Best Practice Guidelines on the Ansys in Building Wind Action Applications
GUILHERME S. TEIXEIRA, MARCO D. DE CAMPOS
Institute of Exact and Earth Sciences,
Federal University of Mato Grosso,
Av. Valdon Varjão, 6390, Barra do Garças, 78605-091, Mato Grosso,
BRAZIL
Abstract: - In the last 30 years, Computational Fluid Dynamics use in Wind Engineering has allowed
researchers to raise its capabilities, and, little by little, it is becoming a reasonable tool because of the
availability of high‐performance computers with large storage capacities. This work offers a short guide to the
twelve tips computer beginners can take on the Ansys in building wind action applications.
Key-Words: - Best practice, guideline, Wind Engineering, ANSYS, computer beginners, CFD, numerical
simulation.
Received: November 15, 2022. Revised: August 25, 2023. Accepted: October 4, 2023. Published: November 1, 2023.
1 Never Use Special Characters or
Spaces in File Naming
In recent decades, new ways of analyzing and
designing structures for wind loads have emerged
due to progress in information technology, data
storage methods, and computational tools.
Among these last, Ansys Workbench (often
ANSYS WB) established itself among researchers
because of its integrity and cost-effectiveness. Next,
twelve best practice guidelines on the Ansys in
building wind action applications will be presented
and discussed.
Possibly, this is the most common mistake made
by beginners in simulations or programming in
general. A computer scientist could use an entire
article to explain why special characters become a
problem in file naming, [1]. In the scope of a
beginner user in Ansys WB, it is enough to say that
some operating systems can assign specific
functions to certain characters as commas, quotes,
ampersands, and parentheses, among others.
Consequently, its use in the simulation file directory
can generate incompatibilities, compromising file
accessibility or even causing it to be deleted or
inaccessible. Choosing inappropriate file names or
addresses can result in two implications. The first is
about the failure of the simulation in Ansys WB due
to its not finding the file directory. The second is the
inoperability between the operating systems since it
is possible to use Ansys collaboratively, sharing the
files of the simulation steps (Figure 1) with other
computers. In the context of a group of researchers,
it is natural to use equipment with different
operating systems, and it may happen that a
particular character accepted in one does not work
in another (as is the case with Windows and Linux,
for example). This way, by simply renaming the
address using only non-special characters, this error
could be eliminated, as well as underlines and
hyphens instead of spaces. It is recommended from
the beginning.
2 Appropriately Model your Control
Volume
In an Eulerian approach, a control volume (CV) is
the region of space through which the fluid flows in
and out, [2]. However, this basic definition in
Computational Fluid Dynamics (CFD) may be
ambiguous for beginners when used in a project to
create a fluid domain in Ansys WB. This fact occurs
because, according to the definition, in the
simulation domain definition, it would be enough to
model only the region through which the fluid
flows. Thus, it would be necessary to model only
the surfaces obstructing the flow, that is, as a unique
solid body (Figure 2). Thus, the control volume
must be created by extracting the geometry of
interest from its interior, causing only one
obstruction in the flow. In other words, there is no
need to insert the extracted geometry again, which
would result in two elements in the simulation.
WSEAS TRANSACTIONS on FLUID MECHANICS
DOI: 10.37394/232013.2023.18.12
Guilherme S. Teixeira, Marco D. De Campos
E-ISSN: 2224-347X
114
Volume 18, 2023
Fig. 1: Computational simulation steps.
Fig. 2: Screenshot of SpaceClaim (Ansys WB CAD platform) showing (a) an inadequate CV, with two solid
bodies in the model, one blue (CV) and one red (building), (b) an adequate CV (note that there is only one body
with an obstruction of the same volume and shape as the building of interest), (c) obstruction filled in the
inappropriate CV (CV 1, top view) and, finally, (d) existing hollow obstruction in the appropriate CV (CV 2,
bottom view).
3 Make Use of Software Features
A good directive to produce an adequate simulation
is to know how to use the software tools. In the
preparation of the geometry, the “Named selections”
in Ansys WB allows the user to name the faces or a
set of them (i.e., INLET, OUTLET, WALL,
WINDWARD ROOF, LEEWARD ROOF, that is,
whatever the user wants) (Fig. 3-a).
Naming the faces according to the lists of each
component of the analysis system (for example,
geometry mesh, or setup) becomes useful for
creating boundary conditions and plotting the
results. On the other hand, unnamed faces showed in
the form of “codes” (like F106.136, F107.136,
F108.36) (Fig. 3-b).
Thus, initially, it is recommended to name the
most important faces of the model in the component
“geometry”. Thus, the time in building the
simulation will be optimized, in addition, to
minimizing errors in the boundary conditions.
WSEAS TRANSACTIONS on FLUID MECHANICS
DOI: 10.37394/232013.2023.18.12
Guilherme S. Teixeira, Marco D. De Campos
E-ISSN: 2224-347X
115
Volume 18, 2023
(a)
(b)
Fig. 3: Screenshot showing (a) the “Named Selection” tool that is accessed by clicking with the mouse
button on the face to be named and (b) a typical list of components of an Ansys WB analysis
component (named and unnamed faces).
4 Prepare your Geometry According
to Available Post-Processing
Improving the quality of the simulation output data
is directly related to the computational model
development according to the expected results. This
fact means not only expecting a physically coherent
result due to the physical behavior of the fluid and
its possible effects on the structure but also how
these results will be presented and treated
Beforehand, it is necessary to determine which part
of the structure (entirely or in part) the variables will
be calculated (Cpe, streamlines, or velocity vectors,
for example). This consideration extends to
streamlines, velocity vectors, or any other parameter
typical of Wind Engineering. This treatment is
called post-processing.
Suppose a hypothetical case in which the user
selects the four facades of a shed and names them
"FACADES" (using the "Named selections" tool).
In this way, it will be not possible to plot the
contours of Cpe only on the front and rear façade,
for example. In plotting the results, the FACADE
must be considered integrally (the four facades
together). However, identifying the four facades
separately can be plotted the results individually or
together.
In addition, other combinations will be possible:
the user could present the contour maps on the four
facades, only on the front facades and, later,
together or only on the leeward roof, in case the
windward is not the object of study, for example.
When plotting the results for some specific parts of
the geometry, it is necessary to prepare the model in
advance. Thus, when Cpe is graphically represented
only on the roofs, excluding the facades, it is
required to name them separately. This
methodology results in greater versatility in the
acquisition and analysis of results of spaces.
WSEAS TRANSACTIONS on FLUID MECHANICS
DOI: 10.37394/232013.2023.18.12
Guilherme S. Teixeira, Marco D. De Campos
E-ISSN: 2224-347X
116
Volume 18, 2023
5 Build Meshes According to your
Processing Power
Although the RAM capacity of the hardware is a
less critical factor than the machine's processor, it is
still a point that deserves attention. Defining the
maximum number of mesh elements to be processed
as a function of the RAM size is a hard decision.
The reason is that this relationship is not direct and
depends, among other factors, on the mesh, the
solution algorithm, numerical precision, and
connectivity between elements. In the case of
hardware from large research groups (in academia
or industry) or even professionals in the area who
work with many different simulation cases, the ideal
is to benchmark the machines to establish some
parameters of the RAM-Mesh ratio.
However, in the case of wind engineering
beginners using Ansys, some recommendations may
be convenient to understand the particularities of
this type of simulation. Although some authors, [3],
recommend a ratio of 1GB for every 1 million mesh
elements, the indication of 2GB for every 1 million
cells is a golden rule in many forums and theme
pages. For this reason, simulation software
developers do not indicate the use of machines with
less than 4GB RAM since this is the minimum value
by Ansys WB.
In this context, the most important thing for the
beginner would be to understand the coherence
between the mesh built for the computational model
and the machine available to solve such a problem.
Initially, you should test values in the range of 1 to
2GB for every million cells and, later, with
experience, be able to establish and analyze the
capacity of the hardware itself.
6 Build Meshes According to your
License Limitations
When using limited licenses, attention is necessary
for the model mesh construction. For the student
version, for example, the mesh limitation is 512000
nodes for fluid simulation (for the latest version at
the time of writing this article).
Ansys Workbench allows the generation of
refined meshes as supported by the hardware.
However, the limitation will appear in the solver
(CFX or Fluent).
When exceeding the software limit, when
solving the computational model, a typical message
will appear (Fig. 4-a), and by not explaining the
problem, it may confuse the novice user. In this
case, to understand the error, it is necessary to check
the simulation out file (Fig. 4-b). For this reason,
before proceeding to the equation solution step, it is
recommended to verify the number of elements and
nodes created in the mesh step, paying particular
attention to the license limitation, if any.
Fig. 4: (a) Screenshot of typical message for several
troubleshooting errors in Ansys Workbench,
including extrapolation of several cells/nodes
limited by license and (b) warning, in the out file,
specifying the error.
7 Equation Discretization Schemes
CFD consists of solving equations through computer
codes, [2], including Computational Wind
Engineering (CWE), [4]. However, the physical
nature of fluids governed by such equations is not
trivial, leading to complex mathematics. Therefore,
an appropriate methodology, including
discretization, is necessary to make the governing
equations of Fluid Mechanics solvable by computer
codes. Thus, these differential equations must be
rewritten as simpler algebraic equations. These
equations have different terms (e.g., temporal term,
advective term, diffusive term, and source term),
and, in Ansys WB, it is possible to choose the
numerical approximation for the advective terms
and the additional turbulence equations. For that,
there are two options: Upwind and High Resolution
(Fig. 5). The first is called first-order discretization
and produces less accurate results than the second;
however, its computational cost is also lower.
Upwind discretizations provide the preliminary
simulation results. However, the literature
recommends that for the final results of your model,
second-order discretizations, called High Resolution
by Ansys WB, be used, [5].
In addition to the computational cost and
accuracy of the results, it is worth mentioning that
the acceptance of the research is also subject to this
boundary condition. Some journals do not accept
simulations whose results do not use high-order
discretization schemes, [6]. Therefore, if possible,
use second-order discretization schemes for your
final results.
WSEAS TRANSACTIONS on FLUID MECHANICS
DOI: 10.37394/232013.2023.18.12
Guilherme S. Teixeira, Marco D. De Campos
E-ISSN: 2224-347X
117
Volume 18, 2023
Fig. 5: Screenshot of the equation discretization
scheme menu using the Ansys Workbench setup
component.
8 Unexpected Interruption of the
Simulation
A common problem in commercial simulation
software occurs when the solution processing stops
unexpectedly. In Ansys WB, with the “solution”
component started, care must be taken that the
software is not closed during this process. If this
happens, due to carelessness on the part of the user,
or even a power outage, or the end of the battery,
the simulation will then be interrupted and, when
returning to the Ansys WB initial screen, a warning
will inform about the end of the processing (Fig. 6).
The user will have to choose between
recovering the files and data created up to the
moment of interruption or abandoning them,
returning with the data from the last savepoint
before the stage of the simulation starts.
In this case, the recommendation is to discard
the data generated up to the moment of interruption,
considering only those already saved. In broken data
recovery, the file may have become corrupted.
In this context, it is also relevant to encourage
beginners in simulation to keep their files updated
periodically during the construction of the
computational model. Also, avoid, when starting a
file, saving it only after post-processing or even
after carrying out a large volume of processing.
Fig. 6: Screenshot of the message when restarting
the file after stopping a numerical solution.
9 Vertical Profiles
Ansys WB, like other software, is based on a
Cartesian coordinate system (x,y,z). When using a
vertical wind profile, such as the Power Law
(function of a z height), the control volume
placement must be correct to avoid physical
inconsistencies in the results. For example, when
building the control volume with the terrain
positioned at a height z<0, consequently, the user
will obtain negative velocities in the input profile. In
this case, a negative velocity vector on the input
face (INLET, i.e., the facade through which the fluid
enters and does not leave) will result in a vector in
the opposite direction to the input plane, which is
considered an inconsistency in the model (Fig 7-b).
This way, there will be an error, and the simulation
will not be complete. Thus, for vertical wind
profiles modeled from Power Law or Logarithmic
Law, when building its geometry, it is necessary to
ensure that the lowest terrain plane (i.e., the face
that represents the terrain in the computational
model) is positioned at z height = 0 (Fig 7-a). This
recommendation applies to the most common cases
of simulation of wind action in buildings, such as
control volumes that include open and flat land, flat
urban areas, among others. It is worth mentioning
that the use of the absolute function abs( ) to prevent
this possible error ends up generating another one
related to the inadequate form of the Power or
Logarithmic Law profile (Fig 7-c).
10 A Warning is not an Error (But it
May be an Indication to Review your
Choices)
When executing some commands, Ansys may issue
alert notices. For example, when inappropriately
choosing a structured mesh model made up of
parallelepipeds for a geometry that would perform
better with an unstructured mesh. In this case, the
user will receive the message that some elements
initially foreseen were not created (Fig. 8).
Sometimes, this amount can be an indication to
review the choice of mesh method or use another
refinement in the geometry. In addition, when
defining an OUTLET-type boundary condition on a
face and verifying a reverse flow during the
resolution of the equation, the software will issue a
warning indicating the change to OPENING, which
allows reverse flow.
Fluid re-entry through the OUTLET face is
defined as overflow by Ansys WB. So, pay attention
to the messages provided by the software and
rethink whether the chosen model choices are
adequate.
WSEAS TRANSACTIONS on FLUID MECHANICS
DOI: 10.37394/232013.2023.18.12
Guilherme S. Teixeira, Marco D. De Campos
E-ISSN: 2224-347X
118
Volume 18, 2023
11 Choose an Appropriate Turbulence
Model
In Computational Wind Engineering (CWE), the
choice of the turbulence model is one of the most
relevant points for a successful simulation. This
boundary condition can vary with the type of
problem, whether pedestrian-level wind
environment, near-field pollutant dispersion, natural
and urban ventilation, structural wind engineering,
or others. Each of these problems requires specific
computational modeling for turbulence.
In addition, commercial software such as Ansys
WB has some options available (Fig. 9). In this
context, some researchers have investigated which
models perform better for different simulation cases,
[7], [8], [9].
For the simulation of wind action on buildings,
some models are widely used as low and high-rise
buildings, industrial buildings, and residential
buildings, among others. Generally, two main
groups, with their variations, are employed: k-ε and
k-ω models, [10]. For the k-ε models, the main
variations applied are the Standard k-ε (Skε), [11],
Realizable k-ε (Rkε), [12], Renormalization Group
k-ε (RNG k-ε), [13]. The k-ε RNG has better
indications in the literature than the Skε and is
usually more used in bluff bodies, [14]. In the k-ω
group, the Shear Stress Transport k-ω, [15], is the
most used. When preparing a simulation, one should
look for references of turbulence model applications
applied to cases similar to the one of interest. This
practice is known as benchmarking.
(c)
Fig. 7: (a) Appropriate and (b) inadequate positioning of the control volume in the Cartesian axes system, and
(c) the physically inconsistent profile generated by using the abs( ) function.
WSEAS TRANSACTIONS on FLUID MECHANICS
DOI: 10.37394/232013.2023.18.12
Guilherme S. Teixeira, Marco D. De Campos
E-ISSN: 2224-347X
119
Volume 18, 2023
Fig. 8: Warning about problems with mesh
generation.
Fig. 9: Turbulence models are available on Ansys
WB.
12 Best Practices Guidelines Known
in The Literature
Other researchers have listed relevant
recommendations in Computational Fluids
Dynamics (CFD). The present text is a contribution
focusing on the commercial software Ansys WB. In
this context, these texts will allow a basis for the
best choices regarding the computational model. For
this reason, we list some authors and their most
famous guidelines, [5], [16], [17], [18], [19], [20],
[21]. In particular, when it comes to Ansys WB, it is
recommended to consult the guides by Ansys Inc.
They are technical texts in which it is possible to
select the topics of interest, [22], [23], [24], [25].
13 Conclusions
Ansys WB is one, among others, a tool that
addresses many engineering problems. This work
presented some good practices related to geometry,
meshes, boundary conditions preparations, and
common software-specific errors.
These guidelines resulted from the authors' personal
experience with Ansys WB and a software-oriented
view of good practices of literature.
In summary, we present the following checklist with
topics and questions that beginners of simulation
with Ansys WB should pay attention to, namely:
Step 1: Check the file's email address
a. Ensure that the address is free of special
characters or empty spaces;
b. Use only letters, numbers, underscores, and
hyphens.
Step 2: Check that the geometry is optimized (any
region of space through which the fluid does not
flow is unnecessary in the computational model.)
Step 3: List your preliminary decisions
a. What variable types do you want to get?
b. How will it be analyzed and presented?
(The answers to these questions will help you build
a targeted model for your CFD solution).
Step 4: Analyze your mesh choice.
a. Check if the mesh type is best suited to your
geometry.
b. Also observe whether the number of elements and
nodes in your mesh are compatible with your
computing power and software license (if any).
Step 5: Understand your boundary conditions.
a. Know the physics involved in the problem;
b. Check the properties of the fluid (density,
viscosity, temperature);
c. Also check the input variables (such as pressure)
and the mathematical expressions for the speed
profiles.
Step 6: Dealing with errors.
a. Check the error description.
b. Then consult the software Help Center.
c. If necessary, check forums on the developer
company's website and independent forums.
This script, associated with the tips detailed
throughout the text, is a manual for beginners in
wind simulation with Ansys WB.
Future work may add suggestions for good
practices aimed at Wind Engineering with Ansys
WB in addition to those explained here and apply
them to other CFD software.
WSEAS TRANSACTIONS on FLUID MECHANICS
DOI: 10.37394/232013.2023.18.12
Guilherme S. Teixeira, Marco D. De Campos
E-ISSN: 2224-347X
120
Volume 18, 2023
References:
[1] M. F. O. Rosenbloom and A. L. and
Carpenter, Macro Quoting to the Rescue:
Passing Special Characters. In: Proceedings of
SAS Global Forum, 2013.
[2] Y. A. Çengel and J .M. Cimbala, Fluid
Mechanics: Fundamentals and Applications.
New York: McGraw-Hill, 2014.
[3] ANSYS, ANSYS Mechanical APDL
Performance Guide, Canonsburg, 2013.
[4] M. Thordal, J. C. Bennetsen and H. H. H.
Koss, Review for practical application of CFD
for the determination of wind load on highrise
buildings, Journal of Wind Engineering and
Industrial Aerodynamics, Vol. 186, 2019, pp.
155-168.
[5] J. Franke, C. Hirsch, A. G. Jensen, H. W.
Krüs, M. Schatzmann, P. S. Westbury, S. D.
Miles, J. A. Wisse and N. G. Wright,
Recommendations on the use of CFD in
predicting pedestrian wind environment,
COST Action C14: Impact of Wind and
Storms on City Life and Built Environment.
Hamburg, COST Office, 2004.
[6] C. J. Freitas, Editorial policy statement on the
control of numerical accuracy, Journal of
Fluids Engineering, Vol. 115, No. 3, 1993,
pp. 339-440.
[7] B. Lia, J. Liua, F. Luoa and X. Man.
Evaluation of CFD Simulation using various
turbulence models for wind pressure on
buildings based on wind tunnel. Procedia
Engineering, Vol. 121, 2015, pp. 2209-2216.
[8] G. K. Ntinas, X. Shen, Y. Wang. Evaluation
of CFD turbulence models for simulating
external airflow around varied building roof
with wind tunnel experiment. Building
Simulation, Vol. 11, 2018, pp.115–123.
[9] M. Xiong, B. Chen, H. Zhang and Y. Qian.
Study on Accuracy of CFD Simulations of
Wind Environment around High-Rise
Buildings: A Comparative Study of k-ε
Turbulence Models Based on Polyhedral
Meshes and Wind Tunnel Experiments.
Applied Sciences, Vol. 12, No. 14, 2022, 12,
paper 7105.
[10] J. Franke, C. Hirsch, A. G. Jensen, H. W.
Krüs, M. Schatzmann, P. S. Westbury, S. D.
Miles, J. A. Wisse , N. G. Wright.
Recommendations on the use of CFD in wind
engineering. In: Proceedings of the
International Conference on Urban Wind
Engineering and Building Aerodynamics,
2004.
[11] B. E. Launder, D. B. Spalding, Mathematical
Models of Turbulence. New York: Academic
Press, 1972.
[12] T. H. Shih, W. W. Liou, A. Shabbir, Z. Yang,
J. Zhu, J., 1995. A new k-ε eddy viscosity
model for high Reynolds Number turbulent
flows-model development and validation.
Computational Fluids, Vol. 24, No. 3, 1995,
pp. 227-238.
[13] V. Yakhot, S. A. Orszag, S. Thangam, T. B.
Gatski, C. G. Speziale,. Development of
turbulence models for shear flows by a double
expansion technique. Physics of Fluids A4,
1992, pp.1510-1520.
[14] T. Potsis, Y. Tominaga, T. Stathopoulus.
Computational wind engineering: 30 years of
research progress in building structures and
environment. Journal of Wind Engineering &
Industrial Aerodynamics, Vol. 234, 2023,
paper 105346.
[15] F. R. Menter, Eddy viscosity transport
equations and their relation to the k-ε model.
Journal of Fluids Engineering, Vol. 119,
1997, pp. 876-884.
[16] J. Franke, A. Hellsten, H. Schlünzen and B.
Carissimo, Best practice guide for the CFD
simulation of flows in the urban environment,
COST Action 732: Quality assurance and
improvement of microscale meteorological
models. Hamburg: COST Office, 2007.
[17] J. Franke, A. Hellsten, H. Schlünzen and B.
Carissimo, The COST 732 Best practice
guideline for CFD simulation of flows in the
urban environment: a summary. International
Journal of Environment and Pollution, Vol.
44, 2011, pp. 419-427.
[18] T. Tamura, H. Kawai, S. Kawamoto, K.
Nozawa, T. Ohkuma. Numerical prediction of
wind loading on buildings and structures —
activities of AIJ cooperative project on CFD.
Journal of Wind Engineering and Industrial
Aerodymics, Vol. 67–68, 1997, pp. 671-685.
[19] T. Tamura, K. Nozawa, K. Kondouma. AIJ
guide for numerical prediction of wind loads
on buildings. Journal of Wind Engineering
and Industrial Aerodymics, Vol. 96, 2008,
pp.1974-1984.
[20] Y. Tominaga, A. Mochida, R. Yoshie, H.
Kataoke, T. Nozu, M. Yoshikawa and
T.Shirasawa, AIJ guidelines for practical
applications of CFD to pedestrian wind
environment around buildings, Journal of
Wind Engineering and Industrial
Aerodynamics, Vol. 96, No. 10-11, 2008, pp.
1749-1761.
WSEAS TRANSACTIONS on FLUID MECHANICS
DOI: 10.37394/232013.2023.18.12
Guilherme S. Teixeira, Marco D. De Campos
E-ISSN: 2224-347X
121
Volume 18, 2023
[21] Architectural Institute of Japan, 2016. AIJ
benchmarks for validation of CFD
simulations applied to pedestrian wind
environment around buildings. Architectural
Institute of Japan, 2016.
[22] ANSYS, CFX-Solver Modeling Guide Ansys,
Canonsburg, 2009, [Online],
https://dl.cfdexperts.net/cfd_resources/Ansys_
Documentation/CFX/Ansys_CFX-
Solver_Modeling_Guide.pdf (Accessed Date:
August 22, 2023).
[23] ANSYS, CFX-Solver Theory Guide Ansys,
Canonsburg, 2009, [Online],
https://dl.cfdexperts.net/cfd_resources/Ansys_
Documentation/CFX/Ansys_CFX-
Solver_Theory_Guide.pdf (Accessed Date:
August 22, 2023).
[24] ANSYS, Meshing User’s Guide Ansys,
Canonsburg, 2010, [Online],
https://dl.cfdexperts.net/cfd_resources/Ansys_
Documentation/Ansys_Meshing/Ansys_Mesh
ing_Users_Guide.pdf (Accessed Date: August
23, 2023).
[25] ANSYS, CFX-Solver Manager User’s Guide
Ansys, Canonsburg, 2016, [Online],
https://www.cfdlectures.com/tutorials/cfxtutor
ial.pdf (Accessed Date: August 22, 2023).
Contribution of Individual Authors to the
Creation of a Scientific Article (Ghostwriting
Policy)
Guilherme Teixeira was responsible for the
methodology. Marco Campos carried out the
conceptualization, review, and editing.
Sources of Funding for Research Presented in a
Scientific Article or Scientific Article Itself
No funding was received for conducting this study.
Conflict of Interest
The authors have no conflicts of interest to declare.
Creative Commons Attribution License 4.0
(Attribution 4.0 International, CC BY 4.0)
This article is published under the terms of the
Creative Commons Attribution License 4.0
https://creativecommons.org/licenses/by/4.0/deed.en
_US
WSEAS TRANSACTIONS on FLUID MECHANICS
DOI: 10.37394/232013.2023.18.12
Guilherme S. Teixeira, Marco D. De Campos
E-ISSN: 2224-347X
122
Volume 18, 2023