Review of OpenFOAM applications in the computational wind engineering: from wind environment to wind structural engineering

Abstract

The use of computational fluid dynamics (CFD) in the wind engineering (WE) is generally defined as computational wind engineering (CWE). Since its foundation in 2004, the use of OpenFOAM in CWE has been increasing progressively and covers nowadays a wide range of topics, from wind environment to wind structural engineering. This paper was drafted in response to the invitation from the organizers of the 18th OpenFOAM workshop held in Genoa (Italy) on 11–14 July 2023, when a technical session on Civil Engineering and Wind Engineering was organized. In this paper the author briefly reviews the history of WE and surveys the evolution, methods, and future challenges of OpenFOAM in the CWE. Topics are here regrouped into three main research areas and discussed from a physical, engineering and purely computational perspective. The study does not cover the Wind Energy and related topics, since this can be considered nowadays as a stand-alone subfield of the WE. This review confirms that OpenFOAM is a versatile tool widely used for WE applications that often require new models to be developed ad hoc by CFD users. It can be coupled easily with numerical weather prediction models for mesoscale-microscale wind and thermal studies, with building energy simulation models to determine the energy demand, with finite element method for structural engineering design. OpenFOAM represents an extraordinary opportunity for all CFD users worldwide to share codes and case studies, to explore the potential of new functionalities and strengthen the network within the CFD community.

1 Introduction

In the last decades and since its birth, several definitions of wind engineering (WE) have been provided by scholars and researchers. Cermak [1] best defined the WE as the “rational treatment of interactions between wind in the atmospheric boundary layer and man and his works on the surface of Earth”. A broad and fascinating definition has been recently provided by Solari [2], who stressed out the dualism property of the wind. Solari [2] defined the wind as the evil when it destroys structures and infrastructures, makes environments uncomfortable, erodes lands by leading to desertification, causes fatalities. On the other hand, the wind may be good because it is the engine of atmospheric motions, it allows the production of green renewable energy through windmills and wind turbines, it blows far away pollutants from cities, and it improves lives of people in deserts and arid lands through natural ventilation. As reviewed by Solari [3], the WE discipline has been evolving and adapting itself through the centuries, by progressively involving more and more topics in which the wind plays a major role. This is also evident from the evolution of session topics scheduled in the WE conferences through the last decades. In 1963, in what we might consider the seed of the International Wind Engineering Conference (ICWE), namely the Symposium on Wind Effects on Buildings and Structures held in Teddington, UK, contributions mainly devoted to wind effects on structures were presented [4, 5]. In 2023, in the most recent 16th International Wind Engineering Conference held in Florence, Italy, a list of thirty-one potential topics spanning from meteorological phenomena to pollution dispersion was presented [6].

Various experimental and numerical techniques have been supporting the WE research studies through different eras (e.g. [7,8,9]). In most of the cases, these techniques have been inherited from other communities (as aerospace and mechanical engineering) and further developed to address WE topics. By overlooking the experimental techniques (as wind tunnels and field measurements) not covered by this review, the numerical technique mostly used by the WE community is certainly the computational fluid dynamics (CFD). As mentioned by Blocken [10], the CFD made its firstly appearance in a WE conference as topic session in 1991, at the 8th International Wind Engineering Conference held in London, Ontario, Canada, and chaired by A.G. Davenport [11]. The use of CFD in WE is generally defined as computational wind engineering (CWE). The scientific literature offers a long list of outstanding review papers focusing on the history and evolution of the CWE (e.g. [8, 12,13,14,15,16,17,18,19,20,21,22,23,24,25,26,27]). The 1st International Symposium on Computational Wind Engineering was held at the University of Tokyo in August 1992, and organized by Prof. S. Murakami also considered as the father of this discipline. In 1997 after 5 years the 1st CWE conference, Prof. Murakami reviewed the progress of CWE focusing on the mainly used numerical approaches, as the steady and unsteady Reynolds-averaged Navier–Stokes (RANS) and large-eddy simulation (LES) [13]. He concluded that although various numerical approaches were used to predict the wind flow around bluff bodies, how to best select such approaches (based on application) was still an open question at that time. He pointed out that albeit LES already gave better results than RANS, the former was too computationally demanding for many applications. Murakami [13] closed the paper by claiming that “… rapid evolution of CPU hardware will surely overcome this restriction, and wide application of LES to CWE problems will certainly be realized in the near future”. It is curious to observe that, despite the rapid growth in computing power of the last two decades, the use of LES in several CWE topics still remains prohibitive for academicians as well as for practitioners. On the other hand, less sophisticated (then less computationally demanding) approaches like the steady RANS became the most used in CWE research and practice through the years (e.g. [7, 10, 28,29,30]). Meantime, extensive best practice guidelines documents have been developed to help the CFD users with the setting of approximate form of governing equations, turbulence model, domain and grid, boundary conditions, discretization schemes, and so on (e.g. [31,32,33,34,35]). Likewise, as reviewed by Blocken [10] the development of verification and validation as well as of uncertainty quantification methods in CFD for WE simulations became crucial to support the activities of both scientists and practitioners (e.g. [36,37,38,39]). On this subject, an exhaustive review has been recently provided by Tominaga et al. [40]. It is worth noticing that if few years ago the mostly used approach (i.e. RANS) was strongly supported by best practice guidelines, nowadays similar guidelines are almost totally missing for one of the most currently used approaches (i.e. the LES). As detailed by Potsis et al. [27], some standardized procedures have been provided about pressure distributions and peak structural response on building (e.g. [24, 40]). However, except for some stand-alone contributions, there is no consensus in the scientific community about the verification and validation process. The state-of-the-art lacks generalized LES best practice guidelines that may help the user in defining (as for RANS) the most relevant computational settings: domain size, grid size (in LES responsible for the cut-off filtering), the choice of the most appropriate inflow method generator (rather relevant in LES), and so on. Moreover, also the validation process (with experimental data) of LES results may be more intricate than RANS results. LES data should rely not only on mean quantities but also on high-order statistics in order to accurately describe the turbulent structures of the flow. Overall, these aspects can be considered as serious concerns that sometimes may limit the applicability of LES to a wide range of numerical studies [30].

The CFD tools historically used in CWE are mainly two: the commercial software ANSYS Fluent [41] and the open-source software OpenFOAM [42, 43]. However, to the best knowledge of the author, a fully dedicated review on scientific CWE studies carried out with OpenFOAM is still missing. This is the innovative scope of the present paper in which CWE topics investigated with OpenFOAM in the last decades are reviewed. Since the 2000s, OpenFOAM has been widely used by wind engineers as well as atmospheric scientists to simulate the wind and airflow. OpenFOAM as well as other open-source codes has some advantages with respect to commercial CFD software (e.g. ANSYS Fluent but not only): (1) the user is not bound to pay any license; (2) codes from the pre-processing to post-processing stage can be manipulated and implemented from scratch; (3) it can be integrated with other open-source codes and vice-versa (e.g. Phyton, Paraview, WRF, etc.); (4) since free-license the user can run simulations in parallel on high-performance computing (HPC) systems with a large number of nodes (i.e. cores) without worrying about license costs. On the other hand, OpenFOAM requires programming skills (e.g. C++) with respect to other commercial tools, making this software not accessible at first glance to users that may lack the required know-how in programming. Moreover, OpenFOAM is not based on a graphical user interface (GUI) and this could make the software generally less intuitive than other commercial CFD tools.

This paper was drafted in response to the invitation from the organizers of the 18th OpenFOAM workshop held in Genoa (Italy) on 11–14 July 2023, for which technical sessions on Civil Engineering and Wind Engineering were organized. For the present review, a database of 289 papers, books and official websites has been assembled. The papers have been selected from well-known website platforms (as Science Direct) by using the most common keywords appeared in the international WE and CWE conferences of the past decades: wind, flow, CFD, OpenFOAM, building, bridge, complex terrain, downscale, mesoscale, microscale, microclimate, wind comfort, wind-driven rain, wind load, windblown sand, snow drift/accumulation, and so on. As expected, most of the papers (about 34%) have been published on the reference journal of the WE and CWE community, that is Journal of Wind Engineering and Industrial Aerodynamics, followed by Computers and Fluids, Building and Environments, Urban Climate, Applied Mathematical Modelling, Boundary-Layer Meteorology, and so on. An overview about the use of OpenFOAM in the CWE is provided in Fig. 1. Three main research areas have been identified in this review: (1) CFD for complex terrain: from mesoscale to microscale, (2) CFD for the built environment, (3) CFD for wind structural engineering. Within these research areas, various topics have been selected in turn. The statistics related to the use of OpenFOAM per research area and topic are reported in Fig. 1a and b, respectively. The percentage indicates the number of papers reviewed per research area (Fig. 1a) and per topic (Fig. 1b), with respect the total number of OpenFOAM studies in CWE considered in this review, namely 188. The histogram of Fig. 1c shows the OpenFOAM studies in CWE published from 2011 to 2023. Some papers have been also published earlier, between 2004 (i.e. the foundation of OpenFOAM) and 2011, but these are considered statistically not meaningful for the final purpose of this plot. Note that the Wind Energy is one of the topics where OpenFOAM is most widely used. However, the Wind Energy can nowadays be considered as a stand-alone WE subfield, with its own community and international conferences worldwide. The same applies also for topics closely related to Wind Energy, dealing with wind and wave effects on off-shore structures (as off-shore/on-shore wind turbines, wave–structure interaction, floating structures, and so on). For this reason, only research studies closely related to wind energy exploitation in the built environment are included in the present review.

Fig. 1

Use of OpenFOAM in the CWE a per research area and b per topic. c Histogram plot illustrating the number of studies in the CWE carried out with OpenFOAM from 2011 to 2023

The geometry and grid generation is a crucial stage to achieve successful CFD results, irrespective of the CWE study under investigation. For sake of brevity, in the present paper the author decided not to focus on very detailed (although important) geometry and grid generation procedures nor on the tool used to generate them. Nevertheless, it is worth noticing that the studies carried out with OpenFOAM and mentioned here do not always use grids constructed with open-source tools/utilities of OpenFOAM (as SnappyHexMesh) or integrated in it (as CfMesh). Conversely, in most of the cases either other open-source tools or commercial tools have been used to construct geometry and grid.

The paper is organized as follows. Section 2 discusses the use of OpenFOAM for complex terrains, from mesoscale to microscale. Section 3 discusses the use of OpenFOAM for the built environment, in particular, for wind and thermal comfort assessment, pollutant/gas dispersion, wind-driven rain, windblown sand and snowdrift. Section 4 addresses the use of OpenFOAM for the modeling of wind effects/loads on bridges, low-rise and high-rise structures as well as photovoltaic panels. Section 5 closes the paper with summary and perspectives.

2 CFD for complex terrains: from mesoscale to microscale

This section focuses on the use of OpenFOAM for the simulation of winds on complex terrains, from the mesoscale to the microscale. The contributions on this topic represent approximately the 12.23% of the total number of OpenFOAM contributions of this review (see Fig. 1a).

When the micro-scale (see [44] for the classification of meteorological scales) model OpenFOAM is applied to simulate real full-scale environmental flows, like wind flows over complex terrain as well as in urban areas, some information concerning the larger-scale (i.e. meso-scale) meteorological conditions is required. This can be obtained either using the micro-scale model in standalone configuration, implementing suitable initial and boundary conditions by means of analytical models or interpolation of the needed variables (e.g., wind velocity, turbulent kinetic energy, energy dissipation rate, temperature, etc.), or coupling OpenFOAM to a meteorological model (or similar proxy like reanalysis) through a process of downscaling of meteorological fields from the larger-scale model to the micro-scale one. In the micro-scale model, the complexity of terrains is reproduced numerically as combination of two stages. The STereo Lithography interface format (STL) is usually used to accurately reproduce the complex orographic condition. The non-homogeneous roughness is generally modeled by means of patches necessary to subdivide the ground in terms of homogeneous aerodynamic roughness length (${z}_{0}$). Additionally, when the orography is very complex and steep (e.g. mountains or hills), it is common practice to add a buffer zone with artificially smoothed orography at the external boundaries to avoid artificial gradients responsible for potential numerical instabilities (e.g. [45, 46]). Urban texture can also be included in the STL file to explicitly model structures and infrastructures. Once the three-dimensional geometry, the computational domain and grid are generated, the minimal approach to run standalone CFD simulations consists in assuming a neutral atmosphere, i.e. thermal energy equation is neglected. In such a case, standard inlet conditions are defined in terms of vertical profiles (e.g. power law, log-law-of-the-wall, and turbulence [34, 47, 48]) for steady/unsteady RANS simulations [49], while inflow generation methods must be adopted for LES simulations. Inflow generation methods have been widely applied in OpenFOAM, as the method of Deodatis [50] used by Ren et al. [45] to simulate wind fields in complex orography and more recently the one proposed by Melaku and Bitsuamlak [51] validated by means of wind-tunnel tests.

Simulating non-neutral atmospheric conditions in standalone micro-scale models is more challenging. The wind field simulation using RANS/URANS requires inlet wind profiles following the Monin–Obukhov similarity as well as modified turbulence model and wall functions to avoid turbulence decay within the computational domain [52]. The consideration of thermal boundary conditions can also require ad-hoc implementations to make the temperature inlet profile consistent with wall functions [53]. For LES applications, inflow generation methods like the method proposed by Xie and Castro [54] exist, these are suitable for neutral as well as unstable atmospheric conditions and were tested by Vonlanthen et al. [55] over a real terrain topography.

The dynamic downscaling approach refers to the use of meso-scale models to explicitly resolve the effects of the larger-scale meteorological phenomena coupled dynamically to micro-scale models to capture the local phenomena of main interest for the CWE. Meso-scale models are usually meteorological models used to forecast weather conditions, also commonly known as numerical weather prediction (NWP) models. In principle, the coupling between NWP models and micro-scale CFD models can be realized through a one-way or two-way technique. For the one-way coupling of NWP models with OpenFOAM steady RANS accounting for thermal effects (i.e. buoyantBoussinesqSimpleFOAM solver), the larger-scale model (the NWP) is used to calculate the steady state of the atmosphere at each output time step, which is typically in the order of few hours. This information is used in turn to evaluate the boundary conditions at different times for the micro-scale model (the CFD) in terms of wind and turbulence profiles using standard analytical function (e.g. [47]) or simply interpolating from the coarse to the fine grid. Accordingly, this approach needs proper post-processing algorithms to extract the required information (e.g. wind, temperature, etc.) from the NWP model and allows running the micro-scale model independently from the larger-scale one, which in theory makes also straightforward the coupling of micro-scale models with available datasets of hindcast or reanalysis. No feedback is expected in one-way coupling from the CFD model to the NWP model. Miao et al. [56], for instance, coupled the Weather Research and Forecast (WRF) by Skamarock et al. [57] to OpenFOAM in order to simulate the pollutant dispersion in Beijing, China. The resolution of the WRF inner domain was of 1 km, equal to the micro-scale domain size, so that only the grid cell nearest to the CFD inlet was used to provide the boundary conditions for CFD simulations. Analogous studies were carried out by various scientists: Wong et al. [58] inestigated the urban microclimate in Singapore; Kadaverugu et al. [59] simulated the wind fields in Nagpur City (India) accounting for the vegetation effects with the porousSimpleFOAM solver; Castorrini et al. [60] and Che et al. [61] applied the one-way coupling approach for wind resource prediction purposes. A systematic analysis of the one-way coupling WRF-OpenFOAM for different turbulence models available in WRF and in OpenFOAM is reported by Temel and van Beeck [62]. By testing various turbulence models for the Askervein Hill project, the authors proposed several closure constants and near-wall treatment suitable for near-neutral conditions [63]. Following up this work, the authors presented a modified version of the PBL BouLac scheme for WRF coupled to OpenFOAM that improves the prediction of velocity and turbulence by using the RANS approach in complex terrain [64]. The authors further refined closure constants and near-wall treatment [65] based on simulations of the Joint Urban 2003 experiment [66]. Based on the OpenFOAM micro-scale RANS simulations of the Askervein and the Joint Urban 2003 field campaigns, García-Sánchez and Gorlé [67] tried to evaluate the wind field uncertainty of the one-way coupling technique with an ensemble approach. Similarly to the ensemble prediction methods used in weather forecast, in the ensemble approach the CFD boundary conditions (calculated from the NWP model) are perturbated and the variability of the CFD results properly quantified. They concluded that the ensemble one-way coupling can be considered satisfactory since it encompasses with high confidence level the true solution.

In the one-way coupling of NWP models with OpenFOAM in URANS or LES cases (i.e. buoyantBoussinesqPimpleFOAM solver), the larger-scale model provides the CFD model with (fixed) initial and (time-varying) boundary conditions. Mughal et al. [68] coupled the WRF-LES model to OpenFOAM-LES using a post-processor to un-staggering the required WRF variables (i.e. velocity, pressure and temperature) on a collocated grid for each available time step (e.g., every 30 s) of the NWP model. Variables are then used as Dirichlet conditions at the OpenFOAM inlet through the timeVaryingMappedFixedValue boundary condition. Ground temperature and thermal fluxes are also assimilated from WRF. Similarly, Piroozmand et al. [69] coupled COSMO-URANS to OpenFOAM-URANS in order to simulate the wind and temperature fields in city of Zurich (Fig. 2). The two procedures are conceptually analogous, with the main exception that in URANS the time-step size can be larger with respect to LES with implications on the Courant number and inlet conditions may differ in the two approaches. Another research study with URANS-URANS one-way coupling of WRF-OpenFOAM was presented recently by Castorrini et al. [70]. The authors applied this approach for wind prediction offshore taking into account also the sea wave formation, which increase turbulence generation at the surface. In the two-way coupling, models exchange information back and forth among each other in such a way that the micro-scale model also influences the NWP forecast. On one hand, this approach may theoretically lead to more accurate results (both at the larger and smaller scales) with respect to the simpler one-way coupling. On the other hand, it is more difficult to implement this approach especially when NWP and OpenFOAM models are involved, since both have to run in parallel with synchronized time step by exchanging information at a fast rate. To the best knowledge of the author, this methodology has not yet been explored in the scientific literature.

Fig. 2

a Computational geometry and domain of the microscale CFD model. b Comparison of OpenFOAM and COSMO contours in terms of hourly average temperature and wind map on the typical summer day, June 23, 2015, at 12–1 p.m. The air temperatures and the wind speeds are shown 2 m and 10 m above the ground, respectively. Figures modified from Piroozmand et al. [69]

Overall, the high flexibility that OpenFOAM provides in a coupling process (with respect to other commercial CFD tools) is crucial to deeply investigate complex atmospheric phenomena at different spatiotemporal resolutions and favor the bridging between the Atmospheric Science and Wind Engineering communities.

3 CFD for the built environment

This section focuses on the use of OpenFOAM for simulation of wind in built environments, which represents approximately the 57.98% of the total number of OpenFOAM contributions of this review (see Fig. 1a). This section is organized into four subsections: wind flow modeling in the built environment (Sect. 3.1) with 19.68% of contributions, pedestrian wind comfort and urban microclimate (Sect. 3.2) with 12.23% of contributions, pollution and gas dispersion (Sect. 3.3) with 11.70% of contributions, wind-driven rain, windblown sand and snowdrift (Sect. 3.4) with 14.36% of contributions (see Fig. 1b).

3.1 Wind flow modeling in the built environment

Most of the best practice guidelines developed in the past two decades emphasized the importance of accurately modeling wind flow in built environment (e.g. [32, 34]). These recommendations have been used in a wide range of research studies, from the pedestrian-level wind comfort assessment to the exploitation of the wind energy by means of small-size wind turbines mounted on buildings’ roof (e.g. [71]). Best practice guidelines have been mostly developed with the aim of modeling by CFD (i.e. by RANS) neutrally stratified ABL winds in natural and built environments. According to Barlow [21] the Urban Boundary Layer (UBL)—the layer of the ABL where most of the population lives—consists of three main parts: the urban canopy layer (UCL), the layer up to the mean roof height where flow channeling occurs along the streets; the urban roughness sublayer (RSL) defined as the region including the UCL where the buildings exert significant drag on the flow and the wind is highly spatially dependent; and the inertial sublayer (IS) located above the RS where turbulence is homogenous and fluxes vary little with height (Fig. 3). The wind flow dynamics is generally quite complex in the UCL, where streets and open spaces (e.g. squares and green parks) may cause the onset of canyoning effects strongly dependent on the approach wind direction and urban fabrics [72]. As reported by previous review papers (e.g. [20, 73, 74]) a large number of studies have been carried out by scientists worldwide in order to investigate the wind flow behavior in the UBL. These studies were mainly targeted at providing new analytical models of vertical wind profiles (in terms of velocity and turbulent characteristics) in and above the UCL by using both experimental and numerical techniques (e.g. [75]). Most of these studies are generally carried out on arbitrary simplified geometries of buildings and cities. This is necessary in order to make the investigation less case specific and construct high-resolution computational geometries and grids that allow in turn to keep under control the number of control volumes. Probably one of the first attempts to simulate wind flow with OpenFOAM on a cluster of realistic buildings was made by Flores et al. [76]. The unsteady RANS and detached eddy simulation (DES) approaches were adopted to simulate the internal ventilation within an open pit including the effects of developed turbulence, buoyancy and stratification. A step forward was made by Carpentieri and Robins [77], who investigated by wind-tunnel tests and CFD simulations the impact of morphological parameters on wind flow in and above the UCL, through a simplified and a more realistic building array. The authors found that the building aspect ratio, the angle between street canyons and reference wind direction, and local geometrical features can significantly influence the flow dispersion. After a few years, a similar study aimed at understanding the impact of geometrical simplifications on wind flow in a realistic urban environment was published by Ricci et al. [78]. Here, results from 3D steady RANS and wind-tunnel tests were compared in terms of mean velocities and turbulent kinetic energy. The results showed that although simplification of geometries is generally possible and sometimes really necessary, more detailed CFD geometries can provide a better agreement with experiments (Fig. 4). Paden et al. [79] further investigated this aspect and proposed a workflow for automatically reconstructing simulation-ready 3D city models. As stated by the authors at the time of publication, the research study was still at an early stage and more work was required to further improve the reconstruction algorithms. Furtak-Cole and Ngan [80] proposed an alternative approach based on the vortex dynamics. This approach was applied to the UCL wind flow and a method for the prediction of mean horizontal velocities was derived. The Improved Delayed Detached Eddy Simulation (IDDES) turbulence model was then used to calibrate the approach on different built environment scenarios, for idealized and realistic canyons. The Delayed Detached Eddy Simulation (DDES) [81] as well as the IDDES that also incorporates the wall modeled LES (WMLES) [82] are among the most recent developments of the DES method [83]. More recently Yao et al. [84] proposed a new approach to characterize by LES the wind flow dynamics in the UCL, by parametrizing the atmospheric surface layer over a real dense city. The authors found that a rougher urban surface may generate eddies with a larger shear length scale, thus enhancing momentum transport.

Fig. 3

a Schematic diagram of daytime convective urban boundary layer with wind flowing from left to right. Dashed lines indicate top of rural and urban boundary layers; solid lines indicate local internal boundary layers. b Schematic diagram of roughness and inertial sublayers. Grey arrows indicate streamlines. Dashed line indicates mean building height H. Figures credit to Barlow [21]

Fig. 4

Impact of geometrical simplifications on the wind flow field and vertical mean velocity profiles. Figures modified from Ricci et al. [78]

While most of the publications dealing with UCL explore the in and above canopy regions, there is a range of scientific studies mainly focusing on the portion of wind flow developing only above the canopy (i.e. over idealized and real urban environments). Recently, Mo and Liu [85] conducted a study to characterize the wind flow in the ISL and RSL over a real urban district of Hong Kong city. Simulated data were then compared to wind-tunnel results for validation purpose. To better understand the turbulent structures of the wind flow developing over the urban city, simulations were carried out with the LES approach. In general, this is an important aspect commonly investigated in the research area of urban wind energy exploitation, as comprehensively reviewed by Toja-Silva et al. [86] and Jie et al. [87]. Back in 2016, Toja-Silva [88] proposed an empirical-heuristic optimization of the building-roof geometry for urban wind energy exploitation. However, these simulations were performed with RANS approach which is unable to properly predict regions of reversal and separation of the flow. For this reason, the same authors in the concluding section of that paper suggested the use of URANS and LES to better assess the unsteadiness of the flow. This is in line with the most recent advances on the subject, as confirmed by Kostadinović Vranešević et al. [89, 90] who used the LES approach to investigate the wind flow pattern around buildings with the aim to maximize energy potential resources.

Given the open-source nature of OpenFOAM, research studies have been also carried out with OpenFOAM to implement new numerical models (e.g. turbulence closure, inflow methods, solvers) and validate their performance on isolated and cluster of buildings in terms of wind flow velocity pattern and turbulence characteristics. RANS approach from OpenFOAM 1.6.x was used by Franke et al. [91] to simulate the wind flow around/over an array of simplified buildings, using different grid types (i.e. structured hexahedral, unstructured tetrahedral, unstructured hybrid grid of tetrahedra and prisms). The results were then validated by means of corresponding experimental results. Similarly, Wang et al. [92] carried out LES simulations to assess the wind flow pattern around an isolated simplified building with three grid types (i.e. hexahedral, tetrahedral and polyhedral cells). In general, they concluded that cases using polyhedral cells provided similar results to the case adopting hexahedral cells, and generally better than those cases using tetrahedral cells. A more extensive parametric study was conducted by Ozake et al. [93] on a 1:1:2 isolated building in the framework of the Architectural Institute of Japan [94]. Various computational grid arrangements, spatial discretization schemes, sub-grid scale (SGS) turbulence models and convergence criteria were tested with the LES. Also Liu et al. [95] and García-Sánchez et al. [96] investigated the performance of various turbulence modeling methods to predict airflow in simplified and realist urban environment. Ricci et al. [97] investigated the impact of turbulence models coupled to RANS approach and the impact of the surface roughness (in terms of equivalent sand-grain roughness height, k_s) on the wind flow pattern in a realistic urban district. They found that the choice of the turbulence model may significantly influence the results in terms of wind speed and turbulent characteristics. The authors concluded that “… the choice of a specific turbulence model may be crucial for a large category of urban physics and wind engineering problems … although it is not a trivial issue to clearly and unambiguously define which one should be definitively used for a specific investigation …”. The setting of inflow CFD conditions is also crucial in research studies focusing on wind in built environments. Back in 2013, Juretić and Kozmar [98] proposed a novel method to prescribe inflow boundary conditions in RANS approach coupled with the standard k–ε turbulence model [99], to simulate a neutrally stratified ABL wind flow. The CFD results showed a good agreement with wind-tunnel data in terms of mean velocity, turbulent kinetic energy and Reynolds stress profiles. 3D steady RANS investigations aimed at understanding the impact of inflow ABL wind conditions were also conducted by Ricci et al. [100, 101]. The authors found that the choice of different neutral ABL wind conditions as well as different formulations from the literature [34, 47] to define the profiles of mean velocity and turbulence characteristics may lead to different results in the UCL. On this subject, García-Sanchez et al. [102] conducted a distinguished research study aimed at quantifying the uncertainties related to three inflow parameters: the wind velocity, the wind direction, the aerodynamic roughness length (z₀) of the logarithmic profile. 3D steady RANS simulations were performed on a realistic urban environment. The uncertainty quantification method revealed a great potential to aid the development of more realistic inflow boundary conditions in atmospheric environment simulations. Unlike RANS simulations, as also stressed in Sect. 2 the definition of inflow conditions for LES simulations may be a challenging task, since it requires the choice of a specific inflow method to perturbate the flow field. Analyzing the numerous inflow methods developed in the past decade for LES simulations is beyond the scope of the present review paper. To support the reader, a non-exhaustive list of publications dealing with this topic is suggested here (e.g. [51, 103,104,105,106]). In these papers, the authors proposed novel inflow methods by comparing their performance with methods already available in the scientific literature for different type of subjects, from open terrains to isolated buildings. Among the others, Mansouri et al. [107] carried out an interesting study in OpenFOAM by testing four types of synthetic turbulence generator methods to provide a neutral ABL wind: digital filter methods, synthetic eddy methods with different shape functions, divergence free synthetic eddy method, and two types of anisotropy turbulent spot method. In general, the authors found that the four methods produced spurious pressure except for the cases using the synthetic eddy method with the Gaussian shape function.

Less traditional solvers (than RANS and LES) are also recently used to predict wind flows in the built environment. An example is offered by Xia et al. [108], who analyzed the performance of the Very-Large Eddy Simulation (VLES) approach [109, 110] to predict turbulent separated flows. In general, the results showed a good performance of the VLES when compared to available LES and experimental data. Li et al. [111] adopted the three fast fluid dynamics (FFD) models [112] with different pressure-correction schemes for solving Navier–Stokes equations in OpenFOAM: the standard incremental pressure-correction (SIPC), the non-incremental pressure-correction (NIPC), the rotational incremental pressure-correction (RIPC). The authors found that the SIPC is faster than NIPC and RIPC if using the same grids, turbulence model and time-step size. On this subject, more recently research studies have been conducted on built environments by using genetic algorithms and neural network methods for the optimization of urban wind conditions at local scales (e.g. [113,114,115,116]).

Overall, the OpenFOAM is largely used to investigate the wind flow development over/through built environments, but also to develop new models and solvers that can improve the prediction of wind characteristics around buildings, cluster of buildings and generally in/above the UCL. Assembling numerical benchmarks validated with experimental data is crucial to support the development of new analytical formulations of vertical wind profiles (velocity and turbulence) in complex environments.

3.2 Pedestrian wind comfort and urban microclimate

The pedestrian-level wind comfort as well as the thermal comfort are among the most investigated topics when dealing with the built environment. This is because the wind comfort and wind safety assessment of pedestrians is nowadays imperative in many countries when designing new buildings (mainly high-rise buildings) amidst historical and well-settled urban layouts. Strong winds in the middle of urban contexts can be extremely dangerous for people and medium/long-term impact on the economy of cities and communities. One of the first paper dealing with this topic was probably published by Jackson [117], who assessed the wind effects on pedestrians by using a pre-assembled database of measurements and questionary survey. Since then, various criteria to evaluate the wind comfort and safety were developed by academicians and practitioners, and numerous review papers on this topic were then published (e.g. [18, 118,119,120,121,122,123,124,125,126,127]). Pedestrian wind comfort studies can be grouped into thermal comfort studies and more simply wind comfort studies, defined by the author of this review as such when referring to the mechanical effect only (by neglecting the temperature variation) of the wind on pedestrians.

In general, the wind comfort studies represent about 52.2% of the comfort research studies (i.e. wind comfort and thermal comfort) here reviewed. About 67% of these wind comfort studies have been carried out with the 3D steady RANS approach. The reason behind this choice may be twofold. Firstly, as stressed by Blocken [8] best practice guidelines have been developed mainly for RANS simulations. Almost no guideline documents exist for LES and this is generally considered a serious limitation by CFD users. Secondly, as claimed in previous review papers (e.g. [30, 34]) the RANS approach can accurately predict high wind speed regions of flow which are mainly responsible for the discomfort. It means that, the inability of RANS in predicting low wind speed regions commonly does not lead to significant mispredictions in comfort analyses. On the other hand, the RANS approach usually requires sensitivity studies to understand how numerical parameters (e.g. geometrical simplification, grid size/type, boundary conditions, turbulence models, etc.) may affect the results. There are various examples of parametric studies on wind comfort carried out with OpenFOAM in the past years. Weerasuriya et al. [128] proposed a new inflow boundary condition to model twisted wind profiles generating from hilly topography upstream of urban environments. The research study was carried out with ANSYS Fluent and OpenFOAM. The authors observed that generally OpenFOAM was more reliable in predicting wind comfort with the newly proposed boundary conditions. Dhunny et al. [129] and Cindori et al. [130] conducted a sensitivity study to assess the pedestrian wind comfort in a tropical city and around an isolated (simplified) building, respectively, by investigating the impact of various k–ε and k–ω turbulence models coupled with RANS. Sensitivity studies with focus on different parameters were carried out by Tsichritzis and Nikolopoulou [131] and Hågbo et al. [132]. Tsichritzis and Nikolopoulou [131] analyzed the impact of morphological characteristics related to building height variation (in a real city) on the wind comfort. Hågbo et al. [132] investigated how different geometry inputs’ (to construct the computational grid) may influence the wind flow field at the pedestrian level. They found that the footprint extrusion model showed significant differences with respect to the national database and the Airborne LiDAR model, possibly affecting in turn the building design decisions in a well-settled urban layout (Fig. 5). However, performing CFD simulations on large-scale domains (like cities) to investigate the impact of several parameters can be very time consuming and sometimes prohibitive especially for practitioners. To overcome this issue, Kaseb et al. [133] proposed an innovative evolutionary-based framework to optimize building heights and plan area densities and improve wind comfort in complex real urban areas. The optimization method is based on a genetic algorithm and particle swarm optimization. The authors concluded that with this framework the computational efforts can be reduced significantly and the wind comfort can be improved in the urban area.

Fig. 5

Comparison of the different building geometry types and corresponding wind comfort classes. Figures credit to Hågbo et al. [132]

In general, the method adopted to define the mean wind speed in the wind comfort assessments may also play an important role, and this can change based on the CFD approach used for simulation. This was the goal of the LES study conducted by Kikumoto et al. [134], who focused on the mathematical interrelation among three mean wind speed types (i.e. mean-vector speed, mean speed, and effective speed) around an isolated building. The comparative analysis revealed that deviations may be significant near the ground surface and in recirculation regions of the flow. Ikegaya et al. [135] adopted the LES approach to simulate the wind flow around a 1:1:2 isolated building. Thus, they analyzed the probability density distribution for each velocity component and wind speed in order to provide a reliable model capable to predict the exceeding wind speeds at the pedestrian level. Likewise, Wang and Okaze [136] proposed a novel statistical method to estimate the low occurrence of strong wind speeds by the mean wind velocity and also the turbulent kinetic energy. In their study two case studies, previously simulated by Okaze et al. [137] with LES in OpenFOAM, were considered: an isolated building and a building array. Lin et al. [138] analyzed the wind comfort with the focus on the “downwash” and “Venturi effect”, previously observed experimentally by Tamura et al. [139]. For this purpose, authors carried LES simulations around square-section buildings with same aspect ratios and different sizes.

Mitigation methods aimed at reducing high wind speed zones in urban areas (i.e. to improve the comfort) are also generally conducted in CFD and validated by experimental data. As thoroughly reviewed by Buccolieri et al. [140], the vegetation (e.g. trees, grass, hedges) is one of the measures commonly used by engineers to improve the pedestrian-level wind comfort in the built environment. In OpenFOAM, the vegetation is often modeled as a porous medium and the solver porousSimpleFoam is therefore used for RANS simulations. However, a very limited number (i.e. three) of OpenFOAM studies [141,142,143] focusing on the mechanical effects (only) have been found by the author of this review paper, and two out of three are conference proceedings.

The thermal comfort studies represent about 47.8% of the total number of comfort studies reviewed in this paper. The majority of these deals with urban microclimate, urban heat island, natural ventilation and building energy simulation (BES). In the past decade, review papers have been published on these subjects (e.g. [144,145,146]) mainly focusing on urban microclimate and impact on the human health. In this regard, as for the wind comfort, mitigation measures have been developed both numerically and experimentally in order to improve the thermal comfort of people under adverse atmospheric conditions, especially in urban environments. The reader can find some interesting and exhaustive review papers recently published in the scientific literature (e.g. [147,148,149,150,151]). While OpenFOAM as well as ANSYS Fluent and ENVI-met [152] are the main CFD-based tools used to simulate atmospheric wind and temperature fields in urban environments, BES simulations for outdoor/indoor analyses are usually conducted with different tools (as EnergyPlus, ESP-r, SPARK). In microclimate analysis, the CFD results (in terms of wind, temperature, humidity, solar radiation, etc.) are generally used as input boundary conditions for BES simulations to determine the energy demand/performance. This process is commonly obtained by one-way CFD-BES coupling. As for the wind comfort, sensitivity studies on specific numerical/geometrical parameters are crucial also in urban microclimate. In general, research studies are primarily carried out on generic and simple geometries, often well-known benchmarks like canyons and building arrays. Once the impact of numerical parameters is well understood, more complex and realistic urban environments are then analyzed. Allegrini et al. [153] and Allegrini and Carmeliet [154] investigated the influence of different simplified urban morphologies (i.e. urban plan and building height) as well as of the buoyancy on the local microclimate. CFD simulations were performed with OpenFOAM while BES simulations were carried out with CitySim [155]. The results obtained in previous fundamental studies further motivated the authors to apply the one-way coupling OpenFOAM-CitySim on a real case scenario (a district of Zürich, Switzerland) to evaluate the increase of wind velocity and surface temperature due the presences of newly designed buildings amidst well-settled urban layout [156] (Fig. 6). Also Mokhatar and Reinhart [157] focused on a realistic scenario by investigating a district of San Francisco in California, United States. The authors proposed an innovative probabilistic, progressive, and accuracy-adaptive modeling approach for faster spatially resolved outdoor thermal comfort estimation. In this study, 3D steady RANS simulations were carried out with OpenFOAM by means of Eddy3D, a toolkit for decoupled outdoor thermal comfort simulations in urban areas [158]. Similary, a sensitivity study mainly focusing on the performance of different BES tools (starting from the same OpenFAOM CFD simulation) was carried out by Heidarinejad et al. [159] who investigated the influence of building surface solar irradiance on environmental temperatures in a simplified urban area. Urban microclimate studies may also be used to calibrate and monitor the performance of reference target buildings. This was the scope of the research conducted by King et al. [160] that analyzed the impact of several wind directions on a cubical building in isolation and in a staggered nine cube array format, with both OpenFOAM and ANSYS Fluent. The comparison was made using methods suggested by guide for ventilation based on internal/external building pressure differences. The authors observed that the ventilation rate of the cubical building in isolation (with single-sided opening) was lower than either of the cross-flow cases, and relationships between air change rate and wind angle were much weaker in the array cases. Miguel et al. [161] used OpenFOAM (for atmospheric simulation) and EnergyPlus (for building energy simulation) to simulate the outdoor conditions and the building energy performance of a reference building by evaluating potential countermeasures to urban heat island effects.

Fig. 6

Two possible design configurations of building geometries in the area under study of Zürich city, in Switzerland. Contours in terms of temperature difference (between the local and the ambient air temperature) made at 2 m above the ground for design A (a, c) and B (b, d), and two approach wind directions. The wind speed is 5 m/s at 10 m above the ground, the albedo is 0.2. Figures modified from Allegrini and Carmeliet [156]

Overall, the two topics introduced in this subsection are based on a different workflow, different analyses, different tools and models. While for the wind comfort assessment the main factor is the wind speed and in few cases also the turbulence, in the thermal comfort coupling the wind and the temperature fields is essential. This latter can rely on a downscaling approach executed by means of open-source tools (e.g. WRF–OpenFOAM–EnergyPlus) with the potential to reach very small scales (e.g. the room scale) through BES simulations.

3.3 Pollution and gas dispersion

The World Health Organization estimates that pollutants and gases have caused about 4.2 million premature deaths around the world and about 99% of the world’s population breaths air exceeding the prescribed limits [162]. As stressed by the United Nations the percentage of the population living in urban area is rapidly increasing. Therefore, making cities more sustainable and resilient to climate change by lowering the carbon emission and increasing renewable energy resources is imperative [163, 164]. In the last two decades, great efforts to investigate the pollutant dispersion/concentration at different spatiotemporal scales have been made by the WE and Atmospheric Science community, under various atmospheric conditions and for a large variety of emitting sources (from traffic emissions to thermal power plants). As observed in Sect. 3.2, most of the research has been and is still conducted on the simplest and most common urban subsystem, that is the urban street canyon. The urban street canyon is an elementary configuration that through the years helped researchers to deeply understand the airflow and pollutant dynamics also in more complex urban environments (as cities) (e.g. [144, 165]). In general, the CFD technique has been widely used in this field to solve advection and diffusion equations of concentration based on the velocity field obtained from the Navier–Stokes equations. As opposite to wind tunnel and field measurements, the CFD allows the monitoring of output data (e.g. pressure, velocity, pollutant concentration, temperature, etc.) at any point of the domain, facilitating the understanding of complex flow dynamics throughout the entire volume/space under investigation (e.g. [8, 166]). Traffic emission sources like cars and trucks are usually modeled by means of ideal lines or points. Recently, an innovative research study has been carried out by Qin et al. [167] with ANSYS Fluent to understand how ideal sources can properly reproduce the emission traffic of realistic car source in terms of pollutant concentration in urban canyons. However, except for this study most of the RANS and LES studies are carried out on simplified urban street canyons and cities with ideal line/point sources, under neutral ABL wind conditions (i.e. with standard logarithmic wind velocity profile at the inlet) and creating thermal stratifications inside the domain (e.g. [168,169,170]). The thermal stratification is obtained by combining the desired reference wind velocity at the inlet and the surface heat flux on the surfaces (e.g. ground as well as buildings), through the evaluation of the Richardson dimensionless number. More complex scenarios than urban street canyon are also analyzed for different engineering purposes. Flores et al. [171] used DES and LES approaches to investigate the pollutant dispersion inside a simplified and realistic open pit mines under intense insolation. The authors found that buoyant currents may foster the exhaust of particles from the pit by modifying the mechanism of the flow recirculation inside the cavity and increasing the atmospheric turbulence. Reiminger et al. [172] used the RANS approach in combination with the Renormalization Group (RNG) k–ε turbulence model [173] to analyze the impact of wind speed and atmospheric stability (i.e. neutral, unstable and stable cases) on the pollution concentration within a street with noise barriers (i.e. like a street canyon).

On simplified urban street canyons, new models have been developed to execute CFD simulations on pollution and thermal stratification. Li et al. [174] proposed a new scheme based on simpleFoam (semi-implicit method for pressure linked equations) algorithm in OpenFOAM, the so-called TimeVarying-SIMPLE, to simulate the time-series flow field under time-varying inflows. The authors performed LES simulations on an ideal street canyon, and compared the wind flow and pollutant dispersion obtained with the new approach with those achieved with pisoFoam (pressure-implicit with splitting of operators) and pimpleFoam (the merge of PISO and SIMPLE) algorithms. Hang et al. [175] developed a new CFD code named APFoam to simulate the integrated processes of both complex photochemical pollutant reaction (NO_x–O₃–VOCs) and dynamic dispersion under two 2D street canyons with different aspect ratios, namely a typical street canyon and a deep street canyon (Fig. 7). Leng et al. [176] proposed an innovative micro-in-meso-scale simulation framework to downscale mesoscale meteorological data (obtained with WRF) at the microscale (by RANS simulations). Results are provided to the final users in terms of wind and pollutant concentration at the local scales (e.g. urban area or a district of it). Research studies using downscaling techniques (e.g. WRF—OpenFOAM) and focusing on gas leakage, gas dispersion, reactive pollutants and the related exposure risk for humans have also been found in the scientific literature (e.g. [177]). Most of these have been carried out on real industrial sites, as offshore platform for subsonic and sonic release [178], thermal power plants surrounded by urban area for comparison with analytical Gaussian plume models [179] as well as on simple and basic urban elements as street canyons [180].

Fig. 7

a and b Computational grid of typical street canyon and deep street canyon. Concentration distribution for the two cases in terms of c and d Co₃, e and f C_NO and g and h Co₃, for U_ref = 3 m/s at t = 5400 s. Figures modified from Hang et al. [175]

As for wind comfort studies, vegetation (e.g. grass, trees, hedges) has been widely used to mitigate the pollutant concentration in urban and surrounding environments. However, as claimed by Janhäll [181] the “… design and choice of urban vegetation is crucial when using vegetation as an ecosystem service for air quality improvements. The reduced mixing in trafficked street canyons on adding large trees increases local air pollution levels, while low vegetation close to sources can improve air quality by increasing deposition…”. This is an important aspect investigated worldwide by CFD simulations, wind-tunnel testing and field measurements at different spatiotemporal scales. While the LES approach is mainly used for urban street canyons, the RANS approach combined to (various) k–ε and k–ω turbulence models is often preferred to simulate large-scale environments (as cities). It is worth noticing that, in this kind of studies the thermal stratification and buoyancy effects are rarely taken into account. Trees and hedges are the green elements more widely adopted and modeled in computational domains. Irrespective of the numerical approach used, trees and hedges in CWE can be (1) explicitly modeled with its components (usually trunk and branches) or (2) implicitly modeled as porous fluid zones. In the latter, an equivalent leaf area density and drag coefficient is assigned to the porous fluid zones and additional source/sink contributions are considered in transport equations [182]. Most of the studies uses the implicit modeling of vegetation. Vranckx et al. [183] investigated the impact of trees (implicitly modeled) on pollutant dispersion in street canyons by RANS and k–ε turbulence model, by using the porousSimpleFoam solver as the majority of RANS studies mentioned below. In line with the Janhäll [181], the authors observed an annual pollutant concentration increase of about 8% for element carbon and about 1.4% for PM₁₀, due to the presence of vegetation. Different results were found by Jeanjean et al. [184,185,186], who investigated the potential of trees (implicitly modeled) as well as buildings facades coated with photocatalytic paint and solid barriers to disperse road traffic emissions in built environments. The cases of Leicester and London, in United Kingdom, were simulated by RANS and k–ε turbulence model. Overall, the authors found that trees may have a beneficial impact on road traffic emissions by reducing the ambient concentration of road traffic emissions of about 7% at pedestrian-level height.

More fundamental research studies were also conducted on this topic. Wang et al. [187] analyzed the performance of explicitly modeled trees in an urban street canyon by using the LES approach. In general, the authors found that pollutant concentration increases significantly with an accumulation of pollution between the trunk and the leeward side of the canyon. For larger inflow wind velocities, the pollutant concentration is generally heavier with respect to the level observed in the absence of trees. McMullan and Angelino [188] proposed a recycling and rescaling turbulent inflow generator method for LES, to assess the performance of trees on the traffic pollutant dispersion in a street canyon. The authors concluded that tree crowns may reduce the effectiveness of the canyon vortex in ventilating the street, by enhancing the mean tracer gas concentration at pedestrian level on the leeward wall. Regardless of numerical settings, the conclusions of Wang et al. [187] and McMullan and Angelino [188] are in line with the conclusions of Vranckx et al. [183], who noted an increase of pollutant concentration when introducing trees in the street canyon. This confirms that there is no general consensus on the efficiency of vegetation to reduce concentration in simple street canyons as well as in urban areas. Thus, further CFD studies are required to deeply understand the basic mechanisms of flow dynamics and pollutant deposition/dispersion under various thermal stratifications.

3.4 Wind-driven rain, windblown sand and snowdrift

This section focuses on the use of OpenFOAM to simulate the wind-driven rain, windblown sand and snowdrift in different environments. These three subtopics have been regrouped within the same subsection because similar numerical methods can be used to model particles.

The publications on wind-driven rain represent about 40.74% of the papers included in this subsection. The wind-driven rain is an important phenomenon largely investigated in the past decades by the WE community. This phenomenon may be responsible of soil and building materials erosion, degradation of building envelops as well as structural damages due to the moisture intrusion [189]. Back in 2004, Blocken and Carmeliet [190] conducted a comprehensive review by presenting the state-of-the-art of this topic in building science. The authors carefully reviewed the main experimental, semi-empirical and numerical methods adopted until then. The use of CFD was also reviewed with main focus on the RANS approach used in combination with k–ε turbulence models. In 2010 and 2022, Blocken and Carmeliet [191] and Gholamalipour et al. [192] presented a new review of the state-of-the-art. Regarding the numerical techniques, they discussed on the use of steady-state and transient CFD approaches (e.g. RANS and LES) as well as the applicability of Lagrangian particle tracking and Eulerian multiphase methods. In general, the Lagrangian and Eulerian methods are often combined with the RANS approach in wind-driven rain simulations, especially for built environments. The Lagrangian method can provide a clear and straightforward overview of the droplet-wall interaction. However, it requires a significant number of raindrops to achieve accurate results, by making this method computationally demanding. The Eulerian method treats the rain as a continuum (as for pollutant, gas, sand, snow), and for each rain class of raindrop size different rain phases are considered [189]. This method is generally way less computationally demanding than Lagrangian.

To the best knowledge of the author, one of the first research studies on wind-driven rain with OpenFOAM dates back 10 years and was conducted by Kulibaly et al. [193]. Here the authors investigated the potential negative impact of this phenomenon on the hygrothermal performance and durability of building facades of an array of low-rise buildings. For this study, the RANS approach was used with the RNG k–ε turbulence model. The Eulerian method was adopted for the spatiotemporal information of the wind-driven rain. CFD results were then validated by means of field measurements. The same case study was numerically reproduced by Kulibaly et al. [194] by LES and Eulerian method, and the simulate data were validated with reduced-scale wind-tunnel data. A similar methodology was then used by Kulibaly et al. [195] to simulate the impact of wind-driven rain on two parallel buildings (Fig. 8) that later became an experimental and numerical benchmark for this kind of studies (e.g. [196]). In particular, the same case study was reproduced also by Xu et al. [197] who proposed an innovative method to define an effective horizontal release plane for Lagrangian particle tracking of raindrops in space. The automatic selection of release plane is based on the analytical solution for unobstructed (empty domain) raindrop trajectories. A scaling factor is then adopted to account for the impact of any physical obstruction.

Fig. 8

a Computational grid used for the CFD simulations of WDR. b Contours and c streamlines of normalized wind speed and d streamlines of rain phases for raindrop sizes d = 0.3 and 1.0 mm at reference wind speed U = 3 m/s in the vertical centerplane for wind from west. e Catch ratio distribution at reference wind speed U = 3 m/s and reference rainfall intensity (R_h = 1 mm/h) for wind from west. Figures modified from Kulibaly et al. [195]

The windblown sand counts about 48.15% of the papers considered in this subsection. The windblown and sand accumulation can create dangerous and harmful conditions to the built environment at various levels, from industrial facilities to railways, making this topic of great interest for engineering disciplines, environmental sciences as well as in applied mathematics and physics [198]. As reported by Bruno et al. [198] who provided the WE community with a comprehensive review on this topic “… A growing demand for windblown sand mitigation design, building and maintenance has been observed in the last decade and it is expected to further increase in the next 20–30 years. The increasing interest in windblown sand mitigation is testified by the growing number of published studies and filed patents in the last years. …”. In this review the authors proposed an original categorization of windblown sand-induced performance deficiencies of the railway systems and prevention techniques to mitigate the windblown sand effects. Experimental (as wind tunnel) and numerical (as CFD) techniques are commonly used to conduct investigations in this field. In particular, the CFD technique played a fundamental role in the analysis of flow dynamics, sediment transport over/around structures (e.g. buildings) and infrastructures (e.g. sand barriers) as well as in aeolian geomorphology applications [199]. One of the first numerical studies on hills and embankments was performed under neutrally stratified ABL winds by Deaves [200, 201]. Zhang et al. [202] utilized the RANS approach in combination with the k–ε turbulence model to simulate the wind flow and investigate the wind-induced erosion of railway embankment. However, in both cases the authors did not provide any indication about the used CFD tools. To the best knowledge of the author, a limited amount of windblown sand studies in the WE literature were conducted with OpenFOAM. Bruno and Fransos [203] performed RANS simulations with shear–stress transport (SST) k–ω turbulence model [204] on sand transverse dune, in order to investigate the wind flow dynamics and the induced sand erosion, transport and deposition. Special focus was laid on the emerging three-dimensional coherent flow structures arising in the wake of the transverse dune. Bruno et al. [205] investigated the aerodynamic effects on the wind flow of innovative and more conventional sand mitigation solid barriers, by means of RANS and SST k–ω turbulence model. Design guidelines were provided through a new proposed empirical dimensionless performance estimator (Fig. 9). Mitigation measures were also systematically analyzed by Horvat et al. [206] who investigated the local wind flow and potential sedimentation patterns around the railways. The knowledge of sedimentation patterns is crucial for preventing sand-induced limit states that may produce in turn serious disruptions on the whole supply chain system. Wind flow field, shear stress field and derived sand sedimentation/erosion patterns were obtained by RANS in combination with the SST k–ω turbulence model. The performance of different railway substructures and track systems was discussed under different reference wind velocities and angles of attack. In general, the sediment transport has been investigated with OpenFOAM also for other types of environments. In particular, Pourteimouri et al. [207, 208] analyzed by RANS how the approach-wind direction and building spacing and shape may affect the wind flow and related sediment transport patterns at the beach. The authors observed that: (i) buildings’ location may have a positive effect on dune growth by steering the airflow and supplying sediment downstream; (ii) buildings can negatively affect the dune growth by obstructing the sediment from moving downstream. Hesp and Smyth [209] used the RANS and RNG k–ε model to simulate various dune scarps (with forward-facing steps), in order to understand the sediment transport pathways from beach to dunes in absence of structures. The authors demonstrated that the scarp morphology and the approach-wind direction can influence the transport pathways.

Fig. 9

Sketch of the barrier profiles: a CN, b JP, c SVW, d IT, e US, f S4S. Corresponding mean streamlines around barriers, structures and characteristic lengths of the local flow. Figures credit to Bruno et al. [205]

The snowdrift covers about 11.11% of total number of papers considered in this subsection. The snowdrift is the result of a very complex interaction between snow particle motion of three processes (i.e. creep, saltation and suspension) and wind blowing on/around the built environment. Investigating the spatiotemporal distribution of snow may help to prevent not only the disruption of services (with troubles to workers and inhabitants) but in the worst-case scenario also the collapse of the structures and infrastructures. Tominaga [210] conducted the first review in WE on CFD modeling of snowdrift around/on buildings later updated in 2018 [211]. As stressed by the authors, in snowdrift while the wind flow is modeled with the Eulerian method, two approaches can used for modeling the snow particle transport: the Lagrangian method or the Eulerian method. As mentioned above, the two methods have advantages and disadvantages. The Lagrangian method can predict the trajectory of individual particles but requires a large number of injected particles (computationally demanding) to obtain reliable statistics. The Eulerian method treats the snow particles as continuum transported passively by the airflow, through the mixture method (passive scalar transport equations) and the drift-flux method. Since 1990s various numerical models to simulate the three processes (i.e. creep, saltation and suspension) of the snowdrift on and around buildings have been proposed (e.g. [212,213,214,215]). Note that, these CFD studies were not carried out with OpenFOAM. In fact, a very limited number of research studies (only three) on snowdrift in built environment have been performed with OpenFOAM, while the majority found in the scientific literature was executed with ANSYS Fluent. One of the reasons may be that OpenFOAM is relatively “young” with respect to ANSYS Fluent. While Fluent in 1990s and 2000s was conventionally used for this kind of investigations, OpenFOAM was not born yet. To the best knowledge of the author, the first “published” research study on snowdrift executed with OpenFOAM dates to 2021 [216]. In this study, the authors performed RANS simulations (with the standard k–ε turbulence model) by adopting the Eulerian–Lagrangian method to quantify the small-scale snow deposition onto Arctic Sea ice. For this purpose, a new Eulerian–Lagrangian model so-called snowBedFoam 1.0 was implemented to simulate the snow transport. This model was developed based on the DPMFoam solver originally implemented in OpenFOAM 2.3.0. In the DPMFoam, the Eulerian continuum equations including particle volume fraction are solved for the fluid phase while Newton’s equations of motion are solved to calculate the trajectory of particles. As mentioned earlier, the coupling between wind and snowdrift can be a very complex phenomenon. In a short or even long period, the wind can cause the re-distribution of snow surface that will induce in turn a change on the approach wind field. To investigate this topic, Chen and Yu [217] proposed a dynamic mesh technology for the simulation of snowdrift to depict its surface evolution under long period. The driftUnsteadyScalarDyFoam was implemented in OpenFOAM and the results were validated by means of several measurement campaigns, including snowdrift on a flat roof and around a building. In order to improve the prediction of snowdrift in presence of obstacles, the same authors [218] developed a Lagrangian–Eulerian method, in particular the MPPICFoamEx solver (which embeds the pimpleFoam) was improved from the MPPICFoam solver. CFD simulations were aimed to assess the wind-induced snow transport on flat terrain and on a roadbed. A comparison with results from the Eulerian–Eulerian method (using the driftUnsteadyScalarDyFoam) and experimental tests was also provided in the paper. The authors concluded that the Eulerian–Lagrangian method provided a better agreement (than Eulerian-Eulerian approach) with the experimental data also in presence of obstacles (Fig. 10).

Fig. 10

Particle Image Velocimetry (PIV) photograph (by Lü et al. [219]) and simulation contours in the regions of windward, roadbed and leeward. The particle concentration in the red framed region of PIV photograph is estimated using Gaussian kernels. In these warm-cold contours, warm color indicates the enrichment of particles. Figures credit to Chen and Yu [218]

All CFD investigations related to windblown sand of this subsection were carried out with the steady RANS approach and not accounting for the particles deposition (e.g. [220]) since beyond the scope of the above-mentioned studies. On the contrary, for wind-driven rain as well as snowdrift studies unsteady simulations were also performed with Lagrangian–Eulerian and Eulerian–Eulerian methods. Nevertheless, as claimed by Horvat at el. [206] and remarked by Bruno, Benli and van Beeck in the mini-symposium Windblown Sand Sciences and Engineering of the 16th International Conference on Wind Engineering (ICWE16) [6], the windblown sand is an emerging issue of WE. There is still room for improvement, to use more sophisticated numerical approaches aimed at improving the prediction of sediment transport. The snowdrift topic has been largely investigated both for flat terrains and built environments (with buildings), with Eulerian–Eulerian and Eulerian–Lagrangian methods. However, this literature review revealed that just few “published” studies were carried out with OpenFOAM, while most of them were performed with ANSYS Fluent. For this purpose, new models/solvers were developed ad hoc and validated through experimental data by the users.

4 CFD for wind structural engineering

This section focuses on the use of OpenFOAM for wind structural engineering studies, which represent approximately the 29.79% of the total number of OpenFOAM studies of this review (Fig. 1a). In the past two decades, OpenFOAM has been widely used to investigate the aerodynamics and structural behavior of a large range of structures here grouped into five main sub-categories: bridges, low- and medium-rise buildings, high-rise buildings, lattice towers, photovoltaic (PV) solar panels. Note that, given the very large amount of research studies conducted with OpenFOAM on this topic, it was not possible to account for all of them. Thus, very comprehensive review papers are suggested here to support the reader. The section is organized into three subsections: wind effects on bridges (Sect. 4.1) with 9.04% of contributions, wind effects on low-rise and high-rise buildings (Sect. 4.2) with 17.02% of contributions, wind effects on PV panels (Sect. 4.3) with 3.72% of contributions (see Fig. 1b).

4.1 Wind effects on bridges

The cylinder (e.g. square and circular sections) is probably the simplest geometry, but also the most fascinating bluff body tested and simulated in the history of WE. This element has been used to understand the fundamental principles of the flow dynamics around bluff bodies, as the velocity and pressure field, the induced aerodynamic forces, the vortex-induced vibrations, and so on. It has been used and it is still used to mimic the behavior of more complex structures and/or its elements, as bridge decks, buildings, poles, etc. In 2008, the Benchmark on the Aerodynamics of a Rectangular 5:1 Cylinder (BARC) was announced during 6th International Colloquium on Bluff Body Aerodynamics and Applications (BBAA VI) hosted by Politecnico di Milano in Italy. Since then, scientists and scholars have been investigating the BARC for different purposes. More details about the research studies on BARC can be found in Bruno et al. [221] that carefully reviewed the extensive research activities and main results on this benchmark from 2010 to 2014. As mentioned above, the results achieved with the BARC may be representative of a wide range of bluff bodies, from bridge deck to sectional model of buildings, and this is probably the main reason this benchmark has been so widely used in the past years worldwide. Studies on cross-sectional bridge decks were carried out in OpenFOAM to investigate the static aerodynamic characteristics and flutter derivatives with URANS coupled to SST k–ω model (e.g. [222]) and LES approach (e.g. [223]). Andersen and Bossen [224] investigated a single bridge deck by URANS with SST k–ω model, with focus on the performance of three modal decomposition techniques for the identification of spatiotemporal structures (as vortex shedding effects) in the pressure field. Lateral barriers can also play an important role in the aerodynamics of bridge decks. Research studies on this subject are commonly conducted by wind-tunnel testing and CFD simulations to optimize the bridge and barrier performance. Investigating the performance of such elements can be extremely challenging by wind-tunnel tests, due to the scaling and the necessity to match similarity criteria. While, sensitivity studies can be performed on a large number of computational parameters (e.g. geometry, grid size/type, turbulence modeling, solvers, etc.) by CFD simulations in a reasonable time (e.g. [8, 27]). Li et al. [225] investigated by RANS (with SST k–ω model) the performance of a twin-winglet system used as an aerodynamic affiliated facility to increase the flutter stability of a box-girder suspension bridge. Xu et al. [226] used the 2D URANS approach to study the performance of porous elements positioned on bridge sections by following two strategies: (1) the pores are explicitly modeled; (2) barriers are implicitly modeled in terms of pressure-jump. The authors concluded that, although the strategy (2) has evident advantages compared to (1) since it allows saving computational resources and time, both strategies have strengths and limitations.

Numerical and experimental studies were also conducted with OpenFOAM on more complex sectional bridge models, as the twin-box bridge decks. Also in this case, parametric CFD studies on the gap distance between girders, on the transversal beams linking the deck girders, on the box geometry shape may be of great support at the early design stage of long-span bridges (e.g. [227,228,229]) (Fig. 11). Long- and medium-span bridges are also simulated in 3D, by reproducing the entire bridge. In particular, atmospheric wind conditions are downscaled from the mesoscale to the local scales (e.g. [230]) in order to understand its interaction with the surrounding environment (e.g. underlying terrain/waterway) as well as the aerodynamic performance of the bridge deck (e.g. [231, 232]). Less common but not less important are the research studies focusing on the effects caused by extreme winds on bridge decks. Hao and Wu [233] simulated the effect of a non-turbulent downburst wind field (modeled as an impinging jet) on a long-span bridge. CFD outputs were then used as dynamic input to the line-element-based 3D finite element model of the long-span bridge, and the downburst-induced transient response was acquired using the computational structural dynamics approach. Qin et al. [234] investigated the interactions between tornado-like vortices and a single-box deck with the LES approach, by focusing on the wind loads and main aerodynamic characteristics. With the LES approach, Chen et al. [235] analyzed the mechanism of the widespread failure of light poles on an elevated highway bridge exposed to Category 4 Hurricane Laura occurred in 2020.

Fig. 11

Computational grid and vorticity magnitude field snapshots at different positions in a cycle of the aerodynamic lift coefficient (C_l) time-history for the one of the gaps considered in the study (i.e. Gap B). Figure credit to Álvarez et al. [227]

Overall, it should be noted that the above-mentioned studies carried out under extreme wind conditions (as tornados, downbursts and hurricanes) do not represent an isolated case in the scientific literature, but on the contrary a new frontier. However, the numerical methods/models developed in the past decades (e.g. inflow methods for LES) to simulate the most common neutral ABL wind conditions are not always suitable to accurately reproduce highly transient winds as tornados and downbursts. Thus, further research studies are required on this subject to better understand the nature of these extreme winds, their impact on bridges, but also to improve the numerical technique. This aspect will be also discussed in Sects. 4.2 and 5.

4.2 Wind effects on low-rise and high rise structures

Buildings are the places where humans spend most of their time. Thus, the design of buildings has always been of primary importance for the WE community. The first benchmark examples of low-rise and high-rise buildings appeared in 1970s. The general scope of these benchmarks was to aid engineers in understanding the flow dynamics around buildings, wind-induced pressure and response of buildings under neutral ABL winds. For instance, the Commonwealth Advisory Aeronautical Research Council (CAARC) building [236] was probably the first benchmark of a single high-rise building and so far also the mostly investigated by the WE community, through experimental and numerical techniques. As stressed by Thordal et al. [24] who recently reviewed the numerical research activities on high-rise buildings, the CAARC has been widely used by scientists through the years to validate (with experimental data) models and settings for the wind loads assessment in structural design. In 1993, Mochida et al. [237] and Stathopoulos and Zhou [238] provided probably the very first numerical studies on subjects that would become shortly thereafter low-rise building benchmarks, for the analyses of wind flow field and wind-induced pressures by means of RANS and LES. The most remarkable aspect of this research activity is probably the use of LES approach “in 1993” for environmental/building simulations, by making the study of Mochida et al. [237] definitively a pioneering CWE research contribution. If the RANS approach in combination with k–ε and k–ω turbulence models has been for decades (from about 1970 to 2010) one of the most used CFD approach also in wind structural applications, the LES has become nowadays the most reliable and therefore widely adopted approach in this topic. This approach can provide users with more accurate turbulence characteristics (than RANS) and consequently a better solution in terms of pressure field, mean wind loads and peaks. However, running LES simulations on a cluster of buildings may be burdensome. In this regard, hybrid approaches have also been developed and used to simulate the wind flow field and loads on buildings. Back in 2011, the hybrid RANS—Kinetic Simulation approach was used by Huang et al. [239] to investigate the wind loads and pressure fluctuations on the CAARC. Similarly, Joubert et al. [240] and Wang and Chen [241, 242] adopted Spalart–Allmaras IDDES and the WMLES approaches, respectively, to investigate the complex time-varying three-dimensional flow field and wind loads on a high-rise building (referred as rectangular prism in [240]). Some studies related to low-rise and high-rise structures were also carried out with RANS and URANS. Nevertheless, these two approaches were either used (1) to simulate “only” the wind flow field around the bluff body for shape optimization process (e.g. [243,244,245]) without venturing a wind pressure/load assessment or (2) to develop machine learning/genetic algorithm frameworks for wind pressure/load assessment in combination with LES databases (e.g. [246,247,248]).

As mentioned earlier, the LES can provide a more accurate solution than RANS for wind load assessment, but the choice of the inflow method generator to reproduce neutral ABL wind conditions is crucial. A review on the numerous LES inflow method generators available in the literature as well as the validation studies and uncertainty quantification is beyond the scope of the present paper. The reader can find in the literature pivotal research studies carried out on open domains with different surface roughness classes, isolated low-rise buildings, high-rise buildings, slender structures and so on (e.g. [103,104,105, 249,250,251,252,253,254,255,256,257]). Note that, since these studies mainly focus on the inflow method generators OpenFOAM is not the only CFD tool adopted by the authors. 

LES studies executed with OpenFOAM on low-rise and high-rise buildings in the structural engineering field can generally pursue multiple goals. Xing et al. [258] analyzed the accuracy and reliability of several computational parameters (i.e. grid size in proximity of the building, numerical schemes, inflow generator method) in LES simulation when predicting wind flow and wind loads on/around a real high-rise building, namely Torre Gioia 22, in Milan, Italy (Fig. 12). Marsland et al. [259] used the LES approach to investigate and reduce the wind-induced vibration by integrating the building with façade opening in service floors. Hasama et al. [260] evaluated the aerodynamic instability of a building through fluid–structure interaction analysis, by combining LES simulations and multi-degree-of-freedom structure model. Liu et al. [261] investigated with LES the performance of horizontal ribs, to be integrated on the facades of a high-rise building, with the aim to mitigate potential dangerous effects of strong winds. Melaku et al. [262] used the LES to assess the wind loads on a cube-shaped equipment mounted on the roof of a low-rise building. The variations of peak drag and uplift force coefficients with different equipment elevations were investigated in detail.

Fig. 12

a Overview of the computational domain and boundary conditions; b and c images of the computational grid with a detailed view on the tower under study; instantaneous flow field at different attack angles d 0°, e 120° and f 240°. Figures credit to Xing et al. [258]

As for wind effects on bridges, in the past few years the increase of extreme meteorological events due to climate change led to a growing number of experimental and numerical studies focusing on the impact of windstorms (as downbursts, tornados, hurricanes) on low-rise structures mainly. This is because, while the ABL wind shows the highest wind speeds at the higher levels from the ground (more meaningful for tall structures), transient winds like downbursts and tornadoes manifest the highest wind speeds near the surface ground (e.g. [2]). Back in 2016, in one of the first CFD studies related to this topic and executed with OpenFOAM, Sim et al. [263] used the steady RANS coupled to the SST k–ω turbulence model to replicate a microburst-like wind as an impinging-jet flow. However few years later Žužul et al. [264], who carefully analyzed the reliability of URANS and Scale Adaptive Simulation (SAS) [265] to reproduce the complex dynamics of a reduced-scale downburst wind flows, recommended the use of more sophisticated approaches (like LES) to better resolve the complex turbulent structures of the flow (Fig. 13). Iida and Uematsu [266] used LES simulations to investigate the non-stationary mechanism causing strong winds close to the building walls and ground surface. With the same numerical approach, Cao et al. [267] simulated a tornado-like vortex to understand the wind-induced pressures and forces on a flat-roofed and gable-roofed low-rise building. The authors concluded that tornado-induced wind pressures have very different characteristics than those caused by synoptic winds like ABL flows.

Fig. 13

a Schematic view of the WindEEE Dome facility reproduced numerically. b Computational domain with an indication of the boundary conditions. c Vorticity contour representation of the downburst-like wind field of the SAS simulation throughout the downburst life cycle. Figures credit to Žužul et al. [264]

A different type of structure that may also be classified as low-rise or high-rise structure (based on the height) are the lattice structures. For lattice structures, very few CFD studies conducted with OpenFOAM have been found in the literature. Nevertheless, given the peculiarity of such structures it may be worth to briefly discuss here some of these research studies. In general, these structures as well as many others have been investigated (e.g. [268]) under different wind conditions, and analytical models have also been derived for the wind-induced response assessment (e.g. [269,270,271,272]). One of the first CFD studies on lattice structures conducted in OpenFOAM probably dates back to 2014. It was carried out by Fabre et al. [273] on a real meteorological mast for which also wind-tunnel tests were performed at 1:20 reduced scale. The RANS simulations helped the authors to calculate the optimum anemometer position by avoiding any possible flow distortion. With respect to more conventional towers, these are peculiar structures generally composed by a large number of sub-elements. Generating a high-resolution computational grid around these structures requires advanced knowledge in geometry/grid modeling and also substantial computational resources, by making these studies commonly computationally demanding. Therefore, modeling only a portion of it to analyze local and most impacting wind effects is sometimes a reasonable “trade-off” for practical engineering applications. This was the strategy of Zhang et al. [274] and Hadane et al. [275] who adopted RANS and Wall-Adapting LES (WALE) approaches, respectively, to analyze the aerodynamic characteristics and wind loads on steel element of a transmission tower. The LES approach was used conversely by Ma and Sun [276] to simulate a hurricane boundary layer turbulence. The obtained wind flow field was then used to analyze the structural response of a power transmission tower.

4.3 Wind effects on photovoltaic panels

The use of renewable energy (as wind, solar and ocean) is crucial to achieve carbon neutrality and satisfy the target of net zero greenhouse gas emissions by the middle of twenty-first century (e.g. [277]). In this perspective, the use of photovoltaic (PV) panels increased significantly in the past years. PV panels are generally ground-mounted in open areas, rooftop-mounted and wall mounted on buildings. Besides their unquestionable and positive impact on the global ecosystem, PV panel systems may suffer from atmospheric and environmental factors, as the dust/particle deposition, rain drop as well as wind effects (e.g. [278]). As for the windblown sand, the investigation of wind effects on PV panels can be considered as an emerging topic in the WE community. As reported by Zhou et al. [278], who reviewed the CFD studies on the interaction between photovoltaic system and ambient environment, “…most studies applied CFD for simulations regarding PV thermal characteristics, PV cooling, and dust deposition and mitigation, whereas less were for investigating airflow and ventilation, wind loading, and microclimate…”. The present review paper confirms the observation made by Zhou et al. [278], since a limited amount of OpenFOAM studies focusing on this topic have been found in the scientific literature and only few of these deal with wind loading. Jubayer and Hangan [279, 280] adopted the RANS and URANS in combination with SST k–ω turbulence model to investigate the wind pressure coefficients, aerodynamic forces and flow structures on a stand-alone and an array of ground-mounted PV system, respectively. The results for the array configuration showed that the first windward row of PV panels experiences the maximum drag and lift forces. In terms of the maximum overturning moment, the 45° and 135° wind directions are the most critical with similar overturning moment coefficients for each row (Fig. 14). Similarly, Sun et al. [281] investigated ground-mounted PV panels by analyzing different scenarios in terms of wind velocities, arrangement of panel arrays like row and column spacing, panel inclination angle. A more sophisticated CFD approach was used by Wang et al. [282], who performed LES simulations for oblique wind directions (i.e. 45° and 135°) on flat-roof-mounted solar arrays to investigate the main dynamic characteristics of conical vortices and their effects on wind pressure distributions. Despite the increase of computational resources, performing sensitivity studies with LES to investigate the impact of numerical/environmental parameters can be burdensome and unpractical for such peculiar structures. To overcome this limitation, Aly and Clarke [283] proposed an innovative method combining RANS and machine learning methods to determine wind loads on PV panels. The study proved that this combination can significantly speed up simulations (up to 10,000 times faster) without losing in accuracy. As mentioned at the begin of this subsection, this is an emerging topic of the WE, where further numerical and experimental analysis are required to gain more knowledge on the wind flow dynamics and wind loads on/around such structures, in order to optimize the aerodynamic shape as well as the material selection/construction process.

Fig. 14

(a) Computational grid for the wind direction 0°; (b) normalized mean velocity magnitude contours with streamlines at the horizontal plane through the center of the panel for α = 0°, α = 45°, α = 135° and α = 180°; (c) Comparison between CFD and Particle Image Velocimetry (PIV) in terms of normalized streamwise (U) and vertical (V) velocity profiles on the surface of the PV panels for the same wind directions. Figures modified from Jubayer and Hangan [280]

Overall, the use of more sophisticated numerical approaches, like LES, is highly required in wind load assessment, if compared to topics analyzed in the previous sections. Although computationally demanding, this approach is essential when dealing with non-synoptic winds (as tornados and downbursts) in order to accurately solve the turbulent structures of the flow. The open-source nature of OpenFOAM can facilitate CFD users with the (1) development of new (LES) inflow method generators required to properly solve the complex turbulent structures and (2) the coupling of CFD simulations with FEM analysis.

5 Summary and perspectives

This review paper provided an overview on CFD research studies carried out by the WE community with the open-source OpenFOAM tool. The WE community and more specifically the CWE includes a wide range of topics and applications, spanning from pollutant/gas dispersion to wind structural engineering. A database of 289 papers, books and official websites has been assembled. Papers have been selected from well-known website platforms (as Science Direct) and by using the most common keywords appeared in the international WE and CWE conferences in the past decades. As expected, most of the papers (about 40%) were published on the reference journal of the WE and CWE community, namely Journal of Wind Engineering and Industrial Aerodynamics. Three main research areas have been identified in this review: (1) CFD for complex terrain: from mesoscale to microscale, (2) CFD for the built environment, (3) CFD for wind structural engineering. Within these research areas, various topics have been selected and discussed in the corresponding subsections.

The Wind Energy is one of the topics where OpenFOAM is most widely used. However, the Wind Energy can nowadays be considered a stand-alone subfield of Wind Engineering, with its own community and related international conferences worldwide. The same applies also for topics closely related to Wind Energy, dealing with wind and wave effects on off-shore structures (as off-shore/on-shore wind turbines, wave-structure interaction, floating structures, and so on). For this reason, only research studies closely related to wind energy exploitation in the built environment were considered in the present review.

The pre-processing of geometry and grid generation is always crucial to achieve successful CFD results, irrespective of the topic. For sake of brevity, although important in the present paper the author did not focus on geometry and grid generation procedures nor on the mostly used tools. Nevertheless, it may be interesting for the reader to know that the majority of the OpenFOAM studies discussed here does not always adopted grids generated with open-source tools/utilities of OpenFOAM (as SnappyHexMesh) or recently integrated in it (as CfMesh). On the contrary, in most of the cases either other open-source tools or commercial tools have been used to construct both geometry and grid. To some extent the lack of a powerful tool fully integrated into the OpenFOAM platform to generate and manipulate geometries and grids may represent a small limitation especially when dealing with wind flows in complex environments.

Similarly, in the past two decades there was a continuous development of the OpenFOAM code from different bodies, as OpenFOAM Foundation [284], OpenFOAM ESI [285], FOAM extend [286]. Analyzing the differences between these versions is out of the scope of the present review. Albeit these versions rely on the same basic algorithms, some differences can be found in terms of models/features/solvers availability by making some variants more versatile and suitable (than others) for specific WE applications. The choice of the version is therefore subjective and entrusted to the CFD user.

Since 2011, different CFD approaches have been used by wind engineers, from RANS to LES. Based on the topic, the CFD models have been often coupled to meteorological forecast models (as WRF), building energy simulation (BES) models, and finite element method (FEM) models. The possibility to couple OpenFOAM with other open-source platforms and establish operational framework procedures makes this tool undoubtably one of the most flexible and suitable CFD tools for research and practical engineering applications.

RANS has been the mostly used numerical approach in the early stage of OpenFOAM, but the rapid increase of computational resources of the last years made the LES one of the mostly used approach in WE nowadays. Nevertheless, RANS remains still the preferred approach for mesoscale simulations (on large-scale domains), pedestrian-level wind comfort assessment (when focusing on areas with high amplification factors, which are often the areas of primary interest in those studies), wind-driven rain, windblown sand and snowdrift (with Eulerian-Eulerian or Eulerian-Langrangian method). The large amount of sensitivity research studies (i.e. on inflow conditions, space and time discretization, turbulence models, algorithm solvers, etc.) carried out through the years with RANS have been crucial to improve the reliability of this approach and to favor in turn the development of best practice guidelines for CFD simulations in WE. On the contrary, there are WE topics for which RANS provides inaccurate solutions (due to well-known limitations). This aspect is particularly sensitive in research studies dealing with wind load assessment on structures (as bridges and buildings), for which the knowledge of the complex turbulent structures of the flow and peak values (velocity and pressure) is crucial both for neutral ABL winds and extreme winds (as downbursts and tornados). Hybrid RANS-LES approaches (e.g. DES, DDES, IDDES, WLES, SAS, etc.) may also represent an alternative option in case of large-scale domains (i.e. large number of control volumes) if the turbulent structures of the flow are sufficiently resolved.

Various inflow generator methods have been developed through the years for LES in OpenFOAM (and other CFD tools) to simulate neutral ABL wind flows with/without buildings. These are essential to properly develop the wind profiles and turbulence characteristics within the domain. However, although these are generally well-established for neutral ABL winds, their reliability to properly reproduce extreme winds (as downbursts and tornados) is still an open question for which more research is needed. To the best knowledge of the author this has a twofold explanation. (1) Tornados and downbursts are more complex to model (because of their transient nature) and validate by experimental data (barely available in the literature). (2) The occurrence of extreme events massively increased in the last years due to the climate change and the WE community is quickly adapting to this change, by focusing more on extreme winds rather than well-known neutral ABL winds. However, while WE standards and codes are fully based on a rational approach (i.e. so-called “Davenport chain”) that ties together synoptic winds (as ABL wind) and wind effects on structures, a similar rational scheme that joins the non-synoptic winds (as thunderstorms) and wind loading into a homogeneous framework is still missing. As stated by Solari et al. [287] “… this happens because the complexity of thunderstorms makes it difficult to establish physically realistic and simple models. Their short duration and small size make few data available. There is a persistent gap between wind engineering and atmospheric sciences …”. In the past few years, the scientific community made a big step forward in the measuring, simulating and modeling of extreme winds for WE applications. A unique initiative to enable a better understanding of fundamental downburst flow features relevant for the structural loading was framed under the umbrella of the European Research Council (ERC) Advanced project THUNDERR [288]. The scope of this project was absolutely novel: “… to detect thunderstorms, create a database of meteorological records and scenarios, conduct unprecedented laboratory tests and numerical simulations, formulate a thunderstorm model appropriate for both atmospheric sciences and structural design, change the format of wind actions, engineering practice and the codification system, make building safer and more sustainable, bring about a profound impact on society and its economy. …”. The research outputs of this project made clear that the open-source nature of weather models (as WRF), CFD codes (as OpenFOAM) and measurements is essential to understand the genesis of such winds. From the computational perspective, a large number of LES simulations under different scenarios are usually required to properly calibrate the model and understand the physics. Therefore, parallelizing the simulations on multiple nodes through HPC systems without paying any license cost may be very beneficial for the CFD user. Another important aspect concerns the coupling of weather forecasting models (necessary for mesoscale simulations) with OpenFOAM CFD simulation of local scales (e.g. buildings). This process may be easier and less costly because of the open-source nature of the utilized codes. Thus, if on the one hand OpenFOAM requires a relatively long training period and specific programming skills (than other commercial CFD tools), the long-term benefit for the CFD user and stakeholders is priceless.

Advanced technologies as artificial intelligence (AI) based schemes (e.g. machine learning) can aid the WE community with the better understanding of physical phenomena [26]. While such advanced technologies are widely adopted by the Fluid Dynamics/Mechanics as well as the Atmospheric Science communities, a limited number of WE studies (about 5.8% of those analyzed here) combining OpenFOAM and AI-based schemes have been found in the scientific literature. Nevertheless, this rate does not look that pessimistic, since about 90.9% of these studies have been recently published (from 2019 to 2023) by indicating an increasing confidence of CWE users in coupling AI-based schemes and OpenFOAM. This is also confirmed by Lamberti and Gorlé [236] on the use of a multi-fidelity machine learning framework to predict wind loads on buildings “… these results demonstrate that multi-fidelity machine learning frameworks provide a route to balancing accuracy and computational cost in the prediction of complex turbulent flow quantities”. In general, if on the one hand the promising results confirm that the CWE community is ready to embrace the AI revolution, on the other hand a “conscious use” of these new technologies in combination with experimental and numerical methods is imperative.

In conclusion, OpenFOAM plays and will play in the coming years a major role in the CWE community. In a totally unique way, it allows CFD users to access and manipulate source codes as well as implement new models/solvers with the support of the theory guide and the OpenFOAM community. OpenFOAM represents an extraordinary opportunity for all CFD users worldwide to share codes and exchange case studies (also through the OpenFOAM journal [289]), to create benchmarks for the development of new best practice guidelines, to explore the potential of new functionalities, to strengthen the network within the CFD community.