Summary of best guidelines and validation of CFD ...

4 downloads 25368 Views 2MB Size Report
marizing the guideline and/or best practice for CFD modeling, the authors addressed the ... 2007; Seo and Lee, 2013; Yu et al., 2010) from livestock buildings.
Computers and Electronics in Agriculture 121 (2016) 180–190

Contents lists available at ScienceDirect

Computers and Electronics in Agriculture journal homepage: www.elsevier.com/locate/compag

Original papers

Summary of best guidelines and validation of CFD modeling in livestock buildings to ensure prediction quality Li Rong a,⇑, Peter V. Nielsen b, Bjarne Bjerg c, Guoqiang Zhang a a

Department of Engineering, Aarhus University, Inge Lehmanns Gade 10, 8000 Aarhus C, Denmark Department of Civil Engineering, Aalborg University, Sofiendalsvej 11, 9200 Aalborg SV, Denmark c Department of Large Animal Sciences, University of Copenhagen, Groennegaardsvej 2, DK1870 Frederiksberg C, Denmark b

a r t i c l e

i n f o

Article history: Received 21 August 2015 Received in revised form 30 October 2015 Accepted 6 December 2015

Keywords: Validation CFD RANS model Numerical method Livestock building

a b s t r a c t Computational Fluid Dynamics (CFD) is increasingly used to study airflow around and in livestock buildings, to develop technologies to mitigate emissions and to predict the contaminant dispersion from livestock buildings. In this paper, an example of air flow distribution in a room with two full scale pig barns was simulated to show the procedures of validating a CFD simulation in livestock buildings. After summarizing the guideline and/or best practice for CFD modeling, the authors addressed the issues related to numerical methods and the governing equations, which were limited to RANS models. Although it is not necessary to maintain the same format of reporting the CFD modeling as presented in this paper, the authors would suggest including all the information related to the selection of turbulence models, difference schemes, convergence criteria, boundary conditions, geometry simplification, simulating domain etc. This information is particularly important for the readers to evaluate the quality of the CFD simulation results. Ó 2015 Elsevier B.V. All rights reserved.

1. Introduction CFD modeling has been increasingly used to study airflow in the livestock buildings (Bjerg et al., 2000, 2002; Blanes-Vidal et al., 2008; Bustamante et al., 2013, 2015; Humbert et al., 2014; Kwon et al., 2011; Lee et al., 2013; Mistriotis et al., 1997; Norton et al., 2010c, 2007; Rahman et al., 2014; Rong et al., 2010a; Sun et al., 2000; Worley and Manbeck, 1995; Zajícˇek and Kic, 2013; Zhu et al., 2012), develop technologies to control the ammonia emissions (Bjerg et al., 2013; Reynolds, 1997; Rong et al., 2011, 2010b; Saha et al., 2011; Sapounas et al., 2009; Wu et al., 2012b, 2013; Zong and Zhang, 2014), natural ventilation of livestock buildings (Bartzanas et al., 2013; Norton et al., 2009, 2010a, 2010b, 2010d; Ntinas et al., 2014; Rong et al., 2015; Sapounas et al., 2013; Saraz et al., 2012; Seo et al., 2009; Shen et al., 2012; Wu et al., 2012a; Zong et al., 2013), and predict the contaminant dispersion (Hong et al., 2011, 2013; Li and Guo, 2006; Lin et al., 2007; Seo and Lee, 2013; Yu et al., 2010) from livestock buildings owing to successful experience observed from indoor climate, environmental engineering, civil and mechanical engineering etc.

⇑ Corresponding author. Tel.: +45 50248562. E-mail address: [email protected] (L. Rong). http://dx.doi.org/10.1016/j.compag.2015.12.005 0168-1699/Ó 2015 Elsevier B.V. All rights reserved.

Good review papers about CFD application in indoor environment can be found in Nielsen (2004, 2015), Chen (2009) and Li and Nielsen (2011). Computational Fluid Dynamics (CFD) modeling has been first introduced by Nielsen in 1970s (Nielsen, 1973) for the prediction of air movement in a ventilated room. Due to the development of efficient numerical discretization methods, ability to implement these methods on computers and great increase of computer power, the CFD modeling has been routinely applied in research and teaching at area of indoor climate and other different research disciplines. It is well recognized that CFD modeling allows full control of the boundary conditions, provides data for each point at the computational domain simultaneously, and can handle the complex geometry well in full scale. Comparing to full scale laboratory measurements, scaled model tests and wind tunnel experiments, CFD modeling is also able to allow efficient parametric analysis of different configuration and for various conditions. However, the CFD modeling has not replaced the experimental method since the experiments can support CFD modeling as benchmark tests (Nielsen, 2015). It is imperative to ensure the accuracy and reliability of CFD modeling and thus perform the verification and validation studies. The accuracy and reliability of CFD modeling is dependent on not only the theoretical fundamentals but also the user’s experi-

L. Rong et al. / Computers and Electronics in Agriculture 121 (2016) 180–190

ence, so it is a theory-based and process-based method (Blocken and Gualtieri, 2012). The fundamental equations of fluid dynamics, that is Navier–Stokes equations, have been known since 19th century, which formed the basis of CFD modeling. In addition, the indoor and outdoor flow is generally turbulent. During the process of CFD modeling, one of the important decisions made by the CFD users is to select the appropriate turbulence models which are solved to describe the turbulent flow. Four modeling approaches have been developed, which are Direct Numerical Simulation (DNS), Large Eddy Simulation (LES), Reynolds-Averaged Navier– Stokes (RANS) and Scale-Resolving Simulation (SRS) (in fact, LES is also one of the SRS). DNS solves the Navier–Stokes equations directly down to the smallest length and time scales without implementing any assumptions and/or sub-models while it is extremely time consuming and limited the application to relatively low Reynolds number. LES uses a filter on Navier–Stokes equation, in which the eddies larger than a certain filter size are directly resolved while the effect of the eddies smaller than the filter size is approximately modeled by subgrid modeling. Although applications of LES are envisaged in engineering design and industry, it is still too computationally expensive to allow routine simulations. RANS are the most widely applied modeling methods which only resolve the mean flow and the turbulence scales is modeled (Chen, 1995; Zhai et al., 2007; Zhang et al., 2007). RANS models have shown strength for modeling wall-bounded flow but not accurate enough for modeling the free shear flow. It is becoming increasingly clear that certain classes of flows should be covered by models in which part of the turbulence spectrum is resolved in a portion of the numerical domain at least. Thus SRS models are developed for improving the accuracy which cannot be achieved by RANS models. More details about the turbulence modeling can refer to Wilcox (2006), Menter (2009), Menter et al. (2011) and Launder and Spalding (1974). In this paper, further introduction of RANS models will be given in Section 2. It is also widely recognized that the CFD users should determine a range of computational parameters which may greatly affect the accuracy of the simulation results besides turbulence models. These parameters include the boundary conditions, computational domain and mesh, discretization schemes, convergence criteria etc. Before running a CFD simulation, a few questions should be considered as stated by Nielsen (2015): ‘Is flow expected to be laminar or turbulent? Which turbulence models should be selected? Is the flow expected to be steady or unsteady? Is the flow expected to have one solution or several solutions? Is the flow 2D symmetrical or 3D asymmetrical?’ Whether the CFD users can make the correct decisions on all these questions influences greatly the accuracy of the CFD modeling. During the past decades, many researchers conducted detailed verification and validation exercises and consequently quite a few best practice guidelines for CFD modeling have been documented. However, our experience of reviewing the papers for journals in research area of livestock buildings and the workshop hold in Wageningen University in January 2015 inspires the idea to complete this paper. It is necessary to provide some guidance for the young researchers and students who are just starting to use CFD modeling for their studies and research in this area. Therefore, this paper is going to (1) summarize the best practice guidelines for CFD modeling; (2) briefly clarify the issues related to RANS models for quality control of CFD modeling; (3) provide a case study of validation for CFD modeling in a full scale pig barn with detailed experimental data. It should be clarified that validation of CFD modeling is not a new topic, but through this effort, we hope that the new CFD users conducting CFD modeling for livestock buildings can obtain some hints when making the important decisions during the CFD modeling and thus the sufficient accuracy of CFD simulations can be ensured.

181

2. Quality control of CFD modeling 2.1. Summarization of best guidelines for CFD modeling Guidelines are needed to implement quality control of CFD modeling so that the sufficient accuracy can be achieved and the reporting results are interpreted clearly to enable readers for judgement of the quality. Indeed, several scientific journals in fluid mechanical engineering and indoor environment have issued policy statements regarding CFD simulation papers. For example, a full assessment of the quality of CFD papers in Indoor Air has been suggested by Sørensen and Nielsen (2003a) because the editors would promote the papers using CFD as a research tool. It required ‘(1) adequate information pertinent to the governing equations and numerical methods and (2) justified estimates of expected accuracy of numerical results’. The editorial board of the Journal of Fluids Engineering, published by the American Society of Mechanical Engineers (ASME), has also issued policy statement for publication of computational results in the journal (Roache et al., 1986) that any papers relating to CFD modeling or numerical simulation would not be accepted for publication if accuracy estimation and truncation error testing was not addressed, and then followed by a more detailed policy statement (Freitas, 1993) with a list of guidelines and criteria for publication of CFD and numerical results in this journal. In 2000, Casey and Wintergerste (2000) edited a Best Practice Guideline for improving the credibility of CFD application in industry. It was published by the European Research Community on Flow, Turbulence and Combustion (ERCOFTC), which has a special interest group on Quality and Trust in Industrial CFD. It summarized the guidelines on turbulence modeling (focus on RANS models), wall functions, definition of geometry, grids, boundary conditions, convergence, discretization schemes, assessment of errors, interpretation and documentation. Although these guidelines were not developed specifically for CFD simulation in livestock buildings, many of these guidelines also apply for it. These guidelines devoted much attention on avoiding errors and uncertainties in CFD simulation from the perspective of the users who use the well-developed and reputational CFD code and/or commercial CFD software. Another valuable guideline for CFD users in the area of livestock buildings can refer to Best Practice Guideline for the CFD Simulation of Flows in the Urban Environment, which was published by Franke et al. (2007). It focused on the improvement and quality assurance of CFD simulation to predict the flow and transport processes in urban and industrial environments. It is beneficial for CFD users who conduct CFD simulation for naturally ventilated livestock buildings and contaminant dispersion. This guideline addressed the selection of target variables, approximate equations of the obstacles, computational domain, boundary conditions, initial conditions, computational grid, time step size (for unsteady simulation), numerical approximations and iterative convergence criteria. This publication is very useful for all CFD users. The other Best Guidelines applied in the research area of open channel and reactor-safety are also available and can be referred to Knight et al. (2005) and Menter (2002). With applying the guidelines, it is also imperative to perform the validation of CFD simulation when submitting an article to a journal. Guides and standards on verification and validation of CFD simulation can be found in AIAA (1998) and Stern et al. (2001). As reported by Roache (1997), verification means ‘solving the equations right’ while validation means ‘solving the right equations’. Computational Fluid Dynamics refers exactly to these two parts. The selection of governing equations for solution of a defined problem i.e. physical properties, boundary conditions, turbulence models etc. is the content of ‘Fluid dynamics’, which is solving the

182

L. Rong et al. / Computers and Electronics in Agriculture 121 (2016) 180–190

right equations. The selection of numerical methods i.e. discretization schemes, computational grid, convergence etc. is referred by ‘Computational’, which is solving the equations right. In this paper, the application of CFD simulation is conducted in a full scale pig barn with slatted floor. We assume that the boundary conditions can be defined appropriately by users. Thus we mainly focus on the issues of governing equations, numerical methods and grid refinement related to RANS models, which are the most widely used in present CFD simulations in livestock buildings. 2.2. RANS modeling The ventilation systems installed in the pig buildings in Denmark is most frequently as a negative pressure system with either side wall jet air supply or diffuse ceiling air supply. The flow in these ventilated buildings is generally incompressible and turbulent due to the velocity level and the dimensions. RANS modeling solves the mean flow variables (contained in the Reynolds stress tensor) by using turbulence transport models. Generally, most of the RANS models assume the turbulence isotropic, known as eddy viscosity models which use Bousinessq assumption, but Reynolds stress model allows for anisotropic turbulence as it models all additional Reynolds stress terms without using Bousinessq assumption. The models by using RANS method consist of zeroequation turbulence model, one-equation turbulence model, twoequation turbulence model, multi-equation turbulence model and RANS Reynolds stress model. In this paper, three of them are introduced briefly and more details about them can be found in the cited references accordingly. The governing equations can be written in a general form as follows

q

    @/ @/ @ @/ j þ S/ þ qu ¼ C/;eff @t @xj @xj @xj

ð1Þ

where / denotes variables, C/;eff denotes the effective diffusion coefficient, uj is the velocity component in j direction and S/ denotes the source term of an equation. In Navier–Stokes equations, C/;eff is leff (effective viscosity) which is the sum of laminar kinetic viscosity (l) and eddy viscosity (lt ). The RANS models solve the higher-order Reynolds stresses by using a turbulent viscosity model which is algebraically related to other turbulence quantities such as turbulent kinetic energy and energy dissipation rate. 2.2.1. Zero-equation turbulence model Zero-equation turbulence model is a relatively simple model. In this model, the eddy viscosity is defined as a constant number or denoted as an algebraic equation without involving turbulence transport equations. Prandtl developed the first zero-equation model by using the mixing-length hypothesis. Although it requires calibrations for each specific type of flow, the mixing-length model has yielded good results in predicting simple turbulent flows (Zhai et al., 2007). Nielsen (1998) showed that zero-equation model can be used to obtain a quick and preliminary solution and even gave a better agreement with experimental data than standard k–e model in a case of prediction for smoke movement once it was calibrated. A further development of zero-turbulence model was conducted by Chen and Xu (1998). This model has been implemented to commercial software for HVAC applications, Airpak. 2.2.2. The k–e turbulence model The k–e turbulence model is the most popular one and has different variations. The standard k–e model is the prevailing turbulence model for prediction of air movement in buildings due to its simple format and robust performance. The model is based on

a transport equation for turbulence kinetic energy k and a transport equation for the dissipation of turbulent kinetic energy e (Launder and Spalding, 1974). This model is also developed (strictly speaking) to be only valid for fully developed turbulent flow and this cannot be always fulfilled in the ventilated room. Meanwhile, the renormalization group (RNG) k–e model (Yakhot and Orszag, 1986) has been also tested by some researchers in an enclosed ventilated room. This model uses RNG techniques to develop a theory for the large scales in which the effects of the small scales are represented by modified transport coefficients. Compared to standard k–e model, RNG has improvements on prediction for separated flow, wall heat and mass transfer etc. Another high Reynolds number k–e model family is realizable k–e model (Shih et al., 1995). It shares the same turbulent kinetic energy equation as the standard k–e model but with an improved equation for dissipation of turbulent kinetic energy, in which the coefficient of C l is variable instead of constant. Compared to standard k–e model, realizable k–e model has improvements on the prediction for rotation, recirculation, planar and round jets and boundary layer under strong adverse pressure gradients or separation. 2.2.3. The k–x turbulence model The k–x two-equation turbulence models have been applied increasingly in industry. This model solves a modified version of k equation used in k–e model and a transport equation for x, which is an inverse time scale that is associated with the turbulence (Wilcox, 1988). The standard k–x model has improvement in predicting equilibrium adverse flows but less robust in wake region and free-shear flows compared to standard k–e model (Menter, 1992). This led to the development of Shear Stress Transport (SST) k–x turbulence model (Menter, 1994), which uses k–x turbulence model in the inner boundary layer and k–e model in the outer regions of and outside of the boundary layer. The switch between k–x turbulence model and k–e model is controlled by blending functions. One of the advantages in SST model is to introduce a limitation of the shear stress in adverse pressure gradient regions. It can also be beneficial to use SST model when the mass and heat transfer between the local air and solid surface is significant. 2.2.4. Reynolds Stress Models (RSM) The above introduced two-equation models assume the turbulence isotropic. If the flow is highly anisotropic such as swirling flows, they could fail for the appropriate predictions. RSM allows development of transport and individual Reynolds stresses by solving the transport equations of Reynolds stresses and fluxes explicitly instead of calculating turbulence viscosity, which leads RSM to be a seven-equation model including six transport equations for the Reynolds stress and one transport equation for the dissipation rate of turbulence energy (Gebremedhin and Wu, 2003; Sørensen and Nielsen, 2003b; Zhai et al., 2007). RSM model is good for accurately predicting complex flows such as cyclone flows, swirling flows, rotating flows, secondary flows, flows involving separation and especially in connection with the ventilation flow in a 3D wall jet (Schälin and Nielsen, 2004). Selecting the appropriate turbulence model for CFD simulation is significant. A few papers about turbulence model selection can be found in Chen (1995), Nielsen (1998), Zhai et al. (2007) and Zhang et al. (2007), which is concerned the application in indoor environment. 2.3. Solving the equations Section 2.2 is related to the selection of the right equations and this section is introducing the discretization both of the space and the equations, which refers to ‘solve the equation right’.

L. Rong et al. / Computers and Electronics in Agriculture 121 (2016) 180–190

2.3.1. Numerical schemes The numerical schemes developed in 1960s were based on central difference (Nielsen, 2004). As Peclet number is bigger than 2, solutions with this scheme for convective terms provide no physical meaning (e.g. oscillatory and wiggly solutions). At that time, by decreasing the grid size could avoid the oscillatory solution but the increased grid number could not be afforded by the computers. Upwind scheme (first order meaning the truncation error is proportional to grid size Dx) developed by Courant et al. (1952) is almost unconditionally stable. It made numerical simulations of flow at high Reynolds number applicable. But later in 1960s it clearly showed large errors in predictions. This error is known as ‘false diffusion’ or ‘artificial diffusion’. The artificial diffusivity is proportional to the velocity and grid size of each computational cell. It reaches the largest when the airflow direction is 45° to the cell face. A good example to show the artificial diffusion of first order upwind scheme is Smith and Hutton problem, which can be found in Sørensen and Nielsen (2003b). Inspired by the first order upwind scheme, a second order upwind scheme has been developed which considers the fact that the upstream conditions have a larger effect on variables than the downstream conditions. Currently, the CFD simulation papers will not be accepted by using first order upwind scheme and generally requires the second order upwind scheme for convective terms at least. In commercial software, higher order of accuracy is also available. The QUICK (Quadratic Upwind Interpolation of Convective Kinematics) scheme developed by Leonard (1979) has greater accuracy than central differencing while remaining the stability of upwind scheme. It also considered that upstream conditions have a larger effect on variables than the downstream conditions. The QUICK scheme has a third order of accuracy and produces lower artificial diffusion. More history and introduction of numerical schemes development can be found in references of Nielsen (2004, 2015) and Sørensen and Nielsen (2003b). 2.3.2. Space discretization It is imperative to discretize the space and time when numerical method is used to solve the coupled partial differential equations which describe the key physics. Then the alerted questions are: ‘Is the mesh good enough?’, ‘Are there criteria that CFD users can follow to ensure a high quality solution by using the generated mesh?’. Ideally, the CFD simulation results should be independent of the computational grid. Unfortunately due to the limitation of the computer power and time, it is almost impossible to obtain a grid-independent solution for three-dimensional flow in full scale pig barns with slatted floor. However, it is meaningful to perform the grid-convergence study. This implies that refining the grid further will not change the results significantly. In 1994, Roache (1994) proposed uniform Grid Convergence Index (GCI) to report the grid refinement studies in CFD. The method provides an objective asymptotic approach to quantification of uncertainty of grid convergence, which is based on a grid refinement error estimator derived from the theory of generalized Richardson Extrapolation. The equation to calculate GCI is expressed as:

GCI ¼ 3jej=ðrp  1Þ

e ¼ ðf 2  f 1 Þ=f 1 r ¼ h2 =h1

ð2Þ ð3Þ ð4Þ

where f 1 is the variable value at a point with fine grid; f 2 is the variable value at the same point with coarse grid; h1 is the representative grid size of fine grid; h2 is the representative grid size of coarse grid; p denotes the numerical scheme order of accuracy, which is 2

183

for second order scheme; ‘3’ is used so that GCI could relate e obtained by any grid refinement to the e with a doubling grid and a second-order method for the same problem because the calculated e by using a grid doubling and a second-order accuracy method revealed the marginal confidence level according to the cumulative experience in the CFD community as stated by Roache (1994). Although doubling grid refinement is preferable (r ¼ 2Þ, it has been argued that this is impractical when the flow is three dimensional with complex geometry e.g. in pig barn with slatted floor. It suggests using a smaller change in grid resolution. But it also suggests using a value of r P 1:1 to avoid the ‘noise’ of incomplete iterative convergence and machine round-off error. It could also be a challenge to apply GCI in practice because it was developed based on the uniform grid. Then it was suggested that r could be 1=3 calculated as: ¼ N fine =N coarse , where N fine and N coarse is the grid number of fine and coarse mesh respectively. If the GCI could decrease with finer mesh at the same numerical accuracy order, it indicates that the mesh refining is on the right track at least. More details about GCI could be referred to the original papers published by Roache (1994, 1997). 2.4. Near wall treatment The k–e turbulence model family is not designed to solve the flow near the wall thus it requires the damping function to simulate the near wall effect, e.g. wall function. For the high Reynolds number k–e model, empirical log-law relations are used and effective when y+ is between 30 and 300. Thus the first node near the wall should be placed there to avoid errors. y+ is defined as: yþ ¼ u y=m, where u denotes friction velocity (m s1), y denotes the distance of the first node to the nearest wall (m) and m is the local kinetic viscosity of the fluid (m2 s1). For the low Reynolds number k–e model, linear relations are used in the boundary sublayer and it requires y+ smaller than 5.0. In reality, y+ normally varies with location and it is difficult to generate a computational grid to ensure the value of y+ within the required range. In some commercial software, enhanced wall treatment is available to implement the hybrid wall functions for varying y+ in CFD simulation, especially useful for the buffer zone where neither linear nor loglaw relations works well. More information about wall treatment can be found in the paper by Knopp et al. (2006). 2.5. Convergence criteria Before starting a CFD simulation, usually the iteration steps and residual can be defined. In commercial software, a default value of residual is given. In practice, the default residual value does not always ensure the converged final solution since solving nonlinear equations to reach the final solution is strongly dependent on the specific problem. In order to obtain sufficiently converged solution, a lower residual value is often required. In addition, values of important variables must be monitored during the simulation for CFD users to judge the completed solution. Conservation of the mass and energy should be also checked after the simulation is completed. 3. Case study In this case study, the procedure to present CFD modeling in a full scale pig barn was presented in this section. In order to validate the CFD simulation with sounding experimental data, the following limitations of this case study should be realized. The experiments were conducted under isothermal cases. No animals were included and no gaseous concentrations were measured. Although the chosen case could not include every detail in an animal barn,

184

L. Rong et al. / Computers and Electronics in Agriculture 121 (2016) 180–190

the authors still believed it would not affect the objectives of this paper. First, the physics of the airflow would not be changed by including animals inside the barn but increasing the complexity of the geometry and leaded to a challenge of mesh generation. Secondly, the prediction of gaseous distribution would be ensured by correct prediction of airflow patterns and velocity distribution due to the fact that the gaseous mass transfer process would not affect the velocity distribution. Some researchers usually compute the velocity field first and then activate the calculation of species equation after the convergence of velocity has been achieved in a complicated case. However, how to define the boundary conditions on the emission surface is still a challenge for prediction of gaseous emissions because a validated emission model is missing from either solid or liquid phase of slurry manure on floor surface and slurry surface in pit. It was realized that challenges such as determination of gaseous boundary condition on the emission surface, detailed building geometry simplification, consideration of the animal’s geometry and movement etc. exist in CFD modeling in livestock buildings, but they are out of the scopes of this paper and will be discussed in a future study. 3.1. Experimental set up The experimental measurements were conducted in one of the sections at the climate laboratory in Aarhus University, Denmark. The schematics of the room, measuring locations and the grid resolution are shown in Fig. 1. The room is 5.68 m in length (x), 4.8 m in width (z) and 2.67 m in height (y), with two full scale pig pens and a corridor. In each pig pen, the floor consists of one-third of drained floor (1.6 m of length, opening ratio of 8.5%) and twothird of slatted floor (3.2 m of length, opening ratio of 16.5%). The experimental measurements were conducted under isothermal conditions with ventilation rate of 2996 ± 75 m3 h1 and side wall jet supply inlet. Before measurement, the ventilation system was turned on for around 2 h to reach steady state condition in the room. During the experiments, the airflow rate was measured by a measuring fan and recorded by a climate control system (Vengsys, Denmark) each minute. Air speed at the measuring points was measured every 0.2 s and averaged every 1.0 s by omnidirectional Air Velocity Transducer (TSI, model 8475) with repeatability of air speed measurements in 2% of the readings. The measurement period at each point was 90 min and the measured data was recorded by CR 1000 data logger (Campbell Scientific Ltd). The room temperature and humidity were continuously measured by the sensors equipped in the room and recorded each minute by the climate control system (Vengsys, Denmark). The measured indoor temperature and humidity was 19.3 ± 0.5 °C and 43.6 ± 1.4% respectively. All this information is important to help readers evaluating the accuracy of the experimental data. 3.2. CFD modeling 3.2.1. Governing equations In livestock buildings, the family of k–e turbulence models are the most widely used, e.g. Bjerg et al. (2000, 2002) and Norton et al. (2009, 2010a). A few studies were also conducted to compare the effect of different turbulence models such as SST and RSM on simulation results (Gebremedhin and Wu, 2003; Shen et al., 2012; Wu et al., 2012b). An agreed turbulence model which might be the most suitable for livestock buildings was not concluded. In this study as an example, three turbulence models were selected, i.e., standard k–e model, RNG k–e model and realizable k–e model which are available in commercial software of Ansys Fluent 15.0. In our opinion, it may not be necessary to present the mathematical expressions of each equation if the models were well-known or standard forms were used in the commercial software. A refer-

Fig. 1. Sketch geometry and grid distribution for CFD modeling.

ence related to the description of turbulence models was sufficient. For example, standard k–e model could refer to Launder and Spalding (1974), RNG k–e model could refer to Yakhot and Orszag (1986) and realizable k–e model could be found in the paper of Shih et al. (1995). It is however important to clearly describe the specific terms which has been included besides the standard terms or the authors would address the importance of certain functions

L. Rong et al. / Computers and Electronics in Agriculture 121 (2016) 180–190

(expressions). In this example, the energy equation was activated automatically due to the computation of species equation. Enhanced wall treatment was selected to solve the flow near the wall since the y+ varied with the locations (e.g. jet area VS vortex area). In this study, the y+ was maintained at the value lower than 120 for the final mesh due to the consideration that some researchers argue that it might bring unreasonable results if y+ reaches 300.

3.2.2. Numerical methods The geometry model was built in a Cartesian coordinate system and the spatial domain was discretized into finite volume control using a structured mesh. Although it saves the time to generate unstructured mesh, it may increase the number of the mesh to ensure the mesh quality due to the large numbers of small slots. The governing equations were discretized using second order upwind scheme over each control volume so that the relative quantity (mass, momentum, energy, species etc.) was conserved in discrete sense for each control volume owing to the finite volume control method. In order to show the effect of different discretization schemes on simulation results, first order upwind and QUICK scheme were also adopted in simulations. The CFD code used SIMPLE method which applies a solution strategy where the momentum equations were solved first and an equation for a pressure correction is obtained using a guessed pressure. A global scaled residual (105 for all the solved equations) as well as velocity monitoring points was defined for purpose of solution monitoring and convergence criteria. The convergence was not assumed to be reached until both the velocity magnitude at the monitoring points and the residual has stabilized. In this example, the residual for mass conservation equation reaches 104 and the residual for other equations arrives at 105. The selection of monitoring points depended on the problem that was to be solved. In this example, two points were chosen in the jet flow and one point was selected near the slatted floor. After the simulation was completed, the balance of mass and energy has also been checked. The mesh was generated in Ansys ICEM. A grid-convergence study was performed and GCI was analyzed. Three mesh files with corresponding numbers of 1.94, 3.66 and 7.04 million were applied. The GCI at a few points as an example were summarized in Table 1. The results showed that the GCI decreased with increasing the grid numbers. It was observed that GCI decreased from 28.2% to 15.6% at P1, from 33.6% to 12.9% at P2 and from 38.2% to 7.3% at P3 when r increased from 1.24 to 1.54. In the paper of Roache (1994), it discussed that the coefficient of 3.0 in Eq. (2) was very conservative when the grid convergence study was conducted under fine mesh. The GCI revealed that refining the mesh leaded to the lower error estimator as well as the error level. What GCI level could be accepted completely depended on the CFD users’ own criteria, the solved problem, computer power and so on. The mesh could be refined (or improved) further but it might exceed the calculation power of our office PC in this study. Therefore, the grid convergence study was finalized at the grid number of 7.04 million and the following results were all based on the simulations using this grid number.

185

Table 2 Boundary conditions. Inlet

Outlet Slurry floor Walls

Velocity inlet: 4.13 m s1, temperature of 19.3 °C, turbulent intensity of 5%, turbulent length scale of 0.0112 (using a factor of 0.07 multiplying the height of the inlet as recommended by Fluent help documents), ammonia mass fraction of 0.0 0.0 Pa Ammonia mass fraction of 4.5E05, temperature of 19.3 °C Non-slip, temperature of 19.3 °C, ammonia mass fraction of 0.0

3.2.3. Boundary conditions A non-slip condition was imposed at solid surfaces. The measured air temperature was defined at inlet as well as on the walls since it was considered as an isothermal case. The concentration of ammonia was defined at the slurry surface (as a tracer gas). No ammonia was brought to the room through the inlet and no ammonia was released from the other walls. In this study, the main

Table 1 GCI calculated for common values of grid ratio (r) and second order upwind scheme. Points

P1 P2 P3

Location

GCI

x

y

z

r = 1.54

r = 1.24

2.07 3.27 4.47

2.6 2.3 0.11

1.2 1.2 1.2

15.6% 12.9% 7.3%

28.2% 33.6% 38.2%

Note: r = 1.24 is the mesh ratio from fine mesh to the middle mesh and r = 1.54 is the mesh ratio from fine mesh to coarse mesh.

Fig. 2. Velocity magnitude and streamline (velocity components of x and y) distribution at plane of Z = 1.2 m. (a) Standard k–e model, (b) realizable k–e model and (c) RNG model.

186

L. Rong et al. / Computers and Electronics in Agriculture 121 (2016) 180–190

purpose of simulating species concentration was to help the authors to evaluate the efficiency of the ventilation system. As mentioned, it was isothermal case and generally it was not supposed to solve the energy equation. But when the species equation was solved, the energy equation was activated automatically. The boundary conditions were summarized in Table 2.

3.2.4. Approximations It was unavoidable to make approximations when using numerical methods to represent a real world. For example, it was necessary to simplify the geometry model instead of including every detail which would lead to huge grid resolution so that the computer power could not afford it. In this study, the feeding system and water spraying system were not included in the geometry of CFD modeling. The poles at the pig contact area were not modeled either and assumed to be a completely open plane.

Fig. 3. Ammonia concentration distribution at the plane of Z = 1.2 m. (a) Standard k–e model, (b) realizable k–e model and (c) RNG model.

Although it was not applicable in this example, it was necessary to simply the geometry of the inlet (e.g. diffuse ceiling) at some cases. Sometimes it was also unavoidable to make assumptions imposed on the boundary conditions such as surface temperature and heat flux on solid surfaces, species concentration on the emission surface if it was related. It was imperative to provide all this information so that the reader could evaluate the CFD modeling from the work. 3.3. Results and discussions 3.3.1. Effect of turbulence models The airflow patterns at the plane of Z = 1.2 m were shown in Fig. 2. At the upper-left area, the vortex was elliptic with standard k–e model and realizable k–e model while it was cone-shape with RNG model. On the left above the slatted floor, a vortex was found with standard k–e model and realizable k–e model white it was not observed with RNG model. Below the slatted floor, different flow patterns were noticed between standard k–e model and realizable k–e model. It seemed that the air flowed from the pit to the room through bigger number of slots on the left with standard k–e model. These results revealed that difference might be found among different turbulence models although the other conditions including mesh resolution, boundary conditions and numerical

Fig. 4. Comparison of simulated and measured velocity magnitude with different turbulence models at three lines at the plane of Z = 1.2 m, STD represents standard k–e model, REL represents realizable k–e model and RNG represents RNG model.

L. Rong et al. / Computers and Electronics in Agriculture 121 (2016) 180–190

methods were the same. Fig. 3 presented the ammonia concentration distribution by using these three turbulence models. Difference of ammonia concentration distribution was observed in the slurry container and the area above the slatted floor due to the different airflow patterns. The simulated results at two vertical lines and one horizontal line below the slatted floor were revealed in Fig. 4. From Fig. 4 (a) and (b), it was observed that the simulated results from standard k–e model and realizable k–e model were closer to each other. By comparing the simulated and measured results in Fig. 4 (a) and (b), these three turbulence models were acceptable although standard k–e model and realizable k–e model was slightly better. But the results shown in Fig. 4(c) indicated that realizable k–e model and standard k–e model predicted the air speed better than the RNG model under the slatted floor. Different air flow patterns were found between the predictions of realizable k–e model and standard k–e model in Fig. 4(c) with X in the range of 3.0– 3.5 m. This might be explained by the air flowing direction at the area close to X = 3.0 m. With realizable k–e model, the air flowed from the room to the pit through the slots at this area and the streamline pointed downward while the flow direction changed to horizontally after penetrating to the pit immediately with standard k–e model. Due to the improvement of predicting the planar and round jets and recirculation flow, the realizable k–e model was selected to perform further investigations.

Fig. 5. Comparison of simulated and measured air speed with three discretization orders at three lines.

187

Generally, it was shown that RNG model could provide better agreement between simulated and measured results in the area of indoor climate. In this study, it showed that realizable k–e model could give better agreement between simulated and measured results. The shortcoming of this validation case was that it was isothermal. The animals were usually enclosed indoor as heat sources. In summer with maximum ventilation rate in Denmark (this is the case here), the difference of indoor temperature between indoor and outdoor was small. Therefore it could still be a case to be referred. With non-isothermal conditions, the emphasis on the boundary conditions should be addressed besides the mentioned issues in Section 2. 3.3.2. Effect of discretization schemes The effect of discretization schemes on simulating results was shown in Fig. 5. Little difference of the air speed was observed between second order upwind and QUICK order in Fig. 5 (a) and (b). Obvious discrepancy was found at the jet flow (Fig. 5 (a) at the height of inlet) between first order upwind and second order upwind as well as QUICK order. At this area, the airflow is not perpendicular to the cell face. Using first order upwind scheme could cause false diffusion which leaded to the error for the simulating results. At the area below the slatted floor, big difference of simulating results was seen between first order and second order

Fig. 6. Comparison of simulated and measured velocity magnitude at three lines, two vertical lines above the slatted floor and one horizontal line below the slatted floor.

188

L. Rong et al. / Computers and Electronics in Agriculture 121 (2016) 180–190

as well as QUICK order. Generally, the simulating results were in better agreement with experimental measurements by using higher accuracy orders. At the range between 3.0 and 3.3 m in Fig. 5(c), discrepancies were also noticed between second order upwind and QUICK order. Due to lack of experimental measurements at this area, it was difficult to conclude if QUICK order predicted better than second order upwind or not. 3.3.3. Comparison of air speed between simulated and measured results The comparison of air speed between simulated and measured results was revealed in Figs. 6 and 7. These results revealed that the

simulated air speed was in agreement with the measurements at most of the points, but discrepancies of air speed at a few points were also found, seen in Fig. 6(a). The measuring results were generally larger than the simulated air speed. It might be caused by excluding the feeding equipment in the simulation. The feeding equipment in experiments, which was located in the middle of the pig barn and near the partitioning wall between two pens, could block the air to some degree and forced the air flowing to the open place in the barn. However, this was not modeled in the CFD simulation for geometry simplification. When the measured locations were moving further away from the feeding equipment, the agreement of air speed between simulation and measurements were becoming better. The agreement of air speed between simulated and measured results was extremely good in Fig. 6(c). Due to the air speed in such a low level at these points, it should also be recognized that the relative error of the hotsphere anemometer measurements might increase.

4. Conclusions This paper summarized the best guidelines for CFD modeling which the CFD users in the research area of livestock buildings would benefit from. Due to the wide application of CFD modeling in livestock buildings, the issues related to RANS modeling have been addressed for quality control of CFD modeling, which includes selection of turbulence models, differencing schemes, grid convergence study, convergence criteria, etc. It is suggested that numerical schemes with a second or higher order of accuracy should be adopted and first order scheme should be avoided for obtaining the final solution. In reality, it is difficult to conduct grid independent study but it is recommended to perform grid convergence study and use the GCI to evaluate the uncertainties caused by grid resolutions. A validation of CFD modeling in a full scale pig room with two barns was presented. The authors strongly recommend that the following aspects should be stated in a paper of CFD modeling:     

Description of governing equations and CFD code. Description of differencing schemes. Description of wall treatment and the range of y+ value. Description of grid topology and resolution. Description of boundary conditions including initial conditions for unsteady simulation.

When describing the governing equations and CFD code, it is suggested to cite the references which are well known by the scientific public. Otherwise, a detailed description should be provided so that the readers have the possibility to reproduce the simulation results. If it is possible, the authors recommend the CFD users to validate the simulation by using experimental measurements. If it is impossible to conduct the measurements, then a reported similar principle flow which could provide well documented experimental data should be adopted to perform the CFD validation process. References

Fig. 7. Comparison of simulated and measured velocity magnitude at the points close to the slatted floor.

AIAA, 1998. Guide: Guide for the Verification and Validation of Computational Fluid Dynamics Simulations (AIAA G-077-1998(2002)). American Institute of Aeronautics and Astronautics Inc. Bartzanas, T., Zhang, G., Norton, T., Wu, W., Papanastasiou, D.K., Kittas, C., 2013. Numerical and experimental assessment of the airflow field and ventilation rates in a naturally ventilated free cubical cattle house with large openings. Precision Livestock Farming 2013 – Papers Presented at the 6th European Conference on Precision Livestock Farming, ECPLF 2013, pp. 652–657. Bjerg, B., Cascone, G., Lee, I.B., Bartzanas, T., Norton, T., Hong, S.W., Seo, I.H., Banhazi, T., Liberati, P., Marucci, A., Zhang, G., 2013. Modelling of ammonia emissions

L. Rong et al. / Computers and Electronics in Agriculture 121 (2016) 180–190 from naturally ventilated livestock buildings. Part 3: CFD modelling. Biosyst. Eng. 116 (3), 259–275. Bjerg, B., Svidt, K., Zhang, G., Morsing, S., 2000. The effects of pen partitions and thermal pig simulators on airflow in a livestock test room. J. Agric. Eng. Res. 77 (3), 317–326. Bjerg, B., Svidt, K., Zhang, G., Morsing, S., Johnsen, J.O., 2002. Modeling of air inlets in CFD prediction of airflow in ventilated animal houses. Comput. Electron. Agric. 34 (1–3), 223–235. Blanes-Vidal, V., Guijarro, E., Balasch, S., Torres, A.G., 2008. Application of computational fluid dynamics to the prediction of airflow in a mechanically ventilated commercial poultry building. Biosyst. Eng. 100 (1), 105–116. Blocken, B., Gualtieri, C., 2012. Ten iterative steps for model development and evaluation applied to computational fluid dynamics for environmental fluid mechanics. Environ. Model. Software 33, 1–22. Bustamante, E., García-Diego, F.J., Calvet, S., Estellés, F., Beltrán, P., Hospitaler, A., Torres, A.G., 2013. Exploring ventilation efficiency in poultry buildings: the validation of computational fluid dynamics (CFD) in a cross-mechanically ventilated broiler farm. Energies 6 (5), 2605–2623. Bustamante, E., García-Diego, F.J., Calvet, S., Torres, A.G., Hospitaler, A., 2015. Measurement and numerical simulation of air velocity in a tunnel-ventilated broiler house. Sustainability (Switzerland) 7 (2), 2066–2085. Casey, M., Wintergerste, T., 2000. Best Practice Guidelines. ERCOFTAC Special Interest Group on Quality and Trust in Industrial CFD. ERCOFTAC. Chen, Q., 1995. Comparison of different k-e models for indoor air flow computations. Numer. Heat Transf. Part B: Fundam. 28 (3), 353–369. Chen, Q., 2009. Ventilation performance prediction for buildings: a method overview and recent applications. Build. Environ. 44 (4), 848–858. Chen, Q., Xu, W., 1998. A zero-equation turbulence model for indoor airflow simulation. Energy Build. 28 (2), 137–144. Courant, R., Isaacson, E., Rees, M., 1952. On the solution of nonlinear hyperbolic differential equations by finite differences. Commun. Pure Appl. Math. 5 (3), 243–255. Franke, J., Hellsten, A., Schlünzen, H., Carissimo, B., 2007. Best Practice Guideline for the CFD Simulation of Flows in the Urban Environment. Meteorological Institute, University of Hamburg. Freitas, C.J., 1993. Editorial. J. Fluids Eng. 115 (3), 339–340. Gebremedhin, K.G., Wu, B.X., 2003. Characterization of flow field in a ventilated space and simulation of heat exchange between cows and their environment. J. Therm. Biol. 28 (4), 301–319. Hong, S., Lee, I., Hwang, H., Seo, I., Bitog, J., Kwon, K., Song, J., Moon, O., Kim, K., Ko, H., Chung, S., 2011. CFD modelling of livestock odour dispersion over complex terrain, part II: Dispersion modelling. Biosyst. Eng. 108 (3), 265–279. Hong, S.W., Lee, I.B., Seo, I.H., Bitog, J.P., Kwon, K.S., 2013. Prediction of livestock odour dispersion over complex terrain using CFD technology: review and simulation study. Acta Horticult. 1008, 29–36. Humbert, U., Wessels, G.J.C., Smit, J.E., Ubbink, O., 2014. Improving broiler lifestyle: a CFD approach. In: 9th South African Conference on Computational and Applied Mechanics, SACAM 2014. Knight, D.W., Wrigh, N.G., Morvan, H.P., 2005. Guidelines for Applying Commercial CFD Software to Open Channel Flow. Knopp, T., Alrutz, T., Schwamborn, D., 2006. A grid and flow adaptive wall-function method for RANS turbulence modelling. J. Comput. Phys. 220 (1), 19–40. Kwon, K.S., Lee, I.B., Han, H.T., Shin, C.Y., Hwang, H.S., Hong, S.W., Bitog, J.P., Seo, I.H., Han, C.P., 2011. Analysing ventilation efficiency in a test chamber using age-ofair concept and CFD technology. Biosyst. Eng. 110 (4), 421–433. Launder, B.E., Spalding, D.B., 1974. The numerical computation of turbulent flows. Comput. Meth. Appl. Mech. Eng. 3 (2), 269–289. Lee, I.B., Bitog, J.P.P., Hong, S.W., Seo, I.H., Kwon, K.S., Bartzanas, T., Kacira, M., 2013. The past, present and future of CFD for agro-environmental applications. Comput. Electron. Agric. 93, 168–183. Leonard, B.P., 1979. A stable and accurate convective modelling procedure based on quadratic upstream interpolation. Comput. Meth. Appl. Mech. Eng. 19 (1), 59– 98. Li, Y., Guo, H., 2006. Comparison of odor dispersion predictions between CFD and CALPUFF models. Trans. ASABE 49 (6), 1915–1926. Li, Y., Nielsen, P.V., 2011. Commemorating 20 years of Indoor Air: CFD and ventilation research. Indoor Air 21 (6), 442–453. Lin, X.J., Barrington, S., Choinière, D., Prasher, S., 2007. Simulation of the effect of windbreaks on odour dispersion. Biosyst. Eng. 98 (3), 347–363. Menter, F., 2002. CFD Best Practice Guidelines for CFD code Validation for ReactorSafety Applications. Menter, F.R., 1992. Influence of freestream values on j–x turbulence model predictions. AIAA J. 30 (6), 1657–1659. Menter, F.R., 2009. Review of the shear-stress transport turbulence model experience from an industrial perspective. Int. J. Comput. Fluid Dyn. 23 (4), 305–316. Menter, F.R., 1994. Two-equation eddy-viscosity turbulence models for engineering applications. AIAA J. 32 (8), 1598–1605. Menter, F.R., Schütze, J., Kurbatskii, K.A., Gritskevich, M., Garbaruk, A., 2011. Scaleresolving simulation techniques in industrial CFD. In: 6th AIAA Theoretical Fluid Mechanics Conference. Mistriotis, A., De Jong, T., Wagemans, M.J.M., Bot, G.P.A., 1997. Computational fluid dynamics (CFD) as a tool for the analysis of ventilation and indoor microclimate in agricultural buildings. Netherlands J. Agric. Sci. 45 (1), 81–96. Nielsen, P.V., 1973. Berechnung der luftbewegung in einem zwangsbelufteten Raum. Gesundheits – Ingenieur 94 (10), 299–302.

189

Nielsen, P.V., 2004. Computational fluid dynamics and room air movement. Indoor Air, Supplement 14 (Suppl. 7), 134–143. Nielsen, P.V., 2015. Fifty years of CFD for room air distribution. Build. Environ. Nielsen, P.V., 1998. Selection of turbulence models for prediction of room airflow. ASHRAE Trans., 1119–1127 Norton, T., Grant, J., Fallon, R., Sun, D.W., 2009. Assessing the ventilation effectiveness of naturally ventilated livestock buildings under wind dominated conditions using computational fluid dynamics. Biosyst. Eng. 103 (1), 78–99. Norton, T., Grant, J., Fallon, R., Sun, D.W., 2010a. Assessing the ventilation performance of a naturally ventilated livestock building with different eave opening conditions. Comput. Electron. Agric. 71 (1), 7–21. Norton, T., Grant, J., Fallon, R., Sun, D.W., 2010b. A computational fluid dynamics study of air mixing in a naturally ventilated livestock building with different porous eave opening conditions. Biosyst. Eng. 106 (2), 125–137. Norton, T., Grant, J., Fallon, R., Sun, D.W., 2010c. Improving the representation of thermal boundary conditions of livestock during CFD modelling of the indoor environment. Comput. Electron. Agric. 73 (1), 17–36. Norton, T., Grant, J., Fallon, R., Sun, D.W., 2010d. Optimising the ventilation configuration of naturally ventilated livestock buildings for improved indoor environmental homogeneity. Build. Environ. 45 (4), 983–995. Norton, T., Sun, D.W., Grant, J., Fallon, R., Dodd, V., 2007. Applications of computational fluid dynamics (CFD) in the modelling and design of ventilation systems in the agricultural industry: a review. Bioresour. Technol. 98 (12), 2386–2414. Ntinas, G.K., Zhang, G., Fragos, V.P., Bochtis, D.D., Nikita-Martzopoulou, C., 2014. Airflow patterns around obstacles with arched and pitched roofs: wind tunnel measurements and direct simulation. Eur. J. Mech. B/Fluids 43, 216–229. Rahman, M.M., Chu, C.M., Kumaresen, S., Yan, F.Y., Kim, P.H., Mashud, M., Rahman, M.S., 2014. Evaluation of the modified chimney performance to replace mechanical ventilation system for livestock housing. Proc. Eng., 245–248 Reynolds, A.M., 1997. A model for predicting airborne dust concentrations within a ventilated airspace. J. Agric. Eng. Res. 66 (2), 103–109. Roache, P.J., 1994. Perspective: a method for uniform reporting of grid refinement studies. J. Fluids Eng. Trans. ASME 116 (3), 405–413. Roache, P.J., 1997. Quantification of uncertainty in computational fluid dynamics. Annu. Rev. Fluid Mech. 29, 123–160. Roache, P.J., Ghia, K.N., White, F.M., 1986. Editorial policy statement on the control of numerical accuracy. J. Fluids Eng. 108 (1). Rong, L., Elhadidi, B., Khalifa, H.E., Nielsen, P.V., 2010a. CFD modeling of airflow in a livestock building. In: IAQVEC 2010: 7th International Conference on Indoor Air Quality, Ventilation and Energy Conservation in Buildings. Rong, L., Elhadidi, B., Khalifa, H.E., Nielsen, P.V., Zhang, G., 2011. Validation of CFD simulation for ammonia emissions from an aqueous solution. Comput. Electron. Agric. 75 (2), 261–271. Rong, L., Liu, D., Pedersen, E.F., Zhang, G., 2015. The effect of wind speed and direction and surrounding maize on hybrid ventilation in a dairy cow building in Denmark. Energy Build. 86, 25–34. Rong, L., Nielsen, P.V., Zhang, G., 2010b. Experimental and numerical study on effects of airflow and aqueous ammonium solution temperature on ammonia mass transfer coefficient. J. Air Waste Manage. Assoc. 60 (4), 419–428. Saha, C.K., Wu, W., Zhang, G., Bjerg, B., 2011. Assessing effect of wind tunnel sizes on air velocity and concentration boundary layers and on ammonia emission estimation using computational fluid dynamics (CFD). Comput. Electron. Agric. 78 (1), 49–60. Sapounas, A.A., Campen, J.B., Smits, M.C.J., Dooren, H.J.C., 2009. Simulating the effect of forced pit ventilation on ammonia emission from a naturally ventilated cow house with CFD. In: Precision Livestock Farming 2009 – Papers Presented at the 4th European Conference on Precision Livestock Farming, pp. 81–89. Sapounas, A.A., Van Dooren, H.J.C., Smits, M.C.J., 2013. Natural ventilation of commercial dairy cow houses: simulating the effect of roof shape using CFD. Acta Horticult. 1008, 221–228. Saraz, J.A.O., Rocha, K.S.O., Tinôco, I.D.F.F., Gates, R.S., Mendes, L.B., Norton, T., Hernandez, R.O., 2012. CFD modeling of air quality inside naturally ventilated broiler barns as a function of barn spatial arrangement. In: American Society of Agricultural and Biological Engineers Annual International Meeting 2012, ASABE 2012, pp. 4553–4561. Schälin, A., Nielsen, P.V., 2004. Impact of turbulence anisotropy near walls in room airflow. Indoor Air 14 (3), 159–168. Seo, I.H., Lee, I.B., 2013. CFD application for estimation of airborne spread of HPAI (Highly Pathogenic Avian Influenza). Acta Horticult. 1008, 57–62. Seo, I.H., Lee, I.B., Moon, O.K., Kim, H.T., Hwang, H.S., Hong, S.W., Bitog, J.P., Yoo, J.I., Kwon, K.S., Kim, Y.H., Han, J.W., 2009. Improvement of the ventilation system of a naturally ventilated broiler house in the cold season using computational simulations. Biosyst. Eng. 104 (1), 106–117. Shen, X., Zhang, G., Bjerg, B., 2012. Comparison of different methods for estimating ventilation rates through wind driven ventilated buildings. Energy Build. 54, 297–306. Shih, T.H., Liou, W.W., Shabbir, A., Yang, Z.G., Zhu, J., 1995. A new kappa–epsilon eddy viscosity model for high reynolds-number turbulent flows. Comput. Fluids 24 (3), 227–238. Stern, F., Wilson, R.V., Coleman, H.W., Paterson, E.G., 2001. Comprehensive approach to verification and validation of CFD simulations—Part 1: Methodology and procedures. J. Fluids Eng. 123 (4), 793–802. Sun, H., Keener, H., Stowell, R.R., Elwell, D., Michel, F.C., 2000. Two-dimensional Computational Fluid Dynamic (CFD) Model of Air and Ammonia Distribution in

190

L. Rong et al. / Computers and Electronics in Agriculture 121 (2016) 180–190

a High-RiseTM Hog Building (HRHB). In: 2000 ASAE Annual International Meeting, Technical Papers: Engineering Solutions for a New Century, pp. 4177–4194. Sørensen, D.N., Nielsen, P.V., 2003a. CFD in indoor air. Indoor Air 13 (1), 1. Sørensen, D.N., Nielsen, P.V., 2003b. Quality control of computational fluid dynamics in indoor environments. Indoor Air 13 (1), 2–17. Wilcox, D.C., 1988. Reassessment of the scale-determining equation for advanced turbulence models. AIAA J. 26 (11), 1299–1310. Wilcox, D.C., 2006. Turbulence Modeling for CFD. DCW Industries Inc. Worley, M.S., Manbeck, H.B., 1995. Modeling particle transport and air flow in ceiling inlet ventilation systems. Trans. Am. Soc. Agric. Eng. 38 (1), 231–239. Wu, W., Zhai, J., Zhang, G., Nielsen, P.V., 2012a. Evaluation of methods for determining air exchange rate in a naturally ventilated dairy cattle building with large openings using computational fluid dynamics (CFD). Atmos. Environ. 63, 179–188. Wu, W., Zhang, G., Bjerg, B., Nielsen, P.V., 2012b. An assessment of a partial pit ventilation system to reduce emission under slatted floor – Part 2: Feasibility of CFD prediction using RANS turbulence models. Comput. Electron. Agric. 83, 134–142. Wu, W., Zong, C., Zhang, G., 2013. Comparisons of two numerical approaches to simulate slatted floor of a slurry pit model – large eddy simulations. Comput. Electron. Agric. 93, 78–89. Yakhot, V., Orszag, S.A., 1986. Renormalization-group analysis of turbulence. Phys. Rev. Lett. 57 (14), 1722–1724.

Yu, Z., Guo, H., Laguë, C., 2010. Livestock odor dispersion modeling: a review. Trans. ASABE 53 (4), 1231–1244. Zajícˇek, M., Kic, P., 2013. Simulation of the broiler house ventilation. Sci. Agric. Bohemica 2013 (1), 32–37. Zhai, Z., Zhang, Z., Zhang, W., 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 and R Res. 13 (6), 853– 870. Zhang, Z., Zhang, W., Zhai, Z., Chen, Q., 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 and R Res. 13 (6), 871–886. Zhu, S., Liu, P., Yang, N., He, J., Ye, Z., 2012. Optimization of local ventilation system for gaseous pollutants removal in broiler house using CFD simulation. In: ASABE – 9th International Livestock Environment Symposium 2012, ILES 2012, pp. 403–408. Zong, C., Wu, W., Zhang, G.Q., Shen, X., Ntinas, G., 2013. A case study of airflow patterns around an arched type agricultural building: investigating mesh convergence of different turbulence models. Acta Horticult. 1008, 69–76. Zong, C., Zhang, G., 2014. Numerical modelling of airflow and gas dispersion in the pit headspace via slatted floor: comparison of two modelling approaches. Comput. Electron. Agric.