Flow and Pollutant Dispersion in Street Canyons,fluent典型错误

Environ Model Assess(2008)13:369–381
DOI10.1007/s10666-007-9106-6
Flow and Pollutant Dispersion in Street Canyons using FLUENT and ADMS-Urban
S.Di Sabatino·R.Buccolieri·
B.Pulvirenti·R.E.Britter
Received:7January2006/Accepted:5May2007/Published online:7July2007
©Springer Science+Business Media B.V.2007
Abstract This paper is devoted to the study offlow within a small building arrangement and pollutant dis-persion in street canyons starting from the simplest case of dispersion from a simple traffic source.Flow results from the commercial computationalfluid dy-namics(CFD)code FLUENT are validated against wind tunnel data(CEDVAL).Dispersion results from FLUENT are analysed using the well-validated atmos-pheric dispersion model ADMS-Urban.The k− turbulence model and the advection-diffusion(AD) method are used for the CFD simulations.Sensitivity of dispersion results to wind direction within street canyons of aspect ratio equal to1is investigated.The analysis shows that the CFD model well reproduces the wind tunnelflow measurements and compares ad-equately with ADMS-Urban dispersion predictions for a simple traffic source by using a slightly modified k− model.It is found that a Schmidt number of0.4is the most appropriate number for the simulation of a simple traffic source and in street canyons except for the case when the wind direction is perpendicular to the street canyon axis.For this last case a Schmidt number equal S.Di Sabatino(B)·R.Buccolieri
Dipartimento di Scienza dei Materiali,
University of Lecce,Lecce,Italy
e-mail:silvana.disabatino@unile.it
B.Pulvirenti
Dipartimento di Ingegneria Energetica,
Nucleare e del Controllo Ambientale,
University of Bologna,Bologna,Italy
R.E.Britter
Department of Engineering,University of Cambridge, Cambridge,UK to0.04gives the best agreement with ADMS-Urban. Overall the modified k− turbulence model may be accurate for the simulation of pollutant dispersion in street canyons provided that an appropriate choice for coefficients in the turbulence model and the Schmidt number in the diffusion model are made.
Keywords Street canyons·Dispersion·Modelling·FLUENT·ADMS-Urban
1Introduction
Air quality in urban areas is of great importance given its direct implications for the health of people living in those areas.Urban building arrangements,in particular the width of streets,their orientation,spacing and the presence of intersections are major factors in the deter-mination of pollution dispersion at street level.Irreg-ular shape buildings contribute to enhance turbulence and vertical mixing in the atmosphere,while W/H ratios(with W the width and H the height)of urban canyons affect street ventilation.More generally,build-ings modify theflowfield,influencing air exchanges and the dispersion of pollutants.In urban areas,in par-ticular,pollution may be the result of emissions from traffic,domestic heating and cooling systems,industry or toxic agents accidentally and/or deliberately released into the atmosphere.
Traditionally,information about concentrations is obtained using wind-tunnel experiments,which provide an opportunity to examine the effects of various para-meters individually or in a controlled combination.For example,Park et al.[18]characterized the dispersion of vehicle emissions by conducting wind tunnel tests and
370S.Di Sabatino et al.
applying tracer gas techniques.They concluded that the dispersion of vehicle emission in street canyons is primarily affected by microscale climatic factors such as the W/H ratio.
Recently,computationalfluid dynamics(CFD)has become an attractive tool to predict concentration fields near buildings.Many works can be found in the literature reporting on the use of computationalfluid dynamics(CFD)techniques to modelflow and pol-lutant dispersion around isolated buildings or groups of buildings[7].However,their use to calculate gas dispersion in urban areas is still limited to isolated cases and to a limited number of sources.The Reynolds averaged Navier–Stokes equation(RANS)methods are amongst the most preferable procedures used to model urban dispersion problems,mainly due to their relatively inexpensive computational par-isons of the RANS results with wind tunnel data show that significant errors could occur in the prediction of concentrations.These errors could come from any inappropriate choice of the turbulence model,numer-ical schemes,grid resolution and so on[24].Recently, Xie et al.[25]investigated the influence of building geometry on pollutant dispersion comparing different k− models with wind tunnel measured data for the optimization of turbulence models.Their comparison showed that the standard k− model[15]was the most optimum choice.On the other hand,integralflow and dispersion models are still the most used tools for the study of pollutant dispersion as they are able to account for a large number of emission sources at the same time;
a result particularly useful to assess air quality in urban areas.
The objective of this study is to compare CFD numerical simulations offlow and pollution concentra-tionfields with predictions from an integral Gaussian-type dispersion model.This work is also an attempt to highlight advantages and disadvantages of two dif-ferent types of modelling for pollutant concentration predictions in a real urban environment.We chose two commercial codes the CFD code,FLUENT[9]and the quasi-Gaussian atmospheric dispersion modelling system(ADMS-Urban)[5].This choice is justified by their extensive use in Europe and in the world.In particular,FLUENT is the world’s most widely used commercial CFD code for a wide range of industrial flow applications.The number of industries that have benefited from using it continues to expand.FLUENT has been used to successfully simulate the atmospheric boundary layer[21]but,at present there are not sufficient validation studies concerning its use for the predictions of pollutants in urban areas[11]. ADMS-Urban is being widely used for calculating gas dispersion into the atmosphere over scales of up to about50km from releases from various sources.The model is able to account for a large number and type of emission sources typically found in urban areas.Several validation studies(see for instance[12]and[3])have shown that,especially overflat terrain,the predictions are consistent with experimental data.The study pro-posed here builds on and extends previous works based on FLUENT and ADMS-Urban model verification and analysis.In particular,a comparison between FLUENT and ADMS3(the industrial version of ADMS-Urban) for atmospheric dispersion modelling from a single point source was analysed by Riddle et al.[21],who found a good agreement using the turbulence Reynolds stress model(RSM)[14]and the Lagrangian particle (LP)method.Their study remarks that CFD simula-tions are not an appropriate alternative to a model such as ADMS for routine atmospheric dispersion studies because of the large run times and the complexity of the setup.More recently,Di Sabatino et al.[8]ex-tended the study to the comparison between ADMS-Urban and FLUENT in an isolated street canyon.They obtained similar results using a slightly modified k− turbulence model and the advection–diffusion(AD) method which,together,are computationally less ex-pensive than other available models.
In this paper we use the three dimensional com-putationalfluid dynamics model FLUENT with both the standard and a modified k− turbulence scheme to examine if the use of a general purpose CFD code can be a practical tool for studying air quality in urban areas.
2Model Availability and General Description FLUENT is a state-of-the-art computer program for modellingfluidflow and heat transfer in complex geometries.The code is available from nationalfluent vendors for both academic and public institutions by acquiring an annual renewable licence.It solves the governing conservation equations offluid dynamics by afinite-volume formulation on a structured,non-orthogonal,curvilinear coordinate grid system using a collocated variable arrangement.Three different spa-tial discretization schemes may be used,that is power-law,second-order upwind,and QUICK,a bounded third-order accurate method.Temporal discretization is achieved by a second-order,implicit Euler scheme. Pressure/Velocity coupling is achieved by the SIM-PLE algorithm resulting in a set of algebraic equations which are solved using a line-by-line tridiagonal matrix algorithm,accelerated by an additive-correction type
Flow and pollutant dispersion in street canyons371
of multigrid method and block-correction.Additional equation solvers are also available to the user. FLUENT models turbulentflows with the standard k− model,an RNG model,and a second-moment closure or Reynolds-stress model(RSM)[9].
ADMS-Urban is a PC based air quality manage-ment system of dispersion in the atmosphere of passive, buoyant or slightly dense,continuous orfinite durations releases from single or multiple sources.The model is available on request directly from the main devel-oper Cambridge Environmental Research Consultants or from national vendors.Both annual and perma-nent licences are available.The model uses an up-to-date parameterisation of the boundary layer structure based on the Monin–Obukhov length and the boundary layer height.Concentration distributions are Gaussian in stable and neutral conditions,but the vertical dis-tributions is non-Gaussian in convective conditions to take account of the skewed structure of the vertical component of the turbulence.A range of modules allow for the effects of plume rise,complex terrain, street canyons,noise barriers and buildings.The street canyon module is based on the largely used OSPM model[13]which considers a trapezoidal recirculation area whose dimensions depend upon the street canyon aspect ratio and wind speed above the street canyon top.Therefore the recirculation area is somehow pre-scribed in models such as ADMS-Urban and this aspect should be kept in mind when comparing results with a CFD code.The parameters for the windfield and the Gaussian plume model are calculated by a meteoro-logical pre-processor.The OSPM model has been ex-tensively tested against measurements at several street locations.Examples of comparison of model results with measurements are given in[2]and[13].
3Methodology
In this work concentration predictions from a traffic source(modelled as a line source with cross-wind di-mension)placed within a regular urban street canyon are investigated.It is recognised that the modelling of a traffic source is straightforward in operational models of the type of ADMS-Urban but it is not with general purpose engineering-type CFD models.In this study we document each step undertaken to achieve thefinal goal in FLUENT with the aim of assessing the validity of results and giving recommendation for the use of commercial generic CFD codes for the prediction of inert pollutant concentrations in street canyons.Sepa-rate simulations are performed to study theflow before proceeding with the modelling of pollutant dispersion.Atfirst we simulate the simplest atmospheric neutral boundary layerflow over a surface with a specified surface roughness length.After,we investigate the best model setup for the simulation of small building arrangements and compareflow results with available wind tunnel data(CEDVAL)[6]to obtain confidence in the CFD simulations.Finally,we study dispersion by modelling afinite traffic source in the atmospheric neutral boundary layer without buildings and after a finite traffic source in a single street canyon for vari-ous wind directions.ADMS-Urban is used to provide benchmark data for the study as it is routinely validated against monitoring data(see for instance[4])and has undergone several validation studies with good datasets (see for instance[12]).
3.1ADMS-Urban General Flow and Dispersion Setup
Initially,ADMS-Urban is run to calculate the boundary layer velocity profiles to use them as the upstream boundary conditions in FLUENT.The velocity(or wind)profile in a neutrally stratified atmosphere is calculated through the logarithmic law:
U(z)=
u∗
κln
z+z0
z0
(1)
where U(z)is the average wind speed at the height z above the ground,z0is the surface roughness,u∗is the friction velocity andκis the von Karman’s constant. As in[21]a neutral boundary layer of height800m is initially used,with a wind speed of5ms−1(at a height of 10m above the ground)and a surface roughness length of0.1m.
The simulation of gas dispersion from a traffic source is done using a line source which is100m long and 1m wide.As an example,a release of CO is chosen with an emission rate of10g/s.A similar emission rate is also used for the simulation of afinite traffic source in a street canyon with aspect ratio(W/H)equal to1, with W=H=20m.In this case the traffic source has dimensions of100×20m.Street canyon aspect ratios from1to0.5correspond to those for which a skimming flow regime[16]develops.This is the most common flow regime found in most European city centres and American cities[19].
3.2FLUENT General Flow Setup
The computational domain used to simulate the neutral atmospheric boundary layer is built using both irregular tetrahedral and hexahedral grids withfiner resolutions close to the ground.The overall number of computa-tional cells used is of the order of one million for most
372S.Di Sabatino et al. cases.The bottom surface(i.e.ground)is specified as
a rigid plane with a specified surface roughness.All
FLUENT simulations are carried out by using a simple
velocity inlet condition(specifying velocity,turbulent
kinetic energy k(TKE)and turbulent dissipation rate
profiles),by specifying an operating pressure at a
point in the middle of theflow domain and by using
outflow conditions at the outlet i.e.the massflow rate is
the same as the inlet.All simulations are carried out
as steady state solutions of the Navier–Stokes equa-
tions and for the conservation of mass species.Second
order discretisation schemes are used to increase the
accuracy and reduce numerical diffusion.The specific
methods are second order upwinding[1]for pressure,
momentum,k and ,the SIMPLE scheme is used for
the pressure-velocity coupling.
FLUENT uses an iterative method to solve the alge-
braic system of equations.Starting from an initial guess
theflow variables are recalculated in every iteration
until each equation is solved up to an user specified
error.The termination criterion is usually based on
the residuals of the corresponding equations.Scaling of
the residuals is usually done with the residuals after the
first iteration.A termination criterion of10−5is used.
Overall,a simulation took about8hours on double
processors of an OPTERON machine.To get steady
state solutions for each case considered in this paper,
residuals reached the chosen level and were stopped
after about100iterations.As certain quantities reached
convergence at a different rate than other quantities,
we checked thatflow values remained unchanged with
respect to the number of iterations.To quantify the
influence of the grid resolution on the solution a grid
convergence study is made.For this,different system-
atically and substantially refined grids are used.The
grid refinement ratio is a minimum of1.1to allow
the discretization error to be differentiated from other
error sources(iterative convergence errors,computer
round-off etc.)[22].
At the inlet,we use a velocity profile equal to the
wind speed profile used in ADMS-Urban(Eq.1)while
turbulent kinetic energy and dissipation rate profiles
are specified as follows:
k=
u∗2
Cμ
1−
z
δ
(2)
and
=u ∗3
1−
z
(3)
whereδis the atmospheric boundary layer depth and Cμis a coefficient used to define the eddy viscosity in k− models[15].
Before proceeding with full three-dimensional simu-lations as will be required when considering a portion of an urban area or street canyons,various simulations are performed using a three-dimensional(3D)flow domain to simulate the simplest atmospheric boundary layer flow over a surface with a specified surface roughness length.A value of Cμequal to0.013is used as suggested by Richards and Hoxey[20]to avoid high near-ground turbulence levels forflow overflat rough surfaces which are typically overestimated in CFD codes.Also this dif-ferent Cμvalue overcome the general difficulty due to the decay of turbulence kinetic energy with the distance downstream often encountered in CFD atmospheric neutral boundary layer with the standard k− model. As a consequence of the alteration of the Cμvalue,also σ (the turbulent dissipation rate Prandtl number)is ad-justed to3.22,in order to satisfy the transport equation for turbulent kinetic energy and turbulent dissipation rate in the k− model.There are some uncertainties regarding the exact values of the simulated surface roughness due to FLUENT’s formulation for surface roughness.This relies on the use of an equivalent sand grain roughness,and a somewhat arbitrary roughness constant C s between0and1.Some tests are also per-formed with different grid sizes tofind the optimum value for K s which is taken to be equal to20,a value which is somewhere in the middle between the value of10and32.6found in literature([23]).The size of the computational domain is5,000by5,000m in the horizontal and800m in the vertical.Figure1shows the velocity profiles obtained at different positions down-wind of the inlet.From thefigure it can be seen that the logarithmic velocity profile is maintained very well
z
[
m
]
u [m s
−1
]
Fig.1Velocity profiles obtained with FLUENT at different positions downwind of the inlet
Flow and pollutant dispersion in street canyons
373
k [m 2 s –2]
z [m ]
10
10
1010
ε [m 2 s 3
–3]
z [m ]
Fig.2k (Top )and (bottom )profiles obtained with FLUENT
at different positions downwind of the inlet
throughout the length of the computational domain.This check should be done before doing any dispersion calculations from a single point or line source in the neutral atmospheric boundary as it likely affects the final concentration at the ground.
Figure 2shows the predicted k (top)and (bottom)profiles generated by the k − model at various posi-tions downwind of the inlet.The predicted TKE levels
tend to become smaller along the domain near ground but they tend to increase above a height of 500m.In the region near the ground (up to 100m),the average TKE values reduce to approximately 75%,while at the ground they reduce to approximately 85%of the inlet values at distance of 5,000m.This reduction over this large distance is much smaller than that found with previous CFD calculations using the standard k − model as reported in [21].Also this reduction in TKE values can be considered acceptable in the context of the modelling we are doing.As before,a check on the performance of the TKE along the entire domain should be done before proceeding with further calcu-lations.The turbulent dissipation rate is maintained very well throughout the length of the computational domain.Based on those results the k − model with the modifications already mentioned is adopted as the main turbulent model.
3.3FLUENT Small Building Arrangement Flow Setup
Several grids are tested for the different simulations performed in
this study.For the comparison of FLU-ENT results with CEDVAL,a geometry of four square shaped rings of model buildings forming an intersection with an offset in one of the two lanes (two buildings are equipped with a slanted roof (45o roof angle)is used.The geometry studied is shown in Fig.3,while a part of the domain and the grid used for FLUENT simulations are shown in Fig.4.
After performing a test to verify that the solution was domain independent and grid shape and size indepen-dent,a structured grid with refined elements near the
Fig.3Sketch of the
geometry of the CEDVAL experiment
374S.Di Sabatino et
al. Fig.4Domain and grid used in FLUENT to simulate the CED-
VAL experiment
ground,inside the intersection,is chosen.The refine-
ment is shown in Fig.4.The smallest dimensions of the
elements near the ground and inside the intersection
are equal to0.5m while they are about2m outside
the intersection.The overall number of computational
cells used is of the order of1.5·106.The bottom surface
(i.e.ground)is specified as a rigid plane with a specified
surface roughness,as for the simulations carried out in
the previous section.Also the velocity inlet profile and
turbulent kinetic energy and dissipation rate profiles
are specified as in the previous section.
3.4FLUENT General Dispersion Setup
Various models are available in FLUENT to model
dispersion of airborne material.In this study only the
advection diffusion(AD)module is used.In turbulent
flows,FLUENT computes the mass diffusion which
satisfies the conservation of mass as follows:
J CO=−
ρD CO+
μt
Sc t
∇Y CO(4)
where D CO is the diffusion coefficient for CO in the
mixture,μt=ρCμk2 is the turbulent viscosity,Y CO is
the mass fraction of CO,ρis the mixture density.In
Eq.4,Sc t=μt/(ρD t)is the turbulent Schmidt number,
where D t is the turbulent diffusivity.
3.5FLUENT Simple Traffic Source Dispersion Setup
Atfirst we study the case of CO dispersion from a
simple traffic source i.e.a traffic source placed in the
neutral atmospheric boundary layer without buildings
in order to assess the validity of dispersion results.
Again as in[21]a reduced computational domain size
of1,000by500m in the horizontal and150m in the
vertical is used for the gas dispersion simulations.The
same inlet CO massflow rate of10g/s set in ADMS-
Urban model is used in FLUENT.The reduced domain
size allowed us to further refine the grid near the release
and downstream of it especially in those regions where
the plume is evolving.The grid elements are about
0.25m in size near the traffic source,and grow with a
ratio of1.2.The traffic source is positioned perpendic-
ular to the wind direction at100m downwind of the
inlet section.The overall number of computational cells
used is of the order of one million.The traffic source
is simulated by separating a volume in the geometry
at the required discharge position and by setting a CO
source term(g/m3-s)for this volume.The area forming
the base of this volume has the same dimensions of the
traffic source set in ADMS-Urban,while the height of
the volume is set to0.5m.Several tests were performed
before choosing this value by verifying the indepen-
dency of FLUENT results from the specific choice of
the height of the volume source.It was found that any
height between0.5and2m would not influence the
final concentration results.
3.6FLUENT Street Canyon Dispersion Setup
We consider the case of CO dispersion from a traffic
source placed in a street canyon of height H and width
W.The aspect ratio of the street canyon is kept con-
stant,W/H=1,for all cases considered in this section.
The street canyon geometry is built by placing at a
distance of100m from the inlet two identical blocks
each being100m long100m wide and20m high.The
same traffic source discussed in the previous section is
used here.All FLUENT simulations for this case use
a domain and grid characteristics similar to those used
to simulate the simple traffic source and the CEDVAL
experiments.
Flow and pollutant dispersion in street canyons375
4Results and Discussion
4.1Comparison with CEDVAL Dataset
Figures5and6show velocity vectors on two vertical planes at y/H=−2and y/H=2respectively(refer to Fig.3).The plane y/H=−2cuts thefirst lane before the intersection.Figure5shows that FLUENT results are in good agreement with CEDVAL measurements. In particular,we observe the sameflow pattern inside and outside the street canyon.Measurements shows that a small recirculation region forms just behind the first slanted roof.This is also predicted by FLUENT. We also observe that both measurements and numer-ical simulations suggest that the slanted roof before the lane deviates airflow and no vortex is observed within the street canyon.The second plane y/H=2 cuts the second lane after the intersection.In this case the downwind roof,taller than the upwind building acts as an obstacle to airflow and the vortex inside the street canyon is enhanced as shown in Fig.6.This is also shown by the numerical
simulations.
Fig.5Velocity vectors from CEDVAL measurements(top)and FLUENT results(bottom)at y/H=−2
plane Fig.6Velocity vectors from CEDVAL measurements(top)and FLUENT results(bottom)at y/H=2plane
Figure7shows the comparison between FLUENT and CEDVAL dimensionless velocity profiles versus dimensionless height z/H.Profiles are obtained along the same y/H=−2and y/H=2planes in the middle of the street canyon.Thisfigure shows that in the case of the presence of a vortex(corresponding to the plane y/H=2)there is a very good agreement between FLUENT results and CEDVAL measurements.In the other case the CFD model slightly underestimates the velocity within the canyon near the ground.Velocity underestimations have been already found when using the k− model to simulateflow in presence of build-ings with roofs[17].
However it should be noted that in the framework of this work the most interesting case is when the vortex forms within the street canyon.This is the case when the k− model performs best.
4.2Simple Traffic Source
From[21]it is known that FLUENT dispersion spread using the algebraic Reynolds stress model(RSM)[10]
376
S.Di Sabatino et al.
u/u
ref
z /H
y/H=2
u/u
ref
z /H
y/H=_2
Fig.7Velocity profiles from CEDVAL measurements (solid
line )and FLUENT results (cross symbols )at the y /H =−2plane (top )and at the y /H =2plane (bottom )
for a high level point source is smaller than that pre-dicted by ADMS-Urban.We found that this is also the case for both the point source and the simple traffic source using the k − model.Therefore we performed some sensitivity tests for the choice of the most suitable Schmidt number in order to artificially increase the plume dispersion.From the sensitivity test the value of 0.4was the most appropriate one.We used this for all subsequent dispersion simulations except for the street canyon simulation with the wind perpendicular to it.For this case the best choice for the Schmidt number was 0.04as will be discussed later.
Figure 8shows the comparison between FLUENT and ADMS-Urban CO concentrations for the case of a simple traffic source.
The profiles are plotted as a function of x both at ground level and at z =10m.Figure shows that there is a good agreement between FLUENT and ADMS-Urban results at ground level for x <300m,while for x >300m FLUENT CO concentrations are about 2times higher than ADMS-Urban ones.A similar obser-vation can be made for results at z =10m.FLUENT maximum concentration value is the same as ADMS-Urban even though its position is about 70m closer to the source.
FLUENT CO concentrations both at ground level and at z =10m tend to the same asymptotic value at large distance from the source.The same behaviour is shown by ADMS-Urban results even if FLUENT asymptotic value is higher than the ADMS-Urban one.Figure 9shows the CO contour plots obtained by FLUENT (left)and ADMS-Urban (right)on two hor-izontal planes,at ground level (a)and at z =10m (c),and on a vertical plane parallel to the wind flow direction (b).
The ADMS-Urban prediction of the vertical and horizontal spread (Fig.9)reaches a width of 500m at a downwind distance of about 300m whereas the width of the FLUENT predicted plume is 350m at the same position.Despite the diminished Schmidt number the plume spread is still smaller than that predicted by ADMS-Urban both in the horizontal and in the vertical.However,the discrepancy between the two models is much smaller than that reported by [21]for which the discrepancy between the models was about 70%.Also it should be pointed out that we obtained those results by using both a k − and AD model which typically run much faster than a combination of an RSM model and a Lagrangian particle tracking (LP)model as used by [21].
4.3Traffic Source in a Street Canyon
In this section dispersion from a traffic source placed within a street canyon is studied for different wind directions.
At first we consider the case of wind direction perpendicular to the orientation of the street canyon.This is the case for which a full bi-dimensional flow
x [m]
C O [u g /m 3
]
Fig.8ADMS-Urban and FLUENT CO concentration profiles as a function of x coordinate,downwind of the source。