Assessing the Effect of Air Ventilation on the Dispersion of Exhaled Aerosol Particles in a Lecture Hall: Simulation Strategy and Streamlined Workflow

Abstract

An efficient solution strategy based on fluid network modeling, computational fluid dynamics (CFD) and discrete particle modeling (DPM) is presented in order to predict and improve air quality, specifically regarding breathing aerosol concentration, in a person-occupied mechanically ventilated room. The efficiency of the proposed workflow is evaluated for the specific case of a lecture hall. It is found that the actual vent system is imbalanced and inefficient in managing the aerosol concentration within the room. Despite a high volumetric exchange rate, aerosol residence times and local aerosol concentrations remain high over an extended period of time, without additional efforts to alter air flow circulation throughout the room. The proposed strategy illustrates how such changes can be efficiently implemented in the basic 1D/3D co-simulation workflow. Analysis of the lecture hall and vent system shows that the execution time for the overall process workflow can be optimized by the following: (1) CAD geometry generation of the room via 3D laser scanning, (2) mesh generation based on the anticipated air discharge behavior from the vent system and (3) by employing HPC resources. Additional simplifications such as the decoupling of vent air flow and room aerodynamics, as observed for the investigated test case, one-way coupling between air flow and aerosol dispersion at low aerosol concentrations and the successive solution of flow field equations can further reduce the problem’s complexity and processing times.

1. Introduction

Many studies on the transmission of pathogens, i.e., infectious microorganisms such as viruses, bacteria or fungi, in closed quarters such as hospitals or office spaces suggest that room ventilation is one of the major methods for reducing and thereby controlling their spread via the airborne route [1,2,3]. Although increasing the ventilation air flow rate does dilute concentrations better when the contaminant source is constant, it does, however, not necessarily increase ventilation’s effectiveness [1].

The outbreak of highly contagious airborne diseases, such as the past COVID-19 pandemic, requires quick actions in implementing various social distancing and other safety measures. This also includes regulations and recommendations for occupancy limits and ventilation requirements for closed public spaces, including public transport, work spaces, doctors’ offices, classrooms and lecture halls [4,5,6]. In the past, room ventilation regulations were limited to specifications for volume exchange rate (based on room volume) and occupancy (based on square-footage per person and independent of room height). Specifics of the room geometry, vent-in and vent-out configuration and the resulting room air flow field characteristics were only considered more recently, since they greatly influence pathogen or aerosol dispersion and local aerosol/pathogen concentrations within a room.

Clearly, the question of if a person’s physical presence in a specific space is safe, with respect to infection with an airborne pathogen emitted from a source (e.g., human host(s)) also present within that room, will not only depend on regulatory parameters, such as the number of occupants, their personal protective measures (such as breathing masks) and room air exchange rates facilitated by the ventilation system, but also on the room’s geometry, the position of the individual(s) in that room and the specifics of the employed venting system, including vent-in and vent-out components.

To answer the prescribed “safety question” for a specific space in a timely fashion under a crisis situation, on-site experimental measurements are impractical, too time-consuming or are simply not possible. On the other hand, virtual simulations of the room aerodynamics and aerosol or pathogen dispersion using computational fluid dynamics (CFD) can be effectively deployed to (a) determine actual aerosol/pathogen concentrations and distribution for a given setting and (b) optimize or modify the vent air inlet/discharge system and the positions of the room’s available seating areas, as well as the positions of additional obstacles or mobile fan or filtrations systems, to control and reduce aerosol concentrations throughout the room [7,8]. In context of item (b), it is important to note that changes to the vent-in/vent-out system will generally also impact the air distribution in the overall vent system itself, thereby modifying the air flow rate through the vent-in/vent-out locations and thereby the room aerodynamics.

A comprehensive review of studies conducted using CFD methods to understand the airborne dispersion and transmission of the COVID-19 virus has been presented by Mohamadi and Fazeli [9]. Some of the recent works that are concerned with aerosol dispersion and air quality in a lecture hall or classroom were presented by Arpino et al. [10], Mahmoud et al. [11] and Zivelonghi and Lai [12]. The aerosol dispersion and effect of facemasks on indoor transmission have also been analyzed numerically by Aderbigbe et al. [13] and Aliyu et al. [14]. These studies analyzed room aerodynamics based on inflow and outflow boundary conditions imposed at the room’s immediate periphery. However, as noted earlier, for actively ventilated rooms, two-way coupling between a room’s aerodynamics and the flow within the vent system, the latter of which can efficiently be described by a 1D flow network model, might occur and has to be accounted for in the overall analysis. This is also relevant and practical in cases where vent inlets and/or vent outlets are not readily accessible for measurements such that boundary-condition values are not directly available for the CFD analysis of the room. In addition, incorporating a flow network model allows one to readily investigate different vent system operating conditions without having to perform measurements at a potentially large number of vent inlets and/or outlets.

While the coupling of 1D flow network models with comprehensive CFD analysis models (1D-3D co-simulation) can be found in the analysis of building energy systems (see for example Wei at al. [15]), as well as in other disciplines such as the modeling of respiratory flows [16] and gas turbine components [17], the authors are not aware of any published study wherein a network model for the ventilation system has been coupled with 3D-CFD simulations as part of the overall workflow to assess the effect of air ventilation on aerosol particle dispersion in a lecture hall.

In the present study, a streamlined process workflow for the coupled analysis of the aerodynamics inside an actively ventilated room and the flow inside the corresponding vent system is presented. The topics addressed include the problem set-up, modeling approach, solution strategy and data post-processing, allowing for an expedited assessment of risk for airborne droplet infection that depends, among other things (see below), on the predicted spatial distribution and concentration of breathing aerosols. See also Mahmoud et al. [18] and Tang et al. [19] in this context. It is noted here that no direct risk assessment was conducted as part of this study, as the primary focus was on analyzing the distribution of exhaled aerosols under forced air ventilation conditions and a suitable efficient workflow to do so. Aside from the distribution of breathing aerosols in the room, assessing a person’s infection risk for pathogens such as viruses within the liquid phase requires additional considerations, including viral activity (which is affected by room temperature and humidity), the specific viral strain(s), exposure duration, virus decay rate(s) and interactions with deposition surfaces and individual immune system responses, excluding indirect transmission from touching contaminated surfaces.

The proposed workflow consists of eight major steps: (1) data collection, (2) vent system analysis, (3) CAD geometry generation of the room, (4) flow-field mesh generation and quality check, (5) CFD solver selection and settings, (6) selection of boundary and initial conditions, (7) stepwise solution process for room aerodynamics and aerosol dispersion and (8) data post-processing. Included in the workflow, also, are process steps relevant for the subsequent mitigation of excessively high local aerosol concentrations leading to higher exposure risks, even though those steps are not being pursued within the present case study. The specific case under consideration here is an actual student lecture hall at the University of Stuttgart, occupied by the maximum allowable number of individuals (based on 2021 COVID state regulations) and subject to air circulation imposed by an existing (unmodified) forced air ventilation system (without heating or cooling). The proposed workflow illustrates the tasks necessary to quickly ascertain both the flow through the vent system and the coupled aerodynamic flow field in the room, the latter of which also provides the distribution of breathing aerosols exhaled by the room’s occupants, thereby allowing one to evaluate the effectiveness of the vent system and the usability of the room if occupied by individuals (at least in part) with a contagious airborne disease.

2. Room and Venting System—Data Collection

The lecture hall depicted in Figure 1 situated at the University of Stuttgart has been considered as a test case to illustrate the streamlined solution strategy presented in Section 3 for determining the airborne aerosol concentration in a room with an installed forced ventilation system.

The hall has a floor area of 417 m², with a normal seating capacity of 396 people. Since our initial university-internal study was conducted during the COVID-19 pandemic, the hall was assumed to be occupied by 32 people, corresponding to the maximum seating capacity based on COVID-19 regulations at the time (May 2021) in the State of Baden-Württemberg (BW), Germany [4]. The present work builds on that initial study and focuses on the workflow for jointly analyzing vent system air flow together with room aerodynamics and the breathing aerosol concentration therein. Hence, the original seating of occupants and room configuration has been retained here. Naturally, the proposed workflow can serve not only for improving an existing indoor air-managing system but also for the design of a room’s interior geometry and vent system from the outset at the planning stage. In either case, this might include the positioning of additional fans/blowers (as analyzed by Rasam et al. [20] and Yang et al. [21]) or using partitioning walls/room dividers (see, for example, Tao et al. [22]). In addition, social distancing in confined spaces remains a valuable and relevant measure in a layered infection prevention strategy, especially where architectural, usage and/or cost constraints prevent the implementation of other measures.

In our test case, occupants were assumed to be seated in uniformly distributed way across the hall, irrespective of the ventilation arrangement. The torso and head of each occupant have been included in a simplified fashion as part of the boundary conditions for determining the room’s aerodynamics. The mouths of the occupants as a source of the aerosol particles were modeled as circular orifices (see Section 5.4 in this context).

The ventilation system of the hall consists of two identical piping branches near the ceiling for air inflow, each comprised of ten swirl nozzles (or swirl diffusers), six jet (or long-throw) nozzles and four air inlet grills. Two outlet vent grills, each connected to an air outflow channel, are situated on either side in the front of the lecture hall. The outflow channels vent the air out of the building and into the atmosphere or alternatively circulate the room air back into the venting. The latter set-up is used during winter-time operation. In the present investigation, the former set-up is in place.

The three types of inflow vents installed in the ventilation system were manufactured by SCHAKO Ferdinand Schad KG, Kolbingen, Germany [23,24,25]. Each type of nozzle or vent produces an air stream with a distinctive flow characteristic and pressure loss. The air streams entering the lecture hall through the various nozzles and vents, and the location and geometry of the outflow vents, dominate the overall air flow pattern in the hall (forced ventilation). The specific characteristics of the flow entering the flow domain through the prescribed nozzles and vents have been captured by the inflow boundary conditions imposed in the room’s simulation model at the respective component outflow cross-sections.

The geometric dimensions of the lecture hall and of the ventilation system were taken directly from the architectural drawings and the Heating, Ventilation and Air Conditioning (HVAC) layout available at the university’s building management and maintenance office. Selected geometric dimensions of the room and the vent nozzles were verified by on-site measurements, using a ruler, calipers and a laser distance-measuring tool (and an electronic inclinometer). Some other equipment in the hall not featured on the available drawings (such as the furniture and some ventilation peripherals) were also measured on site. In a second step, the lecture hall’s geometry was also captured by a laser scanning system (Leica RTC360 manufactured by Leica Geosystems AG, Heerbrugg, Switzerland), providing a 3D point cloud of surface points for further processing. Time requirements for generating the overall room geometry and computational mesh using the two prescribed methods were compared.

The specifics of the venting system geometry not exposed within the room could not be verified directly. The flow or operating conditions of the venting system were provided by the system operators on site in the form of real-time flow rate measurements taken continuously at a specified location within the venting system.

3. Process Workflow

3.1. Overall Flow Field Solution—Room/Vent Coupling (Inner Loop)

The overall flow problem to be solved consists of the air flow within the ducting/venting system and the air circulation within the room. Both flow domains are coupled with each other at the inflow and outflow planes of the vent-in and vent-out components. The characteristic lengths of these components and their geometric features are substantially smaller than the characteristic length of the entire hall. A simultaneous, spatially fully resolved solution of the entire flow domain, comprising the room and venting system, would require a substantial amount of computational resources and computing time. On the other hand, if there is limited (or no) two-way interaction between the air flow within the venting system and the air flow inside the lecture hall, then an iterative but decoupled solution of the two flow domains is possible. Here, coupling only occurs at the flow interfaces, i.e., the vent-in and vent-out planes. Accordingly, the solution process for determining the overall flow field in the present study has been separated into three sequential steps using two different modeling approaches, i.e., 1D-3D co-simulation. The three steps are as follows:

• Step 1: calculation of the flow distribution in the venting system based on a reduced-order flow network model;
• Step 2: analysis of the air flow inside the room/lecture hall by means of computational fluid dynamics (CFD) analysis;
• Step 3: extracting the boundary information from Step 2 and repeating Step 1 with the updated information if the old and new boundary information differ by a pre-defined margin.

In the present test case, it was found that the iterative step (Step 3) was not necessary, since a meaningful two-way coupling between room aerodynamics and venting system air flow does not exist. Specifically, in the investigated case, the outflow air vents and air inflow vents are spatially separated from each other (and amongst themselves) far enough, such that their local flow fields do not interact directly, thereby influencing the overall flow distribution in the venting system. Also, areas in front of the vent locations were not geometrically constrained or blocked by room installations, which might result in flow field fluctuations at these boundaries. Note that as part of Step 3 above, only information on the boundaries common to both the network model and the CFD model is passed between the two solvers. This information exchange can be handled by using a script or a code coupler such as preCICE v2 [26]. Clearly, the network solver and CFD solver solve for the flow in their respective domains independently of each other in Step 1 and 2.

The prescribed use of a network model for the vent system does not only provide for the better convergence behavior of the overall solution in comparison to a fully resolved simulation of both room interior and vent system together; it also reduces the total computational cost and resource requirements, while retaining a detailed flow-field resolution where necessary. Clearly, using the network model eliminates the need for volumetric 3D meshing of the complex vent system geometry, swirl nozzles and air vents. By bypassing the complex flow topology in the vent system and its components and the associated meshing challenges, the overall simulation model achieves better convergence, while at the same time, the omission of spatially resolving the vent components has only a minor impact on the overall room aerodynamics.

In the absence of a temperature difference between room air and vent air and without the warm air exhaled by the room’s occupants, the prescribed (iterative) procedure provides a complete picture of the flow-field aerodynamics within the room as a consequence of the air forced through the room by the venting system. However, since the aim of the investigation is the determination of the breathing aerosol distribution in the room, at least two additional steps, i.e., Steps 4 and 5, have to be taken to determine the latter:

• Step 4: Solution of the energy equation, alongside mass and momentum conservation equations and based on an initialization using the already calculated isothermal flow field from Step 2. This is necessary in order to account for buoyancy effects due to the higher temperature of the exhaled air and thermal plumes as a consequence of heat transfer from the occupants’ bodies;
• Step 5: Tracking of aerosol trajectories, allowing for the determination of the aerosol concentration over time within the room (and on surfaces). Here, it is assumed that the aerosol volume concentration in the room is small, such that the room aerodynamics is not influenced by the presence of the aerosol phase; i.e., a one-way coupling between aerosol phase and gas phase is assumed.

3.1.1. Flow Field in the Venting System

The flow-field solution inside the ventilation system is determined subject to the given operating conditions and ambient/outflow conditions at the vent discharge locations, i.e., at the vents that discharge the vent system air into the lecture hall. A venting or HVAC system consists, in general, of an air handler, heating and cooling components, a thermostat, various valves and the piping system moving the air through the vent “inlets” into the room and managing the air leaving the room through the vent “outlets”. Since in the present case, the vent-out air, i.e., the air leaving the room, is not recirculated (not even in parts) but directly exhausted into the atmosphere, only the portion of the ventilation system delivering the air through the ducting system into the lecture hall needs to be considered. Also, in the investigated configuration, the air admitted to the room is assumed to have a constant temperature. Temperature variations of the air in the lecture hall are assumed to be solely a result of the warm air exhaled by the room’s occupants. The HVAC system is controlled to provide a pre-set total volume flow rate through a pair of identical (open-loop) ventilation branches, subsequently referred to as legs, and the associated periphery. Each leg consists of air ducts, branching components and various reducing and diversion components, along with the discharge nozzles.

The fluid flow through one of the two identical legs is analyzed using a 1D network model and by imposing one-half of the total air volume flow rate at its upstream boundary and atmospheric pressure conditions as the outflow condition at each of the discharge nozzles. Analysis results for the volume or mass flow rates at the various discharge nozzles obtained from the 1D model analysis are then mapped on the corresponding nozzles of the second leg and subsequently used to specify the inflow boundary conditions for the CFD analysis of the lecture hall, i.e., the second step in the prescribed solution process.

When interpreting the results for the room aerodynamics and the spatial aerosol concentration within the room, it should be recalled that the simplified 1D model analysis of the venting system will result in certain inaccuracies with respect to the distribution of the vent air across the various inlets, compared to a detailed CFD analysis of the venting system, thereby affecting also the analysis results for the room flow field and aerosol concentration to a certain extend.

3.1.2. Flow Field Within the Lecture Hall

A steady-state flow-field solution within the lecture hall is computed prior to accounting for the distribution of the airborne aerosol concentration in the room. A commercial computational fluid dynamics (CFD) solver is employed to solve the Navier–Stokes and mass conservation equations for isothermal turbulent flow (as part of Step 2) and the energy equation for non-isothermal flow (as part of Step 4) after spatially discretizing the flow domain. After having determined the steady-state flow-field solution, including turbulence effects and buoyancy effects due to the higher temperature of the air exhaled by the occupants, aerosol particles are injected into the air flow exhaled by the occupants of the room. Lagrangian tracking of the particles in the room is performed using a DPM algorithm and a Random Walk model for turbulent dispersion, from which the aerosol distribution and its concentration can be determined. Droplet vaporization was not considered in the present study, even though it can impact droplet trajectories. It is noted that the vaporization effect could be considered with or without accounting for the generated water vapor by means of an additional transport equation and considering an air–vapor mixture phase in lieu of air.

The flow in both the venting system and in the lecture hall was considered to be incompressible, since the Mach number $Ma$ everywhere in the flow field was substantially lower than 0.3. The maximum fluid velocity was found at the outlet of one of the jet or long-throw nozzles, with a value of 8.58 $\mathrm{m}/\mathrm{s}$. To model buoyancy effects, the well-known Boussinesq model has been used.

3.2. System Modifications—Optimization (Outer Loop)

The solution process described in the previous section provides information on the breathing aerosol distribution in the lecture hall based on a selected seating configuration, assumed occupants’ breathing behavior (e.g., taken from the literature) and for a given vent system operating condition. Based on the analysis results, modifications to the overall set-up might have to be considered in order to reduce the aerosol concentration in the room below acceptable levels and permit continued usage of the room based on given health regulations, for example. There are various modifications that can be considered to achieve this goal, each of which will require changes at different points within the prescribed workflow and different levels of additional modeling efforts to assess their efficacy, following the renewed execution of Steps 1–5 described in the previous section.

Vent System Changes

One possibility to better manage the aerosol concentration within the room is to modify the room’s aerodynamics via changes to the vent system. This concerns changes in the volumetric or mass flow rate of the vent system blower (for example, by increasing the blower speed) or changes to vent system component geometries, e.g., the swirl angle of swirl nozzles, direction of jet nozzles or opening area of air grids.

Modifications of this type will require changes to the network model and, in the latter case, also changes to the inflow boundary conditions within the CFD analysis model for room aerodynamics.

Changes to Room Interior and/or Occupants

This relates to changes in the room conditions in general, in order to change the room’s aerodynamics and thereby also the aerosol concentration throughout the room. These modifications include the addition of room dividers or drop ceiling features, the removal or rearrangement of furniture, the addition of secondary air movers (fans, blowers) with or without filtration features and a change in room occupancy or the position of occupants. Naturally, the prescribed changes are constrained by the need to have a minimal or no impact on the usability of the room for the desired purpose.

Hence, any proposed changes to the room’s architecture (which passively or actively impact the room’s aerodynamics), and their impact on the accessibility of seating areas, visibility and comfort level for occupants or functionality of the room in general, should be evaluated before conducting computationally intensive meshing procedures and CFD simulations. To do so, immersive reality such as a VR headset or a VR Powerwall/CAVE can be useful.

3.3. Workflow Summary

The overall workflow for determining (a) the flow behavior within the room (via CFD modeling) and the venting system (via a 1D network model), (b) the dynamics of aerosol distribution within the room and (c) the process for implementing modifications to the system in order to achieve the desired requirements with respect to aerosol loading within the room is illustrated in Figure 2.

There are four major activity or task blocks, which will be described subsequently in more detail: (1) a data collection block, (2) a network modeling block for the venting system, (3) a CFD modeling block for the room aerodynamics and aerosol distribution and (4) a post-processing block focusing on a detailed analysis of the room’s aerodynamics and the resulting aerosol distribution, based on which changes to the room/vent system are selected if operational requirements are not met. The diagram also illustrates the two feedback loops described previously.

Block 1: Data Collection

As part of the “data collection” activity, Block 1, the geometric and operational data for the room and vent system are collected. The operational data also entail the location and distribution of individuals within the room based on user needs or regulations. While geometric data for a room are in general available from construction or architectural drawings, geometric data for room installations might have to be collected directly on site. One method to collect all the required data might be by 3D laser scanning of the room. For the present investigation, both methods have been employed. Figure 3 shows a picture of the point cloud data collected from laser scanning at one position using a Leica 3D Laser Scanner (model: RTC360).

Block 2: 1D Network Model/Vent System Flow Distribution

The network modeling block (Block 2) determines the quasi one-dimensional flow throughout the vent system and includes a set-up task, defining the vent system network geometry, including vent diameters and lengths, the geometry of bends, contractions and vent outlets (together with relevant wall roughness parameters and loss coefficients) and system operating conditions, including fluid properties and (pressure) boundary conditions at the vent system outlets, corresponding to the vent-in locations of the lecture hall. Assuming the air vented out of the room is not recirculated in the venting system, the room’s vent-in locations provide the only coupling between the network model and the subsequently described CFD-modeling block. After the network model has been set up, it is solved numerically, even though for the cases considered in the present study, an analytical solution would also have been possible. Aside from mean flow velocities within the vent system network, the solution provides mass flow or volume flow rates, leaving the various vent nozzles “feeding” the room with fresh air.

Block 3: CFD Modeling/Room Aerodynamics and Aerosol Distribution

The CFD-modeling block (Block 3) begins with a CAD task in which the room geometry is modeled, including furniture and (to a certain degree of abstraction) the bodies of the occupants seated in the room. The latter should be modeled in a parametric fashion, so that their position can be placed arbitrarily in the room. This also applies to any number of room dividers or secondary air movers potentially placed in the room at a later time (as part of the system optimization pursued in the “outer loop” described earlier). It might be beneficial to make provision for the addition of room dividers as part of the initial room geometry generation process but to consider them to be open to flow initially. The feasibility of the latter will depend on the employed CFD solver and the ability to prescribe “internal face boundaries”. The subsequent CFD set-up tasks follow the best practice guidelines available for incompressible single-phase fluid flows; see, for example, [27]. They consist of suitable geometry simplifications, the generation of a fluid inverse, the generation of an adequate computational mesh and the setting of proper boundary conditions at inlet vents, exit flow vents and solid surfaces. In addition, monitoring points within the room can be set here for monitoring the convergence of the overall room/vent simulation and for post-processing purposes. Once a converged solution has been obtained, best practices requires a mesh convergence study to be conducted as part of the CFD analysis. This can be performed for a fixed set of boundary conditions (provided their changes remain within certain limits as part of the optimization loop) and without coupling with the network model.

As described earlier, the CFD analysis of the room and the prediction of aerosol dispersion can be carried out sequentially, due to the low volume concentration of aerosol. As part of the weakly coupled isothermal room/vent simulation, the steady RANS (Reynolds–Averaged Navier–Stokes) equations for incompressible flow (together with a suitable turbulence model) and the conservation of mass equation are solved within the room. Upon convergence of the overall room/vent air flow, the energy equation is solved, in addition to the other equations and in order to capture the buoyant behavior of the warm air exhaled by the occupants. Upon the renewed convergence of the flow field, now modified by buoyancy effects, aerosol inflow conditions are activated, and the trajectories of aerosol particles/droplets are calculated within the flow field, assuming a one-way coupling (i.e., the effect of the aerosol particles on the flow field is neglected). Tracing the trajectories of the droplet aerosols can be augmented by a model for droplet vaporization and a model for the survivability of pathogens contained in the aerosol droplets once being released by a host/occupant and potentially being deposited onto a surface within the lecture hall.

Block 4: Post-Processing Simulation Data

Aerosol admission to the flow is carried out for a set physical time or until steady-state conditions with respect to the concentration field of suspended aerosols in the room is reached. In the former case, the set physical time might be determined by the usage cycle of the room or set events, upon which changes in the boundary conditions change the flow field within the room, such as the opening of doors or windows. Typical quantities to be analyzed during post-processing are those relevant for determining if usage requirements are met, as well as those needed for validating the computations and those providing guidance for needed flow-field modifications in case the requirements are not met. These include the following: iso-surfaces of aerosol concentration throughout the room, ideally breaking down which local concentration can be attributed to which occupant; aerosol trajectories; aerosol surface deposition rates (potentially with viral activity over time); streamline and vorticity field plots; contour plots of velocity components; and turbulent quantities, as well as various quantities at predefined monitoring points for the purpose of experimental validation of the simulation results. Commonly, post-processing is conducted at a standard desktop; alternatively, post-processing can also be completed in a virtual environment using a VR headset or VR Powerwall or CAVE. Immersive post-processing is especially useful, if in the course of the optimization (outer) loop, room dividers or other obstacles are placed in the room, potentially interfering with its usage, such as visibility to the front of the lecture hall, impacting the well-being of students (e.g., due to air drafts) or the execution of emergency protocols, e.g., the ability to exit the room within a certain amount from any room position. Novel augmented functionality in a VR environment, for example through “wind devices” for skin sensory input of local air velocity, can in the future provide valuable additional information during post-processing [28,29].

Specific details regarding the physical and numerical models employed for the major simulation blocks (CFD and network modeling) as part of the present case study are presented in the following section.

4. Simulation Methods and Models for Test Case

4.1. 1D Network Model—Ventilation System

The ventilation system was analyzed using the commercial software FluidFlow v3.47. The software features a built-in database for fluid properties and loss coefficients for a number of piping system components.

The conservation of mass equation and the extended Bernoulli equation are the underlying governing equations of the model. In the framework of a steady-state fluid network model, this implies that (a) at any junction or node in the network, the incoming and outgoing mass flow has to sum up to zero and (b) the pressure loss between any junction or node is independent of the path taken between the nodes. FluidFlow software calculates the total pressure losses, with the assumption that no energy is dissipated; hence, the total energy needs to be tracked [30]. Mass conservation equations for the various nodes and pressure loss conditions between the nodes based on the prevailing mass flow rates are solved simultaneously and iterated upon. The convergence criteria for pressure and mass flow rate are set at a 0.01% and 0.001% change between two consecutive iterations, respectively.

In the model, air duct pressure loss ${∆p}_D$ $\left[\mathrm{P}\mathrm{a}\right]$ is calculated using the Darcy–Weisbach equation, i.e.,

$${∆p}_D=f_D{\displaystyle \frac{L}{D}}{\displaystyle \frac{\rho V^2}{2}}$$

(1)

where $f_D [-]$ denotes the friction coefficient from the Moody diagram [31], $V$ $[\mathrm{m}/\mathrm{s}]$ is the mean fluid velocity in the duct, $L$ $\left[\mathrm{m}\right]$ the length of the duct section, $D$ $\left[\mathrm{m}\right]$ the hydraulic diameter of the duct section and $g$ $[\mathrm{m}/{\mathrm{s}}^2]$ the acceleration due to gravity.

Constant pressure loss factors $K_N$ $[-]$ for swirl diffusers, jet nozzles and ventilation grills (air grids) were extracted from manufacturers’ data sheets and had to be defined manually in the network model. Pressure loss ${∆p}_N$ $\left[\mathrm{P}\mathrm{a}\right]$ across these components is given by

$${∆p}_N=K_N{\displaystyle \frac{{\rho V}^2}{2}}$$

(2)

Cross-junctions were modeled using the coefficients by Idelchik [32], elbows and various other components according to Crane [33]. At the duct inlet, the volumetric or mass flow rate of air was set, and at the outflow vent components, the static pressure was prescribed. See also Section 5.4 in this context. The solutions from the network model analysis are the volumetric or mass flow rates at the various vent outlets, i.e., nozzles and ventilation grills. Using that information, together with available geometric information for these components, velocity vectors were determined in the respective outflow planes.

4.2. 3D CFD Model—Room Aerodynamics and Aerosol Dispersion

Computational fluid dynamics (CFD) was employed to solve for the flow field and the aerosol concentration inside the lecture hall. The turbulent flow field governing aerosol dispersion was assumed to be steady, thereby excluding large-scale flow unsteadiness, which can potentially lead to bifurcations in flow patterns, for example. Because of the small aerosol particle size and the low aerosol concentration in the flow domain, only one-way coupling was considered for the interaction between fluid flow and the aerosol particle phase within the flow domain. In other words, while the aerosol dispersion in the room is governed by the air flow in the room, the aerosol particles do not impact the fluid velocity nor its turbulent components. In addition, and due to the same reason, particle–particle or rather droplet–droplet interaction has not been considered in this study.

Gas-Phase Governing Equations

The differential forms of the conservation laws for mass, momentum and energy used to solve for the turbulent flow field of an incompressible fluid of a density ρ flow can be written compactly in a generalized form, i.e.,

$$\rho {\displaystyle \frac{\partial \Phi }{\partial \tau }}+\rho div(\overrightarrow{V}\Phi )-div\left({\Gamma }_{\Phi , eff} grad \Phi \right)=S_{\Phi }$$

(3)

with the velocity vector $\overrightarrow{V}=\left(U,V,W\right)$ and $\Phi =1$ for mass conservation, $\Phi =U, V, W$ for conservation of momentum in the x, y and z direction and $\Phi =T$ for conservation of energy. Here, mass, momentum and energy equations have been time-averaged over the turbulent time-scale of the fluid flow, and U, V, W and T denote Reynolds-averaged velocity components (in the x, y and z direction) and Reynolds-averaged temperature, respectively. ${\Gamma }_{\mathsf{\Phi },eff}$ represents an effective diffusivity due to molecular and turbulent diffusion and $S_{\Phi }$ denotes additional (source) terms pertaining to a specific $\Phi$-equation. Their respective values are listed in

Table 1. Effective diffusivities ${\Gamma }_{\Phi ,eff}$ and source terms $S_{\Phi }$ pertaining to mass, momentum and energy conservation equations according to Equation (3).

Equation	$\mathit{\Phi }$	${\mathit{\Gamma }}_{\mathit{\Phi },\mathit{e}\mathit{f}\mathit{f}}$	${\mathit{S}}_{\mathit{\Phi }}$
Continuity	$1$	$0$	$0$
x-momentum	$U$	$\mu +{\mu }_t$	$-{\displaystyle \frac{\partial p}{\partial x}}+\rho g_x+S_x$
y-momentum	$V$	$\mu +{\mu }_t$	$-{\displaystyle \frac{\partial p}{\partial y}}+\rho g_y+S_y$
z-momentum	$W$	$\mu +{\mu }_t$	$-{\displaystyle \frac{\partial p}{\partial z}}+\rho g_z+S_z$
Energy	$T$	$\mu /{\sigma }_l+{\mu }_t/{\sigma }_t$	$S_T$

. Note that in the present investigation, a steady-state flow-field solution is sought. The unsteady term on the left-hand side of the generalized governing equation is employed in a pseudo time-stepping approach to obtain the steady-state solution and vanishes in that limit. It is noted here that the validity of the steady-state assumption was evaluated by performing a time-accurate unsteady simulation after steady-state conditions were reached with the pseudo time-stepping approach. Doing so, the flow field was found to be quasi-steady, with low frequent limited amplitude flow asymmetries along the centerline of the symmetric lecture hall.

Here, $p\left[Pa\right]$ represents the local fluid pressure; $g_x$ $[\mathrm{m}/{\mathrm{s}}^2]$, $g_y$ $[\mathrm{m}/{\mathrm{s}}^2]$ and $g_z[\mathrm{m}/{\mathrm{s}}^2]$ are the components of gravitational acceleration; $S_x[\mathrm{k}\mathrm{g}/{\mathrm{m}}^2{\mathrm{s}}^2]$, $S_y[\mathrm{k}\mathrm{g}/{\mathrm{m}}^2{\mathrm{s}}^2]$ and $S_z[\mathrm{k}\mathrm{g}/{\mathrm{m}}^2{\mathrm{s}}^2]$ denote additional external forces acting on the fluid; and $S_T[\mathrm{J}/{\mathrm{m}}^3\mathrm{s}]$ is due to heat sources within the fluid domain. Note that in the present analysis $S_{x,y,z,T}=0.$ In the ${\Gamma }_{\mathsf{\Phi },eff}$ column of Table 1, $\mu [\mathrm{k}\mathrm{g}/\mathrm{m}\mathrm{s}]$ and ${\mu }_t[\mathrm{k}\mathrm{g}/\mathrm{m}\mathrm{s}]$ are the molecular and turbulent dynamic viscosity and ${\sigma }_l[-]$ and ${\sigma }_t[-]$ represent laminar and turbulent Prandtl numbers, respectively. Since the overall temperature differences are small, buoyancy effects are considered by using the well-known Boussinesq model. The latter accounts for buoyancy forces by expressing the density in gravitational force terms by

$$\rho ={\rho }_0\left[1-\beta \left(T-T_0\right)\right]$$

(4)

where ${\rho }_0 [\mathrm{k}\mathrm{g}/{\mathrm{m}}^3]$ denotes the density at the operating temperature $T_0 \left[\mathrm{K}\right]$ (i.e., the temperature with which the vent air enters the room in the present case) and $\beta$ = 0.00338 [1/K] is the thermal expansion coefficient of air. In all other governing equations, the density is assumed to be ${\rho }_0 [\mathrm{k}\mathrm{g}/{\mathrm{m}}^3]$.

In the present study, the well-known two-equation $k$-ε turbulence model by Launder and Spalding [34] has been employed to calculate the local values of the turbulent or eddy viscosity ${\mu }_t [\mathrm{k}\mathrm{g}/\mathrm{m}\mathrm{s}]$, which is defined as, ${\mu }_t=\rho C_{\mu } k^2/\epsilon$, where $k [{\mathrm{m}}^2/{\mathrm{s}}^2]$ and $\epsilon [{\mathrm{m}}^2/{\mathrm{s}}^3]$ represent local turbulent kinetic energy and its dissipation rate, and $C_{\mu } [-]$ is a model coefficient. Values for k and ε are obtained by solving two additional transport equations, one for k and one for ε. These equations can also be written in the form of Equation (3); the respective values for ${\Gamma }_{\varphi ,eff}$ and $S_{\Phi }$ are listed in

Table 2. Effective diffusivities ${\Gamma }_{\Phi ,eff}$ and source terms $S_{\Phi }$ pertaining to transport equations for turbulent kinetic energy k and turbulent kinetic energy dissipation rate ε according to Equation (3).

Equation	$\mathit{\Phi }$	${\mathit{\Gamma }}_{\mathit{\Phi },\mathit{e}\mathit{f}\mathit{f}}$	${\mathit{S}}_{\mathit{\Phi }}$
$k$-equation	$k$	$\mathsf{\mu }+{\mu }_t/{\sigma }_k$	$G-\rho \epsilon +G_B$
$\epsilon$-equation	$\epsilon$	$\mathsf{\mu }+{\mu }_t/{\sigma }_{\epsilon }$	$\left[\epsilon \left(C_{\epsilon 1}G-C_{\epsilon 2}\rho \epsilon \right)/k\right]+C_{\epsilon 3}{C}_{\epsilon 1}{G}_B(\epsilon /k)$
${\mu }_t=\rho C_{\mu }{k}^2/\epsilon$, $G={\mu }_t(\partial U_i/\partial x_j+\partial U_j/\partial x_i)\partial U_i/\partial x_j$, $G_B=g_i\beta ({\mu }_t/{\sigma }_t) \partial T/\partial x_i$

.

Here, $G [\mathrm{k}\mathrm{g}/{\mathrm{m}\mathrm{s}}^3]$ represents the generation of turbulence kinetic energy due to the mean velocity gradients, and $G_B [\mathrm{k}\mathrm{g}/{\mathrm{m}\mathrm{s}}^3]$ is the generation of turbulence kinetic energy due to buoyancy. $C_{\epsilon 1} [-]$, $C_{\epsilon 2} [-]$ and $C_{\epsilon 3} [-]$ are constants. ${\sigma }_k$ and ${\sigma }_{\epsilon }$ are the turbulent Prandtl numbers for $k$ and $\epsilon$, respectively.

The model constants have been assigned the default values as per [34] and are as follows:

$$C_{1\epsilon }=1.44, C_{2\epsilon }=1.92, C_{\mu }=0.09, {\sigma }_{\epsilon }=1.3 \mathrm{and} {\sigma }_k=1.0.$$

The prescribed governing equations are discretized in ANSYS^® Fluent^® v19.1 based on the finite-volume method with the steady-state flow-field solution being computed via the pseudo-transient solution method, as noted earlier, and subject to the boundary conditions described in Section 5.4. The SIMPLE scheme has been used for pressure–velocity coupling. In

Table 3. Numerical schemes used for spatial discretization in the present study.

Spatial Discretization	Numerical Scheme
Gradient	Least Squares Cell-Based
Pressure	Second-Order
Momentum	Second-Order Upwind
Turbulent Kinetic Energy	Second-Order Upwind
Turbulent Dissipation Rate	Second-Order Upwind
Energy	Second-Order Upwind

, the numerical schemes for spatial discretization in the present study have been summarized. Scaled residuals were used according to [35], and threshold values were set to 1 × 10⁻³ for the conservation equations of mass, momentum and turbulent quantities and 1 × 10⁻⁶ for the energy equation.

Disperse-Phase Model

In general, a dispersed droplet phase such as an aerosol moving in a surrounding gas or fluid phase can exchange mass, momentum and energy with the continuous phase. For the purpose of the present study, this phase coupling is modeled by the so-called discrete phase model (DPM) available in ANSYS^® Fluent^® v19.1. The trajectories of the discrete-phase particles/droplets are tracked within the flow domain in a Lagrangian fashion by integrating the particles’ equation of motion [35]

$$m_p{\displaystyle \frac{d{\overrightarrow{u}}_p}{dt}}=m_p{\displaystyle \frac{\overrightarrow{u}-{\overrightarrow{u}}_p}{{\tau }_r}}+m_p{\displaystyle \frac{\overrightarrow{g}({\rho }_p-\rho )}{{\rho }_p}}+\overrightarrow{F}$$

(5)

together with the kinematic condition

$${\displaystyle \frac{d{\overrightarrow{x}}_p}{dt}}={\overrightarrow{u}}_p$$

(6)

where $m_p \left[\mathrm{k}\mathrm{g}\right]$ is the particle mass; $\overrightarrow{u} [\mathrm{m}/\mathrm{s}]$ and ${\overrightarrow{u}}_p [\mathrm{m}/\mathrm{s}]$ denote the local fluid-phase velocity and particle velocity, respectively; $\rho [\mathrm{k}\mathrm{g}/{\mathrm{m}}^3]$ and ${\rho }_p [\mathrm{k}\mathrm{g}/{\mathrm{m}}^3]$ are the fluid and particle densities; $\overrightarrow{F} [\mathrm{k}\mathrm{g} \mathrm{m}/{\mathrm{s}}^2]$ denotes additional forces acting on the particle aside from gravity and buoyancy; and $m_p{\displaystyle \frac{\overrightarrow{u}-{\overrightarrow{u}}_p}{{\tau }_r}}$ represents the drag force acting from the surrounding flow on the particle, where ${\tau }_r \left[s\right]$ is the droplet or particle relaxation time under the assumption of creeping flow around the particle or droplet (i.e., $Re<1$) [36]:

$${\tau }_r={\displaystyle \frac{{\rho }_p{d}_p^2}{18\mu }}{\displaystyle \frac{24}{C_{D}Re}}$$

(7)

Here, $\mu [\mathrm{k}\mathrm{g}/\mathrm{m}\mathrm{s}]$ is the molecular viscosity of the fluid, $d_p \left[\mathrm{m}\right]$ is the particle diameter, and $Re [-]$ is the particle’s Reynolds number based on the relative velocity between particle and surrounding fluid flow,

$$Re={\displaystyle \frac{\rho d_p\left|\overrightarrow{u}-{\overrightarrow{u}}_p\right|}{\mu }}$$

(8)

and $C_D=24/Re [-]$ denotes the drag coefficient for creeping flow around spherical droplets.

As the density of the continuous fluid phase (air) is considerably lower than that of the dispersed aerosol particles, the so-called “virtual mass” force, i.e., the force required to accelerate the fluid surrounding an aerosol particle, has been neglected. On the other hand, the shear lift or Saffman lift force ${\overrightarrow{F}}_{L,Saff} [\mathrm{k}\mathrm{g} \mathrm{m}/{\mathrm{s}}^2]$ acting on the particle has been considered, i.e.,

$${\overrightarrow{F}}_{L,Saff}=1.615\rho d_p^2\sqrt{\nu }{\displaystyle \frac{\frac{\partial u}{\partial z}}{\sqrt{\left|\frac{\partial u}{\partial z}\right|}}}(\overrightarrow{u}-{\overrightarrow{u}}_p)$$

(9)

The effect of turbulence on particle dispersion has been modeled using the well-known Discrete Random Walk (DRW) model, which describes the interaction of a particle with a turbulent eddy. Here, a randomized fluctuating velocity is imposed onto the mean velocity over a time interval associated with the respective turbulent eddy lifetimes of the turbulent eddies [35]. Since the aerosol particle size considered here is larger than 0.3 $\mathsf{\mu }\mathrm{m}$, Brownian dispersion has been neglected. Note that in the present investigation, droplet evaporation (affecting droplet trajectory) is not considered and $m_p=constant$ in the above equations.

5. Simulation Set-Up

The following section summarizes the model parameters, geometric parameters and boundary conditions specific to the present study, leading to the CFD and network model results presented in Section 6.

5.1. Material Properties

The ventilation air was assumed to be incompressible ideal gas having a temperature of 20 °C, a density of 1.1894 $\mathrm{k}\mathrm{g}/{\mathrm{m}}^3$ and a dynamic viscosity $\mu$ of 1.8232 × 10⁻⁵ Pa·s. The same constant properties were also assumed for the room air at the point of the problem’s initialization. Upon changing the temperature of the air exhaled by the room’s occupants in the course of solving the energy equation within the room, the air density appearing in the gravitational force terms of the momentum equations has been modified according to Equation (4).

Respiratory droplets released by exhaled breathing air consist of saliva and other materials found in the respiratory tract, also including various cell types and, potentially, pathogens such as SARS-CoV-2. As respiratory droplets evaporate, the concentration of non-volatile compounds increases, thereby reducing the droplet evaporation rate. The equilibrium diameter at which no further vaporization takes place is reported to be about 20–40% of its initial value [37]. However, in the present analysis, droplet vaporization has been neglected; the exhaled aerosol particles or droplets were assigned the material properties of water at 34 °C [38] with a density of 998.2 kg/m³.

5.2. Vent System Geometry and Boundary Conditions

The flow through the air venting system has to be modeled in order to determine the air mass flow rates through the various vent components, which discharge the vent air into the lecture hall. These mass flow rates, together with the specific outlet geometries of the employed long-throw jet nozzles, swirl nozzles and air grids/grills, served to define boundary conditions within the subsequent 3D CFD analysis of the air movement inside the lecture hall.

Since the lecture hall’s ventilation system is an open-loop system (i.e., none of the air leaving the room via the vent-out ports is recirculated), and since the air delivery portion of the venting system consists of two identical branches, only one such branch or “leg” is simulated. The network pertaining to this leg is shown in Figure 4 (right) and is comprised of various air discharge components (i.e., vent inlets with respect to the room), whose pressure loss coefficients have been taken from the manufacturers’ technical specifications. Although the pressure loss coefficients are not constant for different flow regimes, the variations were found to be negligible within the considered operating range.

Hence, average values for the pressure loss coefficients of the employed discharge nozzles and ventilation/air grids were considered. Their respective values are listed in

Table 4. Loss coefficients for vent discharge nozzles and vent grids used in the present venting system and employed in the network model.

No.	Component	K Factor
1	Ventilation Air Grid or Grill	1.40
2	Swirl Nozzle/Diffuser	20.00
3	Jet/Long-Throw Nozzle	1.14

.

To limit acoustic noise in the lecture hall to acceptable levels, the ventilation system is run at 70% peak capacity, which corresponds to a volume flow rate of 4800 ${\mathrm{m}}^3/\mathrm{h}$ or 1.586 kg/s of air. Half of this flow rate has been imposed at the 1D vent system branch illustrated in Figure 4. The vent outlets, i.e., nozzles and air grids, have been defined as fixed static pressure outlets, the values of which have been initially set to 101,325 $\mathrm{P}\mathrm{a}$.

Room Geometry/CAD Model

Figure 4 (top left) illustrates the CAD model of the lecture hall with its side walls omitted but including seating areas (gray), the shapes of occupants (red) and the part of the venting system that is located inside the lecture hall. The hall has a total width of 21.92 m, a total length of 19.32 m and maximum height of 5.37 m. The vent pipes are located approximately 0.635 m below the ceiling, and the vent-in boundaries of the swirl nozzles and long-throw nozzle have a distance of 3.9 m and 4 m from the floor. The two cubic sections in the back of the room are the foyers by which the students access and leave the hall. The doors have been assumed to be closed for the simulations. In the front of the hall, there is a slightly elevated stage area occupied by a long rectangular front desk. There are only two square-shaped vent outlets (black) located in the front of the hall, each one situated between a front divider wall and the neighboring side wall at a height of 3 m above the floor and with a cross-sectional area of 0.3416 m². Dimensional information can also be found on the bottom diagram in Figure 4.

In order to keep the size of the computational mesh needed for the CFD analysis of the room manageable, only geometric features essential to the room aerodynamics have been retained. This includes the exact positions and cross-sections of air inflow (vent-in) and outflow (vent-out) boundaries, the walls of the foyer entrances in the back of the room, divider walls near emergency exit doors (which have not been modeled) in front of the room and all seating rows, as well as 32 occupants positioned in every fourth row behind each other and four seats apart from each other within each row. Care has been taken to include the slope of the floor and to precisely position the ventilation duct system within the room; see Figure 4. Geometric features that have been simplified to reduce the meshing time and mesh size include the complexity of the human bodies representing the occupants and details of the seating rows. Each seat within a seating row has been modeled as a separate solid block, and for an occupied chair, the torso and head of the occupant have been approximated as rectangular cuboids sitting atop that block. This has resulted in a considerable reduction in the number of computational mesh elements and a reduction in the complexity of the fluid mesh, the latter of which also had a positive effect on the stability and convergence behavior of the CFD analysis.

Computational Mesh/Discretization of Flow Domain

The geometric or CAD model of the previous section has been used to generate the fluid domain subject to the air flow within the lecture hall. This has been accomplished by using ANSYS^® DesignModeler™ after importing the CAD model from SOLIDWORKS^® 2018. The computational mesh for the fluid domain has been generated using ANSYS^® ICEM-CFD^TM 19.1.

Local mesh resolution was set based on anticipated gradients in flow velocity, which are largest near the jet flows originating from the long-throw/jet nozzles, the swirl diffusers/nozzles, the vent air grids and the occupants’ mouths. For solid surfaces such as the room’s floor, walls and seating positions, wall functions were used to properly and efficiently capture the flow physics in the “near wall” regions. Mesh generation had to be performed with care, since no adaptive re-meshing was employed within the present CFD analysis.

The computational mesh used to obtain the numerical results presented in Section 6.2 initially consisted of approximately 476 million tetrahedral cells and was subsequently transformed into a polyhedral-type mesh. The latter provides better computational efficiency, as well as better accuracy, stability and convergence properties with respect to the numerical solution, in comparison to tetrahedral elements [39]. Special care had to been taken to refine the mesh in the vicinity of the mouths of the occupants, swirl nozzle and jet nozzles; see Figure 5 and Figure 6. After transformation, the total number of polyhedral cells was approximately 85 million.

Cell size dimensions varied from 0.25 mm (in the vicinity of air flow inlets such as swirl and jet nozzles and the mouths of occupants) to 0.1 m. A mesh quality check was conducted. The so-called Cell Squish Index and Face Squish Index are used to assess the mesh quality of polyhedral cells [40,41]. For the exact definition of the Cell Squish Index and Face Squish Index, see [35]. Around 90% of the cells had a squish index below 0.1 and an orthogonal quality index above 0.9, which is considered sufficient for the present study.

5.3. Mesh Sensitivity Study

To ensure that the numerical results for the flow field in the lecture hall are mesh-insensitive, a mesh-independence study was conducted for the non-isothermal case and employing three meshes with a mesh count of 32, 66 and 99 million polyhedral cells, corresponding to a mesh count refinement factor of 2 and 1.5, respectively. Specifically, a GCI (Grid Convergence Index) study was undertaken, as already described in [42,43,44], while considering the velocity magnitude at two meaningful locations within the lecture hall as values of interest or parameters indicative of grid convergence. A GCI value is computed for pairs of grids with successive sizes. For the mesh pair having the two highest resolutions, the GCI is defined as

$$GCI={\displaystyle \frac{F_s\left|\epsilon \right|}{r^p-1}}$$

(10)

where $F_s$ denotes a safety factor, which is commonly assigned a value of 1.25 when three (or more) grids are considered as per Roache [44]. The grid refinement ratio $r$ is defined as the ratio between cell sizes of the two grids being compared, i.e., $r=h_2/h_1$, where $h_1$ denotes the grid spacing of the finer and $h_2$ the grid spacing of the prior (coarser) mesh. According to the NPARC (National Project for Application-oriented Research in CFD) Verification and Validation Guide [43], r ≥ 1.1 is required in order to assess the error due to mesh resolution.

For our unstructured meshes and following Celik et al. [42], we used the volume-equivalent mesh size $h_{vol}$ obtained from the average cell volume for each mesh in order to evaluate r, whereby

$$h_{vol}={\left({\displaystyle \frac{1}{N}}\sum _{i=1}^N{∆V}_i\right)}^{{\displaystyle \frac{1}{3}}}$$

(11)

with $N$ being the total cell count of the mesh and ${∆V}_i$ denoting the volume of the $i^{th}$ cell.

The parameter $\epsilon$ in Equation (10) represents the relative difference (regarding the predicted value of interest (in our case the velocity magnitude at specific points)) between the two meshes. Accordingly, for the mesh pair with the highest resolution

$$\epsilon ={\displaystyle \frac{f_2-f_1 }{f_1}}$$

(12)

Finally, $p$ in Equation (10) represents the order of convergence and is calculated as

$$p={\displaystyle \frac{\ln \left(\frac{f_3-f_2}{f_2-f_1}\right)}{\ln \left(r\right)}}$$

(13)

where $f_1$, $f_2$ and $f_3$ represent the value of the velocity’s magnitude predicted by the finest, medium and coarsest mesh, respectively, at a chosen point of interest in the simulation domain, i.e., the lecture hall. For the present study, two such points, positioned on the line reaching across the lecture hall as depicted in Figure 6, have been chosen. The first point (#P1, indicated by green marking in Figure 6) is located about 20 cm (off center) in front of an occupant’s mouth and within the range of the exhaled air plume. At this location, the local velocity profile plays a critical role in aerosol dispersion. The second point (#P2, indicated by the yellow marking in Figure 6) is situated in the shear layer of one of the air jets emanating from one of the air grids. The accurate prediction of shear layers is of great importance for accurately predicting the overall room aerodynamics.

According to [43], when the ratio $({GCI}_{23}/{(GCI}_{12}·r^p))$ is approximately one, it indicates that the solutions are well within the asymptotic range of convergence. The $GCI$ values for the respective mesh pairs, order of convergence and the ratio indicating asymptotic convergence for both these monitoring points are listed in

Table 5. Summary of the grid convergence study.

Grid	Elements [in Millions]	$\mathbf{Mesh} \mathbf{Size} \mathbf{(}{\mathit{h}}_{\mathit{v}\mathit{o}\mathit{l}}$$\mathbf{)} \mathbf{[}\mathbf{m}\mathbf{]}$	$\mathbf{U} \mathbf{[}\mathbf{m}\mathbf{/}\mathbf{s}\mathbf{]}$		GCI [%]		$\mathit{p}$ [-]		$\frac{{\mathit{G}\mathit{C}\mathit{I}}_{\mathbf{23}}}{\mathbf{(}{\mathit{G}\mathit{C}\mathit{I}}_{\mathbf{12}}\mathbf{·}{\mathit{r}}^{\mathit{p}}\mathbf{)}}$
			#P1	#P2	#P1	#P2	#P1	#P2	#P1	#P2
G1	99	0.0279	0.15	1.79	1.47	0.57	10.97	9.18	1.04	1.01
G2	66	0.0319	0.144	1.77
					6.73	1.99
G3	32	0.0406	0.042	1.54

.

Figure 7 illustrates an exemplary comparison of results obtained for the three meshes (including an additional result for a mesh with 85 million polyhedral cells). Shown are predictions for the velocity’s magnitude along an exemplary straight line inside the lecture hall, which passes through low- and high-speed areas. The chosen line extends from the vicinity of an occupant’s mouth to the close proximity of one of the air grid inlets, as shown in Figure 6. Figure 8 and similar flow-field comparisons throughout the computational domain (not illustrated) show that the mesh with 85 million cells provides a good accuracy at a reasonable computational expense. Hence, this mesh has been used to produce the flow-field results presented in Section 6.2.

5.4. Boundary and Initial Flow-Field Conditions

Inflow conditions related to vent system components, i.e., swirl nozzles, throw nozzles and vent grids, were set according to the locally discharged mass flows predicted by the vent system network model solution. Specifically, velocity inlet conditions were specified to components’ exit flow boundaries (i.e., the respective room inflow boundaries) based on mass flow and the specific component geometry given by the manufacturers’ technical drawings. The calculated velocity vectors were assumed to be constant throughout the boundary surfaces. In the case of the swirl nozzles/diffusers, the exit flow boundary consists of a number of radial slit openings uniformly spaced in the circumferential direction, whereby two sets of internal blades are responsible for the air swirl effect and determine the direction of the velocity vectors at the slit openings. Each slit opening was assigned a specific direction for the air velocity vector, i.e., at 0° or 30° towards the local normal direction. For the present investigation, an angle of 0° was chosen for all swirl diffusers. Defining the boundary conditions for the throw or jet nozzles and vent grids was straightforward.

There are only two vent outlets through which air leaves the lecture hall. These are located at the front wall of the room at a height of approximately 3 m. They are separated by a short divider wall from the area where the blackboards are mounted (see Figure 1). At these boundaries, pressure outlet conditions have been specified, with a static pressure of 101,325 $\mathrm{P}\mathrm{a}$.

To model the occupants’ breathing activity and the release of aerosol particles with the exhaled air, the mouth of each occupant is modeled as a circular orifice having a surface area of 20 ${\mathrm{c}\mathrm{m}}^2$. In the present study, dynamic breathing, i.e., an inhalation cycle followed by an exhalation cycle, or coughing, is not modeled. Instead, continuous exhalation at a volume flow rate of 0.27 L/s is assumed. The latter value corresponds to the mean flow rate of a real exhalation cycle under normal breathing conditions; see [45]. Since the mouth opening is specified as a “velocity inlet” boundary condition, a uniform velocity of 0.135 $\mathrm{m}/\mathrm{s}$ has been imposed here.

No-slip boundary conditions were imposed for solid or impenetrable surfaces; this includes the side walls, floor and ceiling of the room, outer airduct surfaces within the room seating areas and the surfaces of the occupants’ bodies (except for their open mouth surfaces, across which breathing air is exhaled).

A summary of the boundary conditions for mean flow quantities is given in

Table 6. Boundary conditions imposed as part of the CFD analysis of the lecture hall and their respective mean values. Turbulent quantities (k, ε) at velocity inlets obtained from imposed turbulence intensity and viscosity ratios, i.e., 5% and 10, respectively.

Boundary Location	Boundary Type	Value
Occupants’ Mouths	Velocity Inlet	$V_n=0.135 \mathrm{m}/\mathrm{s}$
Inlet Vents	Velocity Inlet	see Table 7
Impermeable Surfaces	No-Slip Wall	$V=0 \mathrm{m}/\mathrm{s}$
Outlet Air Grids	Pressure Outlet	$p_{out}=\mathrm{101,325} \mathrm{P}\mathrm{a}$

and

Table 7. Discharge flow rates and respective mean velocities through various vent system components for the vent network of Section 5.2. Component specification according to the network diagram in Figure 4 (right).

Serial No.	Component Name	Flowrate [m³/h]	Mean Inlet Velocity [m/s]
1	Air Grid A	568.47	2.52
2	Air Grid B	568.47	2.52
3	Swirl Diffuser/Nozzle A	126.91	0.27
4	Swirl Diffuser/Nozzle B	164.49	0.35
5	Swirl Diffuser/Nozzle C	133.93	0.28
6	Swirl Diffuser/Nozzle D	121.56	0.26
7	Swirl Diffuser/Nozzle E	123.33	0.26
8	Jet/Long-Throw Nozzle A	157.21	5.56
9	Jet/Long-Throw Nozzle B	173.14	6.12
10	Jet/Long-Throw Nozzle C	242.49	8.58

. Based on the calculated exit velocities of the swirl diffusers, air grids and long-throw nozzles, a medium turbulence level (with turbulence intensity = 5%) and a viscosity ratio of 10 were assumed for all inflow components. Accordingly, boundary values for $k$ and $\epsilon$ were derived using these assumptions. While this approach is suitable for the swirl diffusers, it may underestimate turbulence for the long-throw nozzles. Nevertheless, at the present Reynolds number, free jet spreading is predominantly influenced by jet–ambient air interactions rather than inlet turbulence, as discussed in [46,47]. Although using varying viscosity ratios for different inflow boundaries could enhance the accuracy, a uniform value was adopted in the present study.

Using conservation of mass and momentum equations (i.e., Equation (3) for $\Phi =(1, U, V, W, k, \epsilon ))$, the steady-state isothermal velocity field within the lecture hall has been determined based on the prescribed boundary conditions and using a pseudo time-stepping approach towards the steady-state solution. The initial velocity, pressure and turbulence field within the room was assumed to be uniform, with (U, V, W, P, k, ε) = (0, 0, 0, 101,325 Pa, 0, 0). After a converged isothermal flow field solution was obtained, the temperature at all vent system inflow boundaries was set to 293.15 K and that of the air exhaled by the occupants was set to 307.15 K (corresponding to the temperature in the human oral cavity). In addition, zero heat flux was imposed at all impermeable surfaces, except for the occupants’ bodies, where a heat flux of $\dot{q}=58 \mathrm{W}/{\mathrm{m}}^2$ was assumed, following DIN EN ISO 7730:2023-04 [48]. Also, before the renewed flow-field solution together with the energy equation ($\Phi =T$ in Equation (3)), the initial temperature on all internal cells was set to 293.15 K.

If the vent or HVAC system generates a temperature difference between the room air and/or room walls, the room aerodynamics can change considerably and the CFD analysis within the room/vent loop workflow now also has to include the solution of the energy equation. If in addition, the room exhaust air is recirculated into the HVAC system, the convergence of the overall flow field, i.e., the room aerodynamics and air flow in the vent network, might be impacted considerably.

Boundary Conditions Aerosol Phase/DPM Set-Up

The distribution of breathing aerosols within the lecture hall has been determined based on the steady-state non-isothermal flow field described earlier and based on the assumption that the aerosol phase does not alter the flow field (i.e., a one-way coupling between the aerosol and gas phase has been assumed).

The calculation of particle trajectories has been performed as described in Section 4.2. According to Hartmann et al. [49], the number of particles emitted through the mouth varies between 134 particles/s and 1018 particles/s. For the present study, we have tracked 10,186 aerosol droplets per person, corresponding to the particles released during a four-second breathing cycle (based on an average release rate of 849 particles per second). Note that for a coughing event, the latter authors measured a mean particle release rate of 13,709 particles/s and a maximum rate of 287,697 particles/s. Particle release positions at the open-mouth boundary were equally distributed across the mouth surface. Based on measured particle size distributions in exhaled air [49,50,51,52], a uniform aerosol droplet diameter of 0.5 $\mathsf{\mu }\mathrm{m}$ was assumed.

An “escape” boundary condition was set at both air outlet vents, i.e., aerosol particles reaching those outflow boundaries are discarded within the simulation. Aerosol particles that reach an impenetrable surface are assumed to be trapped or deposited at that position.

6. Results and Discussion

This section describes the analysis results from the combined analyses of vent system, room aerodynamics and aerosol dispersion within the room for the specific configuration presented in Section 5 and using the models described in Section 4. Flow-field coupling between the vent system and the room air flow, as covered by the process workflow of Section 3 (see also Figure 2), was not observed; i.e., the static pressure of 101,325 Pa, initially imposed at the vent system outlets within the network model, did not meaningfully vary from those predicted within the subsequent CFD analysis.

6.1. Flow Within the Vent System

Simulation results from the network model, subject to the imposed boundary conditions and fluid properties, provide the air flow rate at every vent opening in the ventilation system. These results are summarized in the third column of Table 7. The listed volume flow rates have subsequently been used to determine the velocity inlet conditions at the various vent components (see Table 7) needed for the CFD analysis of the room’s aerodynamics. The velocity magnitudes are listed in column 4 of Table 7.

The calculated mean velocity values were validated by spot-checking the discharge velocity across the outlets of various jet nozzles, air grids and swirl nozzles on site, using a portable vane anemometer. The maximum error between the predicted mean velocities and those calculated from experimental data was 5%.

6.2. Flow Field and Aerosol Dispersion Within the Lecture Hall

Figure 8 shows contour lines of magnitude of velocity (in m/s) in three planes of the fluid domain, cutting either through a set of inlet air grids, a jet/long-throw nozzle or a set of swirl diffusers/nozzles. It can be observed that the air being discharged from the air grids has a major influence on the air circulation in the room. In the front of the room, the two grids directed towards the front wall induce a strong air roller or strong circulation pattern, with air being pushed down the front wall, then back along the elevated stage section towards the front seating rows and from there again upwards; see also Figure 13 (left) in this context. Evidence of the latter is given, also, by the temperature plots shown in Figure 9 and specifically the strongly upwards-directed warm air exhaled by the occupants seated in the front rows. In addition, streamline plots illustrated in Figure 10 show that the left and right sides of the room, down to about half of the room’s length from the front wall, are dominated by air flow originating from the air grids directed towards the front wall.

The air being discharged from the two air grids that are directed towards the center region of the room (i.e., down towards the seating rows) reaches far across the entire room, including the last row of seats with occupants. Air from these two vent grids, together with the air being ejected through six jet nozzles in between the two box-shaped foyers, determines the flow field dynamics in the back of the lecture hall (side wall to side wall), as well as in the center region of the room. Air introduced via the swirl diffusers/nozzles mainly affects the air flow in the center region of the room near the center aisle. Here, flow behavior is also influenced by body plumes, as well as by the surrounding air streams originating from the two inward-directed air grids and by the strong air currents induced by the long-throw nozzles at the back end of the room.

Figure 9 shows contour lines of temperature (in kelvin) in two parallel planes along the length of the lecture hall. Each plane cuts through the circular open-mouth boundary of a series of occupants aligned behind each other in different rows. Due to the higher temperature of the exhaled air, that air experiences a buoyancy force in the upward direction. As a consequence of different surrounding air flow conditions at the various seating positions, the body plumes take different shapes, as can be observed from the temperature contours. The occupants seated in the front row experience the upward flow effect of the air roller discussed earlier; here, the temperature plumes are pointed sharply upwards. The occupants in the second occupied row of seats find themselves below the air current generated by the inward-directed air grids. Here, the flow near the occupants is primarily driven by their body’s thermal plumes. The occupants seated in the last two occupied rows and in line with the air current discharged from the inward-directed air grids experience the strong air flow of this current now approaching the lower area of the room. Here, the temperature plume has nearly disappeared (second to last row) or is washed upwards behind the heads of the occupants towards the back of the room; see Figure 8 (left contour plane) in this context.

Figure 10 illustrates streamlines originating from the air grids, colored by the local magnitude of velocity. As noted earlier, the vent air discharged towards the inner region of the room reaches well across the lecture hall, approaching the room floor at about the last row where occupants are seated. One also observes that a significant portion of that air enters into the left and right back region of the hall without seats. Some of that air first mixes with the air discharged from the downward-directed jet nozzles in the back of the room. Figure 11 shows streamlines originating from the jet nozzles in the back of the room colored by the residence time of virtual massless tracer particles released at time 0 s on the respective starting points of the streamlines. One observes that, after mixing with air from the vent air grids and impinging on the floor, the air from the jet nozzles creates a strong forward- and subsequently upward-directed air current in the central region of the room. This air current also induces a forward air motion above the backward-directed air streams from the vent air grids before being entrapped by these, only to be pushed upwards and forward again along the center aisle later on. Some of the air discharged from the jet nozzles also reaches the side regions in the back of the room. As a consequence of the various prescribed air currents, the air flow surrounding occupants seated in the center and outer region of the second row is mainly driven by natural convection from thermal plumes.

As already noted earlier, much of the air discharged from the air grids towards the front wall of the lecture hall remains confined to the front, i.e., the stage area, where it either drives a rolling air motion between the front wall and the first seating row or is diverted to the right-side and left-side areas between the walls and the seating rows, taking up about one-half of the length of the hall. From there, it can leave the room through the exit flow vents. Alternatively, upon its upward motion along the side walls, that air can enter the central region of the room, where it is again pushed towards the front of the room and then discharged through the exit flow vent or entrained by the air streams and pushed towards the back of the lecture hall.

Figure 12 illustrates streamlines for the air flow discharged from the ten swirl diffusers/nozzles of the vent air distribution system. The air discharged from the four swirl diffusers over the center aisle towards the back of the room (nozzles C and E in Figure 4 for one vent system branch) is pushed downwards and then redirected forwards, due to the influence of the air currents generated by the jet nozzles. The air from the two swirl nozzles in the front of the room (nozzle A in Figure 4 for one vent system branch) is diverted away from the center aisle. The air from the two neighboring swirl diffusers in the center of the room on either side (nozzle B in Figure 4) is entrained by the downward-directed air flow originating from the air grids facing the center of the room and subsequently diverted towards the front of the room.

The air from the outer swirl diffusers in the back of the room (nozzle D in Figure 4) initially moves downwards towards the side walls of the room, followed by an upward motion, at which point the flow splits into a backward-facing (directed towards the jet nozzles) and a forward-facing stream. Note that the upward-directed thermal air currents or body plumes and the downward air currents generated by the swirl diffusers support each other, due to the relative offset between swirl diffuser positions and occupants’ seating positions (in the x-y plane). As a consequence, the breathing aerosols initially rise fairly quickly after being exhaled by the occupants; see Figure 15 (top picture) in this context.

The streamline plots in Figure 10, Figure 11 and Figure 12 provide an insight into the air distribution patterns, which cannot be quickly obtained by cut-plane plots of magnitude of velocity, velocity components or in- or out-of-plane velocity vector plots, for example. An even deeper understanding of room aerodynamics (and aerosol distribution patterns) can be gained from flow field and particle trajectory visualization in a virtual reality (VR) environment. Here, an interactive tracer particle release at arbitrary positions quickly provides an insight into the complex aerodynamics of the room. Unlike VR desktops or headsets, VR Powerwalls or a VR CAVE (as used in the present work; see Figure 13) provide an additional opportunity for working collaboratively in an immersive environment, which can accelerate discussions or decisions on flow-field optimization or the assessment of a room’s usability. For example, flow dividers might be considered for optimizing aerodynamics, but they potentially impact visibility across the room, as well as access to escape routes in case of emergency evacuation. The latter assessment can be more readily be made in VR. In addition, future sensing solutions for immersive VR systems, such as electronic skins [53], will further enhance information concerning an occupant’s well-being, such as the sensation of air drafts when being exposed to a strong air current within the room—information that is otherwise difficult to ascertain.

Figure 13. Three-dimensional visualization of room aerodynamics in fully immersive VR CAVE. Left: streamlines (blue) of air roller in front corner of lecture hall and velocity vectors (white) in horizontal plane near overhead vent air grids. Right: streamlines across the entire lecture hall (view towards the back of the room; high velocities in rose color, low velocities in blue).

Figure 13. Three-dimensional visualization of room aerodynamics in fully immersive VR CAVE. Left: streamlines (blue) of air roller in front corner of lecture hall and velocity vectors (white) in horizontal plane near overhead vent air grids. Right: streamlines across the entire lecture hall (view towards the back of the room; high velocities in rose color, low velocities in blue).

In the following, aerosol dispersion within the lecture hall is discussed. In this context, it is instructive to remember that, here, only one size of aerosols is considered, all having a diameter of 0.5 μm, and that considering other aerosol particle sizes [51,52] and tracking them within the computed quasi-steady flow field would provide a more realistic picture of the overall aerosol load in the room. Figure 14 and Figure 15 illustrate the trajectories of a selected number of aerosol particles (d = 0.5 μm) exhaled by the occupants and colored by their residence time within the room after being released from the occupants’ mouths. One observes that the aerodynamics within the room results in a broadly scattered distribution of aerosol droplets throughout the room, even though the breathing aerosols initially rise fairly quickly towards the ceiling (see Figure 15, top picture). Also, even though the occupants are seated at the same positions on the left and right side of the symmetrically designed lecture hall (including the venting system), with the symmetry axis along its center aisle, the aerosol trajectories differ notably on both sides. This is partly due to turbulent dispersion effects (and the employed Random Walk model) and to a certain extent due to the slight asymmetry of the mean flow velocity distribution with respect to the center aisle.

To describe the aerosol dispersion observed for different seating positions, it is useful to subdivide the occupant pool into (square) blocks of four, i.e., R12C12, representing the two four-person blocks next to the center aisle in the front of the room, and R12S12, representing the two four-person blocks near the front but to the sides of the lecture hall. The blocks R34C34 and R34S34 correspondingly represent the four-person blocks near the center aisle and to the sides in the back of the room; see Figure 15 in this context. Based on this classification, Figure 15 shows that aerosols released from block R34C34 will in general rise upwards and travel towards the front of the room, where they will either be entrained by the air circulation near the front of the room (air roller) or be entrained and “thrown back” towards the room exits (in the back) by the air discharged from the air grids whose openings point inwards into the room. In contrast aerosols released in block R34S34 initially travel mostly backwards (towards the room exits) and are then directly entrained by the long-throw nozzles in the back of the room, or they (initially) might find themselves in the back corners and sides of the room. Aerosols released in block R12C12 are taken up by the air roller established by the air grids discharging their air towards the front of the room. The same is true for aerosols released from the occupants near the center aisle in the front row of block R12S12. Aerosols released by the occupants of block R12S12, which are seated in the second occupied row nearer to the center aisle, can be found (at least initially) within the air circulating in the sides of the room, after being entrained by the air currents originating from the air grids directed towards the inside of the room. Aerosols released from occupants seated in block R12S12 near the wall are either exhausted directly through the vent outlets or indirectly after participating in the air circulation at the side of the room. Overall, based on the actual flow field within the room, only a limited amount of aerosols is directly exhausted through the two exit vents in the front of the room. Evaluation of the residence times and trajectories of aerosol particles shows that after a period of 20 min (starting at t = 0 s), 39% of the aerosol particles released during a four-second period after t = 0 s will leave the lecture hall over the exit vents, while in the same time period the vent air volume admitted to or exhausted from the room corresponds to 1.45 times the total volume of the lecture hall. Figure 16 shows particles suspended in the room 505 s and 1205 s after release from the occupant’s mouth at t = 0 s (for a time period of 4 s). One observes that after 1205 s, the particles are more or less uniformly distributed across the room, while after 505 s streaks of locally higher aerosol concentration can be observed.

Figure 14. Three-dimensional view of aerosol particle trajectories released from the occupants’ mouth openings over a time period of 4 s according to the boundary conditions of Section 5.4. Illustrated are aerosol particle trajectories over a tracking time of 20 min after being released (at t = 0 s). Trajectories colored according to their respective residence times.

Figure 14. Three-dimensional view of aerosol particle trajectories released from the occupants’ mouth openings over a time period of 4 s according to the boundary conditions of Section 5.4. Illustrated are aerosol particle trajectories over a tracking time of 20 min after being released (at t = 0 s). Trajectories colored according to their respective residence times.

Figure 15. Front-to-back view (top picture) and top view (bottom picture) of the 3D aerosol particle tracks within the lecture hall illustrated in Figure 14.

Figure 15. Front-to-back view (top picture) and top view (bottom picture) of the 3D aerosol particle tracks within the lecture hall illustrated in Figure 14.

Figure 16. Locations of suspended aerosol particles within the lecture hall, 505 s (top; particles in blue color) and 1205 s (bottom; particles in red color) after starting release from the occupants’ mouth openings at t = 0 s for a time period of 4 s (each occupant releasing particles at a rate of 849 particles/s). Number of particles suspended after 505 s is 98,500 particles and after 1205 s, 66,200 particles, corresponding to 90% and 61% of the total particles released.

Figure 16. Locations of suspended aerosol particles within the lecture hall, 505 s (top; particles in blue color) and 1205 s (bottom; particles in red color) after starting release from the occupants’ mouth openings at t = 0 s for a time period of 4 s (each occupant releasing particles at a rate of 849 particles/s). Number of particles suspended after 505 s is 98,500 particles and after 1205 s, 66,200 particles, corresponding to 90% and 61% of the total particles released.

Table 8. Wall-clock times for the tasks according to the workflow presented in Figure 2 for the present analysis case of a lecture hall with a forced air vent system.

Task	Time Consumption [h]
Network model	3.5014
Set-up	3.5
Calculation	0.0014
Alternative 1: CAD Generation for Room	26
In situ measurements in lecture hall	4
Measurements of flow conditions	2
HVAC/architecture plan measuring (AutoCAD)	4
CAD generation in SOLIDWORKS®	16
Alternative 2: CAD Generation with 3D-Laserscanner Equipment	13
In situ measurements in lecture hall	3
Measurements of flow conditions	2
Post-processing of point cloud data	8
Mesh Generation	48
Geometry preparation for pre-processing (DesignModeler)	2
Meshing set-up (sizing parameters, refinement)	6
Mesh execution	10
Check mesh quality and improve mesh (3 iterations)	30
CFD Simulation + DPM	16
Conversion of tetrahedral mesh to polyhedral mesh	2
Definition of boundary conditions	1
Selection of numerical models and schemes	1
Run steady simulation without energy equation (5000 iterations); 192 CPU in-house cluster Hydra	4
Coupling flow with energy equation and run simulation (1000 iterations); 192 CPU in-house cluster Hydra	1
DPM set-up	1
Calculation of particle trajectories	6
Post-Processing	12
CFD and DPM results	10
Visualization of results (VR via CAVE)	2
Total Time Consumption	118.5014

summarizes the time requirements for the various work packages of the process workflow shown in Figure 2, specific to the present investigation. Note that, here, no system optimization (“outer loop”) has been included, triggering changes in room or vent geometry, seating positions, vent system volumetric flow rate or other boundary conditions. Also, the pressure conditions predicted by the CFD analysis were consistent with the pressure imposed in the vent system network model; accordingly, no “inner loop” iterations were necessary as part of the present test case.

Regarding the CPU time reported in Table 8 for the CFD analysis, it is noted that the CFD simulations were carried out on a local computing cluster featuring 192 CPU cores (processor model: Intel^® Xeon^® CPU E5-2690 manufactured by Intel Corporation headquartered in Santa Clara, California, USA). The post-processing of the results was performed using ANSYS Fluent and ParaView on a desktop PC, as well as by using COVISE (Collaborative Visualization and Simulation Environment) and a CAVE system available at the HLRS High Performance Computing Center Stuttgart, Germany.

7. Validation of Model Predictions

While not included in the process workflow diagram of Figure 2, any flow-field prediction should naturally be validated against experimental data. To this extent and as noted in Section 6.1, mean velocity values at the vent-in boundaries obtained as part of the network model analysis (and imposed as boundary conditions for the CFD analysis of the lecture hall) were checked by measuring the discharge velocities at selected jet and swirl nozzles and vent air grids using a Ø 3 mm hot ball (thermal) anemometer (manufacturer: Testo SE & Co. KGaA, Titisee-Neustadt, Germany) with a measuring range from 0 to 10 m/s flow velocity and an accuracy of ±0.03 m/s. In addition, predicted flow velocities were compared with measured values at singular positions in the jets discharging from the long-throw nozzles and at vent outlets, with errors ranging from 4 to 5% (see

Table 9. Comparison of calculated velocities (via 1D network model or 3D CFD analysis) with experimentally measured velocities at various positions.

S. No.	Location	Simulation [m/s]	Experiment	Percentage Error
1	Jet/Long-Throw Exit Nozzle C	8.58 (1D network)	8.06–8.3 m/s (±0.03 m/s + 5% of measured value)	4.89%
2	Jet/Long-Throw Nozzle B (measured 1.5 m below the nozzle outlet)	2.72 (3D CFD)	2.74–2.99 m/s (±0.03 m/s + 5% of measured value)	5.06%
3	Outlet 1 (right side of the lecture hall)	3.754 (3D CFD)	3.6–4.2 m/s (±0.03 m/s + 5% of measured value)	3.74%

in this context). Local measurements within the room were not conducted, as the measurements were taken without the presence of occupants. Also, measurements at swirl nozzles could not be performed as they were not safely accessible. Overall, a good agreement between numerical and experimental data was found at the sampled positions.

For a more comprehensive validation of the predicted flow field, laser-based methods like particle image velocimetry and/or laser doppler anemometry are preferred. While these methods are more accurate, their set-up and calibration is elaborate and tedious to execute in a timely manner in a public place. Hence, they have not been employed here. Another method to gage the accuracy of the numerical solution, or rather the predicted major flow patterns, is (a) smoke testing, i.e., the admission of tracers such as smoke or fog, possibly in conjunction with laser-sheet illumination or (b) the timed admission of gases to the vent air and their measurement at various selected positions over time, using suitable sensors.

8. Conclusions

Room ventilation is, aside from personal protection, essential to prevent the spread of any airborne pathogen in closed public spaces such as doctor’s offices, hallways, subways or lecture halls.

While increasing the ACH (air change per hour) is a good approach to decreasing harmful particle concentration in a ventilated room, it is well known that the aerodynamic flow-field pattern within a room, driven by the vent system flow rate (at inlets/outlets), buoyancy effects as consequence of temperature gradients and occupants’ positions (or movement) and their breathing behavior, can have a dominant effect on each individuals’ exposure risk for harmful pathogens released into or entering the room [54,55,56].

While there have been attempts to consider air flow effects by a single lumped parameter for design purposes [57], resolved CFD simulations are needed in order to accurately assess rooms’ air quality and potential exposure risks. Intermediate models, such as RTD (Residence Time Distribution) models [58], multizone air flow network models or, similarly, RN (Reactor Network) models known from gas-turbine design (which can be viewed as network models for a single room), can provide reliable information at a low computational expense, as long as changes in boundary conditions do not result in a change in the overall flow structure, bifurcating flow or bi-/multi-stable flow behavior. However, these models rely on simulations or experimental data to identify characteristic flow-field zones or network nodes.

The present study provides a detailed process workflow for the numerical analysis of a mechanically vented room and its connected vent system, with the emphasis on simulation efficiency. Actual data with regards to the execution/processing time of the various basic workflow tasks is provided for the case of a large lecture hall with a selected student seating arrangement and under normal breathing conditions.

For the considered test case, flow coupling between vent air flow and room aerodynamics did not occur. Steady turbulent flow conditions were assumed for the flow field within the room and modeled by the RANS equations, together with the original k-ε turbulence closure model by Launder and Spalding. Governing equations were solved using the pseudo-transient method in the commercial CFD solver ANSYS Fluent v19.1. Mesh refinement in areas where high-velocity gradients could be expected, and a mesh sensitivity study, resulted in a suitable mesh consisting of 85 million polyhedral cells. Given the low aerosol concentration in the air exhaled by the occupants, and the lack of vent air heating/cooling or heat transfer through walls or windows, a one-way coupled approach between the continuous and disperse phase and the general dominance of forced vs. natural convection could be assumed. Accordingly, the CFD analysis of the room aerodynamics was efficiently performed by a stepwise increasing of the complexity of the flow problem, i.e., (1) solution of mass and momentum conservation equations subject to the given boundary conditions, (2) additional solution of the conservation equations for turbulent quantities k and ε (not necessarily up to full convergence) and (3) additional solution of the energy equation to account for the rising of warm breathing air and thermal plumes generated by the occupants. These successive steps have been performed on a local computing cluster featuring 192 CPUs (Intel^® Xeon^® CPU E5-2690) for a total of 10,000 iterations or pseudo time steps, requiring five hours’ total wall clock time. The Lagrangian tracking of a total of 326,000 monodisperse aerosol particles (d = 0.5 $\mathsf{\mu }\mathrm{m}$) within the calculated turbulent flow field was performed on a local workstation. The results indicate that the vent system air flow entering the lecture hall is imbalanced and inefficiently used. The room aerodynamics is driven by strong, slightly downward-directed air jets discharged from four air grids in the front area of the room. Two of the four jets reach far across the lecture hall and interact with a series of downward-directed throw nozzles at the other end of the hall, driving an air current along the center isle back towards the front of the room and directed slightly upwards. A series of ten swirl nozzles accounts for approx. 28% of the air flow and is distributed across the center region of the room at the height of the air grids. Their positions are generally offset from the seating positions of the occupants below and generate locally downward air currents that support the upward-directed thermal body plumes of the occupants; such breathing aerosols initially rise fairly quickly after being exhaled by the occupants.

Twenty minutes after being released with the air exhaled by the occupants, 61% of the released aerosols are still within the room and mostly suspended in the room’s air. Only 39% have discharged with the vent-out air, while during the same time period the overall volume of air in the room has been changed 1.45 times.

For the considered open (flow-through) vent air system, building the network model accounted for about 3% of the overall process workflow, with a negligible amount of model run time. Control measurements of flow rates and of the basic room geometry, comparison with architectural drawings and CAD data generation using SOLIDWORKS^® 2018 took about 22% of the overall process workflow. Alternatively, performing room measurements with a laser scanning device and using an existing workflow and tools for point cloud processing was considerably more efficient and reduced that time down to 12%. Mesh generation and mesh quality checking accounted for a significant amount of the time, i.e., 40% (not including a mesh sensitivity study), and posed a bottleneck in the overall process workflow. While the mesh preparation step also included estimates for the spreading behavior of freely discharging jet and air streams originating from the vent system (thereby allowing for the selection of a suitable mesh), it shows that streamlining this process will greatly improve overall process turn-around times, provided that enough computational resources are available for the subsequent computing step, especially in the case of large computational meshes. In this context, the use of HPC and Cloud Computing services that also provide CFD software licenses can yield cost-effective and timely solutions. Using the computing cluster available at our institute, the CFD run time for room aerodynamics amounted to 9%, and calculating particle trajectories on a desktop PC to an additional 6%, of the total process time. Data post-processing in order to understand the flow aerodynamics and resulting aerosol concentration accounted for 10%, including both traditional desktop post-processing and post-processing in a VR (Cube) environment. In the latter case, data management and rendering are significantly more efficient if suitable tools for data importing and pre- and post-processing are available and if the user has been properly trained. In fact, developers of high-performing VR systems frequently employ more powerful tools than those used for “traditional” desktop CFD post-processing (e.g., with respect to the cache and buffer optimization). In addition, VR processing allows for the evaluation of features that are not readily accessible otherwise, such as visibility across the room if dividers are placed for the purpose of improving a room’s aerodynamics, for example.

From an engineering perspective, the effective numerical analysis of room aerodynamics and its connected vent flow system requires a careful evaluation/determination of the dominant flow physics, flow coupling and initial mesh generation based on estimates of the expected overall aerodynamics and specifically the extent of forced air streams/jets (and their shear layers) discharged from the vent system. Flow-field meshing retains the largest potential for reducing the overall workflow process time, if sufficient computing resources are available for the problem at hand.