CFD Investigation on the Thermal Comfort for an Office Room

Abstract

Heating, Ventilating, and Air Conditioning (HVAC) systems are important and essential for use in our daily comfort, either in homes, work, or transportation. And it is crucial to study the air movement coming from the inlet diffuser for a better design to enhance thermal comfort and energy consumption. The primary objective of the presented work is to investigate the thermal comfort within a faculty office occupied by two faculty members using the Computational Fluid Dynamics (CFD) methodology. First, an independent mesh study was performed to reduce the uncertainty related to the mesh size. In addition, the presented CFD approach was validated against available experimental data from the literature. Then, the effect of inlet air temperature and velocity on air movement and temperature distribution is investigated using Ansys Fluent. To be as reasonable as possible, the persons who occupy the office, lights, windows, tables, the door, and computers are accounted for in the CFD simulation. After that, the Predicted Mean Vote (PMV) was evaluated at three different locations inside the room, and the approximate total energy consumption was obtained for the presented cases. The CFD results showed that, for the presented cases, the sensation was neutral with the lowest energy consumption when the supply air velocity was 1 m/s and the temperature was 21 °C.

1. Introduction

Heating, Ventilating, and Air Conditioning (HVAC) systems are important and essential in our daily comfort, either in homes, work, or transportation [1]. There have been countless research works carried out by different researchers around the world on the performance of HVAC systems, either in terms of duct sizing or air distribution [2]. HVAC systems have to be designed in a way to improve thermal comfort and reduce energy consumption, especially in hot climates. In Saudi Arabia, the climate is hot and humid, especially in the area near the Red Sea. The electricity consumption due to the use of air conditioning in residential areas in Saudi Arabia is around 50%, which consumed around 130 TWh in 2018 [3]. Thus, studying the thermal comfort of an occupant space in hot weather is advantageous.

To get acceptable thermal comfort, one can look to the American Society of Heating, Refrigerating, and Air-Conditioning Engineers (ASHRAE) standard codes [4]. It is recommended that the temperature difference between the head level and ankle should not exceed 3 °C. In addition, for occupied rooms, it was recommended that the air velocity not exceed 0.2 m/s. It is recommended that the comfortable range of the Predicted Mean Vote (PMV) is within the range of ±0.5.

So, how do we know if a room has reached the thermal comfort zone? It is worth noting that thermal comfort depends on various parameters, including humidity, indoor air temperature, air movement, clothing, and activity within the room. Taleghani et al. [5] reviewed the thermal comfort parameters and their effects on the air quality.

In recent years, the Computational Fluid Dynamics (CFD) approach has been widely applied in various engineering applications, including the analysis of HVAC system performance and air temperature distribution in closed rooms. Recently, researchers have been studying, designing, and optimizing HVAC systems in different scenarios. For example, one question was how thermal comfort would change with changing location and type of the airflow diffuser. Patel and Dhakar [6] investigated a room’s air cooling and temperature distribution by changing the air conditioner duct location using the CFD approach. Three cases of air conditioner locations were studied. The first case was a single air conditioner mounted 2.7 m over the floor, the second used two air conditioners facing each other, and the third used two air conditioners separated by a distance of 2.7 m. They concluded that the third case had better cooling conditions than the other two.

Moreover, Aziz et al. [7] experimentally and numerically investigated the effect of three different types of air diffusers, which were vortex, square, and round diffusers, on thermal comfort and energy consumption inside a room. They concluded that using the vortex diffuser can make the room colder and consume less energy than other investigated diffuser types.

Kokash et al. [8] investigate the effect of diffuser type and location in an elementary classroom on thermal comfort in hot water (cooling) using the CFD approach. The first type is square diffusers placed on the ceiling, and the second type is multi-hole diffusers placed on the walls. They conclude that the multi-hole diffusers increase thermal comfort and reduce energy consumption due to the occurrence of the Coanda effect compared to the square diffusers that were placed on the ceiling.

Barau et al. [9] study the effect of the location of the air conditioning unit on the temperature distribution and airflow velocity using the CFD methodology. The first two cases were when the air conditioner was placed on the walls, and the third case was when the air conditioner was placed in the center of the ceiling. Their findings reveal that a lower temperature distribution was observed when the AC was in the ceiling.

Buratti et al. [10] evaluated the effect of solar radiation on thermal comfort experimentally and numerically using the CFD approach in a classroom at the University of Perugia. They used the outdoor air temperature and solar radiation as input for their CFD setup. However, the indoor air and surface temperatures were measured in the classroom and then used in the CFD setup for validation. The CFD results agreed well with the experimental data using the K-e turbulent model.

Li et al. [11] investigated the airflow velocity distributions in a room using three different types of diffusers, experimentally and numerically, using CFD. The investigated diffuser types were rectangular grille, square grille, and square ceiling diffusers. First, they measured the velocity at different locations inside the room. Then, they used the CFD approach to investigate the velocity inlet boundary conditions by considering it as uniform and non-uniform velocity. The non-uniform velocity inlet boundary condition was used because the diffusers affect the air velocity magnitude and direction. It was shown that there is no significant difference between the two approaches for square ceiling diffusers with an average outflow velocity of less than 1.34 m/s. This method is more convenient when the outflow velocity data at the diffuser are available.

Mahajan and Bartaria [12,13] investigated the effect of the opening location of the air discharge on the air temperature measurements in a conditioned room using thermocouple sensors. The measurements were conducted at an air velocity of 4.5 m/s, with an outside temperature of 32 °C. In their experiments, a window air conditioner was used, and it was connected to a circular pipe duct. The circular pipe duct has three opening locations, which are at the top, middle, and bottom. The opening positions are separated by 1.5 m. They reported a comparison between the air temperature measurements at three different locations, which are at 0.5, 1.5, and 3 m for each circular pipe duct location. It was observed that the reduction of the air temperature was higher at 0.5 and 1.5 m (lower and middle zones of the room) for all three opening locations. In the presented work, the experimental data from Mahajan and Bartaria [12,13] were adopted and used for validating the CFD setup.

The main objective of the presented work is to study the effect of inlet air temperature and velocity on thermal comfort and energy consumption in an office room. To study the thermal comfort, the PMV was evaluated with three different inlet air temperatures and three inlet velocities. In this work, the airflow and temperature distribution inside a work office are investigated using the CFD approach. One of the walls faces the east side; the rest are partitions. The office room is for two faculty members. In addition, the energy consumption was evaluated for each case.

2. CFD Simulation Approach and Setup

ANSYS Fluent with Fluent Meshing version 2023 was used in the presented work to simulate airflow and temperature distribution to study the thermal comfort inside an office room. First, the room’s structure with an area of 14.95 m² was created using the Design Modeler in Ansys Fluent version 2023. The dimensions of the office room are 4.60 m × 3.25 m × 3 m (length × width × height). The office has two windows facing the outside from the east side. The window dimensions are 0.9 m × 1.5 m (width × height). There is one door, which is 0.8 m × 2.2 m (width × height). In the office, there is one air inlet in the room and one return diffuser. The current diffuser type is a square diffuser with 0.29 m² area, which corresponds to 525 mm × 525 mm. The inlet diffuser is located 1.93 m from the right wall and 0.58 m from the front wall to the center of the inlet diffuser. The outlet diffuser is located 2.58 m from the right wall and 1.18 m from the outside wall to the center of the outlet diffuser. To be realistic, the CFD simulation was performed by accounting for the heat transfer from the lights, the wall facing the east side, and the computers used by the faculty, which are two. Figure 1 shows the schematic of the room’s structure. After creating the room’s structure, the air flow was simulated in Fluent.

Table 1. The air flow properties used in the CFD simulations.

Properties	Value
Density (kg/m3)	1.225
Specific Heat [Cp] (J/kg·K)	1006.43
Thermal Conductivity (W/m·K)	0.0242
Viscosity (kg/m·s)	1.7894 × 10−5

shows the air flow properties used in the CFD simulations. The presented CFD study was performed in an office located in hot-climate weather, assuming an outside temperature of 35 °C. The air temperature inside the room when there is no air influx was around 36.5 °C. This value was obtained after performing a CFD simulation for a closed case (without air entering the room).

2.1. Governing Equations and Boundary Conditions

For the investigated case, the indoor airflow and temperature distribution were simulated in Fluent by solving the incompressible Navier–Stokes equations of the continuity, momentum, and energy equations. The steady-state incompressible continuity equation in cartesian form [14] is defined in Equation (1).

$${\displaystyle \frac{\mathsf{\partial }u}{\mathsf{\partial }x}}+{\displaystyle \frac{\mathsf{\partial }v}{\mathsf{\partial }y}}+{\displaystyle \frac{\mathsf{\partial }w}{\mathsf{\partial }z}}=0$$

(1)

where u, v, and w are velocity components in the x, y, and z directions, respectively. The steady-state incompressible momentum equation is defined in Equations (2)–(4).

$$\rho g_{x }-{\displaystyle \frac{\mathsf{\partial }p}{\mathsf{\partial }x}}+\mu \left({\displaystyle \frac{{\mathsf{\partial }}^{2}u}{{\mathsf{\partial }x}^2}}+{\displaystyle \frac{{\mathsf{\partial }}^{2}u}{{\mathsf{\partial }y}^2}}+{\displaystyle \frac{{\mathsf{\partial }}^{2}u}{{\mathsf{\partial }z}^2}}\right)=\rho \left(u{\displaystyle \frac{\mathsf{\partial }u}{\mathsf{\partial }x}}+v{\displaystyle \frac{\mathsf{\partial }u}{\mathsf{\partial }y}}+w{\displaystyle \frac{\mathsf{\partial }u}{\mathsf{\partial }z}}\right)$$

(2)

$$\rho g_{y }-{\displaystyle \frac{\mathsf{\partial }p}{\mathsf{\partial }y}}+\mu \left({\displaystyle \frac{{\mathsf{\partial }}^{2}v}{{\mathsf{\partial }x}^2}}+{\displaystyle \frac{{\mathsf{\partial }}^{2}v}{{\mathsf{\partial }y}^2}}+{\displaystyle \frac{{\mathsf{\partial }}^{2}v}{{\mathsf{\partial }z}^2}}\right)=\rho \left(u{\displaystyle \frac{\mathsf{\partial }v}{\mathsf{\partial }x}}+v{\displaystyle \frac{\mathsf{\partial }v}{\mathsf{\partial }y}}+w{\displaystyle \frac{\mathsf{\partial }v}{\mathsf{\partial }z}}\right)$$

(3)

$$\rho g_{z }-{\displaystyle \frac{\mathsf{\partial }p}{\mathsf{\partial }z}}+\mu \left({\displaystyle \frac{{\mathsf{\partial }}^{2}w}{{\mathsf{\partial }x}^2}}+{\displaystyle \frac{{\mathsf{\partial }}^{2}w}{{\mathsf{\partial }y}^2}}+{\displaystyle \frac{{\mathsf{\partial }}^{2}w}{{\mathsf{\partial }z}^2}}\right)=\rho \left(u{\displaystyle \frac{\mathsf{\partial }w}{\mathsf{\partial }x}}+v{\displaystyle \frac{\mathsf{\partial }w}{\mathsf{\partial }y}}+w{\displaystyle \frac{\mathsf{\partial }w}{\mathsf{\partial }z}}\right)$$

(4)

where the first, second, and third terms from the left are the gravity force, the pressure gradient force, and the viscous diffusion. The right-hand side of Equations (2)–(4) is the acceleration due to convection. The energy equation is defined in Equation (5), where T and α are the temperature and thermal diffusivity, respectively. The thermal diffusivity is defined by Equation (6).

$$u{\displaystyle \frac{\mathsf{\partial }T}{\mathsf{\partial }x}}+v{\displaystyle \frac{\mathsf{\partial }T}{\mathsf{\partial }y}}+w{\displaystyle \frac{\mathsf{\partial }T}{\mathsf{\partial }z}}=\alpha \left({\displaystyle \frac{{\mathsf{\partial }}^{2}T}{\mathsf{\partial }{x}^2}}+{\displaystyle \frac{{\mathsf{\partial }}^{2}T}{\mathsf{\partial }{y}^2}}+{\displaystyle \frac{{\mathsf{\partial }}^{2}T}{\mathsf{\partial }{z}^2}}\right)$$

(5)

$$\alpha ={\displaystyle \frac{k}{\rho c_p}}$$

(6)

where k, $\rho$, and c_p are the thermal conductivity, density, and specific heat at constant pressure, respectively. The CFD simulation was performed in the steady state, and the gravity acceleration was accounted for. The turbulent model used is the K-epsilon turbulent model, which was used with the default constant in Fluent. Other researchers have used the realizable K-epsilon turbulent model, and it has shown good predictions for air simulations inside rooms [15]. The wall function used in the presented study is a scalable wall function, with utilization of viscous heating, and the buoyancy effect was accounted for in the simulations. To account for the radiation heat transfer inside the room, the discrete ordinates (DO) radiation model was utilized. In the DO model, the polar angle (theta) and azimuthal angle (phi) divisions were equal to 5, which produces 25 radiation directions to solve the radiation equations.

First, the simulations were performed using the SIMPLE method for 500 iterations to ensure stable convergence. The convergence criteria for all residuals were set to 1 × 10⁻⁵, except for energy and DO intensity, which were set to 1 × 10⁻⁶. For the first 500 iterations, the discretization of the pressure was solved as standard, the first order upwind for the energy, momentum, and turbulence properties. After the first 500 iterations, the coupled method was used, utilizing the second order for the pressure, momentum, energy, and turbulence properties till it converged. It converged after around 1000 iterations for most of the cases.

The boundary condition for the inlet is an inlet flow velocity. A uniform air velocity magnitude normal to the boundary was assigned at the square ceiling diffuser. The diffuser was used to make the CFD simulation more realistic and to capture the Coanda effect in the room. The outlet gauge pressure is zero. For the nine lights, two persons, two computers, windows, desks, walls, roof, and floor, the wall boundary conditions were assigned for each part separately using either temperature or heat flux, where applicable. The main heat sources inside the room are computers, lights, windows, the wall facing outside, and the two people. The other three walls (partitioned walls), roof, floor, and desks are assumed to be adiabatic walls.

Table 2. Summary of the boundary conditions.

Boundary Name	Location	Type	Value and/or Description
Inlet	Inlet diffuser	Velocity inlet	Ranges from 1 to 3 m/s with a temperature from 16 to 22 °C
Outlet	Outlet diffuser	Pressure outlet	Zero
Wall	Partition walls	Heat flux	Adiabatic wall with zero heat flux
	Door
	Outside wall	Convection	U-value = 0.403 (W/m2·K) with free stream temperature of 35 °C and emissivity (ε) of 90%
	Floor	Heat flux	Adiabatic wall with zero heat flux
	Roof	Heat flux	Adiabatic wall with zero heat flux
	Windows	Convection	U-value = 2.668 (W/m2·K) with free stream temperature of 35 °C and emissivity (ε) of 90%
	Lights	Heat flux	Heat flux = 120 (W/m2) and emissivity (ε) of 90%
	Desks	Heat flux	Adiabatic wall
	Computers	Heat flux	Heat flux = 32 (W/m2) for each computer and emissivity (ε) of 95%
	People	Temperature	The temperature of the faculty (two persons) is assumed to be 36.5 °C with metabolic rate at rest and typing of 1.1 (met) [4] and emissivity (ε) of 95%

summarizes the boundary conditions for the inlet, outlet, windows, light, people, persons, and walls. Table 2 shows the heat flux values used in the thermal boundary conditions. Some of the parameters were adopted from the Saudi Building Codes (SBCs) since the office is located in Saudi Arabia. The U-values of the outside wall and windows were taken from the SBC standard code 602 [16], which are the maximum acceptable U-values in the Jazan region. The U-value is defined as the rate of heat transfer through the building’s components per area and temperature difference between the inside and outside environments of the component (W/m²·K).

There are 9 circular LED lights with a diameter of 30 cm and a power of around 10 Watts. So, it is assumed that the heat flux is around 120 W/m². The heat flux value used in the presented CFD setup of the lights is within the acceptable range [4,17]. For computers, the heat flux boundary condition was used, and it was assumed that the heat flux is 32 (W/m²). Regarding the temperature of the occupants, it was assumed to be 36.5 °C with a metabolic rate of 1.1 (met) at rest. The value of 36.5 °C was assumed for the body temperature, which is similar to the core body temperature.

In the presented study, the air inlet velocity ranges from 1 to 3 m/s; these values were selected to investigate the effect of air velocity on the PMV and energy consumption. These values are within the range of inlet air velocities used in the work that was conducted by Aziz et al. [7], where the inlet air velocity was from 1 to 4 m/s. Also, it is within the recommended range from the SBC 602 standard code [16]. In addition, the effect of the inlet air temperature is investigated, considering inlet air temperatures of 16, 18, 20, 21, and 22 °C. These values are acceptable for offices in hot climates, as per the ANSI/ASHRAE standard code [4]. Also, other researchers have used different values for the inlet air temperature, ranging from 14 to 19 °C [7,18,19,20].

2.2. The Predicted Mean Vote (PMV)-Related Equations and Approach

The PMV was calculated according to the ANSI/ASHRAE 55 standard code [4]. In the presented study, the operative temperature (T_o) was calculated using Equation (7).

$$T_o={\displaystyle \frac{{T_a+T}_{MRT}}{2}}$$

(7)

where T_a is the air temperature, which was taken from the CFD results at the investigated locations. The T_MRT is the mean radiant temperature, which was extracted from the CFD result. In this work, the simplified equation from Fanger [21] was used to determine the T_MRT, which is defined in Equation (8).

$$T_{MRT}=\left(\sum _{i=1}^N{T}_i·S_i\right)·{\left(\sum _{i=1}^N{S}_i\right)}^{-1}$$

(8)

where N, T_i, and S_i are the total number of surfaces considered in the computational domain around the investigated locations, the temperature of each surface, and the area of each surface, respectively. The T_MRT value was calculated after extracting the average temperature of each surrounding surface at the investigated locations from the CFD results. The locations being investigated: the middle of the room, 1.2 m above the floor in front of the face of person 1, and 1.2 m above the floor in front of the face of person 2. The distance of 1.2 m was chosen because it is close to the chest and face region of the people seated in the investigated room. In addition, the air speed was obtained from the CFD results at these locations to obtain the PMV.

After obtaining all the required temperature values and air velocity at the investigated locations inside the room, the PMV was calculated using an external tool available online that was developed by Tartarini et al. [22]. They developed a simple, user-friendly tool that determines indoor thermal discomfort. It is only required to input into the tool the operative temperature, air speed, relative humidity, metabolic rate, and clothing insulation. In the presented study, the relative humidity was assumed to be 60%, the metabolic rate was 1.1 met (for a typing seated person), and the clothing insulation was set at 0.61 clo [22], which represents a person typing and wearing trousers with a long-sleeved shirt. More information on the related equations for determining the PMV can be found in the paper that was published by Tartarini et al. [22].

2.3. Energy Consumption Calculations

The effect of the inlet air velocity and temperature on energy consumption (Q) was examined. The energy consumption considered in this work is the sum of the cooling load obtained from the CFD results of the air conditioning, computers, lights, people, outside wall, and windows, as shown in Equation (9).

$$Q_{total}=Q_{air}+Q_{computers}+Q_{lights}+Q_{people}+Q_{wall}+Q_{windows}$$

(9)

The energy consumption from the air conditioning (Q_air) was obtained using Equation (10).

$$Q_{air}=\dot{m} cp (T_{room}-T_{inlet})$$

(10)

where $\dot{m}$, cp, T_room, and T_inlet are the mass flow rate of air flowing into the room, the specific heat capacity at constant pressure of the air, the room temperature, and the inlet temperature, respectively. The room temperature was considered as the volume-weighted average room temperature. For the other internal cooling loads, Equation (11) was used for each heat source inside the room.

$$Q=q″ A$$

(11)

where q″ and A are the heat flux and the area of the surface where the heat flux was applied.

2.4. Mesh Independence Study

The poly-hexacore mesh was generated using Fluent Meshing. The mesh-independent study was performed to reduce the uncertainty related to the grid size by using a refinement ratio of 20% by adjusting the mesh size in the faces and body. In the mesh-independent study, the air velocity inlet boundary condition was 1.5 m/s. Local face sizing was used for persons, inlets, outlets, lights, computers, tables, and window surfaces. The target mesh size for the local face sizing for mesh#1 is 0.02 m. The local body size method was used for the entire computational domain, equal to 0.07 m for the coarse mesh#1. A 20% refinement ratio was used to generate mesh#2, mesh#3, and mesh#4. For instance, mesh#2 was generated by refining mesh#1 by 20%. Then, mesh#2 was refined by 20% to obtain mesh#3. Mesh#4 was obtained using the same approach. So, four meshes were created: mesh#1 (826,306 cells), mesh#2 (1,468,651 cells), mesh#3 (2,132,074 cells), and mesh#4 (2,995,842 cells). The mesh-independent study was performed on the room’s temperature distribution in a vertical line in the middle of the room, as shown in Figure 2. As can be seen, there is no significant difference in the results between mesh#2, mesh#3, and mesh#4. The maximum absolute temperature difference between mesh#2 and mesh#3 was around 0.3 °C, and between mesh#3 and mesh #4 it was around 0.5 °C. So, the uncertainty due to the mesh size is reduced. It is worth mentioning that mesh#3 showed similar results to mesh#2, but to be more conservative, mesh#3 was used instead for the remaining study in the presented work. Figure 3 and Figure 4 show an isometric view of the computational domain and an inside view of the office room using mesh#3, respectively.

2.5. Validating the CFD Approach with Experimental Data

The presented CFD setup was validated using the available experimental data in the literature, which Mahajan and Bartaria [12,13] produced. The geometry of the room is 6 m × 2 m × 3.55 m. The measured inlet velocity was 4.5 m/s, which was used as the inlet boundary condition. They investigated the effect of the opening location of a circular pipe duct. In the presented CFD validation, only one opening location, which is at the top, is considered. Figure 5 shows the geometry of the investigated room, which includes the inlet, outlet, and the line from which the air temperature distribution was extracted using the CFD. The line is located 2 m from the circular pipe duct, which is similar to the adopted experimental case. The outside temperature was considered to be 32 °C, as was reported by Mahajan and Bartaria [12,13]. The results of the CFD validation are presented in Section 3.1.

3. Results and Discussions

The air velocity, temperature distribution, the Predicted Mean Vote (PMV), and the energy consumption were evaluated to determine the thermal comfort in the office room, using the CFD approach. The following subsections present the results of the CFD validation against the adopted experimental data, air velocity distributions, air temperature distributions, and the thermal comfort analysis.

3.1. Validating the CFD Setup

A CFD simulation was performed using the experimental case from Mahajan and Bartaria [12,13] for the CFD validation. Figure 6a shows the comparison of air temperature distribution between the presented CFD results and the adopted data from Mahajan and Bartaria [12,13] at 2 m from the air discharge pipe. In Figure 6a, the experimental temperature distributions are the recorded temperature with a time interval of 15 min, ranging from 15 to 90 min. As can be seen, the recorded temperature distributions vary over time. The CFD result is in the range of the measured temperature distribution. For the presented CFD validation, the average of these readings was obtained and compared with the CFD result, as shown in Figure 6b. This was carried out because the presented CFD simulation was a steady state. The error bar of the average experimental data is the standard deviation of the readings from 15 to 90 min. The maximum and minimum standard deviations from the experimental temperature distributions are 1.46 °C and 0.76 °C at heights of 0.51 m and 2.5 m from the floor, respectively. As can be seen from Figure 6b, the CFD result is within ±1 °C of the standard deviation. The maximum and minimum absolute temperature differences between the CFD result and the adopted average experimental data are around 1.01 °C and 0.01 °C at heights of 0.51 m and 2.5 m from the floor, respectively.

Table 3. A summary of the comparison between the air temperature from the CFD results and the adopted experimental data from Mahajan and Bartaria [12,13].

Height (Meters)	Average Experimental Data from Mahajan and Bartaria [12,13] (°C)	CFD Results (°C)	Absolute Temperature Difference (°C)
0.12	24.48	25.41	0.93
0.51	24.84	25.85	1.01
1	25.08	25.71	0.63
1.5	24.91	25.74	0.83
2	24.80	25.51	0.71
2.50	25.22	25.21	0.01
3	25.95	25.05	0.90

presents a summary of the absolute air temperature differences between the CFD result and the adopted average experimental data.

3.2. Air Velocity Distributions

The effect of inlet air velocity on the thermal comfort in the office room was investigated. As mentioned before, the air diffuser used in this work was a square diffuser to capture the Coanda effect in the room. Some of the published work only used a square inlet without the diffuser. The air inlet velocity boundary condition at the air inlet diffuser ranged from 1 m/s to 3 m/s, with inlet temperatures of 16, 18, 20, 21, and 22 °C. Figure 7 shows the planes where the air velocity and temperature distribution were studied, which are across the room at the center of the inlet air diffuser and across persons 1 and 2. Figure 8 shows the air velocity contour at the center of the air diffuser with air velocities of 1, 2, and 3 m/s, with the inlet air temperature of 20 °C. As can be seen, the Coanda effect was captured, and the air was uniformly distributed inside the room. The air speed flowing into the room increased when the inlet air velocity increased, which was as expected. Figure 9 and Figure 10 show the velocity contours across persons one and two, respectively. In Figure 9 and Figure 10, the planes across persons one and two were divided to show only the right side of the plane. This was carried out to clearly illustrate the air speed in the range from 0 to 0.35 m/s, where persons one and two are located. As shown in Figure 9 and Figure 10, the air velocity at 1.2 m above the floor in front of the faces and above the heads of persons one and two increases with increasing inlet air velocity. The air speed at 1.2 m above the floor in front of the face of person one is around 0.04, 0.08, and 0.14 m/s with 1, 2, and 3 m/s air inlet velocity, respectively. For person two, the air speeds are around 0.03, 0.08, and 0.14 m/s with 1, 2, and 3 m/s air inlet velocity, respectively. This indicates that, in this particular case, persons one and two experience similar air flow with air inlet velocities of 2 and 3 m/s. However, with 1 m/s inlet air velocity, person two experiences lower airflow compared to person one by around 25%. The low air speed is due to the decrease in the momentum of the supplied air from the diffuser to the occupant. The air speed at the evaluated locations for the thermal comfort is within the accepted range of the ANSI/ASHRAE 55 standard [4], which is less than 0.3 m/s. Figure 11 shows the air streamlines within the office with the inlet air velocity of 2 m/s. It is observed that, with the use of the square diffuser, the Coanda effect enhances the air movement inside the office, and the air is well distributed across the room.

3.3. Air Temperature Distributions

The effect of the inlet air temperature was studied to determine the suitable PMV with lower energy consumption. The inlet air temperature was assigned to be 16, 18, 20, 21, and 22 °C for all selected inlet air velocities (1, 2, and 3 m/s). The temperature distribution was evaluated across the room in three different position planes. The first plane is at the center of the air diffuser, the second is across person one, and the third is across person two.

Figure 12 shows the temperature distribution across the room in the middle of the inlet air diffuser with air inlet velocity of 1 m/s and inlet air temperatures of 16, 18, 20, and 21 °C. As shown, the temperature is uniformly distributed across the room, and the inside room temperature increases with increasing inlet air temperature. When the inlet air temperature increased from 16 to 18 °C, 18 to 20 °C, and 20 to 21 °C, the absolute temperature differences at the center of the room were 1.81 °C, 1.85 °C, and 0.92 °C, respectively. Figure 13 and Figure 14 show the temperature distribution across the room in the middle of the inlet air diffuser with the investigated inlet air temperature and air inlet velocities of 2 m/s and 3 m/s, respectively. Similar observations were obtained for both cases. With 2 m/s inlet air velocity, the absolute temperature differences at the center of the room were around 1.82 °C, 1.88 °C, and 0.94 °C when the inlet air temperature increased from 16 to 18 °C, 18 to 20 °C, and 20 to 21 °C, respectively. Similarly, as shown in Figure 14 with 3 m/s, the absolute temperature differences were around 2, 1.9, and 0.95 °C. As can be seen, the absolute temperature differences increase with increasing inlet air velocity at the center of the room.

Figure 15 shows the temperature distribution across person one with inlet air velocity of 1 m/s and inlet air temperatures of 16, 18, 20, and 21 °C. As observed, the temperature across person one increased with increasing inlet air temperature. At 1.2 m above the floor in front of the face of person one, the absolute temperature difference was around 4.40 °C when the inlet air temperature increased from 16 °C to 21 °C. Figure 16 and Figure 17 show the temperature distribution across person one with inlet air velocities of 2 and 3 m/s, respectively. When the air inlet temperature increased from 16 °C to 21 °C, the absolute temperature differences of the air temperature at 1.2 m above the floor in front of the face of person one were 4.18 and 4.60 °C with inlet air velocity of 2 and 3 m/s, respectively.

Figure 18, Figure 19, and Figure 20 show the temperature distribution across person two with 1, 2, and 3 m/s, respectively. The CFD results across person two showed almost the same results as what was observed across person one. The air temperature was obtained at 1.2 m above the floor in front of the face of person two. It was observed that the air temperature near persons one and two decreases with increasing air velocity. Also, the air temperature across person two increases with the increase in the inlet air temperature. The absolute temperature differences of the air temperature at 1.2 m above the floor in front of the face of person two when the inlet air temperature increased from 16 to 21 °C were 4.40, 4.45, and 4.55 °C for the air inlet velocities of 1, 2, and 3 m/s, respectively.

Table 4. Summary of the effect of the inlet air temperature and velocity on the air temperature at the following locations: (A) center of the room, (B) 1.2 m above the floor in front of the face of person one, and (C) 1.2 m above the floor in front of the face of person two.

Inlet Air Velocity (m/s)	Inlet Air Temperature (°C)	Location (-)	Air Temperature (°C)
1	16	A	18.16
		B	19.87
		C	19.18
	18	A	19.98
		B	21.71
		C	20.90
	20	A	21.83
		B	23.42
		C	22.68
	21	A	22.75
		B	24.27
		C	23.57
	22	A	23.68
		B	25.12
		C	24.46
2	16	A	17.58
		B	19.48
		C	18.45
	18	A	19.41
		B	21.08
		C	20.17
	20	A	21.29
		B	22.80
		C	21.99
	21	A	22.23
		B	23.66
		C	22.90
	22	A	23.24
		B	24.64
		C	23.90
3	16	A	17.22
		B	18.87
		C	17.59
	18	A	19.22
		B	19.66
		C	19.85
	20	A	21.11
		B	21.52
		C	21.69
	21	A	22.06
		B	22.44
		C	22.62
	22	A	23.03
		B	23.41
		C	23.58

presents a summary of the effect of inlet air velocity and temperature on the air temperature at the center of the room, 1.2 m above the ground near persons one and two.

Moreover, the effect of the inlet air velocity on the volume average room temperature with the selected inlet air temperature was investigated, as shown in Figure 21. As can be seen, the volume average room temperature decreases with increasing inlet air velocity for all the presented cases. For 16 °C inlet air temperature, when the air velocity increased from 1 m/s to 3 m/s, the volume average room temperature reduced by 1.07 °C. For 18, 20, 21, and 22 °C inlet air temperatures, the volume average room temperature reduced by 1.06, 1, 0.96, and 0.88 °C, respectively, when the air velocity increased from 1 m/s to 3 m/s.

3.4. Thermal Comfort and Energy Analysis

The Predicted Mean Vote (PMV) and energy consumption were evaluated for different inlet air velocities and inlet air temperatures to determine the suitable condition for the presented office room. The calculations of the PMV were performed using the CBE Thermal Comfort Tool that was developed by Tartarini et al. [22]. The PMV is affected by the operative temperature, air speed, relative humidity, the occupant’s metabolic rate, and the clothing insulation. The standard comfortable range is −0.5 < PMV < +0.5 [4]. The PMV was evaluated at three locations: (A) center of the room, (B) 1.2 m above the floor in front of the face of person one, and (C) 1.2 m above the floor in front of the face of person two. First, the mean radiant temperature was calculated after obtaining the surface temperatures around the investigated locations, using Equation (8). Then, the air temperatures at these locations were obtained from the CFD results and used to calculate the operating temperature. For the PMV calculation, the relative humidity was assumed to be 60%, the metabolic rate 1.1 met (for a typing seated person), and the clothing insulation was set to 0.61 clo [22]. The air velocity used to calculate the PMV is the velocity at the three different locations inside the room.

Table 5. Summary of the results of the Predicted Mean Vote (PMV) and energy consumption for different inlet air velocities and inlet air temperatures at: (A) center of the room, (B) 1.2 m above the floor in front of the face of person one, and (C) 1.2 m above the floor in front of the face of person two.

Inlet Velocity (m/s)	Inlet Temperature (°C)	Measured Locations	Air Velocity at the Measured Locations (m/s)	TMRT (°C)	Operative Temperature (°C)	Predicted Mean Vote (PMV)	Approximate Total Energy Consumption (W)
1	16	A	0.04	21.49	19.83	−1.51	353.54
		B	0.04	23.53	21.70	−0.92
		C	0.03	23.63	21.41	−1.01
	18	A	0.04	23.14	21.56	−0.9	315.27
		B	0.04	25.03	23.37	−0.32
		C	0.03	25.13	23.02	−0.43
	20	A	0.04	24.73	23.28	−0.35	282.72
		B	0.04	26.45	24.93	0.19
		C	0.03	26.54	24.61	0.08
	21	A	0.04	25.53	24.14	−0.07	266.44
		B	0.04	27.16	25.72	0.44
		C	0.03	27.24	25.41	0.34
	22	A	0.04	26.33	25.00	0.21	250.11
		B	0.04	27.87	26.50	0.69
		C	0.03	27.95	26.21	0.6
2	16	A	0.08	20.25	18.91	−1.74	571.36
		B	0.08	21.99	20.74	−1.19
		C	0.08	22.10	20.27	−1.35
	18	A	0.08	21.79	20.60	−1.23	523.07
		B	0.08	23.35	22.22	−0.74
		C	0.08	23.45	21.81	−0.88
	20	A	0.08	23.47	22.38	−0.69	473.71
		B	0.08	24.88	23.84	−0.23
		C	0.08	24.96	23.48	−0.36
	21	A	0.08	24.31	23.27	−0.41	449.00
		B	0.08	25.64	24.65	0.02
		C	0.08	25.72	24.31	−0.1
	22	A	0.08	25.29	24.26	−0.1	423.04
		B	0.08	26.58	25.61	0.32
		C	0.08	26.66	25.28	0.21
3	16	A	0.16	19.55	18.45	−2.11	739.83
		B	0.14	21.07	19.46	−1.72
		C	0.14	21.16	19.61	−1.66
	18	A	0.16	21.21	20.21	−1.54	674.73
		B	0.14	22.57	21.12	−1.18
		C	0.14	22.66	21.26	−1.13
	20	A	0.16	22.93	22.02	−0.95	611.73
		B	0.14	24.16	22.84	−0.64
		C	0.14	24.23	22.96	−0.59
	21	A	0.16	23.79	22.93	−0.66	580.17
		B	0.14	24.95	23.70	−0.38
		C	0.14	25.02	23.82	−0.34
	22	A	0.16	24.72	23.88	−0.37	550.80
		B	0.14	25.83	24.62	−0.1
		C	0.14	25.90	24.74	−0.06

shows the results of the calculated T_MRT, operative temperature, PMV, and energy consumption at different inlet air velocities and temperatures. As can be seen, the inlet air temperature did not affect the air velocity at the investigated locations. The results showed that, with 1 m/s inlet air velocity and a temperature of 16 °C, the PMV is in the cool region at all three locations. When the inlet air temperature increased to 18 °C and 20 °C, the PMV value fell in the neutral sensation region, indicating that the environment complied with the ANSI/ASHRAE 55 standard code [4]. However, with 18 °C at the center of the room, the PMV value is slightly in the cool region compared to the location of persons one and two. This is because the measured location (at the center of the room) is close to the inlet air diffuser. A similar observation was obtained with the inlet air velocity of 2 m/s and temperature of 20 °C. With the inlet air velocity of 2 m/s and temperatures of 16 °C and 18 °C, the PMV values are in a slightly cool region at all three locations. Also, the PMV values are in the cool region at all three locations with the inlet air velocity of 3 m/s and temperatures of 16, 18, and 20 °C. Moreover, the CFD result showed that the PMV values are in the neutral sensation region with the combination of inlet air temperature of 21 °C and inlet air velocity of 1, 2, and 3 m/s. However, with 3 m/s at the center of the room, the PMV value is in the slightly cool region. With an air temperature of 22 °C, the PMV values are in a slightly warm region near persons one and two and neutral at the center of the room with an air velocity of 1 m/s. However, the PMV values are in the neutral region at the investigated locations with 2 and 3 m/s air velocity. This indicates that, by increasing the inlet air velocity, the room temperature will decrease.

The approximate total energy consumption of the room was evaluated for all the presented cases, as shown in Table 5. The CFD results showed that the energy consumption increased with increasing inlet air velocity at a fixed inlet air temperature. In this section, only the results when the PMV values are within the standard range are discussed. The results showed that the conditions suitable for the presented office room are with the combinations of inlet air velocity and inlet air temperature of 1 m/s at 20 °C, 1 and 2 m/s at 21 °C, and 2 and 3 m/s at 22 °C. This is because the PMV values are within the standard comfortable range at all three locations being investigated. Among these cases, the lowest total energy consumption is 266.44 W, obtained with the combination of 1 m/s at 21 °C, which is lower than the other cases when the PMV values are within the acceptable range near the investigated locations.

4. Conclusions

This study focused on investigating the effect of inlet air velocity and inlet air temperature on thermal comfort for an office room using the CFD approach. The investigated inlet air velocity at the inlet diffuser ranged from 1 to 3 m/s at 16, 18, 20, 21, and 22 °C inlet air temperature. First, the mesh independence study was performed to reduce the uncertainty related to the grid size. The mesh study was performed on the temperature distribution at the center of the room. Then, the presented CFD approach was validated against available experimental data. The presented CFD result was shown to be within the measured temperature distribution, and the minimum and maximum absolute temperature differences between the CFD result and the average temperature distribution were 0.01 and 1.01 °C, respectively. Then, the PMV was calculated at three different locations inside the room after obtaining the air speed, surface temperatures, and ambient temperatures around the investigated locations from the CFD results. The CFD results showed that, with the combinations of inlet air velocity and inlet air temperature of 1 m/s at 20 °C, 1 and 2 m/s at 21 °C, and 2 and 3 m/s at 22 °C, the PMV values are within the standard comfort range at all three examined locations. These conditions are suitable for the presented office room. Additionally, the total energy consumption of the room was evaluated for all the presented cases. The most efficient energy consumption for the investigated office was obtained with 1 m/s at 21 °C, which was 266.44 W.

As shown in this work, the CFD has the capability to determine the suitable inlet air velocity and temperature required for a room to achieve better thermal comfort with the most efficient energy consumption. It will be beneficial to use the CFD tool for HVAC applications during the design stages. The findings in this paper help optimize the HVAC design of office environments, especially in hot-climate weather. As was shown for the presented office room, the presented CFD results suggest that thermal comfort can be improved with an inlet air velocity of 1 m/s and an inlet temperature of 21 °C. This can be beneficial for local HVAC guidelines to help achieve buildings with lower energy consumption.

It is worth mentioning that uncertainty may exist in the CFD setup, which could impact the CFD results, including the turbulent model, boundary conditions applied at the wall, light, and windows, and the solution method used in the CFD setup. Thus, for future work, the effect of the turbulence model and the location and angle of the inlet diffuser will be investigated using the CFD methodology. Additionally, the effect of inlet air temperature and time (using transient simulation) on thermal comfort will be investigated.