Chapter 21 Numerical Analysis of Air Flow Around a Hot Water Radiator for Its Structure Improvement

Transcription

1 Chapter 21 Numerical Analysis of Air Flow Around a Hot Water Radiator for Its Structure Improvement Juan Wang, Zhanyong Li, Ruifang Wang, Qing Xu, Wei Tian and Miaomiao Li Abstract Hot water radiators are widely used for indoor heating mainly in North China and a large quantity of fossil fuels are needed for heating energy use every year. Therefore, it is important to analyze thoroughly the characteristic of this type of radiators in order to reduce energy use and associated carbon emissions in the building sector of China. Improper design of heating radiator results in excessive energy consumption with uneven temperature distribution, and dust mark on the wall may occur. For the purpose of energy saving and carbon emission reduction, the numerical simulation of the heat transfer and air flow around radiators within heating rooms is necessary to understand the reason for this dust mark and furthermore to modify the radiator configuration. In this paper, the two-dimensional and three-dimensional models were set up, in which both the Navier Stokes equations and energy equations were solved by using FLUENT software, with the standard κ-ε turbulence model and SIMPLE algorithm. By analysis of the indoor air velocity field and the distribution of temperature field, the influence on fine dust particles distribution due to air flow around the radiator was discussed to explain the cause of dust formation. Then, the external structure of the radiator was modified to change the flow field patterns using numerical simulation, and consequently to minimize the dust formation for energy reduction and improve indoor beautiful appearance. Keywords Radiator Dust formation Structural modification CFD Emission reduction J. Wang Z. Li (&) R. Wang Q. Xu W. Tian M. Li College of Mechanical Engineering, Tianjin University of Science and Technology, Tianjin , China zyli@tust.edu.cn J. Wang Z. Li R. Wang Q. Xu W. Tian M. Li Tianjin Key Laboratory of Integrated Design and On-Line Monitoring for Light Industry & Food Machinery and Equipment, Tianjin , China Springer International Publishing Switzerland 2017 X.-R. Zhang and I. Dincer (eds.), Energy Solutions to Combat Global Warming, Lecture Notes in Energy 33, DOI / _21 435

2 436 J. Wang et al. Nomenclature C P Heat capacity (J kg 1 C 1 ) Greek Letters Ρ Density (kg/m 3 ) k Coefficient of thermal conductivity (W m 1 C 1 ) Ε Internal emissivity β Thermal expansion coefficient 1 Introduction Heating energy accounts for approximately 40 % of the total building energy in China and consequently the fossil fuel used for heating is one of main sources for carbon emissions [1]. The radiators using hot water as heating medium are the main way of heating buildings currently in China, which is expected to continue for a long time [2]. Therefore, it is necessary to understand the characteristics of the hot water radiators in order to reduce energy use for heating and associated carbon emissions from the building sector of China. Heating radiator is commonly used as an end device of heating system to transfer thermal energy carried by the heat medium to indoor air, so as to achieve the aim of maintaining suitable indoor temperature. As a result, it must be operated stably under high temperature and pressure for better heat transfer and thermal properties of fluid inside radiators. Hot water radiators are widely used for indoor heating mainly in North China, but many problems were encountered in practice due to improper design, such as water pipe leakage, corrosion, lukewarm radiator, uneven temperature distribution, and dust formation, which lead to energy wasting and environment pollution. It can be found that there is a lot of dust formation on the upper part of the radiator and the nearby walls after using radiators for a period of time. This apparently affects aesthetic for indoor environment. More importantly, these dusts may also impose a harmful effect on occupants due to the accumulation of dust. The dust removal and wall painting need a large amount of manpower resources. Therefore, analysis of the causes of dust formation and seeking ways to reduce dust formation is necessary for the purposes of both aesthetic and health. In addition, the study of flow fluid in a room can be used to recommend the reasonable place for radiator decoration and furthermore to use the least amount of energy to meet the needs of indoor temperature. The patterns of air flow around the exterior surface of a radiator can be resulted from both natural convection and radiation, which also influences the deposition of contaminant particles because of the different distributions of flow field. In this paper, the computational fluid dynamics and numerical heat transfer method were used to study the velocity field and the distribution of temperature field in a heating

3 21 Numerical Analysis of Air Flow Around a Hot Water Radiator 437 room, and the problem was simplified as high Rayleigh number turbulent natural convection heat transfer within a closed space [3 5]. As a common problem, natural convection within the closed space is widely used in engineering [6, 7]. In recent years, more and more researchers began to pay close attention to this problem. In 1854, Atkinson published a paper in the institution of mining engineers in the north of England, laying a solid theoretical basis for general fluid network theory [8]. Tian and Karayiannis [9] and Betts and Bokhari [10] conducted an experimental study on the natural convection of air in a rectangular cavity, predicted the average temperature distribution and the turbulent velocity distribution of the internal air. Zhen et al. [11] predicted the air flow and temperature field in a room with convective heat source. They compared the simulated results with the experiment results from Howarth [12] obtained by using fluid visualization technology, as well as tracked the trajectories of indoor pollutants and predicted the deposition distribution of different size of particles. Sinha et al. [13] simulated the air flow of a two-dimensional room with and without buoyancy. Posner et al. [4] predicted the air flow inside a room through simulations using the laminar flow, standard κ-ε and RNG κ-ε models. The three-dimension numerical simulation results were compared with the results measured by the laser Doppler velocimeter and the particle image velocimeter. Researchers in the field of domestic buildings also made great contributions in the radiator usage and flow field prediction [14 16]. With an increasing concern of indoor air quality, the predication of indoor distribution of airborne contaminants is becoming a hot topic. Tian et al. [17] investigated the indoor contaminant particle dispersion and concentration distribution in a model room applied three turbulence models standard κ-ε, renormalization group (RNG) κ-ε and RNG-based large eddy simulation (LES) models. Lu et al. [18] simulated the air movement and aerosol particle deposition and distribution in a ventilated two-zone chamber with a small opening connecting the two compartments. Zhao and Wu [19] and Pallares and Grau [20] studied the settling velocity, distribution characteristics, influencing factors and the concentration of the contaminant particles in flow field. Chung and Dunn-Rankin [21] predicated the air currents and the contaminant decay in a small-scale room model using the commercial code FLUENT, the numerical results are validated with flow visualization experiments and local clearance rate measurements by laser extinction. Rouaud and Havet [22] numerically investigated the flow pattern inside a pilot scale room with the aim of efficient contaminant removal using standard and RNG κ-ε turbulence models. Baker et al. [23] gave the CFD simulated characterization of airborne contaminant transport for two practical three-dimensional room air flow fields and predicted the resulting time-dependent concentration evolution throughout the room. The structure [24], location [25] of the radiator and other kinds of heating method [26 28] have also been studied.

4 438 J. Wang et al. However, there are few studies on the local flow field analysis and the influences of the flow field on the deposition of the contaminant particles around radiators. Therefore, the numerical simulation method was used to analyze the local flow field of a heating radiator in this study. Moreover, the external structure of the radiator was modified to change the flow field patterns, which can minimize the dust formation for the purposes of both energy saving and indoor beautiful appearance. 2 Description of the Physical Model The main content of this study is to analyze the flow pattern, velocity field, the distribution of the temperature field, and the deposition of dust particles near radiator in a radiator heating room. This room is assumed to be located in Tianjin, China. Two-dimensional (2D) and three-dimensional (3D) models of a heating room will be created, respectively. The room faces south and there is only exterior wall in the south. Average outdoor temperature is taken as 5 C. The 2D physical model of a room with a hot water radiator is shown in Fig. 1. The room size is 3 3m 2. A single piece of radiator is cm 2 (width height). The whole radiator includes 7 pieces and the space between pieces is 3 cm, situated in the middle of the room. In order to verify the accuracy of the 2D simulation, a 3D model will be also set up as shown in Fig. 2. The size of room is m 3 (length height width) and the thickness of wall is 3 cm. The radiator is cm 3 (length width height), situated in the middle of the room, 5 cm to the left wall, 10 cm high from the ground. The baffle is cm 3 (length width height), fixed on the south wall, 10 cm high from the radiator. Fig. 1 Two-dimensional physical model

5 21 Numerical Analysis of Air Flow Around a Hot Water Radiator 439 Fig. 2 Three-dimensional physical model 3 Simulating Conditions 3.1 Setting of the Solving Model In this paper, FLUENT software was used to carry out the computation in steady state condition. The fluid is assumed to be incompressible, Newtonian, viscous, and the Boussinesq approximation is valid in this case [29]. The 2D/3D steady state calculation model and the implicit finite difference algorithm were chosen. Turbulence was modeled using the standard κ-ε model with buoyancy model enabled [30, 31]. The standard wall function was used near the wall with no-slip wall boundary condition. Radiation was considered in this research and discrete coordinates (DO) radiation model was chosen. 3.2 Material Properties Physical properties of the materials in the model are listed in Table Boundary Conditions According to the actual measurement, the model boundary conditions are shown in Table 2.

6 440 J. Wang et al. Table 1 Properties for the parameters in models Name Density q kg/m 3 Heat capacity C P J/(kg C) Coefficient of thermal conductivity k W/(m C) Fluid (air) Radiator (iron) Interior wall Exterior wall Floor and roof Baffle Internal emissivity ε/thermal expansion coefficient β Table 2 Boundary conditions Boundary Radiator Interior wall Exterior wall Floor and roof Baffle Boundary condition The first-type boundary condition, constant wall temperature 330 K, the internal emissivity is 0.6, the thickness is m The first-type boundary condition, constant wall temperature 288 K, the internal emissivity is 0.9, the thickness is 0.03 m The third-type boundary condition, convection heat transfer coefficient is 5W ðm 2 KÞ, free stream temperature is 268 K, the internal emissivity is 0.9, the thickness is 0.03 m Adiabatic wall boundary condition, heat flow density is 0 W/m 2, internal emissivity is 0.9, the thickness is 0.03 m The first-type boundary condition, constant wall temperature 291 K, the internal emissivity is 0.9, the thickness is 0.02 m 4 Results and Discussion 4.1 Temperature Field Figure 3 presents the temperature distributions in the room space of 2D model, Fig. 4 presents the temperature distributions on plane x = 0 (centerline plane at x = 0 mm) of 3D model. The figure demonstrates that the temperature field presents stratified characteristics along the room height. The highest temperature layer is under the ceiling area. A thermal rising wall jet is produced along the south wall surface above the radiator, where the air temperature is higher and the corresponding isotherm is denser, indicating the temperature gradient is bigger. Therefore, the rising of the hot air created a hot plume above the radiator.

7 21 Numerical Analysis of Air Flow Around a Hot Water Radiator 441 Fig. 3 Temperature profile of 2D Fig. 4 Temperature profile on plane x = 0 of 3D Under the same conditions, the study results show that the temperature ranges from 33.1 to 43.5 C within human activities scope for 2D simulation while 20.6 to 23.4 C for 3D simulation (assuming that the body height is m), the discrepancy may caused by simplification of the physical model, without consideration of the room heat loss, or the mesh used in the simulation is not fine enough. The 3D simulation results show that the indoor temperature distribution is even, the maximum temperature difference from ankle level (0.1 m) to head level ( m) is about 2.8 C, so it can meet the thermal comfort criteria and the requirement of the human body. Compared with the results of 2D simulation, the temperature stratification phenomenon along the height direction of the 3D simulation is more obvious; the indoor temperature distribution is more uniform and has a good accordance with the actual situation of the indoor temperature distribution. Hence, the 3D simulation results can give the real temperature distribution of the indoor air.

8 442 J. Wang et al. Fig. 5 Velocity contour of 2D 4.2 Velocity Field Figure 5 presents the velocity contour of 2D model; Figs. 6 and 7 presents the velocity contour on plane y = cm (centerline plane of the radiator paralleled the south wall) and plane x = 2.8 cm (centerline plane of the radiator perpendicular to the south wall) of 3D model, respectively. The overall indoor air flow trend is that the indoor flow field distributed symmetrically along the center line of the radiator and air near the surface of the radiator is heated by radiator. Since the float lift resulted from temperature rising and density decreasing, a thermal rising wall jet is produced along the wall surface above the radiator, the jet develops into a convective thermal boundary layer along the surface and entrains the cold air from the surroundings. The air in the hot plume flows upwards along the wall surface and changes direction when attaches the ceiling, then some of the hot air disperses downwards to the center parts of the room due to heat exchange, some flows along the ceiling Fig. 6 Velocity contour on plane y = cm of 3D

9 21 Numerical Analysis of Air Flow Around a Hot Water Radiator 443 Fig. 7 Velocity contour on plane x = 2.8 cm of 3D surface and finally bends downwards and strikes the floor, then moves along the floor toward the radiator to complete the circulation. As the temperature of the walls is lower than the indoor air temperature, the hot air will flow down fast along the cold wall (the wall opposite to the radiator) down to the floor, and air circulation vortexes are formed under ceiling and near each wall due to the mixing of hot and cold air and two symmetrical circulations formed along the center line of the radiator. The entrainment of cold air from the surroundings and dispersion of hot air to the room space complete the air circulation and heat exchange [11]. The maximum velocity value appeared in the hot plume area in the upper part of the radiator. The value is m/s from 2D model, and m/s from 3D model, respectively. The result from 3D simulation models is slightly smaller than the 2D simulation results. This may be because the 3D structure is more complex and the space area is larger than the 2D model. On the whole, the results from 3D and 2D simulation models are consistent. In order to verify the accuracy of the simulation, the results were compared with Howarth s results [12]. Figure 8 presents the air movement in the central plane observed by Howarth using a flow visualization technique. The rising convective hot plume (A) flows upward into a buffer zone (B and C) under the ceiling, then some of the air disperses downwards into the core (D) of the room, some strikes and flows along the floor, both subsequently entrained into the rising boundary layer to complete its circulation. Comparing Fig. 7 with Fig. 8, it can be seen that the air flow patterns between prediction and observation are very similar. It also shows that the CFD simulation can capture the main flow features and provide acceptable results. Figure 9 presents the velocity vector from the 2D model. Figure 10 shows the local amplification velocity vector of the 2D. It illustrates that the velocity of the air flow out of the gap between two pieces of radiator is faster, about 0.25 m/s, and the

10 444 J. Wang et al. B C A D Fig. 8 Observed airflow patterns [12] Fig. 9 Velocity vector plot for 2D Fig. 10 Local amplification velocity vector plot of 2D

11 21 Numerical Analysis of Air Flow Around a Hot Water Radiator 445 velocity of the air above the radiator is slower, about 0.08 m/s. Therefore, there are two apparent areas: fast area and slow area from simulation results. Figure 11 shows the velocity vector of plane y = 142 cm (plane near the exterior wall) from the 3D model, with the local amplification above the radiator presented in Fig. 12. The air flow pattern of 3D simulation is similar to the 2D simulation, fast area and slow area also appears in interval, compared with the 2D simulation results, the velocity difference of three-dimensional simulation results is bigger, and the flow speed of the air is faster. This highly uniformity of air flow rate will form a large number of small circulation (eddy current) over the radiator, causing the local velocity drop of the dust particles in the air. Because the temperature of the air near the radiator is higher, there will be a large amounts of dust particles accumulated near the radiator [11], so we can see the phenomenon that a large amount of contaminant particles deposit on the wall near the radiator and the distribution of the dust presents strip-type character, which is in line with the air flow characteristics above the radiator. Therefore, the local speed drop caused by the air vortex results in uneven settlement of the contaminant particles on the wall. Fig. 11 Velocity vector plot on plane y = 142 cm of 3D Fig. 12 Local amplification velocity vector plot on plane y = 142 cm of 3D

12 446 J. Wang et al. 5 Structure Optimization Since the formation of the dust is related to the flow field around the radiator caused by high temperature, so the outer structure of radiator is considered in this paper. Hence, a baffle above a radiator will be installed in order to reduce dust formation. Figure 13 presents the indoor temperature distribution on the plane x = 0 after setting a baffle above the radiator, the figure shows that the baffle block the straight rise of the hot plume, leading the hot air flow to the central parts of the room, which is helpful to the uniformity of indoor temperature distribution to some extent. The whole trend of the indoor temperature distribution has not changed and still presents a layered trend. The temperature would rise as the height increases. The highest temperature appears in the areas between the radiator and baffle, compared with Fig. 4, the temperature distribution in the room has almost no change after setting the baffle, the temperature within the human activities scope is still about 20.1 to 23.5 C. Hence, setting of the damper has little impact on the indoor temperature distribution, which still can satisfy the requirements of the human body. This is because the heat flow turns to the center parts of the room and the uniformity of the indoor temperature distribution increases. This would provide more advantages to occupant comfort. Figure 14 shows the velocity contour on the center plane x = 2.8 cm (centerline plane of the radiator perpendicular to the south wall) after setting the baffle, compared with Fig. 7, the baffle blocks the straight rise of the hot plume, leading the hot air flow to the central parts of the room. Hence, the velocity of the rising air is slower and the contact area with the wall is smaller. However, the flow characteristics of the air in the room did not change. The heat flow continues rising up after bypassing the baffle and then deflects when it reaches the ceiling. Then the hot air will flow down fast along the cold wall after flow through the ceiling, and finally Fig. 13 Temperature profile on plane x = 0 (3D)

13 21 Numerical Analysis of Air Flow Around a Hot Water Radiator 447 Fig. 14 Velocity contour map on plane x = 2.8 cm (3D) flow back toward the radiator to complete the circulation of the indoor air flow. The maximum velocity value appeared in the area between the radiator and the baffle. Figures 15 and 16 show the velocity vector on plane y = 142 cm (plane near the south wall) and the local velocity vector amplification near the radiator respectively, compared with Fig. 12, the baffle blocked the straight rise of the hot plume although there are still apparent fast area between two pieces of radiators and slow area above the radiator. Hence, this baffle blocked the upward movement of the dust particles entrained in the hot air. The flow velocity of the air above the baffle is slower and the difference of velocity between the fast areas and slow areas is reduced, so does the formation of small circulation (eddy current). Thus, the local speed drop of the dust particles is weakened and the dust formation will be reduced. In addition, large amounts of dust particles will be blocked under the baffle, achieving the goal of focus sedimentation of the dust particles to make dust more clustered between the baffle and the radiator. This is not only benefit for indoor beautiful appearance, easy dust removal, but also gaining the aim of emission reduction. Fig. 15 Velocity vector plot on plane y = 142 cm (3D)

14 448 J. Wang et al. Fig. 16 Local amplification velocity vector plot on plane y = 142 cm (3D) 6 Conclusions A CFD modeling of convective airflow in a room heated by a radiator has been presented in this paper. By analyzing the numerical simulation, the following conclusions can be drawn: (1) Formation and distribution of the dusts were influenced by the flow field around the radiator. The local speed drop caused by the air vortex resulted in uneven settlement of the contaminant particles on the wall. (2) The thermal wall jet created by a radiator greatly influences the airflow pattern and the temperature distribution. The air flow inside the room formed two symmetrical circles and the temperature field presented stratified characteristics along the room height. (3) The dust formation on the wall was minimized by modifying the external structure of the radiator (e.g., setting baffle above the radiator) to change the flow field patterns. References 1. Mo LQ, Song WM, Xiao YR (2007) Exploration of the development direction of heating radiator in China. Heating Radiator 32:2 36 (in Chinese) 2. Qi JH, Wang M, Wang X (2006) The present situation existing problems and development prospects of heating radiator in China. Issue Qual Inspection 28:52 53 (in Chinese) 3. Eftekhari MM, Marjanovic LD, Pinnock DJ (2003) Air flow distribution in and around a single-sided naturally ventilated room. Build Environ 38: Posner JD, Buchanan CR, Dunn RD (2003) Measurement and prediction of indoor air flow in a model room. Energy Build 35: Saury D, Rouger N, Djanna F, Penot F (2011) Natural convection in an air-filled cavity: experimental results at large Rayleigh numbers. Int Commun Heat Mass Transfer 38:

15 21 Numerical Analysis of Air Flow Around a Hot Water Radiator Xu W, Chen Q, Nieuwstadt FTM (1998) A new turbulence model for near-wall natural convection. Int J Heat Mass Transf 41: Yang HX, Zhu ZJ (2008) Numerical study of three-dimensional turbulent natural convection in a differentially heated air-filled tall cavity. Int Commun Heat Mass Transfer 35: Wood DJ, Ormsbee LE (1989) supply identification for water distribution system. J AWWA 7: Tian YS, Karayiannis TG (2000) Low turbulence natural convection in an air filled square cavity, part I: the thermal and fluid flow fields. Int J Heat Mass Transf 43: Betts PL, Bokhari IH (2000) Experiments on turbulent natural convection in an enclosed tall cavity. Int J Heat Fluid Flow 21: Zhen LW, Andrew TH, Alan PJ (1997) Prediction of airflow and temperature field in a room with convective heat source. Build Environ 32(6): Howarth AT (1985) The prediction of air temperature variations in naturally ventilated rooms with convective heating. BSER&T 6: Sinha SL, Arora RC, Roy S (2000) Numerical simulation of two-dimensional room air flow with and without buoyancy. Energy Build 32: Zhu BR, Yue XM (2011) Numerical simulation of indoor temperature and velocity distribution in radiator heating room. Build Energy Environ 30:92 94 (in Chinese) 15. Zhai JP (2006) The distribution of the air flow and temperature in the common heating rooms. Sci Tech Inf Dev Econ 16: (in Chinese) 16. Fan RY, Wang Q, Yang SR (2006) Numerical simulation of natural convection in a large enclosed space. Water Conservancy Electr Power Mach 28:29 36 (in Chinese) 17. Tian ZF, Tu JY, Yeoh GH (2006) On the numerical study of contaminant particle concentration in indoor airflow. Build Environ 41: Lu W, Howarth AT, Adam N, Riffat SB (1996) Modeling and measurement of airflow and aerosol particle distribution in a ventilated two-zone chamber. Build Environ 31: Zhao B, Wu J (2007) Particle deposition in indoor environments: analysis of influencing factors. J Hazard Mater 147: Pallares J, Grau FX (2012) Particle dispersion in a turbulent natural convection channel flow. J Aerosol Sci 43: Chung IP, Dunn-Rankin D (1998) Using numerical simulation to predict ventilation efficiency in a model room. Energy Build 28: Rouaud O, Havet M (2002) Computation of the airflow in a pilot scale clean room using κ-ε turbulence models. Int J Refrig 25: Baker AJ, Roy S, Kelso RM (1994) CFD experiment characterization of airborne contaminant transport for two practical 3-D room air flow fields. Build Environ 29: Jing JH, Lan ZQ (2009) On the design of the water-heated radiators. Shan Xi Archit 35:25 26 (in Chinese) 25. Park HJ, Holland D (2001) The effect of location of a convective heat source on displacement ventilation: CFD study. Build Environ 36: Myhren JA, Holmberg S (2008) Flow patterns and thermal comfort in a room with panel, floor and wall heating. Energy Build 40: Witry A, Al-Hajeri MH, Bondok AA (2005) Thermal performance of automotive aluminium plate radiator. Appl Therm Eng 25: Myhren JA, Holmberg S (2009) Design considerations with ventilation-radiators: comparisons to traditional two-panel radiators. Energy Build 41: Ganguli AA, Pandit AB, Joshi JB (2009) CFD simulation of heat transfer in a two-dimensional vertical enclosure. Chem Eng Res Des 87: Launder BE, Spalding DB (1972) Lectures in mathematical models of turbulence. Academic, New York 31. Hsieh KJ, Lien FS (2004) Numerical modeling of buoyancy-driven turbulent flows in enclosures. Int J Heat Fluid Flow 25: