Conference PaperPDF Available

Streamlining meshing methodologies for annual urban CFD simulations



For environmental CFD simulations, it is considered best practice to use a box-shaped wind tunnel as simulation domain. A box-shaped wind tunnel, however, shows drawbacks when it comes to simulating air flow from several wind directions-remeshing and additional preprocessing steps may be necessary and can be considerable time constraints. We utilize a routine implemented in Grasshopper to create a cylindrical computational mesh that allows for the simulation of arbitrary wind directions in a streamlined manner with the open source software OpenFOAM. We estimate the time savings that are possible along with specific mesh properties to take advantage of the proposed method. For validation purposes, commonly used wind tunnel data are presented. A proof of concept tool is implemented in the Rhinoceros CAD modeling environment and will be released publicly.
Streamlining meshing methodologies for annual urban CFD simulations
Patrick Kastner, Timur Dogan
Cornell University, Ithaca, NY, USA
For environmental CFD simulations, it is considered best practice to use a box-shaped wind tunnel as simulation
domain. A box-shaped wind tunnel, however, shows drawbacks when it comes to simulating air flow from several wind directions
— remeshing and additional preprocessing steps may be necessary and can be considerable time constraints. We utilize a
routine implemented in Grasshopper to create a cylindrical computational mesh that allows for the simulation of arbitrary
wind directions in a streamlined manner with the open source software OpenFOAM. We estimate the time savings that are
possible along with specific mesh properties to take advantage of the proposed method. For validation purposes, commonly
used wind tunnel data are presented. A proof of concept tool is implemented in the Rhinoceros CAD modeling environment and
will be released publicly.
Keywords: CFD, meshing, urban, cylindrical, box-shaped, annual, wind tunnel
Urbanization and population growth, along with a massive
predicted construction volume can be seen as a unique op-
portunity to improve the built environment and quality of
life through integrated, and well-informed architectural ur-
ban design processes. Such processes lead to high quality,
climate-adaptive architecture that uses passive means to pro-
vide comfortable environments which in turn are character-
ized by smaller carbon footprints. In areas where the largest
construction volumes are expected, notably in subtropical
and tropical climates, natural ventilation (NV) is one of the
most efficient ways of cooling and promises a significant
energy saving potential. In such areas, studies have shown
the possibility of saving up to 50 % energy compared to me-
chanical ventilation (Cardinale et al.,2003;Oropeza-Perez
and Østergaard,2014).
Architectural design for good NV supply remains challeng-
ing due to its many physical and computational variables
involved and the expert knowledge needed. As a result, the
simulations are expensive, and they are usually not employed
until the very end of the design process — often resulting in
design alterations no longer being feasible. Thus, to incorpo-
rate natural ventilation analysis into early design stages, the
workflows for annual wind analysis need to be (1) stream-
lined; and (2) the time to produce actionable results needs
to be reduced. In this study, we propose a novel methodol-
ogy to reduce the overall preprocessing and simulation time
of annual urban wind simulations by utilizing the Compu-
tational Fluid Dynamics (CFD) software OpenFOAM and
optimizing the shape and the creation of the simulation do-
main. Moreover, we investigate meshing issues that might
occur while employing cylindrical meshes for urban CFD
simulations. In doing this, we hope to create a robust work-
flow that expedites annual wind flow analysis into existing
urban energy simulations as shown in figure 1.
Building energy modeling (BEM) packages like Energy Plus
and TRNSYS come with capable airflow network (AFN)
solutions for natural ventilation evaluation in multi-zone
building energy models. These solutions rely on pressure
coefficient arrays for different wind directions and exterior
simulation nodes. For simple box-shaped buildings without
contextual obstructions, lookup tables and fast methods for
surface-averaged pressure coefficient generation exist. For
instance, two examples are EnergyPlus (Swami and Chan-
dra,1988) or the wind-pressure distribution model CpGen++
developed for COMIS (Grosso,1992). Since then, many
attempts have been made to deal with air flow sheltering ef-
fects for simplified urban geometries and there is an evolving
literature about wind pressure coefficients for sheltered build-
ings that is summarized extensively by (Costola et al.,2009).
For specific sites, however, further attention is needed to
avoid geometric oversimplification (Cheung and Liu,2011).
In such cases, computationally expensive Fluid Dynamics
(CFD) analysis is required. The expertise to perform such
an analysis and the associated simulation overhead, often
hinder a wider use of AFN based natural ventilations studies
in urban and building scale design workflows.
CFD is a numerical methodology to calculate desired flow
variables on a number of grid points within a simulation do-
main by solving discretized Navier-Stokes equations (NSE).
The usual steps of a recurrent CFD analysis for an optimiza-
tion process for the built environment consist of:
1. Modeling the building geometry with CAD software
2. Meshing the building geometry and topography
Simulating the problem with appropriately assigned
boundary conditions
Proceedings of eSim 2018, the 10ᵗʰ conference of IBPSA-Canada
Montréal, QC, Canada, May 9-10, 2018
ISBN 978-2-921145-88-6
wind CFD
Urban CAD model
wind data
Simulation software
Scope of this work
Airflow networks
cpvalues for every
5° wind direction
Estimation of annual
air change rates
Outdoor comfort
Air velocities with a high
spatial resolution
Figure 1: Schematic of how the scope of this study integrates
with existing workflows.
Post-processing the variables of interest, likely followed
by design alterations and referring back to 1., based on
the results obtained
The geometric optimization of the built environment through
CFD warrants particular attention, especially when it comes
to efficient meshing methodologies. Although several best
practice guidelines for environmental flow problems have
been published over the years (Franke et al.,2004;Franke,
2006;Franke and Baklanov,2007;Franke et al.,2010;Tom-
inaga et al.,2008;Blocken,2015;Ramponi and Blocken,
2012), all of which propose best practices with respect to
domain dimensions, convergence criteria and relaxation fac-
tors. Little focus, however, has been put on how to best
approach annual wind simulations, let alone utilizing results
from CFD studies for more complex analysis like outdoor
comfort studies.
For basic urban CFD simulations, it is considered best prac-
tice to construct a box-shaped virtual wind tunnel with pre-
defined dimensions with respect to the building geometry
that shall be simulated. A widely used best practice pro-
posed by (Tominaga et al.,2008) suggests the size of the
simulation domain to be
z= 6Hmax
l= 20Hmax
given by a blocking ratio of
, where z, l, and w are
the dimensions of the domain and
is the height of the
tallest building in the building agglomeration to be simu-
lated. The blocking ratio is defined as the ratio of the area
of the building perpendicular to the inlet to the total area
Figure 2: Wind rose of annual wind data from Ranchi, East
of the inlet. A visual representation of those suggestions is
illustrated in figure 4(a).
The result, a box-shaped wind tunnel, however, shows draw-
backs when it comes to simulating air flow from several
wind directions, which may vary from 0
to 359
over the
course of one year depending on the local wind directions.
A seasonal climate without a clear prevalent wind direction
for which simulations from many directions are necessary is
illustrated in figure 2.
As a result, remeshing and/or additional preprocessing steps
with regard to the geometry may be necessary and can be a
considerable overhead, especially for larger urban scale mod-
els and software without a graphical user interface (Open-
FOAM). While (re)meshing of single, exposed building
geometries for few wind directions is manageable, more
complex problems (annual wind analysis with surrounding
urban context) become increasingly complicated to handle.
For such annual analysis, one would usually simulate the
building geometry for a number of wind directions that are
considered to be viable, followed by postprocessing steps
to account for the gaps. There are two viable approaches to
account for different wind directions: one can either alter
the orientation of the building geometry that is placed in the
so-called artificial wind tunnel figure 3(a) or set up an en-
tirely new simulation domain as well as boundary conditions
for each wind direction figure 3(b).
Evidently, both options come with disadvantages. For the
first option, the geometry needs to be remeshed for every
additional wind direction since x and y coordinates of build-
ing elements change respectively. For the second option,
the boundary conditions need to be adjusted to account for
the alteration in wind directions, thus possibly violating the
dimensional rules put forth by (Tominaga et al.,2008). To
circumvent remeshing the geometry for every wind direction,
and thus to reduce overhead, we propose a cylindrical com-
putational mesh that allows for simulating arbitrary wind
Proceedings of eSim 2018, the 10ᵗʰ conference of IBPSA-Canada
Montréal, QC, Canada, May 9-10, 2018
ISBN 978-2-921145-88-6
(a) (b)
Figure 3: Top-view of two approaches to account for differ-
ent wind directions. The black square represents the building
directions in a streamlined manner, see figure 4(b).
Furthermore, the proposed method automates setup of new
boundary conditions so that a significant amount of time
will be saved to change the boundary conditions in case of
an annual wind analysis (up to 72 or more wind directions).
More specifically, every lateral cylinder patch represents
a 5
change and can be assigned to either inlet or outlet
conditions depending on the wind direction, see figure 9.
Given that, the mesh is reusable for any wind direction that
might be of interest later in time.
By employing a cylindrical mesh while making sure not
to violate the aforementioned best practice dimensions, the
ground area of the mesh is larger and thus characterized
by a higher cell count than one would anticipate with the
conventional approach shown in figure 4(a). The goal of
this study is to quantify the time differences by reducing
overhead with respect to the corresponding mesh proper-
ties. To estimate advantages and drawbacks, we conduct a
Richardson Extrapolation for four stages of mesh refinement
and investigate both a commonly used wind tunnel reference
case by Jiang et al. (2003) for one of those refinements.
CFD simulations are highly sensitive about their BC and the
fineness of the mesh used. Therefore, we validated one of
the three simulation cases against measured data to be able
to examine the accuracy of the results.
All numerical simulations are based on the open source CFD
library OpenFOAM, using its steady-state RANS models
and solvers in combination with a
model. While we are aware of the limited applicability of
the RANS equations for environmental flows, it is impor-
tant to emphasize that this study focuses on early design
methods for the built environment, thus emphasizing the
interest in simulation time rather than strict accuracy. The
pressure-velocity coupling was calculated with the SIMPLE
algorithm using three non-orthogonal correctors. Buoyancy
effects were neglected due to air velocities that are well
1.8 m s−1
(Tecle et al.,2013;Boulard et al.,1996).
Furthermore, we assumed that convergence was obtained
when reaching residuals of
1×10−4 f
1×10−5 f
the remaining parameters. The relaxation factors were cho-
sen to be 0.7 for pand 0.3 for U,kand ω.
All simulations were done 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 Open-
FOAM 4.1. At most, we ran a maximum of four OpenFOAM
instances at a time on single CPUs on separate threads to
avoid simulation times being affected by other processes
hogging resources.
Jiang et al. (2003) conducted an extensive study in an atmo-
spheric boundary layer (ABL) wind tunnel (WT) in which
a scale model had been investigated experimentally. One
scale model that had been used is a cuboid with two open-
ings for investigations of the ”cross-ventilation” behavior,
see figure 5. The geometry in figure 5was modeled in
Rhinoceros 5
with infinitesimally thin walls, neglecting the
wall dimensions of the wind tunnel scale model of
6 mm
The plugin Grasshopper was used to automate the pre-
processing, including the assignment of boundary condi-
tions. The mesh was created by using the blockMesh utility
for the background mesh and snappyHexMesh to subse-
quently snap the background mesh to the building geometry.
The dimensions of the box-shaped simulation domain are
5.75 ×1.16 ×1.5 m
. The domain inlet was set to an ABL
profile for
, and
. At the outlet of the computational
domain, a constant pressure is assumed, while the other vari-
ables 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 pres-
sure and wall functions for
. For the
, an intelligent
wall function was used. The front, back, and top faces are
set to symmetry boundary conditions for all variables. The
kinematic viscosity,
, was set to
1.5 ×10−5
. The turbu-
lence inlet parameters were calculated using the following
κ(zzmin +z0)(2)
Cmu ·k(3)
is the friction velocity, and
is a constant
for the turbulence model being
. The values used are
summarized in table 1.
Proceedings of eSim 2018, the 10ᵗʰ conference of IBPSA-Canada
Montréal, QC, Canada, May 9-10, 2018
ISBN 978-2-921145-88-6
3 % blocking ratio 3 % blocking ratio15 Hmax /
15 Hmax
6 Hmax
6 Hmax
5 Hmax
(a) (b)
Figure 4: Top-view of the (a) proposed dimensions of simulation domain by (Tominaga et al.,2008) for an arbitrary urban area;
(b) proposed cylindrical simulation domain accounting for the same requirements. The perimeter of the cylindrical domain
consists of 5 straight line segments. A more detailed illustration of the resulting mesh is given in figure 9.
(a) (b)
h = 0.25 m
Figure 5: (a) Schematic of the reference model that was investigated in the wind tunnel by (Jiang et al.,2003). The dimensions
are given in meters. (b) Vertical section through validation domain for mesh sensitivity purposes.
Proceedings of eSim 2018, the 10ᵗʰ conference of IBPSA-Canada
Montréal, QC, Canada, May 9-10, 2018
ISBN 978-2-921145-88-6
Table 1: Turbulence boundary conditions used for the vali-
dation study.
Parameter Value
k0.034 56
The approach to model the ABL in OpenFOAM is based on
the following equations (Wallace and Hobbs,2006):
κln zzmin +z0
ln Zref +z0
is the friction velocity,
is the von Karman con-
stant being
= 0.41
is reference velocity at reference
is the reference height and
is the aerodynamic
roughness length.
The atmospheric boundary layer profile of the inlet velocity
in the WT 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 or the
resulting z0. Thus, a value of z0= 0.005 was used.
To compare the OpenFOAM results in a quantitative manner,
the data was digitalized as well as interpolated using 50 sam-
pling points. The axis are normalized by height =
0.25 m
12 m s−1
. For later comparison, the vertical, stream-
wise measurements by Jiang et al. (2003) were taken at
, as
the most significant deviation from the measured data was
found there, see figure 5. The results were then sampled with
the sample utility using the cellPoint interpolation scheme in
OpenFOAM. Finally, the sampled results were compared to
the experimental values by plotting them against each other
as well as by calculating the coefficient of determination
R2= 1 PN
i=1(yi¯yi)2,with 0R21(6)
The refined meshes were created by varying the size of the
background mesh by factors of two in each direction of the
coordinate system, while keeping the levels of surface and
feature refinements constant. The mesh size for each refine-
ment stage is summarized in table 2, the meshes themselves
are illustrated in figure 6.
The results of the mesh refinement study are depicted in
figure 8in which the normalized domain height is plotted
over the normalized reference velocity. By comparing the
of each refinement stage, it is evident that the accuracy
of the solution increases for finer grids. The finest grid,
however, underpredicts the normalized velocity, especially
in the opening section. In the interest of time and given its
reasonable accuracy, we decided to use the ”coarse” grid
refinement for the subsequent time comparisons.
To provide a standard and consistent approach to report re-
sults of grid convergence studies as well as error estimations,
Roache (1994) suggests to calculate the grid convergence
index (GCI) for the selected grid. 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 with a further refinement of the grid.
A small GCI indicates that the values are within the asymp-
totic range. The results of the spatial convergence study are
depicted in table 2.
Thus, we may state that the volumetric flow rate for an
ideal mesh would be
0.046 m3h−1
with a numerical error
band of
7 %
with respect to the second finest grid. In
the experiment done by Jiang et al. (2003), a volumetric
flow rate of
0.045 m3s−1
was measured which confirms the
results obtained in this study.
Mesh refinements studies for cases with large meshes are
not a trivial task, as the simulation time grows exponentially
with the number of cells. Thus, this method is useful to
estimate the numerical error without conducting a full re-
finement study especially for large-scale simulations. To put
this effort into perspective, we would like to emphasize that
this paper focuses on the comparison of two meshing ap-
proaches, not the accuracy of the results themselves. Hence,
the Richardson Extrapolation shows that the refinements
strategy follows commonly accepted guidelines and that it is
sufficient for our purpose to continue with the coarse mesh.
Detailed information on the grid refinement study may be
found in Kastner (2016).
Figure 9summarizes the dimensions of the box-shaped and
the cylindrical mesh for both case studies. To ensure fair con-
ditions between both approaches, we created the blockMesh
with equal cell sizes in the areas where the buildings were
placed and used identical mesh refinement levels. A visual
representation of both domains after the background mesh
was created is given in figure 9.
For each simulation case presented, we ran only one wind
direction until the convergence criteria was reached. Table 3
provides a summary of the time comparison between the box-
shaped and the cylindrical wind tunnel of the investigated
mesh refinement. Figure 11 depicts the achieved residuals
of both cases. Figure 10 shows the vertical plot of
both cases. The slightly higher
in Figure 10 vs. figure 8
was achieved by employing three mesh layers for the ground
and the building surfaces.
The implementation of the cylindrical simulation domain
Proceedings of eSim 2018, the 10ᵗʰ conference of IBPSA-Canada
Montréal, QC, Canada, May 9-10, 2018
ISBN 978-2-921145-88-6
(a) very coarse (b) coarse (c) normal (d) fine
Figure 6: Excerpt of the mesh sizes used in the mesh refinement study.
Table 2: Parameters of grid convergence study. The study was conducted for 4 different mesh sizes: very coarse, coarse, normal
and fine.
is the grid refinement ratio and
is the normalized grid spacing. Moreover, the Richardson Extrapolation (RE)
predicts the flow rate for an ideal mesh (continuum), estimating the magnitude of the numerical error.
shows the flow rate
through the windward opening obtained. exp.
experiment by (Jiang et al.,2003). cont.
continuum. The grid convergence
index refers to the grid number indicated and the subsequent finer grid respectively. The coarse mesh shows reasonable
accuracy and is therefore chosen for further studies.
# type case cell # h r ˙v[m3s−1 ] error (exp.) error (cont.) GCI [%]
1 sim. very coarse 124 456 8 1.3 0.0540 17 % 15 % 11.04
2 sim. coarse 263 919 4 1.6 0.0505 11 % 10 % 6.82
3 sim. normal 1 165 733 2 1.6 0.0485 7 % 6 % 4.94
4 sim. fine 4 940 280 1 - 0.0471 4 % 3 %
- calc. RE - 0 - 0.0456
- meas. experiment - - - 0.0450
Figure 7: Richardson extrapolation of the volumetric flow
rate based on a grid refinement study. The symbol
to the grid sizes in table 2. The symbol
depicts the less
accurate values than the previous refinement stages and
therefore was not used to determine the continuum. The
is the extrapolated value for the volumetric flow
rate with the discretization error eliminated. The symbol
shows the value obtained in the experiment by (Jiang et al.,
Figure 8: Results of the grid refinement study. Vertical
sample of
at h
for different mesh sizes. Depicted as
is the sample from measurements in the wind tunnel.
Proceedings of eSim 2018, the 10ᵗʰ conference of IBPSA-Canada
Montréal, QC, Canada, May 9-10, 2018
ISBN 978-2-921145-88-6
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 9: The table compares the dimensions of both mesh-
ing approaches considering best practice guidelines. The
illustration shows the corresponding simulation domains
after creating the background mesh with blockMesh.
resulted in a 21 % higher cell count compared to the box-
shaped domain. As expected, the cylindrical domain was
characterized by a higher meshing time; cell count and mesh-
ing time, however, do not scale linearly (21 % vs. 5 %). Fur-
ther, the cylindrical simulation domain is characterized by
a lower simulation time than the box-shaped simulation do-
main. This can most likely be attributed to the differences in
convergence behavior which was worse for the box-shaped
domain, see figure 11. By evaluating the first 200 iterations,
the simulation time per iteration is 16 s for the box-shaped
case and 21 s for the cylindrical case.
It is evident that the box-shaped simulation domain achieves
slightly better accuracy (R2= 96.7%) than the cylindrical
simulation domain (
R2= 94.1
%). Both domains under- or
overestimate regions with high pressure gradients which is
known as a deficiency of the steady-state RANS model.
As a result, for this particular simulation setup, the cylin-
drical domain would be of advantage over the box-shaped
domain from a simulation time perspective.
Table 3: Summary of meshing and simulation times on a
single CPU until convergence criteria was reached. M =
meshing, S = simulation. The units for time are given in
Box-shaped Cylindrical
coarse 00:10:51 15:10:47 00:11:25 14:24:19
Figure 10: Comparison of the box-shaped and the cylindri-
cal simulation domain based on the coarse case. Vertical
sample of
at h
for different mesh sizes. Depicted as
is the sample from measurements in the wind tunnel.
0 1000 2000 3000 4000 5000
0 1000 2000 3000 4000 5000
Figure 11: Residuals of box-shaped domain (top) and cylin-
drical domain (bottom).
Proceedings of eSim 2018, the 10ᵗʰ conference of IBPSA-Canada
Montréal, QC, Canada, May 9-10, 2018
ISBN 978-2-921145-88-6
The results presented show that it is possible to employ a
cylindrical simulation domain for urban CFD simulations.
The residuals of the cylindrical case show that the proposed
approach shows solid convergence behavior which is similar
to conventional box-shaped simulation domains.
Where high-pressure gradients are expected, the mesh has to
be appropriately refined to capture important flow features
and to adequately resolve the boundary layer. Consequently,
for box-shaped domains, one needs higher mesh resolution
around all building geometries as well as at the ground
boundary. A cylindrical domain needs to be created in a way
that flows from all directions can be sufficiently resolved.
Since the building geometries are identical for both cases, a
significant amount of additional cells (21 %) is introduced
at the ground boundary for the cylindrical domain. This
disadvantage is illustrated in figure 9.
The results show that the cylindrical domain shows better
simulation times which is very likely due to the differences
in convergence behavior illustrated in figure 11 — and which
we believe happened coincidentally for this particular case.
Given the higher mesh count of the cylindrical case, the time
per iteration for a cylindrical domain is higher than for a
box-shaped domain. Thus, by extrapolating those iteration
times, one can infer that the only possibility to achieve
faster simulation times than with a cylindrical domain would
be to achieve better convergence behavior, meaning that
fewer iterations will yield the same results. If this is not
the case, a cylindrical simulation domain will always be
at a disadvantage over the box-shaped domain in terms of
simulation time.
Aside from that, the nature of the annual wind analysis
problem warrants another, more holistic comparison: for
this purpose we assume identical convergence behavior and
that every wind direction simulation starts with a ”positive
budget” which equals the meshing time of a corresponding
box-shaped case. This budget, in this case, would be 10 min
and 51 s or 651 s. This budget of 651 s is exhausted after 131
iterations of simulation time for the cylindrical domain. In
other words, the simulation time of the cylindrical domain
may be 651 s longer to still win over the box-shaped case.
By extrapolating both iteration times for
3000 iterations,
we yield a total simulation time of 13.3 and 17.5 h for the
box-shaped and the cylindrical domain respectively. The
fact that the
of both total times is far greater than
651 s
we believe that hardly any considerable time advantages
could be achieved with different mesh densities.
However, the advantages of a cylindrical domain outweigh
the disadvantages in some cases. First, in practice with real
geometries, the scale of most urban CFD simulations sug-
gests to run those overnight or over the weekend. Given
those time-spans, improvements in simulations time are
desirable but only magnitudes in simulation time improve-
ments would change the way of working with such large-
scale simulation cases. On the contrary, incorrect simulation
setups or non-reliable simulation cases might result in a
weekend of lost simulation time.
Aside from differences in meshing time, we would like
to emphasize that CFD simulations are highly sensitive to
the input mesh and its quality. The creation of such high-
quality meshes often requires time-consuming and tedious
preprocessing efforts, mostly for cleaning the geometries.
Considering these efforts, one can make use of the inherent
advantages of a cylindrical simulation domain. In using a
cylindrical domain with a high-quality mesh, one can use it
for all subsequent simulations of different wind directions.
The simulation of each wind direction may be started in par-
allel after one single mesh is created. This possibility might
help to identify problems in the buildings’ design before
one might happen to reach the particular wind direction that
reveals problems with a sequential simulation approach. Fur-
thermore, CFD analysis for the built environment is usually
characterized by iterative design alterations which have been
outlined above. Every design alteration is likely to introduce
new mesh inconsistencies that, for the box-shaped domain,
might elicit meshing issues for every new wind direction
that is required to be studied. In contrast, these hindrances
do not exist for the cylindrical domain. Consequently, one
requirement we see for the further automation of CFD work-
flows in the field of building performance simulation is the
reliability to achieve robust, converging simulation cases.
Apart from mixed polyhedral meshes that were used in this
study, other commonly used meshes include hexahedral-
only, tetrahedral-only meshes. We are aware of the advan-
tages that those might have in terms of accuracy or simula-
tion time. Unfortunately, none of the latter ones have been
implemented in OpenFOAM in a robust manner at the time
of writing this manuscript. As soon as those meshes become
available, the presented cylindrical meshing approach could
take advantage of them.
In this study, we proposed a cylindrical mesh for urban wind
simulations. We showed that cylindrical simulation domains
for urban CFD simulations are feasible with OpenFOAM.
We examined a commonly used validation case for which
we compared the box-shaped computational domain with
the cylindrical simulation domain, both by considering the
best practice dimensions for environmental flows. Meshing
and simulation time comparisons showed that it is recom-
mendable to use the box-shaped approach if no annual wind
analysis is intended. A cylindrical simulation domain is
likely to have advantages over the box-shaped approach
from a methodological standpoint and if further simulations
with the same mesh may be necessary for different wind
directions at a later point in time. In future work, we plan
to validate the results of the urban wind case in a further
study and envision to link the results from the annual wind
Proceedings of eSim 2018, the 10ᵗʰ conference of IBPSA-Canada
Montréal, QC, Canada, May 9-10, 2018
ISBN 978-2-921145-88-6
study with Building Energy Simulation software for more
accurate natural ventilation potential estimations.
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
ABL atmospheric boundary layer
AFN air flow networks
BC boundary condition
BEM building energy modeling
CAD Computer-aided design
CFD Computational Fluid Dynamics
GCI grid convergence index
NV natural ventilation
RANS Reynolds-averaged Navier-Stokes
Semi-Implicit Method for Pressure Linked
SST Shear Stress Transport
WT wind tunnel
cppressure coefficients
hnormalized grid spacing
Cmu constant
turbulence dissipation rate, m2s−3
κvon Karman constant
ppressure, kg m−1 s2
rgrid refinement ratio
R2coefficient of determination
Uvelocity, m s−1
uref reference velocity, ms−1
Ufriction velocity, m s−1
˙vvolumetric flow rate, m3s−1
ωspecific dissipation rate, s−1
yivalues of choice
ˆyipredicted values of choice
¯yimean values of choice
zheight, m
z0surface roughness length, m
zmin min. coordinate value in z-direction, m
zref reference velocity, ms−1
Blocken, B. (2015). Computational fluid dynamics for urban
physics : Importance , scales , possibilities , limitations
and ten tips and tricks towards accurate and reliable simu-
lations. Building and Environment 91, 219–245.
Boulard, T., J. Meneses, M. Mermier, and G. Papadakis
(1996). The mechanisms involved in the natural ventila-
tion of greenhouses. Agricultural and Forest Meteorol-
ogy 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 Environ-
ment 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 Ham-
Franke, J., A. Hellsten, H. Schl
unzen, and B. Carissimo
(2010). The Best Practise Guideline for the CFD simu-
lation 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 build-
ings: a parametrical model. Energy and Buildings 18(2),
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, Tech-
nische Universit¨
at M¨
Proceedings of eSim 2018, the 10ᵗʰ conference of IBPSA-Canada
Montréal, QC, Canada, May 9-10, 2018
ISBN 978-2-921145-88-6
Oropeza-Perez, I. and P. A. Østergaard (2014). Energy sav-
ing 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: Im-
pact of computational parameters. Building and Environ-
ment 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 pres-
sure distribution on buildings and calculation of natural-
ventilation airflow. ASHRAE transactions 94(3112), 243–
Tecle, A., G. T. Bitsuamlak, and T. E. Jiru (2013). Wind-
driven natural ventilation in a low-rise building: A Bound-
ary Layer Wind Tunnel study. Building and Environ-
ment 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 envi-
ronment 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.
Proceedings of eSim 2018, the 10ᵗʰ conference of IBPSA-Canada
Montréal, QC, Canada, May 9-10, 2018
ISBN 978-2-921145-88-6
... The mesh was created by OpenFOAM's blockMesh utility for the background mesh and snappyHexMesh to subsequently snap the background mesh to the building geometry. For the background mesh, we used a cylindrical simulation domain approach discussed in (Kastner and Dogan, 2018). This meshing approach allows for reusing the same computational mesh for every subsequent wind direction. ...
... The Grasshopper plugin called Eddy3D was used to automate the pre-processing, including the assignment of boundary conditions. Depending on the wind direction, we mapped the inlets to a one-half circle of the simulation domain and the outlet on the opposite side as described in (Kastner and Dogan, 2018). The half circular domain inlet was set to a uniform profile for U, k, and ω, and a roughness length z 0 = 1 that corresponds to "regular coverage with large size obstacles with open spaces roughly equal to obstacle heights, suburban houses" (Wallace and Hobbs, 2006), according to equations 3-5. ...
... While this seems plausible for a tropical climate, it is worth reiterating that microclimate maps will likely suffer greatly from a reduced number of simulated wind directions in colder climates (Bröde et al., 2013). Although additional wind directions increase the simulation time for the engine that is already the bottleneck in simulation procedure, the RANS method is state-of-the-art in terms of an accuracy/efficiency/robustness-trade-off for outdoor comfort mappings, especially when additional measures are taken into account (Kastner and Dogan, 2018). However, one area for further research might be to replace the RANS method with an engine that is based on Lattice Boltzmann methods which can be solved less expensively. ...
Conference Paper
Full-text available
Global warming and increasingly dense cities lead to poor outdoor thermal comfort that may not only be detrimental to our health and well-being but also decreases social and commercial activities. Although workflows for the analysis of thermal comfort exist, they have yet transitioned into the quotidian architectural design process. Our work-flow allows for annual outdoor comfort analyses that are seamlessly integrated into a commonly-used CAD environment. We simulated the annual outdoor thermal comfort on a university campus and discuss which simplifications seem appropriate by means of preliminary on-site measurements. The results exemplify the possibility to conduct such analyses within reasonable time and accuracy if some simplifications to the UTCI estimation are acceptable.
... 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). ...
For urban CFD simulations, it is considered a best practice to use a box-shaped simulation domain. 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 behaviour. 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.
... Cylindrical simulation domain: To circumvent re-meshing of the simulation domain for every wind direction and to reduce manual and computational overhead, a cylindrical mesh is used to facilitate the simulation of arbitrary wind directions, see Figure 1 (B). The modeling approach has been validated against three cases with measured data showing insignificant differences compared to the best practice box-domain approach (Kastner & Dogan, 2018). Furthermore, the proposed method automates the setup of boundary conditions so that a significant amount of time will be saved to change the boundary conditions in case of an annual wind analysis. ...
Conference Paper
Full-text available
Energy modeling packages such as EnergyPlus and TRNSYS come with capable airflow network solvers for natural ventilation evaluation in multi-zone building energy models. These approaches rely on pressure coefficient arrays of different wind directions based on simple box-shaped buildings without contextual obstructions. For specific sites, however, further attention is needed to avoid geometric oversimplification. In this study, we present an automated and easy-to-use simulation workflow for exterior airflow simulation based on OpenFOAM to generate pressure coefficient arrays for arbitrary building shapes and contextual situations. The workflow is compared to other methods commonly used to obtain pressure coefficients for natural ventilation simulation.
In Design of high-rise structures, Wind is considered as one of the important horizontal forces that have significant impact on the response of building. Due to rise in population, the demand for tall buildings is increasing day by day. Wind Load on such structures are calculated using pressure coefficients and force coefficients which are available in various international codes and standards. However, these international codes and standards give information about regular shape buildings such as square, rectangle, circular or octagonal.With the technological advancement, composite plan shape buildings such as square and circular, circular and hexagonal and square and octagonal etc. have been considered by many architects keeping in view of aesthetics of Building. The wind flow around a tall building with composite plan shapes having different height ratio variation differs from what we get in regular shape analysis. Since, data is not available regarding such buildings, the need to carry wind tunnel testing or CFD become important for analyzing wind effect on such buildings. CFD (Computation Fluid Dynamics) for determining wind responses is becoming immensely popular.
The architectural community needs holistic, evidence-based planning tools to promote urban resilience in the face of global warming. To ensure maximum impact, simulation-driven microclimate analysis methods must be integrated early in the design process. With Eddy3D, we present a toolkit to simulate outdoor thermal comfort (OTC) metrics with a decoupled approach. We motivate the decoupled systems framework with meteorological measurements and local and global sensitivity analyses of three different climates. For a real-world case study on a university campus, we present results for both wind velocity and mean radiant temperature simulations. Finally, we discuss the advantages and disadvantages of a decoupled simulation approach considering design aiding and the architectural. Our findings support reduced simulation time and flexibility, with the caveat of reduced accuracy due to neglecting forced convection, albeit this being less relevant in the early stages of design. The framework presented in this manuscript has been implemented and released as Eddy3D, a plugin for Rhino & Grasshopper.
Conference Paper
Full-text available
The present work deals with the determination of thermal comfort maps in large enclosures. Currently no specific approach is proposed to this end as building simulation relies on a nodal approach, where the computed scalar values (e.g. temperature, humidity, solar flux) are homogeneously distributed in zones whatever their size. We present here a method allowing for the calculation of a spatial distribution of thermal comfort, enhancing the classical approach by a precise determination of indoor solar fluxes and isothermal air velocities.
With increased awareness of sustainability, natural ventilation has become a strategy to reduce energy consumption in the built environment while providing comfortable indoor air quality. The main aim of this thesis was to apply the CFD software OpenFOAM, to investigate the wind-induced natural ventilation potential of classrooms. Relevant ventilation metrics such as air change rates, age of air, andCO2 concentrations were implemented. External and internal wind flow was simulated in one domain to assess the natural ventilation potential via RANS turbulence modeling. A case setup for a simple cross-ventilation geometry was validated against wind tunnel measurements in accordance with CFD guidelines for the built environment. Based on the validation, a case study was conducted for BRAC University—located in subtropical Asia. The validation study revealed that OpenFOAM was able to accurately predict the flow field and flow rates for the cross-ventilation geometry. Further, OpenFOAM’s passive scalar transport method is able to predict CO2 concentrations with a reasonable error range, while the workflow can be highly automated. Applying these results to the case study, we suggest a number of geometry modifications to optimize the natural ventilation potential of classrooms for BRAC University. These include specific placement based on the wind direction and either relocation or shape optimization of adjacent staircases. Additionally, we suggest the use of operable windows to accommodate temporal fluctuations throughout the year. Finally, passive scalar transport methods, which derive metrics like the age of air or CO2 concentrations, provide additional valuable information that should not be overlooked when evaluating design principles. In the future, it may be possible to employ tools based on the implemented ventilation metrics to automate the search for optimized building geometries for maximizing the natural ventilation potential.
Urban physics is the science and engineering of physical processes in urban areas. It basically refers to the transfer of heat and mass in the outdoor and indoor urban environment, and its interaction with humans, fauna, flora and materials. Urban physics is a rapidly increasing focus area as it is key to understanding and addressing the grand societal challenges climate change, energy, health, security, transport and aging. The main assessment tools in urban physics are field measurements, full-scale and reduced-scale laboratory measurements and numerical simulation methods including Computational Fluid Dynamics (CFD). In the past 50 years, CFD has undergone a successful transition from an emerging field into an increasingly established field in urban physics research, practice and design. This review and position paper consists of two parts. In the first part, the importance of urban physics related to the grand societal challenges is described, after which the spatial and temporal scales in urban physics and the associated model categories are outlined. In the second part, based on a brief theoretical background, some views on CFD are provided. Possibilities and limitations are discussed, and in particular, ten tip and tricks towards accurate and reliable CFD simulations are presented. These tips and tricks are certainly not intended to be complete, rather they are intended to complement existing CFD best practice guidelines on ten particular aspects. Finally, an outlook to the future of CFD for urban physics is given.
The objective of this article is to show the potential of natural ventilation as a passive cooling method within the residential sector of countries which are located in warm conditions using Mexico as a case study. The method is proposed as performing, with a simplified ventilation model, thermal–airflow simulations of 27 common cases of dwellings (considered as one thermal zone) based on the combination of specific features of the building design, occupancy and climate conditions. The energy saving potential is assessed then by the use of a new assessment method suitable for large-scale scenarios using the actual number of air-conditioned dwellings distributed among the 27 cases. Thereby, the energy saving is presented as the difference in the cooling demand of the dwelling during one year without and with natural ventilation, respectively. Results indicate that for hot-dry conditions, buildings with high heat capacity combined with natural ventilation achieve the lowest indoor temperature, whereas under hot-humid conditions, night ventilation combined with low heat capacity buildings present the best results. Thereafter, an average aggregated saving potential of 4.2 TW h for 2008 is estimated, corresponding to 54.4% of the Mexican electric cooling demand for the same year. The practical implications of the study are that the results contribute to an assessment of the economic and environmental benefits for using natural ventilation rather than an active method such as air conditioning. Thereby, the average economic saving is estimated at US$ 900 M and the environmental benefit at an annual average mitigation of 2 Mt CO2eq, both for 2008.
This paper proposes the use of a Grid Convergence Index (GCI) for the uniform reporting of grid refinement studies in Computational Fluid Dynamics. The method provides an objective asymptotic approach to quantification of uncertainty of grid convergence. The basic idea is to approximately relate the results from any grid refinement test to the expected results from a grid doubling using a second-order method. The GCI is based upon a grid refinement error estimator derived from the theory of generalized Richardson Extrapolation. It is recommended for use whether or not Richardson Extrapolation is actually used to improve the accuracy, and in some cases even if the conditions for the theory do not strictly hold. A different form of the GCI applies to reporting coarse grid solutions when the GCI is evaluated from a ''nearby'' problem. The simple formulas may be applied a posterior by editors and reviewers, even if authors are reluctant to do so.
This report describes the theoretical development of work done within task group “wind pressure distribution” of the COMIS Workshop. The paper is divided into three Sections with an introductory part on the physical fundamentals. The first Section entails the objectives and the meaning of modelling wind pressure distribution as an integrated part of multizone airflow modelling. A literature review is presented, on calculation techniques and wind tunnel tests, and a description of the evaluation of an existing numerical model. The second Section is related to the development of the Cp calculation model. Objectives, characteristics and methodology of the parametrical approach chosen for the analysis are depicted, together with a description of the reference data, the regression technique, the algorithm, and the structure of the calculation model. The third Section is a detailed report of the results of the regression analysis. The curve-fitting process is explained with reference to the main factors affecting the wind pressure distribution on a building envelope: terrain roughness, surrounding buildings, aspect ratios, and wind direction. Figures of the curves are shown. In the Appendix, equations and relevant coefficients of the curve-fitting are presented.
Although natural ventilation is one of the major mechanisms that controls the greenhouse climate, our understanding of the underlying processes remains insufficient to allow accurate prediction of the rates of such exchanges.This paper deals with the physical mechanisms involved in natural ventilation of a greenhouse equipped with continuous lateral windows, and uses the following experimental procedures: •• air exchange rate measurements, using tracer gas or heat and water balance techniques;•• direct determination of the air and heat flows through an opening, using an eddy correlation system, comprising a sonic anemometer and a fine wire thermocouple;•• measurements of mean and turbulent pressure differences at ground level between inside and outside.The methods employed allow the prediction of greenhouse air exchange rates as well as the characterization of its components: a steady effect resulting from the combination of both mean wind-related and stack effects and a turbulent effect linked to wind speed fluctuations.Local estimations of total, mean and turbulent flows are provided: a wind parallel to the greenhouse axis produces an inflow at the leeward half and an outflow at the windward half. The mean flow of sensible heat is estimated between 55% and 80% of the total flux so that the turbulent flow does not exceed 45% of the total.Local estimations of total, mean and turbulent flows are compared with air exchange rate measurements using the decay rate method and a good agreement between both approaches is demonstrated.
Accurate CFD simulation of coupled outdoor wind flow and indoor air flow is essential for the design and evaluation of natural cross-ventilation strategies for buildings. It is widely recognized that CFD simulations can be very sensitive to the large number of computational parameters that have to be set by the user. Therefore, detailed and generic sensitivity analyses of the impact of these parameters on the simulation results are important to provide guidance for the execution and evaluation of future CFD studies. A detailed review of the literature indicates that there is a lack of extensive generic sensitivity studies for CFD simulation of natural cross-ventilation. In order to provide such a study, this paper presents a series of coupled 3D steady RANS simulations for a generic isolated building. The CFD simulations are validated based on detailed wind tunnel experiments with Particle Image Velocimetry. The impact of a wide range of computational parameters is investigated, including the size of the computational domain, the resolution of the computational grid, the inlet turbulent kinetic energy profile of the atmospheric boundary layer, the turbulence model, the order of the discretization schemes and the iterative convergence criteria. Specific attention is given to the problem of oscillatory convergence that was observed during some of these coupled CFD simulations. Based on this analysis, the paper identifies the most important parameters. The intention is to contribute to improved accuracy, reliability and evaluation of coupled CFD simulations for cross-ventilation assessment.