind Eng. Ind. Aerodyn.96, 389 –411.
Tominaga, Y., Mochida, A., Murakami, S., and Sawaki, S. (2008a), “Comparison of various revised k–ε
models and LES applied to flow around a high-rise building model with 1:1:2 shape placed within the
surface boundary layer”, Jnl. of Wind Eng. Ind. Aerod., 96(4), 389-411.
Tominaga, Y., Mochida, A., Yoshiec, R., Kataokad, H., Nozu,T., Masaru, Yoshikawa, M., Shirasawa, T.
(2008b), “AIJ guidelines for practical applications of CFD to pedestrian wind environment around
buildings”, Jnl. of Wind Eng. Ind. Aerod., 96, 1749–1761.
Tutar, M., and Celik, I. (2007), “Large eddy simulation of a square cylinder flow: Modelling of inflow
turbulence”, Wind and Structure, 10(6), 511-532.
Werner, H., Wengle, H. (1991), “Large-eddy simulation of turbulent flow over and around a cube in a
plate channel”, Proceedings of the 8th Symposium on Turbulent Shear Flows 19 (4), 155–165.
Wardlaw, R.L., Moss, G.F. (1970), “A standard tall building model for the comparison of simulated
natural winds in wind tunnels”, CAARC, C.C.662m Tech; 25 January.
Wright, N.G., Easom, G.J. (2003), “Non-linear k– turbulence model results for flow over a building at
full-scale”, Applied Mathematical Modelling, 27(12), 1013-1033.
Yoshiea,R., Mochida,A., Tominaga,Y., Kataoka,H.,Harimoto, K., Nozu, T., Shirasawa, T. (2007),
“Cooperative project for CFD prediction of pedestrian wind environment in the Architectural Institute of
Japan”, Jnl. of Wind Eng. Ind. Aerodyn. 95, 1551–1578
Zhang, N., Jiang, W., and Miao, S. (2006), “A large eddy simulation on the effect of buildings on urban
flows”, Wind and Structures, 9(1), 23-35.
17
Agerneh K. Dagnew 1, Girma T. Bitsuamalk2, Ryan Merrick3
Research Assistant, Civil and Environmental Engineering department (CEE), International
Hurricane Research Center (IHRC), Florida International University (FIU), Miami, Florida,
USA, [email protected]
1
2
Assistant Professor of Wind/Structural Engineering, CEE, IHRC, FIU, Miami, Florida, USA
[email protected]
3
Senior Technical Coordinator, RWDI USA LLC, Miramar, Florida, USA,
[email protected]
ABSTRACT
At present, the wind engineering toolbox consists of wind-tunnel testing of scaled models, limited
full-scale testing, field measurements, and mechanical load/pressure testing. The evolution of
computational wind engineering (CWE) based on computational fluid dynamics (CFD)
principles are making the numerical evaluation of wind loads a potentially attractive
proposition. This is particularly true in light of the positive development trends in hardware and
software technology, as well as numerical modeling. The present study focuses on numerical
evaluation of wind pressures on tall buildings by using the Commonwealth Advisory
Aeronautical Council (CAARC) building model (Melbourne, 1980). The CARRC model has been
used extensively to study wind loading on tall buildings in wind tunnel studies and is usually
adopted for calibration of experimental techniques. Numerically obtained pressure coefficients
on the surface of CAARC building under different configurations of adjacent building are
compared with wind tunnel data collected at the RWDI USA LLC laboratory for the present
study and from literature. The present numerical simulation uses mostly Reynolds Averaged
Navier- Stokes equations (RANS) and Large Eddy Simulation (LES) for selected few cases.
KEY WORDS: Computational fluid dynamics, boundary layer wind tunnel, wind pressure, tall
building, RANS, LES
INTRODUCTION
Buildings, bridges, large span roof structures and other civil structures must be able to withstand
the external loads imposed by nature, at least to the extent that the disastrous damage of natural
force reduced to the acceptable limit (Irwin, 2007). Wind is one of the major forces responsible
for the catastrophic failure and loss of life. Therefore, accurate evaluation and prediction of wind
loads and proper mitigations are very important in reducing the adverse effects of wind in the
built environment. In addition to the mean and the background (due to turbulent fluctuations)
loads on rigid buildings, flexible structures will be subjected to resonant wind loads as well. The
primary source of the along-wind motion is the pressure fluctuations in the windward and
leeward faces due to the fluctuation in the approach flow and its interaction with the building.
Building codes and Standards usually provide loads along the wind direction for common shapes
1
in open and suburban terrain category perhaps with the exception of the AS-NZ 2002 code which
attempts to provide provisions in for the cross-wind direction as well. The cross-wind motion is
mainly caused by fluctuations in the separating shear layers. Torsional motion can be caused due
to imbalance in the instantaneous pressure distribution on each face of the building either due to
oblique wind directions, unsteadiness in the approaching flow, partial sheltering and interference
from surrounding buildings or due to own shape and dynamic structural properties. Studies
shows that for many high-rise buildings, the crosswind and torsional response may exceeds the
along wind response in terms of both limit state and serviceability requirements (Kareem, 1985).
Nevertheless, most existing standards, including ASCE07-05, only provides procedure for
evaluation of along-wind effects. For complex cases, the standards refer to physical model
testing in boundary layer wind tunnel (BLWT) facility.
The success of application of computational fluid dynamics (CFD) in aeronautical engineering is
very encouraging. Acknowledging the difference between streamlined and bluff body flows, the
use of computational fluid dynamics for predicting wind effects in the atmospheric boundary
layer appears very promising. This is particularly so considering the recent advances in hardware
and software technology, development of reliable sub-grid turbulence models and numerical
reproduction of inflow turbulence (Tamura 2008). At this stage of CWE application, however, a
systematic validation of CWE models through comparison with wind tunnel experiments shall
continue to enhance the confidence and warrant its use for practical applications.
Significant progress has been made in the application of CWE to evaluate wind loads on
buildings (e.g. Murakami and Mochida 1988; Selvam 1997; Stathopoulos 1997; Wright et al.
2003; Camarri et al. 2005; Tamura 2006; Tutar and Celik 2007; El-Okda et al. 2008; Tominaga
et al. 2008a; Cóstola et al. 2009 and others). Significant progress has also been made on the
evaluation of wind load modifications due to topographic elements (Bitsuamlak et al. 2004,
2006; Poggi and Katul 2007). Some countries have already established working groups to
investigate the practical applicability of CWE and develop recommendations for their use for
wind resistant design of actual buildings and for assessing pedestrian level winds, within the
framework of the Architectural Institute of Japan (AIJ) (Tamura et al. 2008, Tominaga et al.
2008b`) and the European cooperation in the field of scientific and technical (COST) research
(Franke et al. 2004). Further, AIJ provides methods for predicting wind loading on buildings by
the Reynolds Averaged Navier Stokes equations (RANS) and LES. Practical applications of
CWE are widespread in areas such as pedestrian level wind evaluation Chang (2006), Lam and
To (2006), Blocken and Carmeliet (2008), Yoshie et al. (2007), and Tablada et al. (2009), where
only the mean wind speeds are required for evaluating pedestrian comfort (Stathopoulos and Hu
2004). CWE applications for wind driven rain are reported by researchers such as Choi (2000),
and Blocken and Cameliet (2004). Some CFD wind flow studies for urban neighborhood
include Zhang et al. (2006), Huang et al. (2006), and Jiang et al. (2008). While most of studies
mentioned above focus on straight winds, studies by Lin and Savory (2006), and Hangan and
Kim (2008) focused on simulation of downburst. Other common uses of CWE, include
augmentation of experimental wind engineering research: Sengupta and Sarkar (2008)
augmented their microburst and tornado wind simulator facility with numerical simulation;
Merrick and Bitsuamlak (2008) used numerical simulation to facilitate selection of an artificial
surface roughness length to be applied on curved surfaced buildings during wind tunnel testing
as a means to compensate for High Reynolds number effects that is usually missing from low
wind speed tunnels.
2
The majority of numerical prediction of wind pressure loads on buildings devoted on the basic
cube shape, because of its geometrical simplicity yet representing the complex features of
building aerodynamics and availability of experimental data (Stathopoulos 2002; Nozawa and
Tamura 2002; Lim et al. 2009). These include full-scale low-rise building structures such as
Silsoe Cube (Wright and Easom 1999, 2003), Texas Tech University (Senthooran et al. 2004)
and Wall of Wind test building (Bitsuamlak et al. 2008). Some of the computational studies for
Tall Buildings include studies by Nozawa and Tamura (2002), Huang et al., (2007), Tominaga et
al., (2008), Tamura (2008) and Braun et al. (2009). Huang et al. (2007) and Braun et al. (2009)
focused on the aerodynamics of Commonwealth Advisory Aeronautical Council (CAARC)
building model and investigate the flow pattern and mean and rms pressure coefficient. CAARC
tall building is considered as one of the most extensively studied building model and popular in
wind tunnel researcher community as well (Wardlaw and Moss 1970 as referenced by Braun et
al. 2009; Melbourne 1980; Obasaju 1992). As a result, the present study also uses the CAARC
building model both for the numerical as well as boundary layer wind tunnel investigation thus
allowing a comparative study among different researcher results which is required perhaps at this
stage of CWE application for building aerodynamics. Different from previous CAARC studies in
literature which focuses on isolated building, the present study include experimental and
numerical aerodynamic analysis of CAAR building model under different orientation of adjacent
building conditions. While the numerical simulation uses Fluent 6.3 commercial software and
employs mostly RANS and LES (for limited case) turbulence models, the experimental part
include boundary layer wind tunnel experiments conducted at RWDI USA LLC, Miramar FL for
the present study.
Unlike flow around streamed line object, analysis of flow around sharp edged bluff-body
involves many difficulties as pointed out by Murakami (1998) and Stathopoulos (1997).
Intensive studies have been done on the suitability of various turbulence models (Murakami and
Mochida 1989; Murakami 1998; Castro and Graham 1999; Saha and Ferziger 1996, 1997).
RANS has been used in wind engineering application due to their simplicity in modeling and
reduced computational cost. Despite the computational cost, LES (large eddy simulation) is
believed to have reached the stage where analysis can be carried out within a reasonable
computational time for complicated turbulent flow around actual buildings and should be
considered as a complementary tool for wind loads evaluation (Tamura, 2008).
NUMERICAL MODEL
Based on a preliminary exploratory study on surface mounted cube, different turbulence models
from literature have been examined for their relative suitability for the present bluff body
application. Figure 1 shows comparison between numerically obtained pressure coefficients on
surface mounted cube by several researches with experimental results. As expected LES
provides superior results that agree well the experimental data obtained from wind tunnel and
full-scale tests. From RANS family of models the RNG k- provides relatively better result
compared to the standard k- model. In the present study RNG k- has been therefore opted due
to its relatively good agreement with BLWT compared to Standard k- and relatively lower
computational resource demand compared to LES. Only for comparison purpose LES has been
applied for Case 1A and Case 1B. Due to the chaotic nature of flow around bluff bodies, the
turbulence flows significantly affected by the presence of walls. The near-wall treatment has a
great impact on the result of the numerical simulation. Murakami et al. (1999) discussed the
difficulty in using no-slip boundary condition at solid walls for flows with high Reynolds
3
number, such as the present case. For such flow environment, Werner and Wengle (1991) wall
functions in the viscous sub layer (as provided by Fluent 6.3), which will reduce the use of
excessive fine meshes around the solid walls can be used. While for Case 1A, very fine meshes
are used in the near-wall region in attempt to resolve the low Reynolds number flow up to the
wall surface and Werner and Wengle (1991) wall functions are applied for Case 1B. Case 2 and
3 uses non-equilibrium wall functions as described in FLUENT user manual (2006).
1.5
Bitsuamlak et al., 2008 (K-e)
Wright and Easom, 2003 (K-e)
Wright and Easom, 2003 (RNG)
1
Wright and Easom, 2003 (NL)
Lim et al., 2009 (LES)
0.5
Wind tunnel (Holscher et al., 1998)
Wind tunnel (Richards et al., 2007)
Full Scale (Richards et al., 2007)
Cp
0
-0.5
-1
-1.5
-2
A
B
C
D
Figure 1 Comparison of mean pressure coefficients by several researchers using several turbulence models.
NUMERICAL AND WIND TUNNEL MODEL SETUPS
The geometrical modeling for the numerical simulation of CAARC building model mimics the
1:400 scale rigid model of the wind tunnel testing. The CAARC model has a rectangular
prismatic shape with dimensions 100 ft (x) by 150 ft (y) by 600 ft (z) height. The flow is
described in a Cartesian coordinate system (x, y, z), in which the x-axis is aligned with the
stream-wise direction, the z-axis is in the perpendicular direction and the y-axis is in the vertical
direction. The computational domain dimensions, boundary conditions and the wind tunnel
configurations and are given in Fig. 2. The driver (inlet), lateral and downstream boundaries are
extended laterally to minimize blockage issue on the aerodynamics of the test building. The
Reynolds number based on building height H and inflow velocity UH at z H is 3.8 x10 5 . Open
exposure velocity profile with power low exponent of 0.16 is used during the present BLWT test.
4
Table 1: Study cases
Case
Case 1A
Case 1B
Case 1C
Case 1D
Case 2A
Case 2B
Case 2C
Case 2D
Case 3A
Configuration
Velocity profile
Isolated
Isolated
Isolated
Isolated
full height adj. bldg upwind of CAARC
full height adj. bldg upwind of CAARC
full height adj. bldg downwind of CAARC
full height adj. bldg downwind of CAARC
half height adj. bldg upwind of CAARC
BLWT (Huang 2007)
BLWT (present)
ASCE (exposure B)
ASCE (exposure C)
ASCE (exposure B)
ASCE (exposure C)
ASCE (exposure B)
ASCE (exposure C)
ASCE (exposure B)
Scale
1:250
1:400
In the present study, three building configurations under four different flow fields have been
investigated. Table 1 describes all cases considered for the numerical simulation of CAARC
building model. Case 1 simulates wind effects on the isolated building without considering the
interference action of the surroundings. Case 2 simulates CAARC building with an adjacent
surrounding building having similar height with the test building placed upwind and downwind
of the study building. Case 3 simulates similar to Case 2 but the adjacent building has only half
height of the CAARC model.
The computational domain contains non uniform grid points and the grid stretching ratio for LES
simulation is less than 1.1 to avoid cut-off wave number between neighboring grids, see Fig. 3.
High mesh resolution is used in the low Reynolds viscous sub-layer zone. The inlet velocity
boundary condition comprising four different mean profiles as shown in Fig. 4 has been
simulated. For transient flow simulation generation of inflow turbulence for LES analysis (Case
1A), the velocity fluctuation is generated using spectral synthesizer available in Fluent. Free out
flow boundary conditions are imposed as the downstream of the computational domain. Wall
treatments as described in Numerical Model section are used at the building wall and the ground
surface. At the top and side boundaries are assumed to have zero velocity gradient and
symmetric boundary conditions are applied.
5
(a) Computational domain and boundary conditions: Case 1.
Isolated test
building
(b) Wind tunnel configurations.
6
(c) Computational domain: Case 3.
(d) Computational domain: Case 2.
Figure 2 Computational and wind tunnel set up.
Vertical section
Horizontal section
Figure 3 Typical grid used in the present study: Case 1A.
7
1.6
BLWT (Huang et aL., 2007)
BLWT (Present study)
1.4
ASC E (Exposure - C)
ASC E (Exposure - B)
Z(m) - Model scale
1.2
1
0.8
0.6
0.4
0.2
0
8
9
10
11
12
13
14
15
16
U(m/s)
Figure 4 Inflow boundary condition (velocity profiles) used in the present study.
RESULT AND DISCUSSIONS
For validation and comparison purposes, both standard and LES simulations have been used
for Case 1A and Case 1B. Measurements of mean pressure coefficients normalized by the
dynamic pressure at the building height are compared with the present BLWT data as well as
those obtained from literature. The mean pressure coefficients, Cp, on the upper windward,
sidewall and leeward faces are extracted for the isolated building case at 2/3H of the building as
shown in Fig. 5 for various inflow boundary conditions. As shown in Fig. 5, there is a good
agreement between the present LES as well as Braun’s (2009) and Huang’s (2007) numerical
simulation results of the current study with the experimental results on the windward face. The
agreement deteriorates slightly at the sidewalls and improves at the lee-ward wall. The standard
method over-predicts the pressure coefficient at the stagnation point and at flow separation
point.
8
1.5
Present study (ke - Case 1A )
Present study (LES - Case 1A)
Figure 2. Comparison of mean pressure
coefficient.
1
Present study (LES - Case 1B)
Braun et al., (2009)-numerical
Huang et al., (2007)-numerical
0.5
Wind tunnel (B LW T- P resent study)
Wind
tunnel
(Tong
Ji University)
Figure 3. Mean velocity contour at mid-vertical
and
2/3 H
horizontal
section.
Cp
0
-0.5
-1
-1.5
-2
0
0.5
1
1.5
2
2.5
3
3.5
4
X '/Dx
Figure 5 Measurements of mean pressure coefficients over the perimeter at Z/H =2/3: Velocity pressure
normalized by UH (12.7m/s)
Windward wall
Leeward wall
Figure 6 Contour plot of mean pressure distribution over the building walls (Case 1A)
9
Figure 6 shows mean-pressure contour pots of the windward and leeward face of configuration
Case 1A. The horseshoe vortex shape contour generated on the front wall agrees well with
Huang et al. (2007) and Braun et al. (2009) flow field investigation. To asses the effects of
inflow boundary conditions, the present work studies four different inflow conditions as outlined
in table 1. Where each of the categories varies in their velocity profile, turbulence intensity and
turbulence integral length scale. Figure 7 exhibits the comparison of mean pressure coefficients
obtained by numerical simulation with the wind tunnel data. Among all, there is reasonable
agreement between Case 1C and the experiment on the windward face. As expected there is
substantial increase in prediction of mean Cp by the numerical method.
1.5
Case 1B (RNG )
1
Case 1C (Exposure-B )(RNG)
Case 1D (Exposure-C)(RNG)
Wind Tunnel (P resent study)
Mean Cp
0.5
0
-0.5
-1
-1.5
-2
0
0.5
1
1.5
2
2.5
3
3.5
4
4.5
5
X'/Dx
Figure 7 Measurements of mean pressure coefficients over the perimeter at Z/H =2/3 (Case 1): Velocity
pressure normalized by UG (14.63 m/s)
Effect of adjacent building plays an important role on the aerodynamic response of buildings.
Each building site is unique and needs to be examined case by case. In the present study a
limited attempt was made to assess the effect of different adjacent building with different height,
Case 2 with same height as with the study building and Case 3 with half height. The numerical
as well as the wind tunnel test results, reveals the sheltering effect due to the presence of tall
structures upwind of the study building as shown in Fig. 8. Approximately a 150% reduction in
mean pressure coefficient has been observed relative to the isolated case. Figure 9 presents the
same case but when the adjacent building is placed in the leeward direction of the flow. In this
case the interference has no significant on the front wall pressure distribution but there is
10
0
0
1
2
3
4
5
-0 .2
-0 .4
-0 .6
M e an C p
-0 .8
W ind Tu nne l (P re se nt stud y)
-1
C a se 2 A (E xp o sure -B )(R NG )
-1 .2
C a se 2 B (E xp o sure -C )(RN G )
-1 .4
-1 .6
-1 .8
-2
X '/D x
Figure 8 Comparison of mean pressure coefficients over the perimeter at Z/H =2/3 (Case 2A & 2B): Velocity
pressure normalized by UG (14.63 m/s).
1.5
W ind tunne l (P re se nt stud y)
1
C a se 2 C (E xpo sure -B )
C a se 2 D (E xpo sure -C )
Me a n C p
0.5
0
-0.5
-1
-1.5
-2
0
0.5
1
1.5
2
2.5
3
3.5
4
4.5
5
X '/D x
Figure 9 Measurements of mean pressure coefficients over the perimeter at Z/H =2/3 (Case 2C & 2D):
Velocity pressure normalized by UG (14.63 m/s)
11
reduction in suction pressure coefficient. The presence of the half height adjacent building have
less significant impact on the mean pressure load compared to the effect of full height adjacent
building as can be expected.
1.5
Case 1B (BLWT - Present study)
Case 1B (Exposure - B)(RNG)
1
Case 2 (BLWT - Present study)
Case 2A (Exposure - B)(RNG)
Case 3 (BLWT - Present study)
0.5
Mean Cp
Case 3A (Exposure - B)(RNG)
0
-0.5
-1
-1.5
-2
0
0.5
1
1.5
2
2.5
3
3.5
4
4.5
5
X'/Dx
Figure 10 Comparison of mean pressure coefficients over the perimeter at Z/H =2/3: Surrounding
interference effects
Mean pressure contours on the building surface are shown in Figs 11a and 11b for Cases 2 and 3
respectively. Flow modification due to complex fluid structure interactions including the
adjacent buildings are also shown in Figs. 11c and 11d for Cases 2 and 3 respectively. Flow
separation points, down washes on windward walls, recirculation behind buildings that are
signature of tall buildings are clearly depicted in these figures. These capabilities of CFD
simulations are very useful in explaining aerodynamics phenomena among wind engineers and to
structural engineers and architects.
12
(a) Case 2
Mean pressure coefficients
(b) Case 3
(c) Velocity path lines: Case 2
(d) Velocity path lines: Case 3
Figure 11 Mean pressure coefficient and velocity path lines: Case 2& Case 3
13
CONCLUSIONS AND FUTURE WORKS
Several comparisons between CFD and experimental analysis have been discussed in order to
better understand the current state-of-the-art and assess the potential use of numerical wind load
predictions approaches for practical use. In the past, consistent efforts have been made to make
CFD a better tool for evaluation of wind loads. The application of CFD techniques to predict
wind load, on CAARC model and with different surrounding conditions reveals the suitability of
CFD tools for preliminary assessments and detail explanation of complex building aerodynamic
characteristics. Consistent to reports in literature, numerical data comparison with
measurements in boundary wind tunnel carried out in the present study suggests that an accurate
time-dependent analysis, such as LES analysis is very vital. Planned future studies include detail
LES analysis of buildings incorporating various orientation of surrounding effects.
ACKNOWLEDGMENT
The support from National Science Foundation (through NSF Career award to the second author)
is gratefully acknowledged.
REFERENCES
American Society of Civil Engineers, American National Standard: Minimum design loads for buildings
and other structures, ASCE 7-05.
AS/NZS 1170.2:2002, Australian/New Zealand Standard: Structural Design Actions Part 2: Wind Actions
Standards.
Bitsuamlak, G.T. (2006), “Application of computational wind engineering: A practical perspective”,
Third National Conference in wind Engineering, January 5-7, Kolkata, India.
Bitsuamlak, G.T., Dagnew, A.K., Gan Chowdhury, A. (2008), “Computational blockage and wind
simulator proximity effects assessment for a new full-scale testing facility”, 4th International
Conference”, Advances on Wind and Structures (AWAS08), Jeju, Korea.
Bitsuamlak, G.T., Stathopoulos, T., and Bédard, C. (2006), “Effect of upstream hills on design wind load:
a computational approach”, Wind and Structures. 9 (1), 37-58.
Bitsuamlak, G.T., Stathopoulos, T., Bédard, C. (2004), “Numerical evaluation of turbulent flows over
complex terrains: A review”, Journal of Aerospace Engineering, 17(4), 135-145.
Blocken, B. and Carmeliet, J., (2008), “Pedestrian wind conditions at outdoor platforms in a high-rise
apartment building: generic sub-configuration validation, wind comfort assessment and uncertainty
issues”, Wind and Structures. 11(1), 51-70.
Blocken, B., Carmeliet, J. (2004), “A Review of Wind-driven Rain Research in Building Science”, Jnl. of
Wind Eng. Ind. Aerod., 92(13), 1079-1130.
Braun, A.L. (2009), “Aerodynamic and aeroelastic analyses on the CAARC standard tall building model
using numerical simulation”, Computer and Structures 87. 564-581.
Camarri, S., Salvetti, M.V., Koobus B.,and Dervieux, A. (2005), “Hybrid RANS/LES simulations of a
bluff-body flow”, Wind and Structure, 8(6), 407–426.
14
Castro, I.P., Graham, J.G.R., (1999), “Computational wind engineering: the way ahead?”, Proc. Inst.
Civil Eng. Struct. Build. 134, 275–277.
Chang, C. (2006), “Computational fluid dynamics simulation of pedestrian wind in urban area with the
effects of tree”, Wind and Structures, 9(2), 147-158.
Choi ECC (2000), “Variation of Wind-driven Rain Intensity with Building Orientation”, Journal of
Architectural Engineering; 6, 122–130.
Cóstola, D., Blocken, B. and Hensen, J.L.M. (2009), “Overview of pressure coefficient data in building
energy simulation and airflow network programs”, Building and Environment, In press.
El-Okda, Y.M, Ragab, S.A., and Hajj, M.R. (2008) “Large-eddy simulation of flow over a surfacemounted prism using a high-order finite-difference scheme”, Jnl. of Wind Eng. Ind. Aerod., Vol. 96,
Issues 6-7, pp 900-912.
Franke, J., Hirsch, C. Jensen, A.G., Krus, H, W., Schatzmann, M., Westbury, P.S., Miles, S.D., Wisse, J.A.
and Wright, N.G. (2004), Recommendations on the Use of CFD in Wind Engineering. In van Beeck,
J.P.A.J., ed., Proceeding of the International Conference on Urban Wind Engineering and Building
Aerodynamics: COST Action C14- Impact of Wind and Storm on City Life and Built Environment. RohdeSaint-Genese: Von Karman Institute for Fluid Dynamics. C.1.1.-C.1.11.
Hangan, H. and Kim, J.D. (2008), “Swirl ratio effects on tornado vortices in relation to the Fujita scale”,
Wind and Structures, 11(4), 291-302.
Holscher, N., Niemann, H.J., 1998, “Towards quality assurance for wind tunnel tests: A comparative
testing program of the Windtechnologische Gesellschaft”, Jnl. of Wind Eng.Ind. Aerod., 74, 599-608.
Huang, H., Kato, S. and Ooka, R. (2006), “CFD analysis of ventilation efficiency around an elevated
highway using visitation frequency and purging flow rate”, Wind and Structures, 9(4), 297-313.
Huang, S., Q.S Li, and S. Xu. (2007), “Numerical evaluation of wind effects on a tall steel building by
CFD”. Journal of Constructional Steel Research 63, 612-627.
Irwin, P.A. (2008), “Bluff body aerodynamics in wind engineering”, Jnl. of Wind Eng. Ind. Aerodyn.96,
701–712.
Kareem ,A.(1985), “Lateral-torsional motion of tall buildings to wind loads”, Jnl. of Struct. Eng., ASCE
111 (11),(2479–2496.
Lam, K.M. and To, A.P. (2006), “Reliability of numerical computation of pedestrian-level wind
environment around a row of tall buildings”, Wind and Structures, 9(6), 473-492.
Lin, W. E. and Savory, E. (2006), “Large-scale quasi-steady modelling of a downburst outflow using a
slot jet”, Wind and Structures,9(6), 419-440.
Lim, C.H., Thomas, T.G., Castro, I.P. (2009), “Flow around a cube in a turbulent boundary layer: LES
and experiment”, Jnl. of Wind Eng. Ind. Aerod., In press
Merrick, R., and Bitsuamlak, G.T. (2008), "Control of flow around a circular cylinder by the use of
surface roughness", 4th International Conference”, Advances on Wind and Structures (AWAS08), Jeju,
Korea.
15
Melbourne, W.H. (1980), “Comparison of measurements of the CAARC standard tall building model in
simulated model wind flows”, Jnl. of Wind Eng. Ind. Aerodyn. 6:78–88.
Murakami, S., Mochida, A. (1989), “3-D numerical simulation of airflow around a cubic model by means
of the k-e model”, Jnl. of Wind Eng. Ind. Aerodyn.,Vol 31, 283-303.
Murakami, S. (1993), “Comparision of various turbulence models applied to a bluff body”, Jnl. of Wind
Eng. Ind. Aerodyn. 46-47, 21-36.
Murakami, S. (1998), “Overview of turbulence models applied in CWE”, Jnl. of Wind Eng. Ind. Aerodyn.
74-76, 1-24.
Murakami,S., 1997. Current status and future trends in computational wind engineering. Jnl. of Wind
Eng. Ind. Aerodyn. 67&68, 3-34.
Nozu, T., Tamura, T., Okuda, Y., Sanada, S. (2008), “LES of the flow around building wall pressures in
the center of Tokyo”, Jnl. of Wind Eng. Ind. Aerodyn.96, 1762-1773.
Nozawa, K., Tamura, T. (2002), “Large eddy simulation of the flow around a low-rise building immersed
in a rough-wall turbulent boundary layer”, Jnl. of Wind Eng. Ind. Aerodyn. 90, 1151–1162.
Obasaju, E.D. (1992), “Measurement of forces and base overturning moments on the CAARC tall
building model in a simulated atmospheric boundary layer”, Jnl. of Wind Eng. Ind. Aerodyn.40, 103-126.
Poggi, D. and Katul, G.G., 2007, “Turbulent flows on forested hilly terrain: the recirculation region”,
Quarterly Journal of the Royal Meterological Society, 133: 1027–1039.
Richards, P.J., Hoxey, R.P., Connell, B.D., Lander, D. P. (2007), “Wind-tunnel modelling of the Silsoe
Cube”, Jnl. of Wind Eng. Ind. Aerod., 95, 1384–1399.
Shah, K.B., Ferziger, J.H. (1996), “Large-eddy simulations of flow past a cubical obstacle”,
Thermosciences Division Report TF-70, Department of Mechanical Engineering, Stanford University.
Shah, K.B., Ferziger, J.H. (1997), “A fluid mechanician’s view of wind engineering: large-eddy
simulation of flow past a cubical obstacle”, Jnl. of Wind Eng. Ind. Aerodyn. 67&68, 211–224.
Senthooran,S., Lee, D. D., Parameswaran ,S. (2004),“A computational model to calculate the flowinduced pressure fluctuations on buildings. Jnl. of Wind Eng. Ind .Aerodyn. 92, 1131–1145
Selvam, S.P. (1997), “Computation of pressures on Texas Tech university building using large eddy
simulation”, Jnl. of Wind Eng. Ind. Aerod., 67&68, 647-657.
Sengupta, A., and Sarkar. (2008), “Experimental measurement and numerical simulation of an impinging
jet with application to thunderstorm microburst winds”, Jnl. of Wind Eng. Ind. Aerod., 96(3), 345-365.
Stathopoulos, T. (1997), “Computational wind engineering: Past achievements and future challenges”,
Jnl. of Wind Eng. Ind. Aerod., 67-68, 509-532.
Stathopoulos, T. Wu, H. (2004), “Using Computational Fluid Dynamics (CFD) for pedestrian winds”,
Proceedings of the 2004 Structures Congress, Nashville, TN.
16
Stathopoulos, T. (2002), “The numerical wind tunnel for industrial aerodynamics: Real or virtual in the
new millennium?”, Wind and Structures. Vol. 5, No. 2~4, 193-208.
Tablada,A., Troyera,F. D., Blocken, B., Carmeliet, J., Verschure, H .(2009), “On natural ventilation and
thermal comfort in compact urban environments – the Old Havana case”, Building and Environment, In
Press.
Tamura, T., Nozawa, K., and Kondo, K. (2008), “AIJ guide for numerical prediction of wind loads on
buildings”, Jnl. of Wind Eng. Ind. Aerod., 96, 1974–1984.
Tamura, T. (2006), “Towards practical use of LES in wind engineering”, The fourth international
symposium in Computational Wind Engineering (CWE2006), Yokohama, Japan.
Tamura, T. (2008), “Towards practical use of LES in wind engineering”, Jnl. of Wind Eng. And Ind.
Aerodyn. 96, 1451–1471.
Tominaga, T., Mochida, A., Murakami, S., Sawaki, S. (2008), “Comparison of various revised k–e
models and LES applied to flow around a high-rise building model with 1:1:2 shape placed within the
surface boundary layer”, Jnl. of Wind Eng. Ind. Aerodyn.96, 389 –411.
Tominaga, Y., Mochida, A., Murakami, S., and Sawaki, S. (2008a), “Comparison of various revised k–ε
models and LES applied to flow around a high-rise building model with 1:1:2 shape placed within the
surface boundary layer”, Jnl. of Wind Eng. Ind. Aerod., 96(4), 389-411.
Tominaga, Y., Mochida, A., Yoshiec, R., Kataokad, H., Nozu,T., Masaru, Yoshikawa, M., Shirasawa, T.
(2008b), “AIJ guidelines for practical applications of CFD to pedestrian wind environment around
buildings”, Jnl. of Wind Eng. Ind. Aerod., 96, 1749–1761.
Tutar, M., and Celik, I. (2007), “Large eddy simulation of a square cylinder flow: Modelling of inflow
turbulence”, Wind and Structure, 10(6), 511-532.
Werner, H., Wengle, H. (1991), “Large-eddy simulation of turbulent flow over and around a cube in a
plate channel”, Proceedings of the 8th Symposium on Turbulent Shear Flows 19 (4), 155–165.
Wardlaw, R.L., Moss, G.F. (1970), “A standard tall building model for the comparison of simulated
natural winds in wind tunnels”, CAARC, C.C.662m Tech; 25 January.
Wright, N.G., Easom, G.J. (2003), “Non-linear k– turbulence model results for flow over a building at
full-scale”, Applied Mathematical Modelling, 27(12), 1013-1033.
Yoshiea,R., Mochida,A., Tominaga,Y., Kataoka,H.,Harimoto, K., Nozu, T., Shirasawa, T. (2007),
“Cooperative project for CFD prediction of pedestrian wind environment in the Architectural Institute of
Japan”, Jnl. of Wind Eng. Ind. Aerodyn. 95, 1551–1578
Zhang, N., Jiang, W., and Miao, S. (2006), “A large eddy simulation on the effect of buildings on urban
flows”, Wind and Structures, 9(1), 23-35.
17
