Revista Ingeniería de Construcción Vol. 29 N^{o}1, Abril de 2014www.ricuc.cl PAG. 22-45

**CFD modeling of basic convection cases in enclosed environments: Needs of CFD beginners to acquire skills and confidence on CFD modeling**

**Magdalena Cortés*, Paul Fazio**, Jiwu Rao**, Waldo Bustamante³***, Sergio Vera¹*****

* Pontificia Universidad Católica de Chile, Santiago. CHILE

** Concordia University, Montreal, Quebec. CANADA

*** Center for Sustainable Urban Development (CEDEUS). Pontificia Universidad Católica de Chile, Santiago. CHILE

**ABSTRACT**

Prediction of airflow pattern velocities, temperature, moisture and pollutants concentration is required to design healthy and comfortable indoor environments. Computational Fluid Dynamics (CFD) is the most advanced technique to model and predict the airflow in enclosed environments. However, the main errors in CFD models and their results are linked to the human factor. Beginners on CFD modeling do not account with skills, experience and engineering judgment to generate robust and reliable CFD models. This process is not intuitive and new CFD users need guidance. This paper aims to provide more complete information on CFD modeling of basic natural, forced and mixed convection cases that would allow CFD beginners to acquire skills and confidence. CFD modeling includes mesh generation, setting convergence criteria and under-relaxation factors, and evaluating different turbulence models for each convection case. Results show that users´ expertise is needed in each step of CFD modeling, even for these basic convection cases.

**Keywords:** CFD, enclosed environments, new CFD users, turbulence models, CFD validation

**1. Introduction**

Indoor air distribution in buildings has significant impacts on thermal comfort, indoor air quality and energy efficiency. Important indoor air parameters are temperature and relative humidity; pollutants concentration such as carbon dioxide (CO2) and volatile organic compounds (VOC); indoor surface temperatures; and distribution of air velocity and air turbulence intensity (Zhai et al., 2007). Indoor airflow in building can be natural, forced or mixed and driven by different forces such as wind-induced infiltration, thermal buoyancy, and mechanical ventilation.

Computational Fluid Dynamics (CFD) technique has had a rapid advance since its first application to simulate indoor airflows by Nielsen (1974). Similarly to building energy simulation tools, nowadays, CFD is extensively and intensively applied in the design stage of buildings. It is a well suited tool to model indoor air conditions for research and design because CFD modeling might save time and effort (Hajdukiewicz et al., 2013). However, this involves an important risk of obtaining erroneous results due to lack of user skills on CFD modeling and expertise to deal with indoor air specific engineering problems. Therefore, CFD codes and user skills need to be verified and validated to obtain successful simulations and reliable results (AIAA, 1998).

Mainly, CFD modeling requires expertise to:

• Decide how to model a specific engineering problem. For instance, the physics of the problem could be represented as 2D or 3D and steady-state or transient.

• Define the geometry that represents the indoor environment engineering problem.

• Generate a proper mesh which includes deciding about size and meshing topology as well as testing grid independence.

• Set the fluid properties.

• Set the boundary condition such as wall boundary conditions (surface temperature, heat flux), air supply and outlets, heat and moisture sources and sinks, etc.

• Define solution algorithms, such as pressure or density based solution methods.

• Choose a proper turbulence model that provides reliable results for the characteristic airflow of the problem.

• Establish the numerical parameters such as differencing schemes, under-relaxation factors, time-step in case on transient problems, number of iteration, convergence criteria; etc.

Since several CFD codes have been already widely verified, errors to simulate indoor environments via CFD technique are mostly linked to the human factor. These errors are associated to user's attitude and their experience and training (Casey & Wintergeste, 2000). It often happens that inexperienced users may not realize that results are wrong due the high accessibility to commercial software with friendly user interfaces and colorful results which increases the risk of false confidence.

The "Best Practice Guidelines for Quality and Trust in Industrial CFD" (Casey & Wintergeste, 2000) shows the training need for CFD users and provide guidelines to do this. Also, the guidelines for CFD modeling of AIAA (1998), ERCOFTAC (Casey & Wintergeste, 2000), ASHRAE (Chen & Srebric, 2001), and Oberkampf and Trucano (2002) show procedures to validate CFD models based on comparing CFD simulation results for various turbulence models experimental data. Both procedures would help new CFD users to acquire confidence and expertise on modeling of indoor environments.

However, the disadvantage of these procedures is that the main focus is to evaluate different turbulence models for enclosed environments, but they do not provide detailed information about parameters used on these CFD models, the engineering judgments applied to define the modeling parameters and how to generate a representative model of reality. This information is useful for new CFD user to acquire skill and confidence on CFD modeling.

In consequence, this paper aims to provide more complete information on CFD modeling of basic natural, forced and mixed convection cases. CFD validation of five k-ε and k-ω turbulence is followed to show the criteria and engineering judgments used to model the cases of Ampofo and Karayiannis (2003) for natural convection (NC), Restivo (1979) for forced convection (FC) and Blay et al. (1992) for mixed convection (MC). The CFD validation process and datasets shown in this paper could be used as training exercises for new CFD users to acquire skills and expertise on CFD modeling.

**2. Review on evaluating turbulence models and experimental studies**

This paper proposes that CFD validation process according to CFD guidelines (i.e. AIAA, ASHRAE, etc.) and complemented with information about parameters used and the engineering judgments applied is a proper methodology for training of inexperienced CFD users. CFD validation has focused in a major part of the last two decades to evaluate different turbulence models. This requires experimental datasets to compare CFD results of predicted quantities with experimental measurements (i.e. air velocity, temperature, turbulent kinetic energy, etc.). The following sections summarize most recently studies in evaluating turbulence models, as well as basics experimental setups for NC, FC and MC that will be modeled on CFD as training exercises for new CFD users.

**2.1. Evaluation of turbulence models**

There is a large amount of work on evaluating turbulence models for indoor environments. Many works have focused on evaluating the capabilities of different turbulence models *k*- ε estándar, *k*-ε RNG, *k*-ε realizable, *k*-ε estándar, SST k-ω, etc.) to predict the airflow pattern and indoor environmental parameters for natural, forced and mixed convection flows in laboratory enclosed cavities and in real offices or atriums. Table 1 summarizes some of these studies which cover a broad range of turbulence models, from simpler turbulence models such as zero-equation model of Chen and Xu (1998) to more advanced models such as detached-eddy simulation models of (Shur et al. 1999). The table provides a performance evaluation of different turbulence models to predict temperature and velocity from "A" to "D" according to the information provided in the revised studies. "A", "B", "C" and "D" mean that errors between measurements and simulations are less than 20%, between 20 and 30%, between 30 and 40%, and over 40%, respectively.

**Table 1.** Literature review on performance of turbulence models

It is observed that several authors have evaluated k-ω standard and k-ω SST models for NC, showing very good performance of these turbulence models to predict temperature and velocity. A couple of studies (Choi & Kim, 2012; Zhang et al., 2007) have also shown very good performance of v2f and its variation v2f-dav for NC.

For FC, k- ε standard and k-ε RNG models show very good results for temperature and slightly lower performance for velocity. Zhang et al. (2007) showed that the v2f-dav and LES models also provide very good predictions of indoor air conditions for FC. The k-ω SST model was evaluated by Cao et al. (2011) and Zhang et al. (2007) but their results have been extremely different. In fact, while Cao et al. (2011) found the k-ω SST model provides excellent results, Zhang et al. (2007) found that its performance was poor.

For MC, evaluation errors fall under "A" or "B" ranges for all turbulence models. Rohdin and Moshfegh (2011) evaluated several variants of k-ε models (standard, RNG and Realizable) in large industrial rooms. While all these turbulence models predict well the airflow conditions, the RNG showed the best results even for pollutant transport in large rooms. Zhang et al. (2007) found that the zero-equation, k-ε RNG and v2f-dav models predict well airflow conditions in enclosed cavities with low Raleigh number. Stamous and Katsiris (2006) evaluated several turbulence models in offices. They concluded that all evaluated models predict well temperature and velocity, however, the k-ω SST model performs better when a proper mesh is used.

**2.2 Experimental studies**

Complete datasets for experimental studies on indoor air conditions in enclosed cavities are needed to be able to validate CFD models and evaluate different two-equation eddy-viscosity models. This paper shows the validation procedure for fundamental cases of natural, forced and mixed convection according to ASHRAE guidelines (Chen and Srebric 2001).

Figure 1 shows the enclosed cavities for each convection flow, which are briefly described as follows:

• Natural convection: Ampofo and Karayiannis (2003) carried out a natural convection experiment in a square cavity where 2D flow occurs. This experiment consists in a cavity of 0.75 x 0.75 m and 1.5 m deep (Figure 1a) with hot and cold side walls at 50°C and 10°C, respectively; thus Ra number is 1.58x10^{9}. The top and bottom walls are highly insulated. The fluid properties are Cp = 1006.43 J/kg·°K, λ= 0.0242 W/m·°K, *µ* = 1.7894x10^{–5} kg/m·s, and a molecular mass of 28.966 g/mol.

• Forced convection: The isothermal Annex 20 room of Restivo (1979) and described in Nielsen (1990) consists in a room with 2D forced convection flow (Figure 1b). The air supply is provided by an inlet slot at air velocity of 0.455 m/s and air temperature of 20°C. The room is 9.0 x 3.0 m, the inlet height is 0.168 m and the outlet height is 0.48 m. The kinematic viscosity of inlet air is 15.3x106 m2/s, thus Re is 5.000 based on the inlet height and its air conditions. According to Nielsen (1990), the turbulent intensity based on inlet conditions is 4%.

• Mixed convection: Blay et al. (1992) developed an experimental apparatus of 1.04 x 1.04 x 0.7 m giving a 2D flow (Figure 1c). Air is supplied from the inlet slot at temperature and air velocity of 15°C and 0.57 m/s, respectively. The outlets are placed at the floor level on the opposite wall. The wall temperature is 15°C while the floor temperature is 35.5°C. Thus, Re based on the inlet condition is 684. The measured turbulence intensity at the inlet is 6%.

**Figure 1.** Experimental cavities for NC, FC, and MC cases (length dimensions are in mm)

**3. CFD modeling of basic convection cases**

The evaluation of five two-equation eddy-viscosity models for each convection case shown in Figure 1is presented in this section. Each case is an opportunity for CFD beginners to acquire skills and confidence on modeling indoor environments. Five models are evaluated using the latest version of FLUENT:

• k-ε standard (Launder & Spalding., 1974)

• k-ε RNG (Yakhot & Orszag, 1986)

• k-ε Realizable (Shih et al.,1995)

• k-ω standard (Wilcox, 1988)

• k-ω SST (Menter, 1994)

For each convection case, the validation procedure follows the processes shown in Figure 2, which is an adaptation of the validation process proposed by Hajdukiewicz et al. (2013). The first step consists of generating an initial CFD model and test grid independency. This test consists of verifying that simulated results do not vary significantly for different mesh sizes. Thus, a mesh size is choosing among mesh sizes that passed the test balancing accuracy of results and computing time.

This initial model requires several inputs such as geometry that represents the problems, boundary conditions, parameters related to the physics of the problems (i.e. 2D or 3D, steady state or transient), initial mesh and turbulence model. To start verifying grid independency, a coarse mesh is set initially. Then, the number of mesh elements is increased consecutively and grid refinement is performed in certain zones (i.e. regions close to walls, inlet). Mesh size independency is achieved when close results are obtained. Once grid independency is obtained, a mesh size is chosen balancing accuracy of simulated results and computing time.

Then, the validation procedure is carried out. This implies that some parameters of the initial CFD model might need to be modified (i.e. under-relaxation factors, mesh refinements, etc.) to accommodate requirements of each model. Since the mesh is tested for independency of the results, the under-relaxation factors are modified in this study for each convection case and turbulence model to allow convergence and accurate simulation results.

** Figure 2.** Process flow for CFD validation as excercise for new users to acquire CFD modeling skills

**3.1 Natural convection (NC)
3.1.1 Initial CFD model**

The experiment shown in Figure 1a was modeled as 2D base don information reported by Ampofo and Karayiannis (2003). It was not possible to reach convergence when the problem was defined as steady-state. This result agrees with similar studies that have modeled the same experiment (Rundle & Lighstone, 2007). Thus, the problem was modeled as transient with a time step size of 0.19 s. It is worthy to notice that time step setting is not straight forward. Smaller time-steps could allow more accurate results but it is more difficult to reach convergence. The initial turbulence model was set as k-ω standard because it shows good performance according to the literature review shown in Table 1. Table 2 shows the main CFD setup parameters for the initial CFD model.

The hot and cold temperatures (Th and Tc in Figure 1a) were set as boundary conditions of the hot and cold side walls, respectively. The top and bottom walls were set as adiabatic because they were highly insulated, thus heat flows through them are supposed to be negligible.

**Table 2.** CFD setup parameters of NC case

Convergence criteria were 10-³ for all parameters except for energy. ANSYS (2012) recommends a convergence criterion for energy of 10^{–6}. However, it was not possible to obtain convergence with this criterion, thus, it was increased to 10^{–4} to reach convergence. Moreover, default under-relaxation factors needed to be modified to obtain convergence. The sum of residual errors met convergence criteria at 2,023 iterations as shown in Figure 3. At this iterations number results were not satisfactory and simulations were performed until 4,000 iterations. Although the fluid flow is developed at 2,000 iterations as shown in Figure 4, the temperature distribution is right after 4,000 iterations only. Hot air rises along the hot wall while cold air drops down along the cold wall, and temperature stratification occurs.

**Figure 3.** Residuals for NC case with k-ω standard

**Figure 4.** Temperature distribution for NC case at different iterations with k-ω standard

**3.1.2. Verification of grid independency**

Since the simplified geometry of the experiment of Ampofo and Karayiannis (2003), the mesh is composed for quads elements in a uniform distribution (structured mesh) as shown in Figure 5a. The mesh was refined close to the walls to be able to transfer properly the boundary conditions to the air domain. In fact, large gradients of temperature and velocity occurs in the zone close to the walls, thus a finer mesh allow predicting these gradients more accurately. A coarser mesh is observed in the center of cavity where the air parameters show very low variation.Grid independency verification was carried out for mesh sizes of 79x79, 94x94, 125x125 and 188x188. Figures 6a and 7a shows the temperature and velocity at midheight of the square cavity (Y/H = 0.5). It is observed that all mesh sizes predict well the velocity and temperature in the center of the cavity at Y/H = 0.5. The maximum difference between the simulated and experimental data is 0.23% for mesh 94x94, which is negligible.

Nevertheless, Figure 6b shows that the CFD model with mesh 125x125 predicts better the temperature drop close to the hot wall. On the other hand, Figure 7b shows that the coarsest mesh predicts very well the velocity close to the hot and cold walls, while the other meshes underpredict it significantly between X/L 0.01 and 0.05. Based on the overall performance, the mesh size of 125x125 is chosen to proceed with the CFD validation process.

**Figure 5.** Mesh grid initial CFD model for NC, FC and MC cases

**Figure 6.** Grid independency test: a) Dimensionless temperature along Y/H=0.5. b) Dimensionless temperature close to the hot wall

**Figure 7.** Grid independency test a) Velocity along Y/H=0.5. b) Velocity close to the hot wall in m/s

**3.1.3 CFD model validation**

CFD validation is carried out comparing the simulation results for the five turbulence models and experimental data reported in Ampofo and Karayiannis (2003) for temperature and velocity at Y/H = 0.5. Overall, Figures 8a and 9a show that all evaluated turbulence models predict very well the temperature and velocity distribution at midheight of the square cavity. The five two-eddy viscosity models are able to predict the large variation of temperature and velocity close to the hot and cold walls as well as the constant temperature and velocity at the middle section of the cavity.

Despite this good overall performance of all evaluated k-ε and k-ω models, their performance vary significantly in the region close to walls. Figure 8b shows that k-ω standard predicts better the temperature variation close to the hot wall, while the model k-ω SST presents the largest variation from the experimental results. Furthermore, Figure 9b shows that both variation of k-ω model (standard and SST) do not predict the variation of velocity close to the hot walls as well as the k-ε models. The k-ω SST overpredicts the peak velocity and underpredicts the velocity drop in the outer border of the boundary layer. The simulated results with k-ω SST show differences up to 13.4% with experimental data, which is the largest difference among evaluated two-eddy viscosity models. Similar limitations of k-ω SST to predict velocity in the boundary layer were found also by Rundle and Lighstone (2007) and Zitzmann et al. (2005). On the other hand, the k-ε RNG and Realizable show excellent performance predicting the air velocity close to the hot and cold walls.

These results show that convergence was difficult to reach even for this basic NC case. The problem needed to be modeled as transient and under-relaxation factors and convergence criterion for energy were modified to get convergence and reliable results. Modification of these factors is not intuitive and requires specialized knowledge.

Also, it was found that simulated results in the region close to walls vary significantly among turbulence models. Accurate predictions of what happen in this region are crucial because the heat and mass transfer between walls and air occurs in this zone. This could have great influence on the predicted room air conditions (temperature, velocity, moisture content, pollutant concentration). This fact emphasizes the need of CFD beginners to be aware that choosing the right turbulence model to indoor environmental conditions. New CFD users need to get experience on CFD modeling. Otherwise, the CFD model and results may not be reliable.

**Figure 8.** Performance of two-eddy viscosity models for NC: a) Dimensioless temperature along Y/H=0,5. b) Dimensionless temperature close to the hot wall

**Figure 9.** Performance of two-eddy viscosity modles for NC: a) Velocity along Y/H=0,5. b) Velocity close to the hot wall

**3.2. Forced convection (FC)**

Since a similar process to NC case was carried to create the initial CFD model and verification of grid independency for FC case, this section focuses on the validation procedure via the evaluation of the turbulence models. Table 3 shows the main CFD setup parameters for the k-_ RNG model. The experimental setup of Restivo (1979) was modeled as 2D and steady-state. Since this setup is isothermal, the air inlet supply is the main factor that influences the airflow pattern. Figure 5b shows a structured grid of 40x120 quad elements. The mesh was refined close to the walls and inlet supply to properly transfer the heat and mass flow from the boundaries to the air domain.

**Table 3.** CFD setup parameters of FC case

The same under-relaxation factors used for NC case were used in this CFD model. Although convergence criterion for energy was more stringent than that for NC case, convergence was obtained in short time (650 iterations). Figure 10 shows the comparison of the airflow pattern for the initial CFD model. It is observed a clockwise airflow with a strong jet throw under the ceiling due to the air inlet. This result is in good agreement with other CFD simulation studies (Olmedo and Nielsen 2010).

**Figure 10.** Airflow pattern for initial CFD model for FC

The evaluation of the five turbulence models is carried out for velocity at the vertical plane at X = 2 m. Results of each turbulence model and experimental data reported in Nielsen (1990) are shown in Figure 11. It can be observed that all turbulence models predict the general airflow pattern, a jet throw close to the top wall of the experimental cavity, and a reverse flow close to the bottom wall. Overall, velocities predicted by all evaluated k-ε and k-ω models are in good agreements with velocities along the cavity height at X = 2 m. However, significant differences on predicted velocities among turbulence models are observed close to the top and bottom walls. In this zone, the k-ε standard and RNG predict very well the reverse flow close to the floor and the jet throw close to the ceiling, showing the best performance with differences lower than 7% (or 0.009 m/s) with the experimental data. Otherwise, the k-ε Realizable model shows the largest differences, 21.3% or 0.05 m/s.

**Figure 11.** Performance of two-eddy viscosity models to predict temperature along X=2m for FC case

Similarly to NC case, significant variation of simulated air velocity close to the floor is found among turbulence models, and the k-ε RNG predict well the whole air domain. In contrast with NC case, k-ε Realizable shows poor performance predicting air velocity. This result evidences that the performance of turbulence models could strongly depend on the quantity predicted and airflow type.

**3.3 Mixed convection (MC)**

The mixed convection experiment of Blay et al. (1992) is modeled via CFD technique. This experiment has been widely used to validate new CFD models. The airflow is influenced by inertia forces due to the air supply and buoyancy forces due to the temperature differences on the walls.

Figure 5c shows the mesh of 60x60 elements used to model this experiment. Table 4 summarizes the main setup parameters of CFD modeling with the k-ε Realizable. Convergence was obtained at 350 iterations. However, different under-relaxation factors were used to allow obtaining accurate results.

**Table 4.** CFD setup paramenters of MC case

Figure 12 shows the flow pattern obtained with different turbulence models and those observed experimentally by Blay et al. (1992). It is observed that all evaluated turbulence models predicts well the clockwise airflow pattern. However, k-ε Realizable and both k-ω models predict a large eddy in the upper-right corner of the cavity that is not predicted by the k-ε standard and RNG models. Due to the lack of more detailed experimental data showing this eddy, it is not possible to get conclusions about the accuracy of the turbulence models to predict this particular feature of the airflow.

** Figure 12.** Comparison of airflow pattern for different turbulence models and experiment

This section focuses on validation procedure and evaluation of the turbulence models. In this case, the validation is based on the velocity and temperature measurements carried out by at the middle height (Y = 0.52 m) and middle width (X = 0.52) of the cavity as shown in Figure 1c. Figures 13 and 14 shows the temperature and velocity at X = 0.52 and Y = 0.52, respectively. In Figures 13a and 14a, it is observed that k-ω models significantly underpredict the temperature by 1°C along the midwidth and midheight of the cavity. On the other hand, the simulation results of temperature for k-ε models are in good agreement with experimental data. Among the k-ε models, the Realizable variant shows a better performance because it accurately predicts the temperature distribution close to the boundary layer and along the core of the cavity. The maximum differences between the experimental and simulation data for k-ε Realizable are 0.97% and 1.3% at Y = 0.52 m and X = 0.52 m, respectively.

Velocity profiles at X = 0.52 m and Y = 0.52 m are shown in Figures 13b and 14b. It is observed that all turbulence models predict the general pattern of the airflow but large discrepancies occur close to the walls. The standard versions of the k-ε and k-ω models predict better the air velocities in the regions far from the walls. Also, both turbulence models predicts well the air velocities close to the top wall at X = 0.52 and close to the right wall at Y = 0.52 m. However, these models significantly underpredict the reverse flow close to the bottom wall at X = 0.52 m and the vertical velocity close to the left wall at Y = 0.52 where maximum differences are close to 0.1 m/s. In these zones where large velocity gradients occur, the k-ε RNG model performs better.

In these case, it can observed similar results than that for NC and FC cases. However, performance of turbulence models to predict temperature across de air domain varies more significantly. It is notorious that k-ω models underpredict temperature not only close to walls but also across the cavity core.

**Figure 13.** Performance of CFD model to predict temperature and air velocity at X=0.52m for MC case

**Figure 14.** Performance el CFD model to predict temperature and air velocity at Y=0.52m for MC case

**4. Discussion and final remarks**

CFD modeling is not an intuitive process and requires taking decisions about several parameters such as representative geometry, mesh size and topology, convergence criteria, under-relaxation factors, turbulence model, among others. The main source of errors in CFD modeling is the lack of users´ expertise.

The main objective of this study was to provide more complete CFD modeling information of basic natural, forced and mixed convection flows that allows CFD beginners to acquire skills and confidence on CFD modeling. This paper provides a procedure, criteria and engineering judgment to evaluate five k-ε and k-ω turbulence models. Modeling these three basics flow in enclosed environments with different two-eddy viscosity models is proposed as exercise for new CFD users to obtain expertise on CFD modeling.

The results evidences that reliable and robust CFD results require users' skills on CFD modeling, even for the basics indoor airflows studied in this paper. The main general conclusions that can be drawn from this study are:

• Overall, the five evaluated k-ε and k-ω model performs well predicting air velocity and temperature. However, their accuracy depends on the convection type, quantity predicted and regions of the air domain. Therefore, the use of the right turbulence models is crucial to obtain reliable results. Literature review provides evidence about which turbulence models perform better for different cases. However, studies from different authors is not always in good agreement due to particularities of the case studied and other CFD modeling parameters that also influences the results (i.e. mesh size and topology).

• Predicted indoor conditions for temperature and air velocity in the boundary layer region might vary significantly among k-ε and k-ω models. Accurate predictions of what happen in this region are crucial because the heat and mass transfer between walls and air occurs in this zone. This could have great influence on the predicted room air conditions (temperature, velocity, moisture content, pollutant concentration). This fact strongly support that new CFD users need to acquire skills on CFD modeling even for the basic convection flows reviewed in this paper.

• Convergence cannot be given for granted, especially for natural convection cases. The setting up of time step and under-relaxation factors is needed, which involves advanced knowledge and expertise of the CFD modeler even for basic indoor environmental problems.

• The basic convection cases studied in this paper are good exercises to get skills on CFD modeling of indoor environments. This paper provides information and engineering judgment that allow new CFD users to properly model these cases and obtain robust and reliable CFD models and results.

**5. Acknowledgements**

This work was funded by the National Commission for Science and Technological Research (Conicyt) of Chile under the grants Fondecyt 11100120 and supported by the research project CONICYT/FONDAP 15110020.

**6. References**

** AIAA (1998),** Guide for the Verification and Validation of Computational Fluid Dynamics Simulations. American Insitute of Aeronautics and Astronautics.

** ANSYS (2012), **Ansys FLUENT Theory Guide: Release 14.0. ANSYS, Inc.

** Ampofo F. and Karayiannis T. (2003),** Experimental benchmark data for turbulent natural convection in an air filled square cavity. International Journal of Heat and Mass Transfer , 3551-3572. doi: http://dx.doi.org/10.1016/S0017-9310(03)00147-9.

** Blay D., Mergui S. and Niculae C. (1992),** Confined turbulent mixed convection in the presence of a horizontal buoyant wall jet. In Fundamentals of Mixed Convection, ASME HTD 213.

** Cao G., Ruponen M., Paavilainen R. and Kurnitski J. (2011),** Modelling and simulation of the near-wall velocity of a turbulent ceiling attached plane jet after its impingement with the corner. Building and Environment, 46 (2), 489-500. doi: http://dx.doi.org/10.1016/j.buildenv.2010.08.012.

** Casey M. and Wintergeste T. (2000),** ERCOFTAC Special Interest Group on Quality and Trust in Industrial CFD - Best Practice Guidelines.

* Chen Q. and Xu W. (1998),* A zero-equation turbulence model for indoor airflow simulation. Energy and Buildings, 28(2), 137-144. http://dx.doi.org/10.1016/S0378-7788(98)00020-6

** Chen Q. and Srebric J. (2001),** How to Verify, Validate and Report Indoor Environment Modeling CFD Analyses. Atlanta: ASHRAE.

** Choi S. K. and Kim S. O. (2012),** Turbulence modeling of natural convection in enclosures: A review. Journal of Mechanical Science and Technology , 283-297. doi: 10.1007/s12206-011-1037-0.

** Choi S.-K., Kim E.-K., Wi M.-H. and Kim S.-O. (2004),** Computation of a turbulent natural convection in a rectangular cavity with the low-reynolds-number differential stress and flux model. KSME International Journal , 18, 1782-1798. doi: 10.1007/bf02984327

** Hajdukiewicz M., Geron M., and Keane M. M. (2013),** Formal calibration methodology for CFD models of naturally ventilated indoor environments. Building and Environment , 56, 290-302. doi: http://dx.doi.org/10.1016/j.buildenv.2012.08.027.

** Klobut K. and Sirén K. (1994), **Air flows measured in large openings in a horizontal partition. Building and Environment , 29 (3), 325-335.

** Launder B. and Spalding D. (1974),** The numerical computation of turbulent flows. Computer Methods in Applied Mechanics and Energy, 3, 269-289. http://dx.doi.org/10.1016/0045-7825(74)90029-2

** Menter F. (1994),** Two-equation eddy-viscosity turbulence models for engineering applications. AIAA Journal , 32, 1598-1605. doi: 10.2514/3.12149.

** Moureh J. and Flick D. (2003), **Wall air-jet characteristics and airflow patterns within a slot ventilated enclosure. International Journal of Thermal Sciences, 42, 703-711. http://dx.doi.org/10.1016/S1290-0729(03)00037-1.

** Nielsen P. V. (1974),** Flow in air conditioned room. Copenhagen.: Technical University of Denmark.

** Nielsen P. V. (1990),** Specification of a two-diemnsional test-case. Department of Building Technology and Structural Engineering, Aalborg University, Denmark.

** Oberkampf W. L. and Trucano. T. G. (2002),** Verification and validation in computational fluid dynamics. Progress in Aerospace Sciences , 38 (3), 209-272. doi: http://dx.doi.org/10.1016/S0376-0421(02)00005-2.

** Olmedo I. and Nielsen P.V. (2010),** Analysis of the IEA 2D test. 2D, 3D, steady or unsteady airflow? Department of Civil Engineering, Aalborg University (DCE Technical Reports; No.106).

** Omri M. and Galanis N. (2007),** Numerical analysis of turbulent buoyant flows in enclosures: Influence of grid and boundary conditions. International Journal of Thermal Science, 46(8), 727-738. doi: http://dx.doi.org/10.1016/j.ijthermalsci.2006.10.006.

** Posner J. D., Buchanan C. R. and Dunn-Rankin D. (2003),** Measurement and prediction of indoor air flow in a model room. Energy and Buildings , 35, 515-526. doi: http://dx.doi.org/10.1016/S0378-7788(02)00163-9.

** Restivo A. (1979), **Turbulent Flow in Ventilated Room. London: Ph.D. Thesis, University of London.

** Rohdin P. and Moshfegh B. (2011),** Numerical modelling of industrial indoor environments: A comparison between different turbulence models and supply systems supported by field measurements. Building and Environment, 46, 2365-2374.doi: http://dx.doi.org/10.1016/j.buildenv.2011.05.019

** Rundle C. A. and Lighstone M. F. (2007),** Validation of turbulent natural convection in square cavity for application of CFD modelling to heat transfer and fluid flow in atria geometries. 2nd Canadian Solar Building Conference. Calgary, Canada.

** Rundle C., Lightstone M., Oosthuizen P., Karava P. and Mouriki E. (2011),** Validation of computational fluid dynamics simulations for atria geometries. Building and Environment , 1943-1353. doi: http://dx.doi.org/10.1016/j.buildenv.2010.12.019.

** Shih T., Liou W., Shabbir A., Yang Z. and Zhu J. (1995),** A new k-_ eddy viscosity model for high reynolds number turbulent flows. Computers & Fluids , 24, 227-238. doi: http://dx.doi.org/10.1016/0045-7930(94)00032-T.

** Shur M., Spalart P., Strelets M. and Travin A. (1999),** Detached-eddy simulation of an airfoil at high angle of attack. Engineering turbulence modelling and experiments -4. Proceedings of the 4th International Symposium on Engineering Turbulence Modeling and Experiments, 669-678.

** Stamou A., and Katsiris I. (2006),** Verification of a CFD model for indoor airflow and heat transfer. Building and Environment , 41, 1171-1181. doi: http://dx.doi.org/10.1016/j.buildenv.2005.06.029.

** Susin R. M., Lindner G. A., Mariani V. C. and Mendonça K. C. (2009),** Evaluating the influence of the width of inlet slot on the prediction of indoor airflow: Comparison with experimental data. Building and Environment, 44, 971-986. doi: http://dx.doi.org/10.1016/j.buildenv.2008.06.021.

** Vera S., Fazio P. and Rao J. (2010),** Interzonal air and moisture transport through large horizontal openings in a full-scale two-story test-hut: Part 2 - CFD study. Building and Environment , 45 (3), 622-631. doi: 10.1016/j.buildenv.2009.07.021.

** Voigt L. K. (2000),** Comparison of Turbulence Models for Numerical Calculation of Airflow in an annex 20 Room. . International Centre for Indoor Environment and Energy.Department of Energy Engineering.Technical University of Denmark.

** Wilcox D. (1988),** Reassessment of the scale-determining equation for advanced turbulence models. AIAA Journal , 26, 1299-1310. doi: 10.2514/3.10041.

** Yakhot V. and Orszag S. (1986),** Renormalization group analysis of turbulence. Journal of Scientific , 1, 3-51.

** Zhai Z., Zhang Z., Zhang W. and Chen Q. (2007),** Evaluation of Various Turbulence Models in Predicting Airflow and Turbulence in Enclosed Environments by CFD: Part 1- Summary of Prevalent Turbulence Models. HVAC&R RESEARCH , 853-870. doi: 10.1080/10789669.2007.10391459

** Zhang Z., Zhang W., Zhai Z. J. and Chen Q. Y. (2007),** Evaluation of Various Turbulence Models in Predicting Airflow and Turbulence in Enclosed Environments by CFD: Part 2-Comparison with Experimental Data from Literature. HVAC&R Research , 13 (6), 871-886. doi: 10.1080/10789669.2007.10391460.

** Zitzmann T. and Cook M. P. (2005),** Simulation fo steady-state natural convection using CFD. Building Simulation. Montréal, Canada.

E-mail: svera@ing.puc.cl

Fecha de Recepción: 22/01/2014 Fecha de Aceptación: 04/03/2014

### Refbacks

- There are currently no refbacks.

Copyright (c)