Numerical modeling and optimization of an air handling unit

energies Article Numerical Modeling and Optimization of an Air Handling Unit JoséLopes 1, João Silva 1,2,* , Senhorinha Teixeira 2and JoséTeixeira 1   Citation: Lopes, J.; Silva, J.; Teixeira, S.; Teixeira, J. Numerical Modeling and Optimization of an Air Handling Unit. Energies 2021,14, 68. https:// dx.doi.org/10.3390/en14010068 Received: 21 November 2020 Accepted: 18 December 2020 Published: 25 December 2020 Publisher’s Note: MDPI stays neutral with regard to jurisdictional claims in published maps and institutional affiliations. Copyright: © 2020 by the authors. Licensee MDPI, Basel, Switzerland. This article is an open access article distributed under the terms and conditions of the Creative Commons Attribution (CC BY) license (https://creativecommons.org/ licenses/by/4.0/). 1MEtRICs Research Centre, University of Minho, 4800-058 Guimarães, Portugal; [email protected] (J.L.); [email protected] (J.T.) 2ALGORITMI Research Centre, University of Minho, 4800-058 Guimarães, Portugal; [email protected] *Correspondence: [email protected] Abstract: Concerns about the efficiency of Heating, Ventilating, and Air Conditioning systems, including Air Handling Units (AHUs), started in the last century due to the energy crisis. Thenceforth, important improvements on the AHUs performance have emerged. Among the various improvements, the control of the AHUs and the redesign of the fans are the most important ones. Although, with increasingly demanding energy efficiency requirements, other constructive solutions must be investigated. Therefore, the objective of this work is to investigate, using a computational fluid dynamics (CFD) tool, the fluid flow inside an AHU and to analyze different constructive solutions in order to improve the AHU performance. The numerical model provided a reasonable agreement with the experimental results in terms of air flow rate, despite the assumed simplifications. Regarding the constructive solution concept, the CFD results for the two different flow control units (FCUs) showed improvements in terms of fan static pressure rise. Under real conditions, improvements of 15.1% when compared with the case without the FCU were obtained. Nevertheless, it was concluded that the axial component of the air velocity, at the fan exit, can have a determinant impact on the FCU viability. Finally, an improved FCU geometry, with a new body shape, which resulted in an additional improvement of 6.1% in the fan static pressure rise. Keywords: air handling unit; computational fluid dynamics; flow control unit; modeling 1. Introduction About 90% of a person’s day is spent inside closed spaces, so, it is necessary systems that guarantee the buildings breathe and healthy and safe conditions to the people who live inside them, who study or work there. This need has grown and, coupled with environment concerns with increasing energy consumption there are stringent requirements for energy consumption in buildings. In fact, HVAC systems are responsible for approximately 40% of the total energy consumed in buildings, according to the Heating, Ventilation, and Air-Conditioning High-Efficiency Systems Strategy (HVAC HESS) working group. In a factsheet published by the HVAC HESS working group in 2013, it is shown that the air circulation is the most demanding process in an HVAC system, representing 34% of the total energy consumption of a typical HVAC system. Thus, manufacturers of air treatment and conditioning equipment have been investing in finding more eco-friendly and efficient solutions. As one of the HVAC components, the air handling units (AHU) are a major source of energy consumption [1]. An AHU also called an air handler, is a part of an HVAC system that handles and conditions certain air flows. This equipment allows creating the necessary conditions for the good health of any building and the people who use it. In other words, AHU conditions and treats certain air flows to ensure the desired conditions. For this, this unit allows combining of air circulation, filtration, heating, cooling, humidification, dehumidification, energy recovery between flows, among other features [ 1 ]. Generally, AHUs are connected to air ducts, through which conditioned and treated air is distributed, as well as the return air. These units can be used in all general ventilation systems where it Energies 2021,14, 68. https://dx.doi.org/10.3390/en14010068 https://www.mdpi.com/journal/energies Energies 2021,14, 68 2 of 16 is required to provide adequate indoor air quality, reduce internal heat loads, temperature and humidity control, or particle concentration control [1]. Relatively to the air circulation process in an AHU, fan manufactures have been working on different ways to improve overall efficiency in their products. This century, the efficiency improvements obtained in fans were, mostly, in their controlling systems. Besides that, the redesign of the fans using bionic science allowed them to achieve more efficient turbomachines. Particularly in the redesign process, the importance of computational tools for fluid dynamics analysis has increased. These have been used more and more at an initial or even final stage of project development, as a complement to experimental tests. For instance, Chunxi et al. [ 2 ], Rong et al. [ 3 ], Madhwesh et al. [ 4 ], and Shen et al. [ 5 ] are examples of numerical investigations to study the influence of some design details and to optimize a specific centrifugal fan. This is an important aspect since an improper configuration of the flow produces increased flow resistance and higher power consumption by the exhaust fan will be necessary [ 6 ]. Although, the air circulation effectiveness in an AHU is not just dependent on the fan static efficiency but also on the manner that the air flow is conducted through the AHU. As increasing fan efficiency will become gradually difficult to achieve, it is necessary to think of solutions that potentially can improve the air conducting the process in an AHU [ 7 – 9 ]. However, studies on the literature regarding this issue are very limited. In the 90 0 s, Nilsson [ 10 ] made a study in HVAC systems regarding their performance in terms of specific fan power. At that time, with good design practices and life-cycle cost optimization, the specific fan power for each fan should be between 0.5 and 1 kW m−3s−1 . Using data from nearly 1000 audited fans used in HVAC systems, including AHUs, in Sweden, an average measured value of 1.5 kW m −3 s −1 was obtained. Apparently, this scenario was found in other countries too. Nowadays, in the more demanding projects in terms of energy efficiency requirements, the requested specific fan power for an AHU, for instance, can reach 0.1 kW m −3 s −1 . By analyzing the contract forms used by Swedish builders and consultants’ design practices, the two most important causes were identified. First, the lack of energy performance specifications by the builders due to the nonexistence of economic incentives and knowledge. Then, the builder has a first-cost minimization incentive, which combined with the first cause ends with the installation of HVAC systems with low initial cost rather than systems with an optimized life-cycle cost. In order to assist further investigations in AHUs control, operation, fault detection, and diagnosis, Li and Wen [ 11 ] developed a dynamic AHU simulation model. Being capable of creating operational data for the most common AHUs configurations at that time, the proposed model was developed using HVACSIM+ software. This model, based on two previous ASHRAE projects, was applied to an AHU and four building zones that were served by the AHU. After the determination of the key parameters directly from experimental data, a good agreement between the experimental and simulation results was obtained. Schito [ 9 ] performed a dynamic simulation of an AHU installed in a museum. By building a routine as a MATLAB script linked to a TRNSYS model, the behavior of the components was reproduced using the suitable ε -NTU relations. By comparing the results between the model and the experimental data from one month of monitoring at the exhibition room, the model is considered validated. Azem et al. [ 12 ] studied a centrifugal fan mounted inside of an AHU is through on-site measurements and CFD simulations. In order to decrease the turbulence levels downstream of the centrifugal fan, a cuboid-shaped body is installed at the exit zone of the centrifugal fan. With this solution, most of the conduct area is covered, leaving only a small channel for the air at the near zone of the conduct walls to pass. The use of this geometry allowed to increase the fan efficiency by reducing the vorticity downstream of the fan, transferring a substantial part of the kinetic energy into pressure energy. The CFD simulations are performed using ANSYS CFX software, with a hybrid numerical grid and a simplified free running centrifugal fan model. By comparing both cases (empty duct Energies 2021,14, 68 3 of 16 and with the cuboid-shaped body), an improvement of 5.06% was obtained in terms of maximum static pressure difference. It is from the need of solutions to improve the air conducting the process in an AHU that arises the motivation for the present work. Thus, the aim of this study is to study the air flow behavior inside an AHU manufactured by a national company designed to circulate an air flow between 3700 and 5800 m 3 /h. For this purpose, a numerical model using the ANSYS Fluent software was developed. Furthermore, to improve the performance of the AHU, an analysis of other constructive solutions are evaluated to decrease the pressure drop in future products and, consequently, decrease their specific fan power. 2. Air Handling Unit 2.1. Description of the Air Handling Unit The AHU in analysis provides clean air to a gymnasium in Braga, Portugal. The main dimensions of the AHU in the study are 4398 mm × 1135 mm × 1660 mm, and it weighs 834 kg. This machine is a double-deck type with partial recirculation of the air, due to the heat wheel and the mixing box that possesses, respectively. For this project, an air flow of 3850 m 3 /h both in insufflation and extraction was required, to handle the air inside of the corresponding space. The AHU presented is equipped with a heat wheel, water heating, and cooling coils, mixing box, filters, fans, dampers, and a condensed tray. This is a very standard layout for a common AHU. Beyond the mentioned equipment, the AHU has panels, doors, top coverings, chassis, among others. Figure 1shows the AHU under analysis. Energies 2021, 14, x FOR PEER REVIEW 3 of 17 simulations are performed using ANSYS CFX software, with a hybrid numerical grid and a simplified free running centrifugal fan model. By comparing both cases (empty duct and with the cuboid-shaped body), an improvement of 5.06% was obtained in terms of maximum static pressure difference. It is from the need of solutions to improve the air conducting the process in an AHU that arises the motivation for the present work. Thus, the aim of this study is to study the air flow behavior inside an AHU manufactured by a national company designed to circulate an air flow between 3700 and 5800 m 3 /h. For this purpose, a numerical model using the ANSYS Fluent software was developed. Furthermore, to improve the performance of the AHU, an analysis of other constructive solutions are evaluated to decrease the pressure drop in future products and, consequently, decrease their specific fan power. 2. Air Handling Unit 2.1. Description of the Air Handling Unit The AHU in analysis provides clean air to a gymnasium in Braga, Portugal. The main dimensions of the AHU in the study are 4398 mm × 1135 mm × 1660 mm, and it weighs 834 kg. This machine is a double-deck type with partial recirculation of the air, due to the heat wheel and the mixing box that possesses, respectively. For this project, an air flow of 3850 m 3 /h both in insufflation and extraction was required, to handle the air inside of the corresponding space. The AHU presented is equipped with a heat wheel, water heating, and cooling coils, mixing box, filters, fans, dampers, and a condensed tray. This is a very standard layout for a common AHU. Beyond the mentioned equipment, the AHU has panels, doors, top coverings, chassis, among others. Figure 1 shows the AHU under analysis. Figure 1. AHU under analysis and their respective components. The AHU has two centrifugal fans, one in the supply deck and the other in the exhaust deck. These are dimensioned and selected considering the pressure drop of the components, from each deck, and the installation system pressure drop. Given by the manufacturers, the pressure drops associated with the upper and lower part of the AHU are 549 Pa and 306 Pa, respectively. Along with these, the pressure drop of the supply and exhaust installations are presented. Based on the pressure drop values, the point of operation for each fan was estimated. Table 1 presents the nominal operating conditions of the two centrifugal fans. Table 1. Nominal operating conditions of the centrifugal fans. Parameter Supply Fan Exhaust Fan Air volume flow rate (m 3 /h) 3850 3850 Pressure rise (Pa) 729 308 Figure 1. AHU under analysis and their respective components. The AHU has two centrifugal fans, one in the supply deck and the other in the exhaust deck. These are dimensioned and selected considering the pressure drop of the components, from each deck, and the installation system pressure drop. Given by the manufacturers, the pressure drops associated with the upper and lower part of the AHU are 549 Pa and 306 Pa, respectively. Along with these, the pressure drop of the supply and exhaust installations are presented. Based on the pressure drop values, the point of operation for each fan was estimated. Table 1presents the nominal operating conditions of the two centrifugal fans. 2.2. On-Site Measurements In order to obtain data for the numerical simulations and to validate the CFD model, experimental measurements were made on site. It was important to make measurements of the relative pressure in different points of the AHU and the air volume flow rate in circulation. The pressure measurements in the AHU were made, typically, from pressure tips placed in different parts of the machine. The pressure tips located in filters play an important role in the overall maintenance of the AHUs. By measure the filter’s pressure Energies 2021,14, 68 4 of 16 drop, it is possible to estimate their real level of dirtiness. The dirtier the filter is, the higher is the corresponding pressure drop. When a filter is becoming dirty throughout the machine operation, the fan working point changes. Due to the increase of pressure drop, the fan angular velocity also increases to overcome the extra pressure drop. This way, the energy costs due to ventilation increase. Table 1. Nominal operating conditions of the centrifugal fans. Parameter Supply Fan Exhaust Fan Air volume flow rate (m3/h) 3850 3850 Pressure rise (Pa) 729 308 Fan static efficiency (%) 61 50.6 Working angular velocity (rpm) 2342 1941 Nominal angular velocity (rpm) 2600 2140 Electrical power input (kW) 1.28 0.65 Nominal electric power input (kW) 1.7 1 In this way, to measure the values of relative and differential pressure in the different places, a multifunction measuring instrument, the testo 435-4 (accuracy ± 0.02 Pa) was used. This equipment is an air conditioning measurement instrument with a differential pressure gauge integrated. In each measurement test, five measurements were made in order to consider the instrument reproducibility since repeating the measurements, the uncertainty caused by random errors can be determined. Accordingly, to the American Society of Mechanical Engineers guidelines for test uncertainty in instruments, it is recommended that the results are presented with uncertainty for a 95% confidence interval. Therefore, an expanded uncertainty should be calculated through the multiplication of the standard deviation of the mean by an expansion factor (based on a t-student distribution for 95%). More details about the methodology can be found in [ 13 ]. In this sense, Table 2presents the average results complemented with the experimental data uncertainty. Table 2. Results of the experiments with an uncertainty for 95% confidence interval. Local Pressure (Pa) Fan inlet −212.40 ±1.42 Fan outlet −1143.80 ±8.80 Bag filter inlet 238.60 ±7.83 Bag filter outlet 78.40 ±3.68 Measurements at the fan outlet were not possible. However, being the distance between the supply fan and the bag filter entry about 434 mm, it is reasonable to approximate the pressure at the fan outlet to the bag filter inlet pressure. Thus, to compare with the fan technical data from the AHU in the study, the static pressure difference between the fan inlet and the bag filter inlet is considered as the fan static pressure increase. Furthermore, based on these measurements, the air flow rate can be estimated by Equation (1): Q=k×p∆p(1) where ∆ p, is the differential pressure, Qis the air volume flow rate worked by the fan and kis a factor that considers the specific properties of the inlet ring of the corresponding fan. Depending on the fan reference, the manufacturers assign different kvalues for each turbomachine. Thus, the instant air volume flow rate supplied by the fan can be calculated. In Table 3, the fan operating conditions from the AHU from the on-site measurements are presented. Energies 2021,14, 68 5 of 16 Table 3. Real operating conditions of the supply fan. Parameter Value Air volume flow rate (m3/h) 4534 Pressure rise (Pa) 451 Fan static efficiency (%) 55 Working angular velocity (rpm) 2227 Electrical power input (kW) 1.03 It is possible to verify that, the supply fan is not working under project conditions. There are some reasons that can explain this, as changes in the air flow demand, differences between the project installation layout and the installed layout, or differences between the filters pressure drop during the AHU selection and their real pressure drop in the measurements. In this way, as the fan is working further from its nominal working point, the static efficiency is lower when compared with project conditions. Table 3. shows the operating conditions of the supply fan. 3. Numerical Model 3.1. Mathematical Model and Fan Modeling The air flow inside the AHU was assumed to be incompressible and turbulent. Although the flow is steady, due to numerical convergence issues the unsteady solution was performed. The unsteady Reynolds-averaged Navier-Stokes governing equations, averaged in a time interval together with the transient term, are applied in the numerical calculation performed by the CFD software (ANSYS Fluent v16.2). Since the flow through the filters passes through a porous media, a source term represented by the term S is added to the momentum equation. Regarding the turbulent field, the realizable k-ε and RNG (Re-Normalization Group) model were considered as both of the models have shown satisfactory results when it comes to flows that include strong streamline curvatures, vortices, and rotation [ 14 ]. By doing a preliminary CFD simulation with these two models and comparing their results with the experimental data, it is concluded that the realizable model allows to achieve better results under the conditions of the study. Furthermore, the full buoyancy effects option is enabled to account for the air dynamic of going from lower pressure zones to higher pressure zones. Therefore, the realizable kε with a standard wall function is selected because this model is capable to take into account the effects of mean rotation in the turbulent viscosity [ 14 ]. The description of these models is presented in detail in the ANSYS Fluent User’s guide [14]. The governing equations were discretized using the Finite Volume Method using a second-order upwind spatial discretization. The computational models were solved using a transient formulation, as in terms of prediction of turbulent flows and swirl phenomena allow better results than steady-state simulations, based on a first-order implicit method and the convergence criterion of 1 × 10 −3 for continuity and 1 × 10 −4 for energy, momentum, and turbulence equations. The pressure-velocity coupling is solved with the Semi-Implicit Method for Pressure Linked Equations (SIMPLE) algorithm, using the standard initialization. The SIMPLE algorithm provides more efficient and robust singlephase flows. The pressure is modeled with a pressure staggering option (PRESTO scheme). The contribution of the gravity acceleration was implemented in a downwards direction. The simulation of this project was computed in the 12-core processor, with approximately 32 GB of memory RAM required. The simulation time condition was considered unsteady to predict all the movement of gas inside the AHU and the bag filter. The time step size was automatically calculated by the solver upon the previous time step calculation. This algorithm considers the value of the Courant number for the fluid, deciding the next time step size for the simulation. Subsequently, the results are time-averaged after the simulation reaches a pseudo steady-state by means of a long transient simulation. In all cases, 6 s were enough for the simulation time as after this time the results are stable, varying less than 1%. Energies 2021,14, 68 6 of 16 Regarding the air flow inside the AHU process where the air is induced by a fan, CFD application, generally, takes one of three approaches to model the turbomachine: Fan Boundary Conditions (FBC) [ 12 ], the Moving Reference Frame (MRF) model [ 2 , 5 ], and the Sliding Mesh model [4]. The FBC model is also referred to as the body force model (BFM) in investigation works. The FBC model is used to determine the fan impact, with certain characteristics, in a flow field. In this case, the fan geometry is not considered, instead, the operating fan curve is introduced in the software. This empirical curve represents the relationship between the fan static pressure rise and the air velocity at the fan inlet, under certain operating conditions. Concerning the second approach, the MRF model, these are steadystate approximations used in problems involving moving parts, such as rotating blades, impellers, and other types of moving parts. Unlike the FBC, MRF models take into account the geometry of the rotating or moving part under analysis. Finally, instead of all the previously presented models, the Sliding Mesh model is an unsteady approach where the transient interactions between the stationary and moving components are accounted for. When modeling turbomachines components, where the interaction between rotor and stator is important, this approach must be used to compute the unsteady flow field. Being the most accurate model for simulating flows in multiple moving reference frames, this is also the one that requires the most computational effort [14]. In this work, the FBC model is used to simulate the air induced by the fan inside the AHU. As mentioned previously, one of the key inputs in this approach is the fan curve equation. To obtain the fan curve equation the similarity between fans is used. The fan manufacturer provides the datasheet from the fan, including several working points at different angular velocities. Using the provided nominal data of the fan, a tendency curve at the real operating conditions is generated. In this way, the real fan working curve, based on the experimental measurements, is presented in Figure 2. It shows the pressure increase as function of the inlet velocity at real operating conditions. Energies 2021, 14, x FOR PEER REVIEW 6 of 17 Subsequently, the results are time-averaged after the simulation reaches a pseudo steady-state by means of a long transient simulation. In all cases, 6 s were enough for the simulation time as after this time the results are stable, varying less than 1%. Regarding the air flow inside the AHU process where the air is induced by a fan, CFD application, generally, takes one of three approaches to model the turbomachine: Fan Boundary Conditions (FBC) [12], the Moving Reference Frame (MRF) model [2,5], and the Sliding Mesh model [4]. The FBC model is also referred to as the body force model (BFM) in investigation works. The FBC model is used to determine the fan impact, with certain characteristics, in a flow field. In this case, the fan geometry is not considered, instead, the operating fan curve is introduced in the software. This empirical curve represents the relationship between the fan static pressure rise and the air velocity at the fan inlet, under certain operating conditions. Concerning the second approach, the MRF model, these are steady-state approximations used in problems involving moving parts, such as rotating blades, impellers, and other types of moving parts. Unlike the FBC, MRF models take into account the geometry of the rotating or moving part under analysis. Finally, instead of all the previously presented models, the Sliding Mesh model is an unsteady approach where the transient interactions between the stationary and moving components are accounted for. When modeling turbomachines components, where the interaction between rotor and stator is important, this approach must be used to compute the unsteady flow field. Being the most accurate model for simulating flows in multiple moving reference frames, this is also the one that requires the most computational effort [14]. In this work, the FBC model is used to simulate the air induced by the fan inside the AHU. As mentioned previously, one of the key inputs in this approach is the fan curve equation. To obtain the fan curve equation the similarity between fans is used. The fan manufacturer provides the datasheet from the fan, including several working points at different angular velocities. Using the provided nominal data of the fan, a tendency curve at the real operating conditions is generated. In this way, the real fan working curve, based on the experimental measurements, is presented in Figure 2. It shows the pressure increase as function of the inlet velocity at real operating conditions. Figure 2. Pressure increase as function of the inlet velocity at real operating conditions. As represented in Figure 2, the tendency curve obtained is a fourth-degree polynomial, being the correlation coefficient near unity. Therefore, this curve is used in fan modeling. ANSYS Fluent software calculates the entry velocity at the fan zone, being this value used as an input in the polynomial equation. The pressure increase value is then obtained, and the static pressure values of the adjacent elements to the fan surface are calculated. In this case, a single pressure increase value is determined for the adjacent elements because the option calculates pressure-jump from average conditions is enable [14]. The massFigure 2. Pressure increase as function of the inlet velocity at real operating conditions. As represented in Figure 2, the tendency curve obtained is a fourth-degree polynomial, being the correlation coefficient near unity. Therefore, this curve is used in fan modeling. ANSYS Fluent software calculates the entry velocity at the fan zone, being this value used as an input in the polynomial equation. The pressure increase value is then obtained, and the static pressure values of the adjacent elements to the fan surface are calculated. In this case, a single pressure increase value is determined for the adjacent elements because the option calculates pressure-jump from average conditions is enable [ 14 ]. The massaveraged velocity normal to the fan is determined, and the single pressure-jump value is estimated [14]. The other required inputs for the application of the FBC model were the tangential and radial velocity which were considered as 29.5 and 10.1 m/s, respectively. It is important to Energies 2021,14, 68 7 of 16 note that to reach the values of tangential and radial velocity a real blade angle had to be considered. In this case, a real blade angle of 25◦was considered. The bigger disadvantage of this fan modeling approach is the fact that air flow at the fan outlet is purely radial and tangential. It gains even more important as the exit blade angle of the fan is bigger. Using the FBC model, it is not considering the axial velocity component at the fan outlet. Thus, in the CFD simulations that are presented in the next sections, all the conclusions taken presuppose this limitation. 3.2. Computational Domain, Mesh and Boundary Conditions The AHU module in the study is only the supply deck (upper part of Figure 1) and it can be divided into four sections: fan inlet, fan outlet, bag filter, and AHU exit. The fan inlet section is defined according to the real distance between the water heating coil, the upstream component of the fan, and the fan inlet zone. The other sections respect the real dimensions of the AHU module, being the AHU exit the zone between the bag filter outlet and the installation conducts. Between the fan inlet and the fan outlet sections is the supply fan, which modeling strategy and considerations are mentioned in the previous section. Furthermore, it is important to note that the considered geometry is defined according to the type of mesh pretended for this case. To improve the stability of the overall simulation process, a structured mesh it is adopted. In this way, in terms of casing constitution, the protrusions from the rails, rivets, and other components are not considered. Thus, each surface respective to all sections is totally flat, being compared to empty sheet metal boxes. The pressure tips, at the top of the fan and bag filter sections, are also not considered. Regarding the fan modeling, this is modeled as a simple disk. This comes because of the fan modeling approach used, where the real geometry of the fan is not needed. Thus, the diameter of the disk is equal to the real impeller diameter, as well as its depth. Furthermore, the fan volute, which is of conic nature, is modeled as a cylinder due to mesh issues. Finally, the fan electric motor is not considered or modeled due to its minor influence on the flow pattern. Moving into the bag filter modeling, this is assumed as a regular box where geometric details are not modeled. This simplification is possible due to the ability of ANSYS Fluent software of defining a pressure drop in a body, over a certain direction, in the function of its length. Taking into account these considerations, Figure 3a presents the geometry considered for the CFD simulations with the indication of the boundary conditions. The yellow line presented in Figure 3a, which crosses the whole system, is represented since a curve of the static pressure evolution over the system length will be carried out to better interpretation and comparison of the different CFD results. Figure 3b shows the mesh used in the study. Energies 2021, 14, x FOR PEER REVIEW 8 of 17 (a) (b) Figure 3. Representation of the: (a) AHU geometry and (b) mesh used in the simulation. The strategies assumed in the geometric modeling are based on the need of building a structured mesh. In this sense, to better control the structured mesh features, some splits over the geometric model were performed. An isometric perspective of the mesh obtained is presented in Figure 3b). Mesh refinements were performed in specific zones where there are high gradients of velocity or pressure. Thus, higher mesh resolutions in the regions with higher gradients allow defining better transition zones. In terms of mesh quality evaluation, there are some crucial mesh parameters commonly used in the literature, as orthogonality, skewness, and aspect ratio. These parameters were evaluated, and it was possible to conclude that the mesh is in lined with all the main quality parameters regularly used in the literature. After this analysis, a mesh dependency study was carried out. This study allows for the assessment of the dependency of the CFD results in the mesh resolution (number of elements), without changing the mesh quality standards. Four different meshes were developed and preliminary simulations were done and at the end of the simulation, the air flow rate was computed. Figure 4 presents the results, and it is possible to see that the maximum difference between the air flow rate is less than 1%. Furthermore, the air flow rate stabilizes, approximately, at 3971 m 3 /h and, therefore, to reduce the computation time and effort, only 560,784 hexahedral elements are necessary. Figure 4. Mesh dependency study. Figure 3. Representation of the: (a) AHU geometry and (b) mesh used in the simulation. Energies 2021,14, 68 8 of 16 The strategies assumed in the geometric modeling are based on the need of building a structured mesh. In this sense, to better control the structured mesh features, some splits over the geometric model were performed. An isometric perspective of the mesh obtained is presented in Figure 3b). Mesh refinements were performed in specific zones where there are high gradients of velocity or pressure. Thus, higher mesh resolutions in the regions with higher gradients allow defining better transition zones. In terms of mesh quality evaluation, there are some crucial mesh parameters commonly used in the literature, as orthogonality, skewness, and aspect ratio. These parameters were evaluated, and it was possible to conclude that the mesh is in lined with all the main quality parameters regularly used in the literature. After this analysis, a mesh dependency study was carried out. This study allows for the assessment of the dependency of the CFD results in the mesh resolution (number of elements), without changing the mesh quality standards. Four different meshes were developed and preliminary simulations were done and at the end of the simulation, the air flow rate was computed. Figure 4presents the results, and it is possible to see that the maximum difference between the air flow rate is less than 1%. Furthermore, the air flow rate stabilizes, approximately, at 3971 m 3 /h and, therefore, to reduce the computation time and effort, only 560,784 hexahedral elements are necessary. Energies 2021, 14, x FOR PEER REVIEW 8 of 17 (a) (b) Figure 3. Representation of the: (a) AHU geometry and (b) mesh used in the simulation. The strategies assumed in the geometric modeling are based on the need of building a structured mesh. In this sense, to better control the structured mesh features, some splits over the geometric model were performed. An isometric perspective of the mesh obtained is presented in Figure 3b). Mesh refinements were performed in specific zones where there are high gradients of velocity or pressure. Thus, higher mesh resolutions in the regions with higher gradients allow defining better transition zones. In terms of mesh quality evaluation, there are some crucial mesh parameters commonly used in the literature, as orthogonality, skewness, and aspect ratio. These parameters were evaluated, and it was possible to conclude that the mesh is in lined with all the main quality parameters regularly used in the literature. After this analysis, a mesh dependency study was carried out. This study allows for the assessment of the dependency of the CFD results in the mesh resolution (number of elements), without changing the mesh quality standards. Four different meshes were developed and preliminary simulations were done and at the end of the simulation, the air flow rate was computed. Figure 4 presents the results, and it is possible to see that the maximum difference between the air flow rate is less than 1%. Furthermore, the air flow rate stabilizes, approximately, at 3971 m 3 /h and, therefore, to reduce the computation time and effort, only 560,784 hexahedral elements are necessary. Figure 4. Mesh dependency study. Figure 4. Mesh dependency study. Another important aspect concerning the mesh resolution, the y + value was considered during the mesh execution. In this regard, the fact that the flow pattern in the analysis is dominated by swirl, the need for high resolution meshes is lower and this was taken into account. Consequently, the turbulence stresses are dominant relative to the Reynolds shear stresses (the y + can be higher than 30 to capture the fully turbulent layer which is where turbulent stress dominates the flow). Thus, with the mesh resolution considered, the values of wall y+ are higher than 30 in all wall zones, and, consequently, a standard wall function was used to accurately predict the flow in the boundary layer. In terms of boundary conditions, its values were defined considering the experimental measurements (Table 4). A pressure inlet and outlet were defined at the inlet and outlet, respectively. Table 4 also presents the condition defined for the fan and bag filter wall. Furthermore, the bag filter region was modeled as a box, by defining a pressure drop in the function of its length, in the direction of the air flow (zdirection). Considering the pressure drop obtained on-site measurements, a source term in the Z Momentum equation is defined as 413.2 N/m3. Energies 2021,14, 68 9 of 16 Table 4. Boundary conditions defined in the numerical model. Location Boundary Condition Parameter Value Inlet Pressure inlet Gauge total pressure (Pa) −212 Turbulent intensity (%) 3.8 Hydraulic diameter (mm) 814.9 Outlet Pressure outlet Gauge pressure (Pa) 78 Back flow turbulent intensity (%) 3 Hydraulic diameter (mm) 814.9 Fan wall Wall Stationary wall—no slip - Bag filter frame Wall Stationary wall—no slip - 4. Results and Discussion 4.1. Validation of the Numerical Model to Nominal Operating Conditions To analyze the accuracy of the FBC model, the CFD simulation was developed from the data provided by the on-site measurements. By defining a longitudinal plane, xz plane, located at medium height, it is possible to observe the static pressure and velocity contours, as represented in Figures 5and 6, respectively. Energies 2021, 14, x FOR PEER REVIEW 9 of 17 Another important aspect concerning the mesh resolution, the y + value was considered during the mesh execution. In this regard, the fact that the flow pattern in the analysis is dominated by swirl, the need for high resolution meshes is lower and this was taken into account. Consequently, the turbulence stresses are dominant relative to the Reynolds shear stresses (the y + can be higher than 30 to capture the fully turbulent layer which is where turbulent stress dominates the flow). Thus, with the mesh resolution considered, the values of wall y+ are higher than 30 in all wall zones, and, consequently, a standard wall function was used to accurately predict the flow in the boundary layer. In terms of boundary conditions, its values were defined considering the experimental measurements (Table 4). Table 4. Boundary conditions defined in the numerical model. Location Boundary Condition Parameter Value Inlet Pressure inlet Gauge total pressure (Pa) −212 Turbulent intensity (%) 3.8 Hydraulic diameter (mm) 814.9 Outlet Pressure outlet Gauge pressure (Pa) 78 Back flow turbulent intensity (%) 3 Hydraulic diameter (mm) 814.9 Fan wall Wall Stationary wall—no slip - Bag filter frame Wall Stationary wall—no slip - A pressure inlet and outlet were defined at the inlet and outlet, respectively. Table 4 also presents the condition defined for the fan and bag filter wall. Furthermore, the bag filter region was modeled as a box, by defining a pressure drop in the function of its length, in the direction of the air flow (z direction). Considering the pressure drop obtained on-site measurements, a source term in the Z Momentum equation is defined as 413.2 N/m3. 4. Results and Discussion 4.1. Validation of the Numerical Model to Nominal Operating Conditions To analyze the accuracy of the FBC model, the CFD simulation was developed from the data provided by the on-site measurements. By defining a longitudinal plane, xz plane, located at medium height, it is possible to observe the static pressure and velocity contours, as represented in Figures 5 and 6, respectively. Figure 5. Static pressure contour at medium height of the AHU. Figure 5. Static pressure contour at medium height of the AHU. The static pressure in the fan volute reaches very low values. In this zone, the dynamic pressure component is also important due to the high passing air velocity. In terms of static pressure field calculated, it is seen, as mentioned previously, that an average value of static pressure is set in the fan zone boundary. Furthermore, it is understood that the fact that the air flow at the outlet is purely radial and tangential, makes that the zones with higher static pressures are located at the near-wall zones. This phenomenon creates “death zones” where the static pressure levels are lower, and around where swirl formation takes place. Finally, the pressure drops defined for the bag filter over zdirection, in the function of its length, can also be observed in Figure 5. Figure 6shows the velocity field inside the AHU: (a) velocity contour and velocity vectors at medium height and (b) velocity streamlines inside the AHU. Energies 2021,14, 68 16 of 16 decreasing of the pressure drop at the fan exit. Although, experimental tests need to take place to clearly see the reaction of the centrifugal fan to the mounting of an FCU. Author Contributions: Conceptualization, J.L.; J.S.; J.T.; methodology, J.L.; J.S.; J.T.; investigation, J.L.; J.S.; writing—original draft preparation, J.L.; J.S.; J.T.; S.T.; writing—review and editing, J.L.; J.S.; J.T.; S.T.; supervision, J.T.; S.T. All authors have read and agreed to the published version of the manuscript. Funding: This work was supported by Portuguese Foundation for Science and Technology (FCT) within the R&D Units Project Scope UIDB/00319/2020 (ALGORITMI) and R&D Units Project Scope UIDP/04077/2020 (MEtRICs). Acknowledgments: The second author would like to express his gratitude for the support given by FCT through the Grant SFRH/BD/130588/2017. Conflicts of Interest: The authors declare no conflict of interest. Nomenclature kfactor for each turbomachine, - ppressure, Pa QAir flow rate, m3/s References 1. Shahsavar Goldanlou, A.; Kalbasi, R.; Afrand, M. Energy usage reduction in an air handling unit by incorporating two heat recovery units. J. Build. Eng. 2020,32, 101545. [CrossRef] 2. Chunxi, L.; Ling, W.S.; Yakui, J. The performance of a centrifugal fan with enlarged impeller. Energy Convers. Manag. 2011 , 52, 2902–2910. [CrossRef] 3. Rong, R.; Cui, K.; Li, Z.; Wu, Z. Numerical Study of Centrifugal Fan with Slots in Blade Surface. Procedia Eng. 2015 ,126, 588–591. [CrossRef] 4. Vasudeva Karanth, N.M.K.; Yagnesh Sharma, N. Effect of innovative circular shroud fences on a centrifugal fan for augmented performance—A numerical analysis. J. Mech. Sci. Technol. 2018,32, 185–197. 5. Shen, Y.; Li, Y.; Wang, H.; Shen, W.; Chen, Y.; Si, H. Numerical simulation and performance optimization of the centrifugal fan in a vacuum cleaner. Mod. Phys. Lett. B 2019,33, 1950440. [CrossRef] 6. Bleier, F.P. Fan Handbook: Selection, Application, and Design; McGraw Hill Higher Education: New York, NY, USA, 1998. 7. Bozkaya, B.; Zeiler, W. The energy efficient use of an air handling unit for balancing an aquifer thermal energy storage system. Renew. Energy 2020,146, 1932–1942. [CrossRef] 8. Yun, G.Y. Influences of perceived control on thermal comfort and energy use in buildings. Energy Build. 2018 ,158, 822–830. [CrossRef] 9. Schito, E. Dynamic simulation of an air handling unit and validation through monitoring data. Energy Procedia 2018 ,148, 1206–1213. [CrossRef] 10. Nilsson, L.J. Air-handling energy efficiency and design practices. Energy Build. 1995,22, 1–13. [CrossRef] 11. Li, S.; Wen, J. Development and Validation of a Dynamic Air Handling Unit Model, Part I; ASHRAE Transactions United States of America: Atlanta, GA, USA, 2010; Volume 116. 12. Azem, A.; Mathis, P.; Stute, F.; Hoffmann, M.; Müller, D.; Hetzel, G. Efficiency increase of free running centrifugal fans through a pressure regain unit used in an air handling unit. Energy Build. 2018,165, 321–327. [CrossRef] 13. ASME. Test Uncertainty PTC 19.1—2018(R2018); ASME: New York, NY, USA, 1998. 14. ANSYS. ANSYS FLUENT Theory Guide; ANSYS: Canonsburg, PA, USA, 2013.