Content uploaded by Patrick Kastner
Author content
All content in this area was uploaded by Patrick Kastner on Apr 18, 2025
Content may be subject to copyright.
Content uploaded by Patrick Kastner
Author content
All content in this area was uploaded by Patrick Kastner on Feb 27, 2023
Content may be subject to copyright.
ARTICLE TEMPLATE
A Cylindrical Meshing Methodology for Annual Urban Computational Fluid
Dynamics Simulations
Patrick Kastneraand Timur Dogana
aCornell University, Ithaca, NY, USA
ARTICLE HISTORY
Compiled December 7, 2020
ABSTRACT
For urban CFD simulations, it is considered a best practice to use a box-shaped simulation do-
main. Box-shaped domains, however, show drawbacks for airflow from several wind directions
as remeshing and additional preprocessing steps become necessary. We introduce a routine
to create a cylindrical mesh that expedites the simulation of arbitrary wind directions using
OpenFOAM. Results computed with the cylindrical domain are validated against wind tunnel
data. We report that the cylindrical method yields comparable results in terms of accuracy and
convergence behavior. Further, run time comparisons in a real-world scenario are conducted
to discuss its advantages and limitations. Based on the findings, we recommend using the
cylindrical approach if at least eight wind directions are analyzed for which we report 18 % run
time savings. The cylindrical domain along with automated best practice boundary conditions
has been implemented in Eddy3D — a plugin for Rhinoceros.
KEYWORDS
CFD; urban; meshing; box-shaped; cylindrical; multi-directional
Introduction
Urbanization and population growth, along with a massive predicted construction volume can
be seen as a unique opportunity to improve the built environment and its quality of living
through integrated and well-informed architectural urban design processes. Such processes lead
to high quality, climate-adaptive architecture that uses passive means to provide comfortable
environments with smaller carbon footprints. Not only in Mediterranean countries but also in
countries with subtropical and tropical climates where the largest construction volumes are
expected, natural ventilation (NV) is one of the most efficient ways of cooling and promises a
significant energy saving potential. In such regions, studies have shown the possibility of saving
up to
50 %
in energy compared to air conditioning (Cardinale et al., 2003; Oropeza-Perez and
Østergaard, 2014).
Author Email: pk373@cornell.edu
To evaluate such savings, building energy modeling (BEM) packages like EnergyPlus and
TRNSYS come with capable airflow network (AFN) solutions for natural ventilation evaluation
in multi-zone building energy models (Huang et al., 1999; Weber et al., 2003). These solutions
rely on pressure coefficient arrays for different wind directions and exterior simulation nodes. For
simple box-shaped buildings without contextual obstructions, look-up tables and fast methods
for surface-averaged pressure coefficient generation exist (Grosso, 1992; Swami and Chandra,
1988). Since then, many attempts have been made to deal with airflow sheltering effects for
simplified urban geometries, and there is evolving literature about wind pressure coefficients
for sheltered buildings that are summarized by Costola et al.. For unique geometries, and if
surrounding buildings exist, further attention is needed to avoid geometric oversimplification
(Cheung and Liu, 2011). This is especially important when it comes to annual analyses, that
is, analyses for all hours of the year, for which multi-directional CFD simulations are needed.
In these multi-directional conditions, computational fluid dynamics (CFD) analyses are used,
either as a standalone tool or to inform the AFN method with more accurate pressure coefficient
(
𝑐𝑝
) input data. CFD is a numerical methodology to calculate desired flow variables on a lattice
within a simulation domain by solving the Navier-Stokes equations (NSE). The usual steps of a
recurring CFD analysis in a design process for the built environment consist of:
(1) modeling the building geometry with CAD software;
(2) meshing the building geometry and topography;
(3)
simulating the problem with appropriately-assigned boundary conditions for multiple
wind directions;
(4)
postprocessing the variables of interest, likely followed by design alterations that lead
back to (1) if goals or constraints have not been met.
The expertise needed to perform such analyses and the associated preprocessing overhead often
impedes a wider use of natural ventilation studies in building and urban scale design workflows.
As a result, NV studies are expensive and usually are only undertaken late in the design process
when significant changes to improve the NV potential are often no longer feasible. Hence, to
incorporate natural ventilation analyses into early design stages, the workflows for annual wind
analysis need to be (1) streamlined, and (2) the time to produce actionable results needs to be
reduced.
In this study, we propose a novel methodology to reduce the preprocessing and simulation time
of annual urban wind simulations by utilizing the CFD library OpenFOAM. For this, we use a
cylindrical simulation domain that allows for a seamless assignment of boundary conditions for
arbitrary wind directions. Further, we discuss meshing issues that might occur when cylindrical
meshes for urban CFD simulations are used. We introduce a robust workflow that expedites
annual wind flow analyses that are relevant for applications shown in figure 1. We investigate
the convergence behavior, accuracy, and run times in two studies:
(1)
In a validation study, we conduct a grid convergence study for four stages of mesh
refinement. Then, we evaluate the accuracy and convergence behavior of both the box-
shaped and cylindrical domains for a reference case by Jiang et al. (2003) from the previous
grid convergence study.
(2)
In a more detailed annual study, we use a square-shaped building array to assess the
differences to complete both meshing and simulation referred to as run time.
Annual wind
CFD methodology
Urban CAD model
Annual
wind data
Building Performance
Simulation
Scope of
this work
Airflow networks
analysis
cpvalues for every 5°
wind direction increments
Estimation of annual
air change rates
Outdoor thermal
comfort analysis
Air velocities at
high spatial resolution
Pedestrian wind
comfort analysis
Figure 1.: Collocation scheme of the investigated approach within the urban simulation process.
Background
When it comes to spatial analysis and decision aiding for the built environment with CFD,
particular attention should be paid to meshing methodologies. Several best practice guidelines
for urban flow problems have been published over the years (Franke et al., 2004; Franke,
2006; Franke and Baklanov, 2007; Franke et al., 2010; Tominaga et al., 2008; Blocken,
2015; Ramponi and Blocken, 2012), all of which propose best practices concerning domain
dimensions, convergence criteria, and relaxation factors. Little focus, however, has been put on
how to best approach the meshing of a simulation domain for annual wind simulations.
For urban CFD simulations that take into account a single wind direction, it is considered best
practice to construct a box-shaped wind tunnel (WT) with predefined dimensions in relation
to the building geometry. A commonly-used practice proposed by Tominaga et al. suggests a
simulation domain size of
𝑧=6·𝐻𝑚𝑎 𝑥
,
𝑙=20 ·𝐻𝑚𝑎 𝑥
and
𝑤
given a blocking ratio of
≤3 %
,
where
𝑧
,
𝑙
, and
𝑤
are the dimensions of the simulation domain and
𝐻𝑚𝑎 𝑥
is the height of the
tallest building in the building agglomeration. The blocking ratio is defined as the ratio between
the projected facade area of the buildings perpendicular to the inlet to the total area of the inlet
in wind direction.
There are two approaches to account for different wind directions: one may either rotate the
building geometry that is placed in the simulation domain (figure 2 (a)), or set up an entirely
new simulation domain with corresponding boundary conditions for each additional wind
direction (figure 2 (b)). In each subfigure, the dashed lines represent the wind tunnels and
wind directions after an arbitrary rotation. Both options come with disadvantages. In the first
case, the entire simulation domain needs to be remeshed for every additional wind direction.
However, as the height of the WT depends on a constant
𝐻𝑚𝑎 𝑥
, a change in the windward-facing
projected facade area introduced by rotation, results in a different width of the WT. In manual
preprocessing setups, width adjustments for adequate blocking ratios are often neglected. As
a result, the same WT width is used for all wind directions, which may lead to convergence
problems (figure 2 (a)). For the second approach shown in figure 2 (b), the coordinates of
the WT and the boundary conditions need to be adjusted to account for changes in wind
directions, thus likely violating the best practice dimensions for the WT width if omitted.
Hence, box-shaped simulation domains show drawbacks when many wind directions need to
be simulated because of the given climate data. While (re)meshing of single, exposed building
geometries for few wind directions is manageable, more involved problems (many directions
with surrounding urban context) become increasingly complex to handle.
(a) (b)
Figure 2.: Top view of simulation domains to account for different wind directions.
To avoid the creation of a new mesh for every wind direction, we propose a cylindrical
computational mesh that allows for a streamlined simulation of arbitrary wind directions,
see Case C and C’ in figure 3. Further, the setup of boundary conditions is automated such
that a significant amount of time will be saved for the setup of an annual wind analysis (up
to 32 or more wind directions). More specifically, every lateral cylinder patch represents
an individually defined angular increment and can be assigned to either an inlet or outlet
boundary condition depending on the particular wind direction (figure 4). Moreover, the angular
increment determines the block size of the inner rectangle. This makes the same mesh reusable
for the simulation of any arbitrary wind direction. Case A and A’ in figure 3 illustrate the
box-shaped wind tunnel, whereas Case B/B’ and C/C’ illustrate a square-shaped and cylindrical
simulation domain, each of them with best practice dimensions imposed. Little is known
about cylindrical meshes for this purpose, hence, a thorough study of accuracy, convergence
behaviors, and actual computational speed gains are required.
Methodology
Validation study
This section consists of two analyses: first, we conducted a grid independence study for a
box-shaped domain for a single wind direction and a single building geometry. With the
sufficiently-refined grid, we compared its accuracy and convergence behavior to a mesh
Case A Case B Case C
15 Hmax
Hmax
5 Hmax
s.t. blocking ratio = 3 %
6 Hmax
15 Hmax
15 Hmax
Building geometries
inlet
outlet
15 Hmax
15 Hmax
Projected
facade area
Top vi ew Front vi ew Top vi ew Front view
Case A’ Case B’ Case C’
15 Hmax
Hmax
5 Hmax
s.t. blocking ratio = 3 %
6 Hmax
15 Hmax
15 Hmax
Building geometries
inlet
outlet
15 Hmax
15 Hmax
Projected
facade area
Top vi ew Front vi ew Top vi ew Front view
Figure 3.: Top row: top views of the simulation domain for an arbitrary urban area; Case A
shows a conventional simulation domain, Case B shows a square-shaped simulation domain,
and Case C shows a cylindrical simulation domain, each for a wind direction of 0
°
. Bottom
row: Cases A’-C’ for wind directions of 45°. The illustrations are not true to scale.
produced with the cylindrical approach.
Jiang et al. (2003) conducted an extensive study in an atmospheric boundary layer (ABL) WT
in which a cuboid with two openings had been investigated experimentally to estimate the
cross-ventilation behavior (figure 5).
The geometry in figure 5 (a) was modelled in
Rhinoceros
with infinitely thin walls, neglecting
the
6 mm
wall thickness of the scale model. The Grasshopper plugin Eddy3D was used to
automate the preprocessing, including the assignment of boundary conditions. The mesh
was created by using the blockMesh utility for the background mesh and snappyHexMesh to
subsequently snap the background mesh to the building geometry, producing a mixed polyhedral
mesh. The dimensions of the box-shaped simulation domain are
(5.75 ·2.75 ·1.5) m
. When
using a cylindrical mesh, while ensuring not to violate the best practice dimensions for length,
width, and height, the ground area of the mesh is larger. It is characterized by a higher cell
count than one would anticipate with the conventional approach shown in figure 3 for Case A.
To ensure a fair comparison between both approaches, we created the blockMesh with identical
Lateral patch
Angular
increment
Cylindrical patches
with inlets/outlets
imposed
Figure 4.: Top view of the lateral cylinder patches. A coarse setting is shown left, a substantially
finer mesh is shown on the right.
(a) (b)
h = 0.25 m
h/2
0 h
Figure 5.: (a) Schematic of the validation wind tunnel geometry; (b) Vertical section through
validation domain with geometry spanning from 0to ℎ.
cell sizes in the areas where the buildings were placed and used identical mesh refinement
levels. Figure 6 illustrates both the box-shaped and the cylindrical domains considering best
practice guidelines as they were created in Grasshopper. In this example, the lateral patches of
the cylindrical domain consist of 5°straight line segments.
The domain inlet was set to an atmospheric boundary layer profile for
𝑈
,
𝑘
, and
𝜔
. At the
outlet of the computational domain, constant pressure is assumed, while the other variables
are assumed to be zero-gradient. The ground and the building walls use the same boundary
conditions: a no-slip condition for velocity, a zero-gradient condition for the pressure, and wall
functions for
𝑘
and
𝜔
. For
𝜈𝑡
, the intelligent wall function called nutUSpaldingWallFunction
was used. The front, back, and top faces are set to symmetric boundary conditions for all
variables. The kinematic viscosity,
𝜈
, was set to
1.5 ×10−5
. The turbulence inlet parameters
were calculated using the following equations:
𝑘=(𝑈∗)2
√𝐶𝑚𝑢
(1)
𝜀=(𝑈∗)3
𝜅(𝑧+𝑧0)(2)
𝜔=
𝜀
𝐶𝑚𝑢 ·𝑘(3)
box-shaped WT cylindrical WT
x[𝑚]y[𝑚]z[𝑚]radius [𝑚]z[𝑚]
2.75 5.75 1.5 4.125 1.5
Figure 6.: 3D visualization of box-shaped wind tunnel (WT) and cylindrical WT.
where
𝑈∗
is the friction velocity, and
𝐶𝑚𝑢 =0.09
is a constant for the turbulence model. The
values used are summarized in table 1.
Table 1.: Turbulence boundary conditions used for the validation study.
Parameter Value
𝑘0.034 56
𝜖0.0835
𝜔10.42
The approach to model the ABL in OpenFOAM is based on the following equations (Wallace
and Hobbs, 2006):
𝑈=
𝑈∗
𝜅𝑙𝑛 𝑧+𝑧0
𝑧0(4)
𝑈∗=𝜅𝑈𝑟 𝑒 𝑓
𝑙𝑛 𝑧𝑟 𝑒 𝑓 +𝑧0
𝑧0(5)
where
𝑈∗
is the friction velocity,
𝜅
is the von Karman constant,
𝑈𝑟 𝑒 𝑓
is the reference velocity
at the reference height
𝑧𝑟 𝑒 𝑓
, and
𝑧0
is the aerodynamic roughness length. In the original
experiment, the atmospheric boundary layer profile of the WT’s inlet velocity was created
by placing Lego Duplo blocks on the windward side of the scale model. Unfortunately, no
visual documentation is provided to estimate the size of the resulting
𝑧0
, hence, a value of
𝑧0=
0.005 m
has been used in this study. All numerical simulations are based on OpenFOAM’s
steady-state simpleFoam solver in combination with a
𝑘−𝑤−𝑆𝑆𝑇
RANS turbulence model.
The pressure-velocity coupling was established with the SIMPLE algorithm using three
non-orthogonal corrector loops. Buoyancy effects were neglected due to air velocities that
are well above
1.8 m s−1
(Tecle et al., 2013; Boulard et al., 1996). Furthermore, we assumed
that convergence was obtained when reaching residuals of
1×10−4f
or
𝑝
and
1×10−5f
or the
remaining fields. For each case, we simulated until the convergence criteria were reached. The
relaxation factors were chosen to be
0.7
for
𝑝
and
0.3
for
𝑈
,
𝑘
and
𝜔
. All simulations ran on
an AMD Ryzen Threadripper 1950X 16-Core Processor running Windows 10. We used the
Docker Version 17.12.0-ce-win47 (15139) to run OpenFOAM 4.1. At most, we ran a maximum
of four OpenFOAM instances at a time on single CPUs on separate threads to avoid affecting
the run times by other processes. All other values including the discretization schemes not
specifically mentioned here were selected according to current best practice guidelines (Franke,
2006).
To compare the OpenFOAM results of both meshing methodologies against the WT data,
measurements by Jiang et al. (2003) were digitized and subsequently interpolated to yield
50 sampling points. The axes were normalized by
ℎ=0.25 m
and
𝑢𝑟 𝑒 𝑓 =12 m s−1
. For
later comparison, vertical, stream-wise velocity measurements were taken at
ℎ
2
, as the largest
deviation from the measured data was found there, see figure 5. First, the results for the
refinement study were sampled with the sample utility using the cellPoint interpolation scheme
in OpenFOAM, which is a linear-weighted interpolation using cell values. The sampled results
were then plotted against the experimental data and the coefficient of determination (
𝑅2
) was
calculated:
𝑅2=1−Í𝑁
𝑖=1(𝑦𝑖−ˆ𝑦𝑖)2
Í𝑁
𝑖=1(𝑦𝑖−¯𝑦𝑖)2,with 0≤𝑅2≤1(6)
To verify and report grid independence, refined meshes were created by increasing the number
of divisions of the background mesh by factors of two in each Cartesian direction while keeping
the levels of surface and feature refinements constant. To provide a standard and consistent
approach to report the results of grid convergence studies (GCS) and error estimations, we
adopted the concept of the grid convergence index (GCI) by Roache which is based on a derived
variable. The derived variable, in our case, is the volumetric flow rate through the opening.
The GCI measures the percentage that the computed value is deviating from the asymptotic
numerical value which is to be interpreted as an error band. In other words, it measures how
much the solution would change by further refining the grid. Moreover, we use Richardson
Extrapolation (RE) to predict the flow rate for an ideal mesh (continuum), thereby estimating
the magnitude of the numerical error. The mesh size for each refinement stage is summarized
in table 2, and the meshes themselves are illustrated in figure 7.
Annual study
A previous study found that a singled out, cubic building geometry is not adequate to highlight
the benefits of the proposed method in terms of overall run times (Kastner and Dogan, 2018). To
establish a more real-world-like scenario, we created simulation domains for a square-shaped,
equidistant building array consisting of cubes with a
20 m
edge length. To ensure a fair
comparison between the meshes, the refined regions in the center of the simulation domain are
identical and the surrounding coarser regions were set up with the same cell divisions. For
this study,
𝑢𝑟 𝑒 𝑓
was arbitrarily chosen to be
5 m s−1
and the turbulence values were calculated
according to equation 1 - 3.
The Cases A and A’ exemplify a rotation of the simulation domain (0
°
and 45
°
representing the
two extremes in terms of the projected facade area) according to the best practice rules if the
blocking ratio is fixed at
3 %
. This leads to an increase in the size of the simulation domain
for Case A’. By simulating these two extreme cases, a full 360
°
study is reproduced with 45
°
stepwise rotations by exploiting the rotational symmetry of A and A’. Moreover, we assessed
a square-shaped simulation domain suggested by Franke and Baklanov (Case B), which is
characterized by automatically-generated inlet and outlet boundary conditions identical to Case
C. This approach, often used as a workaround for expedited case setups, also benefits from
only having to be meshed once no matter which wind direction is imposed. Finally, Case C
represents the cylindrical approach that we propose in this study. To estimate the final run times
of a set of hypothetical wind directions, we summed up the meshing and simulation times and
multiplied them by the corresponding number of wind directions (or rotations). Hence, the
meshing time was taken into account multiple times for Case A and A’, whereas only a single
time for Case B and C.
Results
Validation study
(a) very coarse (b) coarse (c) normal (d) fine
Figure 7.: Excerpt of refined mesh sizes for the validation study.
Figure 7 shows a cropped stream-wise section around the building geometry for each mesh
refinement. For each of the meshes, the vertical velocity samples are depicted in figure 8,
in which the normalized domain height is plotted over the normalized reference velocity
𝑢𝑦
.
By comparing the
𝑅2
of each refinement stage, it is evident that the accuracy of the solution
increases for finer grids. The finest grid, however, under-predicts the normalized velocity,
especially in the opening region.
0.50 0.25 0.00 0.25 0.50 0.75 1.00 1.25 1.50
uy
uref [ ]
0.00
0.25
0.50
0.75
1.00
1.25
1.50
1.75
2.00
z
h[ ]
Wind tunnel
Boxvery coarse,
R
2= 0.921
Boxcoarse,
R
2= 0.946
Boxnormal,
R
2= 0.962
Boxfine,
R
2= 0.952
Figure 8.: Coefficients of determination (
𝑅2
) for vertical velocity probes
𝑢𝑦
at
ℎ
2
for different
mesh sizes.
In the experiment conducted by Jiang et al. (2003), a volumetric flow rate of
0.045 m3s−1
was
measured for the opening of the building geometry. Contrary to the vertical velocity probes, all
stages of the grid refinement confirm the measurement of that derived variable in a converging
manner toward the finer grids (figure 9 and table 2). By evaluating the GCS, the volumetric flow
rate for an ideal mesh would be
0.047 m3s−1
, which is in good agreement with the experimental
results of
0.045 m3s−1
. Furthermore, the ratios of the CGIs confirm that the volumetric flow
rates reported in the GCS are well within the asymptotic range of convergence (Kastner, 2016).
Given the reasonable numerical error band of
∼10 %
, we decided to continue with the “coarse”
grid for the subsequent accuracy comparison.
Table 2.: Parameters of the grid convergence study for four different mesh sizes: very coarse,
coarse, normal, and fine.
Case Cell count ℎ𝑔𝑟¤𝑣[m3s−1] Error (experiment) Error (continuum) GCI [%]
very coarse 124 456 8 1.3 0.0540 17 % 15 % 11.04
coarse 263 919 4 1.6 0.0505 11 % 10 % 6.82
normal 1 165 733 2 1.6 0.0485 7% 6 % 4.94
fine 4 940 280 1 - 0.0471 4 % 3 % -
RE - 0 - 0.0456 - - -
Experiment - - - 0.0450 - - -
To compare the accuracy of the box-shaped and the cylindrical method, the vertical, stream-wise
probes
𝑢𝑦
are plotted at
ℎ
2
, for the “coarse” mesh setting, see figure 10. It is evident that the
012345678
Normalized grid spacing (h) [ ]
0.045
0.046
0.047
0.048
0.049
0.050
0.051
0.052
0.053
0.054
Volumentric flow rate [m3/s]
v (
h
= 8, 4, 2)
v (
h
= 0, RE)
Not considered for RE
Experiment
Figure 9.: Richardson Extrapolation (RE) of the volumetric flow rate
¤𝑣
through the windward
opening based on the grid convergence study.
box-shaped simulation domain achieves a marginally higher
1
accuracy (
𝑅2=96.7 %
) than
the cylindrical simulation domain (
𝑅2=94.1 %
). However, both approaches either under-
and/or overestimate regions with high-pressure gradients which is known as a deficiency of the
steady-state RANS model.
0.50 0.25 0.00 0.25 0.50 0.75 1.00 1.25 1.50
uy
uref [ ]
0.00
0.25
0.50
0.75
1.00
1.25
1.50
1.75
2.00
z
h[ ]
Wind tunnel
Cylinder,
R
2= 0.94
Box,
R
2= 0.97
Figure 10.: Vertical sample
𝑢𝑦
at
ℎ
2
for the box-shaped and the cylindrical simulation domain.
Figure 11 depicts the residuals reported for both cases. Here, the cylindrical domain shows
better convergence behavior for the particular convergence criteria (figure 11 (b)). This results
1
The marginally higher
𝑅2
(
94.6 %
vs.
96.7 %
) in figure 10 vs. figure 8 stems from using three additional mesh boundary layers
for the ground and the building surfaces.
in a simulation that converges after
∼2900
iterations for the cylindrical case, whereas the
box-shaped WT converges after ∼4100 iterations.
10-8
10-7
10-6
10-5
10-4
10-3
10-2
10-1
100
0 1000 2000 3000 4000 5000
Residual
Iteration
Ux
Uy
Uz
p
omega
k
10-8
10-7
10-6
10-5
10-4
10-3
10-2
10-1
100
0 1000 2000 3000 4000 5000
Residual
Iteration
Ux
Uy
Uz
p
omega
k
(a) (b)
Figure 11.: Residuals of box-shaped (a) and cylindrical simulation domain (b).
Annual study
The annual study is concerned with evaluating the run times for a square-shaped, equidistant
building array. The top row in figure 12 shows the top view of the meshes after the blockMesh
routine in OpenFOAM. A detailed summary of the three simulation domains is given in table 3.
For Case A/A’, the width of the WT varies with the angle of the approaching wind (which is
largest in the particular Case A’) due to the constraint to keep the blocking ratio constant. The
bottom row in figure 12 shows horizontal velocity plots at
2 m
above the ground plane. This
confirms visually that all simulation domains are comparable in capturing the flow field, as
shown before.
Figure 13 provides an extrapolation of the individual meshing and simulation time for an annual
analysis of an urban area depending on the number of wind directions. For the individual
meshing times, we report a significantly higher meshing time for Case A’ compared to the three
other cases. The extrapolation in figure 13 reveals that the cylindrical simulation domain (Case
C) yields
18 %
better run times compared to the conventional approach (Case A/A’) if 8 or
more wind directions are simulated. Moreover, Case C shows
39 %
better overall run times
compared to the square-shaped approach (Case B) regardless of the number of wind directions.
Table 3.: Geometry and mesh information about the cases A, A’, B, and C.
Case Dimensions Mesh
In flow
direction [𝑚]⊥to flow
direction [𝑚]
Ground area
[𝑚2]
Projected facade
area [𝑚2]
Cell count Cells per ground
area [𝑐𝑒𝑙𝑙𝑠/𝑚2]
A 1.200 399 4.79E+05 4.000 8.1E+05 1.69
A’ 1.200 1.408 1.69E+06 10.182 1.4E+06 0.83
B/B’ 1.600 1.600 2.56E+06 10.182 1.3E+06 0.51
C/C’ 1.600 1.600 2.01E+06 10.182 9.7E+05 0.48
Case A Case A’ Case B’ Case C’
Figure 12.: Top row: meshes after the blockMesh routine. Case A and A’ correspond to a
box-shaped tunnel for 0 and 45
°
, Case B’ corresponds to a square-shaped approach, and Case
C’ corresponds to a cylindrical approach. Bottom row: horizontal velocity plots at 2 m above
the ground plane.
Discussion
The results show that it is possible and beneficial to employ a cylindrical mesh for annual/multi-
directional urban CFD simulations with OpenFOAM. Where high-pressure gradients are
expected in the simulation domain, the mesh has to be appropriately refined to capture
important flow features and to adequately resolve the boundary layer. We estimated the
numerical error resulting from our validation mesh setting to be
∼10 %
with the help of a grid
convergence study (GCS). GCSs for large meshes are not a trivial task, as the simulation time
grows exponentially with the number of background mesh divisions. However, this method is
useful to both estimate the numerical error and to confirm an adequate convergence behavior
0
500
1000
1500
2000
2500
3000
1 2 4 8 16 32
Time [min]
Number of wind directions
A/A'
B/B'
C/C'
Case Time [min]
Meshing Simulation
A 2.2 47.0
A’ 11.4 60.7
B/B’ 3.5 81.0
C/C’ 2.3 49.7
.
Figure 13.: Meshing and simulation times for cases A/A’, B/B’, and C/C’
by utilizing a reasonable number of mesh refinements. To put this effort into perspective, we
would like to emphasize that this study focuses on the comparison of two different meshing
approaches, not to achieve the best overall accuracy. Here, the GCS confirms that the refinement
strategy follows commonly-accepted guidelines and that the coarse mesh is sufficient for the
goals of this study.
Further, we show that for the coarse mesh, the box-shaped simulation domain achieves a
marginally better accuracy
(𝑅2=96.7 %)
than the cylindrical simulation domain
(𝑅2=94.1 %)
while both domains either under- and/or overestimate regions with high-pressure gradients.
The deficiency in accuracy in high-pressure regions can be attributed to the steady-state RANS
model. While we are aware of the limited applicability of the RANS approach for urban flows,
it is noteworthy that the application of the method proposed in this study focuses on early
design exploration for the built environment. Thus, we emphasize the interest in overall feasible
run times rather than accuracy. However, the cylindrical meshing approach presented can be
used independently of the solver. Therefore, such deficiencies could be avoided by using more
advanced LES or DNS solvers, should the need for very accurate results arise.
In figure 13, we summarize the run time comparisons for an annual analysis with multiple
wind directions that are extrapolated from the individual meshing and simulation times. Here,
the run times reported for Case A and A’ were linearly interpolated to estimate the theoretical
run times in the case of 16 and 32 wind directions and the necessary rotations. For Case A
and A’, it is sufficient to adhere to the best practice dimensions from the wind direction of that
simulation instance (either
0°
or
45°
), whereas a cylindrical domain needs to be created in
a way that wind from all directions can be simulated appropriately. Hence, additional cells
are introduced at the ground surface of the cylindrical domain, see figure 6. Considering that
trade-off, we suggest that simulation domains according to Case A/A’ be used for analyses with
<
8 wind directions
2
. For
≥
8 wind directions, the fact that the cylindrical domain only needs
to be meshed once makes up for the additional number of cells in the simulation domain. Thus,
for ≥8 wind directions, we suggest using the cylindrical approach.
However, it should be emphasized that the advantages of a cylindrical domain may outweigh
the disadvantages even in cases with fewer than 8 wind directions as CFD simulations are
highly sensitive to the quality of the CAD input geometry. First, in practical use with real-
world problems, the scale of most urban geometries suggest overnight or over-the-weekend
simulations. Given these time-spans, improvements in simulations time are indeed desirable
but only magnitudes in run time improvements would change the way of working with such
large-scale simulations. On the contrary, malfunctioning simulation setups that stem from
manually changing the boundary conditions might result in weekends of wasted computing
time. Furthermore, the creation of robust, high-quality meshes often requires time-consuming
and tedious preprocessing efforts, mostly for cleaning the CAD geometries. CFD analyses
for the built environment are usually characterized by iterative design changes that have been
2
In an earlier study, a less optimistic result had been reported which neglected the effect that the rotation enforces by increasing
the width of the WT while keeping the blocking ratio constant (Kastner and Dogan, 2018).
outlined above. Every change is likely to introduce new mesh inconsistencies that, for Case
A and A’, might elicit meshing or convergence issues for every additional wind direction.
Considering these impediments, we suggest making use of the inherent advantages of a
cylindrical simulation domain. Here, the simulation domain only needs to be validated once,
which subsequently guarantees valid simulation results from all directions. Moreover, the
simulations for all wind directions may even be started in parallel after the single mesh is
created. This possibility might help to identify problems in a buildings’ design early on before it
might be discovered with a sequential simulation approach. Consequently, one requirement we
see for the prospective automation of CFD workflows for the built environment is the ability to
produce robust, converging simulation cases. As a first step in that direction, we suggest using
a cylindrical simulation domain if the meshing process of the particular building geometry
seems to be unstable and likely to fail in the case of further geometry rotations.
Apart from mixed polyhedral meshes that were used in this study, other commonly used meshes
include hexahedral-only, tetrahedral-only meshes. As the two latter are known to achieve
better performance in terms of meshing time, future work should investigate whether such
an approach might affect the conclusions drawn. From an implementation perspective, the
cylindrical meshing approach could take advantage of faster meshing times.
In future work, we plan to use the results from such annual wind studies as input for BEM
software to inform the prediction of the natural ventilation potential of buildings.
Conclusion
In this study, we propose a cylindrical mesh for urban wind simulations and show that such
simulation domains are feasible and beneficial with OpenFOAM. We examined a commonly-
used validation case for which we compared the box-shaped computational domain to the
cylindrical simulation domain while considering best practice dimensions for urban CFD
studies. Meshing and simulation time comparisons show that it is recommended to use the
box-shaped approach if fewer than 8 wind directions are intended to be studied. We show
that the cylindrical simulation domain shows better overall run times in the case of 8 or more
wind directions. Concluding, we discuss how a cylindrical simulation domain may likely have
advantages over the box-shaped approach from a methodological perspective, even if fewer
than 8 wind directions are studied.
Acknowledgment
The authors would like to acknowledge the financial support by the Cornell University David
R. Atkinson Center for a Sustainable Future and the Cornell Center for Transportation,
Environment, and Community Health which funded this research.
Nomenclature
ABL Atmospheric boundary layer
AFN Air Flow Networks
BC Boundary condition
BEM Building energy modeling
CAD Computer-aided design
CFD Computational Fluid Dynamics
DNS Direct numerical simulation
GCI Grid convergence index
GCS Grid convergence study
NV Natural ventilation
LES Large eddy simulation
RANS Reynolds-averaged Navier-Stokes
SIMPLE Semi-Implicit Method for Pressure Linked Equations
SST Shear stress transport
WT Wind tunnel
𝑐𝑝Pressure coefficients
ℎHeight, m
ℎ𝑔Normalized grid spacing
𝐶𝑚𝑢 Constant
𝜖Rate of dissipation of turbulence energy, m2s−3
𝑘Turbulence kinetic energy, m2s−2
𝜅von Karman constant
𝑝Pressure, kg m−1s2
𝑟Grid refinement ratio
𝑅2Coefficient of determination
𝑈Velocity, m s−1
𝑢𝑟 𝑒 𝑓 Reference velocity, m s−1
𝑈∗Friction velocity, m s−1
¤𝑣Volumetric flow rate, m3s−1
𝜔Specific dissipation rate, s−1
ˆ𝑦𝑖Predicted values
¯𝑦𝑖Mean values
𝑧Dimensions along z-axis, m
𝑧0Surface roughness length, m
𝑧𝑟 𝑒 𝑓 Reference velocity, m s−1
References
Blocken, B. (2015). Computational fluid dynamics for urban physics : Importance , scales ,
possibilities , limitations and ten tips and tricks towards accurate and reliable simulations.
Building and Environment 91, 219–245.
Boulard, T., J. Meneses, M. Mermier, and G. Papadakis (1996). The mechanisms involved in
the natural ventilation of greenhouses. Agricultural and Forest Meteorology 79(1-2), 61–77.
Cardinale, N., M. Micucci, and F. Ruggiero (2003). Analysis of energy saving using natural
ventilation in a traditional italian building. Energy and Buildings 35(2), 153 – 159.
Cheung, J. O. P. and C. H. Liu (2011). CFD simulations of natural ventilation behaviour in
high-rise buildings in regular and staggered arrangements at various spacings. Energy and
Buildings 43(5), 1149–1158.
Costola, D., B. Blocken, and J. Hensen (2009). Overview of pressure coefficient data in
building energy simulation and airflow network programs. Building and Environment 44(10),
2027–2036.
Franke, J. (2006). Recommendations of the COST action C14 on the use of CFD in predicting
pedestrian wind environment. In The Fourth International Symposium on Computational
Wind Engineering, pp. 529–532.
Franke, J. and A. Baklanov (2007). Best practice guideline for the CFD simulation of flows in
the urban environment: COST action 732 quality assurance and improvement of microscale
meteorological models. University of Hamburg.
Franke, J., A. Hellsten, H. Schlünzen, and B. Carissimo (2010). The Best Practise Guideline
for the CFD simulation of flows in the urban environment : an outcome of COST 732. In The
Fifth International Symposium on Computational Wind Engineering (CWE2010), Chapel
Hill, pp. 1–10.
Franke, J., C. Hirsch, A. G. Jensen, H. Krus, M. Schatzmann, P. S. W. Miles, S. D., J. A. Wisse,
and N. G. Wright (2004). Recommendations on the Use of CFD in Wind Engineering.
Technical report, Joint publication.
Grosso, M. (1992). Wind pressure distribution around buildings: a parametrical model. Energy
and Buildings 18(2), 101–131.
Huang, J., F. Winkelmann, and F. Buhl (1999). Linking the COMIS Multizone Airflow Model
with the EnergyPlus.
Jiang, Y., D. Alexander, H. Jenkins, R. Arthur, and Q. Chen (2003). Natural ventilation
in buildings: Measurement in a wind tunnel and numerical simulation with large-eddy
simulation. Journal of Wind Engineering and Industrial Aerodynamics 91(3), 331–353.
Kastner, P. (2016). Customizing OpenFOAM to assess wind-induced natural ventilation
potential of classrooms: A case study for BRAC University. Master’s thesis, Technische
Universität München.
Kastner, P. and T. Dogan (2018). Streamlining meshing methodologies for annual urban CFD
simulations. In eSim 2018.
Oropeza-Perez, I. and P. A. Østergaard (2014). Energy saving potential of utilizing natural
ventilation under warm conditions – a case study of mexico. Applied Energy 130, 20 – 32.
Ramponi, R. and B. Blocken (2012). CFD simulation of cross-ventilation for a generic isolated
building: Impact of computational parameters. Building and Environment 53(0), 34–48.
Roache, P. J. (1994). Perspective: A Method for Uniform Reporting of Grid Refinement Studies.
Journal of Fluids Engineering 116(3), 405.
Swami, M. and S. Chandra (1988). Correlations for pressure distribution on buildings and
calculation of natural-ventilation airflow. ASHRAE transactions 94(3112), 243–266.
Tecle, A., G. T. Bitsuamlak, and T. E. Jiru (2013). Wind-driven natural ventilation in a low-rise
building: A Boundary Layer Wind Tunnel study. Building and Environment 59, 275–289.
Tominaga, Y., A. Mochida, R. Yoshie, H. Kataoka, T. Nozu, M. Yoshikawa, and T. Shirasawa
(2008). AIJ guidelines for practical applications of CFD to pedestrian wind environment
around buildings. Journal of Wind Engineering and Industrial Aerodynamics 96(10-11),
1749–1761.
Wallace, J. M. and P. V. Hobbs (2006). Atmospheric Science: An Introductory Survey (2 ed.).
Academic Press.
Weber, A., M. Koschenz, V. Dorer, M. Hiller, and S. Holst (2003). TRNFLOW, a new tool for
the modelling of heat, air and pollutant transport in buildings within TRNSYS.
