Application of lattice Boltzmann method in indoor airflow simulation.
Indoor air can be many times more polluted than outdoor air. Ineffectively designed indoor airflows could significantly impact occupant's health and productivity, and even a building's energy efficiency. In modern buildings, many mechanical ventilation systems are designed to circulate fresh air to maintain good indoor air quality in rooms. The airflow patterns in rooms can be very complex, as it might involve different flow types such as forced, natural, and/or mixed convection (Hsu et al. 1997). It has been well recognized that an in-depth understanding of the indoor airflow characteristics is critical for indoor air quality improvement, which calls for the need of accurate predictions tools (Turiel et al. 1983; Lee and Awbi 2004).
Indoor airflows are generally considered as low-Reynolds-number flows, which might be in laminar, transitional, or turbulent regimes, depending on the ventilation flow rates and geometries. The complexity of indoor airflow makes high-quality experimental investigation not only difficult but also expensive (Rey and Velasco 2000; Jiang et al. 2009). During the last decades, the technique of computational fluid dynamics (CFD) has been widely adopted to investigate indoor airflows, with good successes. Traditional CFD approaches start with a mathematical description of a fluid at the continuum level using the Navier-Stokes equations. The governing equations are usually discretized on a structured or unstructured mesh by finite-difference, finite-volume, or finite-element methods. Much work has been done with these CFD methods to study indoor airflows under various physical and geometrical conditions. Chen (2009) and Chen et al. (2010) provided overviews of the related methods and recent applications. Stamou and Katsiris (2006), Karimipanah et al. (2007), and Li et al. (2009) used CFD to explore the best locations of air supply diffusers and return outlets and the flow rates needed to create an acceptable indoor air quality. Other recent CFD work includes Sorensen and Nielsen (2003), Yang et al. (2004), Lin et al. (2005), Zhang (2005), Zhai (2006), Srebric et al. (2008), Ezzat et al. (2008), Abdilghanie et al. (2009), and Yan et al. (2009), to name a few. In these works, CFD has been used primarily to predict contaminant transport on the bases of flow fields, and has provided valuable information about indoor air quality in built environments.
In recent years, the lattice Boltzmann method (LBM) has emerged as a powerful alternative computational approach for simulating fluid flows and physics (Chen and Matthaeus 1992; Chen and Doolen 1998; Succi 2001; Sukop and Thorne 2005). Unlike traditional CFD methods, LBM solves the discrete Boltzmann equation to simulate the flow of a fluid by using collision models, such as Bhatnagar-Gross-Krook (BGK). By simulating streaming and collision processes across a limited number of particles, the intrinsic particle interactions evince a microcosm of viscous flow behavior applicable across the greater mass. In LBM, the need to explicitly solve pressure dynamics is eliminated. LBM scheme is particularly successful in applications that require a parallel implementation or the ability to handle arbitrarily complex geometry (D'Humiere et al. 2002; Geller et al. 2006; Seta et al. 2006; Andreas et al. 2007). Based on these works, parallel lattice Boltzmann models can be easily implemented in modern supercomputers with several hundreds of processors to simulate large-scale problems, since all variables in the discretized algorithm depend solely on nearest-neighbor information. By defining different values for density distribution functions at the solid side of the media, the domain's complex boundary conditions can be easily implemented through collision rules of the fluid particles with the surfaces. LBM has been used extensively in the areas of porous media flows (Andreas et al. 2007), multiphase flows (Lee and Lin 2005), phase-change heat transfer (Kono et al. 2000), and acoustics (Tsutahara et al. 2008). Crouse et al. (2002) was the first and perhaps the only one to attempt to apply LBM in indoor convective airflow analysis. The potential benefits of LBM in indoor airflow modeling have not been fully explored (Grouse et al. 2002). Much work is still needed before LBM become a viable computational tool in indoor airflow applications. Particularly, LBM's advantages and disadvantages compared to those of traditional CFD have not been quantitatively investigated in the context of indoor airflows.
In this article, LBM is used to simulate the isothermal airflows in indoor environments. Experimental data for a model room are primarily used to validate the LBM simulation. LBM application in indoor airflow is then further demonstrated through simulations of a model ward with multiple beds. We intend to compare LBM with the traditional CFD method in predicting and understanding the basic flow behavior in two different types of rooms: one with a partition and another with ten beds. The pros and cons of LBM simulation are discussed.
Traditional CFD Method
Most traditional CFD methods are concerned with numerical solutions of the Navier-Stokes equations, which include the continuity equation and momentum equation in partial differential equation (PDE) form. For incompressible fluids, the steady Navier-Stokes can be expressed as
[nabla] * u = 0 (1)
u * [nabla]u = - [1/[rho]][nabla]p + v[[nabla].sup.2]u (2)
where v is kinematic viscosity, u is the velocity vector of the fluid parcel, p is pressure, and [rho] is fluid density. For flow with temperature gradients, the energy equation must be solved simultaneously. When flow is in turbulent regime, turbulence transport equations need to be solved as well. In this article, the RNG k-[epsilon] turbulence model proposed by Yakhot and Orszag (1986) was used to compare with simulation of lattice Boltzmann method. The selection of RNG turbulence model is based on previous study by Chen (1995) who had found that RNG k-[epsilon] model predicts the flow pattern well compared to other turbulence model.
The traditional CFD method uses a numerical technique, such as the finite-volume method (FVM), to discretize all the governing equations, which can be written in the following general form:
[nabla]([rho]u[empty set]) = [nabla]([GAMMA] * [nabla][empty set]) + S (3)
where [empty set] represents variables, such as velocities, and S and [GAMMA] are the source term and the diffusion coefficient, respectively. The computational domain is first subdivided into a number of control volumes or cells V by grids. Then, the integration of Equation 3 is applied to these cells. Volume integrals in the equation that contain a divergence term can be converted to surface A integrals, using the divergence theorem. The resulting integral equations will be of the following form:
[[integral].sub.V]n * ([rho]u[empty set])dV = [[integral].sub.A]n * ([GAMMA] * [nabla][empty set])dA + [[integral].sub.V]SdV (4)
The terms in Equation 4 are then evaluated with specifically designed numerical schemes under different boundary conditions. Thus, a set of algebraic equations for all the nodes in the domain can be obtained, and can be solved either directly or iteratively. Coupling between velocity and pressure can be treated by the SIMPLE algorithm proposed by Patankar (1980).
Lattice Boltzmann Method
LBM originated from the lattice gas automata (LGA) method (Frisch et al. 1986; Wolf-Glad-row 2000). It can be considered as a simplified fictitious molecular dynamics model, in which space, time, and particle velocities are all discrete. In LGA, there can be either zero or one particle at a lattice node moving in a lattice direction. After a time interval, each particle moves to the neighboring node in its direction; this process is called the propagation or streaming step. The main motivation for the transition from LGA to LBM was the desire to remove the statistical noise by replacing the Boolean particle number in a lattice direction with its ensemble average density distribution function [[florin].sub.i].
The lattice Boltzmann model with the BGK collision term is time-dependent, and can be described as
[[florin].sub.i](x + [c.sub.i][DELTA]t, t + [DELTA]t) = [[florin].sub.i](x, t) - [1/[tau]][[[florin].sub.i](x, t) - [[florin].sup.eq](x, t)] (5)
The left-hand side of Equation 5 is the streaming part and the right-hand side is the collision term (Succi 2001). [c.sub.i] is the particle discrete velocity and can be taken as [c.sub.i] = [[DELTA]x/[DELTA]t, where [DELTA]x, [DELTA]t are the lattice spacing and step size in time, respectively.
In the present study, we used a standard 3D lattice D3Q19 (shown in Figure 1), which has 19 discrete particle velocities, and can be written as follows:
[MATHEMATICAL EXPRESSION NOT REPRODUCIBLE IN ASCII]
[FIGURE 1 OMITTED]
Fluid particle collision is considered as relaxation towards local equilibrium. The equilibrium distribution for this model is defined as [[florin].sub.i.sup.eq], and can be computed by
[[florin].sub.i.sup.eq] = [rho][[omega].sub.i][1 + 3([c.sub.i] * u) + [9/2][([c.sub.i] * u).sup.2] - [3/2](u * u)] (6)
where [[omega].sub.i] is weight depending on the underlying lattice structure, which takes the following values:
[MATHEMATICAL EXPRESSION NOT REPRODUCIBLE IN ASCII]
[tau] is the dimensionless relaxation time related to viscosity seen in Equation 5. For the continuum flow, it is given by [tau] = [upsilon]*/([c.sub.s.sup.2][DELTA]t) + 0.5, where v* is the lattice kinematic viscosity and [c.sub.s] is the speed of sound (He et al. 1997).
To some extent, the convergence criteria used in LBM are similar to those in the traditional CFD method. In CFD simulation, we can monitor residuals changes, whereas in LBM we can monitor kinetic energy changes to prefixed levels before computational convergence. A larger Reynolds number usually requires more lattices to get a certain value of relaxation time, which plays an important role on the rate of convergence and the stability. However, the simulation time takes a toll if the length of a lattice cell is too small.
Beginning with the initial equilibrium distribution and the distribution at time t = 0, which can be taken as the initial equilibrium distribution, the computational cycle of the LBM can be divided into two steps:
1. Propagation: the populations propagate along the discretized velocity vectors [c.sub.i] to the next neighbors.
2. Collision: they collide according to the right-hand side of Equation 3 at the nodes.
When the distribution functions are computed, macroscopic variables such as density and momentum can be easily determined at each node by sums over the distribution functions:
[rho] = [[SIGMA].sub.i][[florin].sub.i], [rho]u = [[SIGMA].sub.i][[florin].sub.i][c.sub.i] (7)
The boundary conditions treatment could affect numerical accuracy and stability. This study used the "full-way-bounce-back" scheme to model the no-slip boundary on the walls. With this scheme, incoming particle populations at the boundary are treated as follows: each population is replaced by the value of the population with a velocity vector pointing in opposite direction. This completes the collision step, and the propagation step is executed directly after. The result of this operation is well defined, because all unknown populations leave the computational domain. On the outlet boundaries, outflow condition was used.
RESULTS AND DISCUSSION
In this study, low-Reynolds flows in two model rooms, with one having a partition, and another having ten beds, were simulated using both LBM and traditional CFD. All computations were carried out on a Linux Cluster in the University of Tennessee's Computational Fluid Dynamics Laboratory.
Before the results about the indoor airflow are presented, we first discuss a basic validation study with experimental data using a classic wall-bounded flow (i.e., flow in a channel).
Flow in a Channel
Figure 2 shows the schematic and dimensions of the channel, 30 [micro]m x 300 [micro]m x 25 mm (0.00118 in. x 0.0118 in. x 0.000984 in.). Fluid flow in the micro-sized channel was measured experimentally using Meihart et al.'s (1999) PIV method. The flow rate is 200 [micro]L/h (2.78 x [10.sup.-10] [m.sup.3]/s) (0.000017 [in.sup.3]/s), which results in very low speed flow in the channel. Flow is incompressible. We simulated only a section of length of 2.5 mm. Because this length is longer than the entrance length, we can assume that flow at the outlet is fully developed. A uniform velocity was imposed at the inlet. The LBM grid used in this case is 10 x 100 x 833. Figure 3 shows the comparison between LBM simulation and PIV measurement; the simulation results agreed with experimental measurement fairly well.
[FIGURE 2 OMITTED]
[FIGURE 3 OMITTED]
Model Room with Partition
In the first part of our work about indoor airflow, we simulated the partitioned model room that was experimentally studied by Posner et al. (2003). Figure 4 shows the diagram of the 3D model room. It is 94 cm (37 in.) long, 45.7 cm (18 in.) wide and 30.5 cm (12 in.) tall. The inlet and outlet on the ceiling are both 0.16 x 10.16 [cm.sup.2] (4 in.[.sup.2]) square. A partition half as tall as the room height is located at the center of the room. According to the flow rate, to maintain good indoor air quality (ASHRAE 1996), the inlet Reynolds number based on the hydraulic diameter of the inlet and outlet (10.16 mm or 4 in.) is estimated at 1600, which dictates an inlet velocity of 0.25 m/s (0.82 ft/s). The air density is 1.18 kg/[m.sup.3] (0.0737 [lb.sub.m]/[ft.sup.3]), and the viscosity used in this case is 1.72 x [10.sup.-5] kg/m*s (1.156 x [10.sup.-5] [lb.sub.m]/ft*s). The grid size of 130 x 194 x 389 was used for the LBM simulations. The time step size for LBM is 4.34 x [10.sup.-8] s. For incompressible flow, low Mach number suggests that the time step size is of the second order of grid size in LBM. Because LBM is an inherently time-dependent scheme, computations proceed until computed variables reached steady state. We consider the solution to be converged primarily based on the value of the kinetic energy in the domain (i.e., when it becomes constant). For CFD simulation, a grid size of 42 x 48 x 70 was used after a grid-independent study. The convergence criteria are that scaled residuals for all variables are less than [10.sup.-6].
[FIGURE 4 OMITTED]
Figure 5 shows the inlet jet centerline axial velocity (y component) profiles by LBM and the traditional CFD/FVM with RNG k-[epsilon] turbulence model, as compared to the experimental data reported by Posner et al. (2003). The horizontal coordinate of the figure is the distance from the inlet. We can see that the LBM simulation's results agree very well with the CFD solutions and experimental measurements. Along with the direction of air entering the inlet, the velocity increases slowly in a period of time, and begins to drop at a distance of about 0.23 m (9.06 in.) from the inlet. The velocity results predicted by CFD with the RNG k-[epsilon] model decrease slightly earlier than the experimental values, whereas those calculated by LBM agree better with experimental data in this region. Note that there might be other CFD turbulence models that perform better than the one used in this study. Because our focus is on LBM applications, testing additional turbulence models are beyond the scope of this article.
[FIGURE 5 OMITTED]
Comparison of the vertical velocity along the horizontal line at mid-partition is shown in Figure 6. Both numerical results by CFD with the RNG k-[epsilon] model and LBM agree reasonably well with the general trends of experimental data. The two peak velocities measured in the experiment are 0.115 m/s (0.377 ft/s), near the wall, and 0.109 m/s (0.358 ft/s), caused by the partition. LBM overpredicts the peak value, whereas the CFD RNG k-[epsilon] model underpredicts it. The largest dip in the velocities has an experimental value of -0.273 m/s (-0.896 ft/s), with calculated values at -0.21 m/s (-0.689 ft/s) by CFD with the RNG k-[epsilon] model and -0.264 m/s (-0.866 ft/s) by LBM. This resulted in errors of 23.0% (CFD with RNG k-[epsilon]) and 3.3% (LBM) at this largest dip point. Also, careful examination of the curves in the figure reveals that the LBM model predicts the subtle changes of the velocity along the x direction much better than the CFD with RNG k-[epsilon] model: the experimental data show that velocity varies subtly, especially along the horizontal direction in Figure 6. Based on these results, we can see that LBM has the potential to predict flow velocity distribution with better resolution than traditional CFD method.
[FIGURE 6 OMITTED]
The simulated steady-flow velocity vector fields at the middle plane using the two methods are shown in Figure 7. A comparison of these figures shows that there are some differences in the airflow patterns predicted by the two models. However, both methods predicted very similar strong air circulations at the right corner near the floor. As shown in the experimental image (Figure 8), the partition generates a small vortical structure as air flows over it. Here, the LBM is able to predict the vortical structure very well, as seen in Figures 7b and 7c. Because both LBM and CFD solutions are grid-independent, it is believed the grid-resolution, although different in the two methods, is not a factor here.
[FIGURE 7 OMITTED]
[FIGURE 8 OMITTED]
Figure 8a shows a laser sheet flow visualization image of the airflow pattern in the experiment, Figure 8b shows the velocity contours map generated by LBM, and Figure 8c shows the velocity contours map generated by CFD for the middle plane of the model room. The technique used to take and process the flow image was reported by Posner et al. (2003). Both the CFD and LBM results are considered steady, although an unsteady scheme is used in LBM. In Figure 8a, there actually is recirculation at the corner due to the presence of the wall. We suspect that the recirculation zone was not shown clearly on the experimental image primarily because of poor illumination in the corner during the experiment. We can see clearly that the LBM predicts the experimental flow pattern with fairly good details. Particularly, the LBM, which is based on an unsteady procedure, is able to resolve the complex flow structures (such as the vortical flow structure and the jet/ambient air interface), as well as the behavior of air moving over the partition. Such kinds of detailed flow structures tend to be smoothed out by the steady Reynolds-averaged Navier-Stokes (RANS) turbulence models that are used in traditional CFD simulations. Also, compared to LBM, the CFD simulation overpredicted the size or diameter of the jet flow.
Model Ward with Ten Beds
In the second part of our numerical study, we applied the validated LBM model to the study of airflows in a model hospital ward. It was also simulated by the traditional CFD method with the RNG k-[epsilon] turbulence model for comparison. The ward has a length of 7.5 m (24.6 ft), a width of 6.0 m (19.7 ft), and a height of 2.7 m (8.86 ft), as shown in Figure 9. The inlet on the ceiling and the outlet on the side walls are both squares with areas of 0.36 [m.sup.2] (3.88 [ft.sup.2]). The distance between the bottom of the outlet and the floor is 0.8 m (2.62 ft). Ten beds of the same sizes are located on the floor of the room; each of them is 2.0 m (6.56 ft) long, 1.0 m (3.28 ft) wide, and 0.5 m (1.64 ft) high. The beds are uniformly distributed in two rows, and are against the side walls. The inlet velocity is 0.263 m/s (0.863 ft/s). The air density is 1.18 kg/[m.sup.3] (0.0737 [lb.sub.m]/[ft.sup.3]), and the viscosity is 1.72 x [10.sup.-5] kg/m*s (1.156 x [10.sup.-5] [lb.sub.m]/ft*s). The grid is 140 x 310 x 864 in the LBM simulation. The time step size for LBM is 1.02 x [10.sup.-8] s. For the incompressible flow, low Mach number suggests that the time step size is the second order of grid size. For CFD simulation, a grid size of 50 x 89 x 106 was used after a grid-independent study. For this case, no experimental data are available.
[FIGURE 9 OMITTED]
Figures 10 to 14 compare the velocity vector fields at several different cutting planes in the ward predicted by both the LBM and CFD with the RNG k-[epsilon] turbulence models. These flow patterns are expected from a fluid dynamics standpoint. In general, the simulation results of the two models agree well. Flow field differences are caused by the use of two computational methods that use fundamentally different techniques in the computations. Consistent with the finding in the model room with a partition, the results of the CFD method with RANS-based k-[epsilon] approach look smoother than those of the LBM. The LBM reveals additional flow structures, particularly the various vortices in the computational domain, as compared to the traditional CFD method.
[FIGURE 10 OMITTED]
[FIGURE 11 OMITTED]
[FIGURE 12 OMITTED]
[FIGURE 13 OMITTED]
[FIGURE 14 OMITTED]
Figure 15 compares vertical velocity profiles along the centerlines of the vertical inlet and near the wall with the outlet, as predicted by both LBM and the traditional CFD with RNG k-[epsilon] model. It can be seen that vertical velocity begins to drop sharply at y = 1.5 m (4.92 ft), as shown in Figure 15a, with the results of RNG model decreasing slightly faster than those of the LBM. This is similar to what happened in the airflow in the first case of our study (i.e., the partitioned model room without beds). In Figure 15b, we can see that the vertical velocity changes direction because of the existence of the outlet. The significant differences of the predicted velocities between the two computational methods become larger when approaching the outlet. For the results along the centerlines of the vertical inlet (Figure 15a), the maximum magnitude deviation between the two models is about 19% relative to values of the CFD with RNG k-[epsilon] model. Near the wall with outlet (Figure 15b), the extreme (or peak) results of CFD and LBM are -0.078 m/s (-0.255 ft/s) and -0.031 m/s (-0.102 ft/s), respectively. This resulted in the maximum deviation of 60.3% for LBM relative to CFD method.
[FIGURE 15 OMITTED]
The numerical results by LBM and the CFD with RNG k-[epsilon] model are found in better agreement in terms of the general trends of vertical velocity on top of the beds and along the center of the outlet, as shown Figure 16. For the data that are compared on the top of beds, it is at the middle plane along the x direction. The traditional CFD with RNG k-[epsilon] model predicts a smooth velocity profile; in contract, the LBM scheme predicts a curved profile, revealing a certain level of detail about the flow velocity distribution.
[FIGURE 16 OMITTED]
Using the computers in our laboratory, the traditional CFD simulations took 7 h for the model room and 9 h for the hospital ward, while the LBM simulations took about 11 h and 16 h, respectively. This shows that the LBM approach requires on average 1.7 times the CPU time as the traditional CFD with RNG k-[epsilon] model for the cases investigated in this paper.
In this paper, the lattice Boltzmann method, which uses an unsteady procedure, was first applied to the simulation of airflows in a ventilated model room with partition. For this case, the steady LBM result was validated with the available experimental data and compared to traditional steady CFD simulation using the standard RNG k-[epsilon] turbulence model. Agreement between LBM results and experimental data for this case was very good. The LBM model was then used with the CFD approach to simulate a model ward with multiple beds to demonstrate its application in a more complex environment.
Within the investigated parameter ranges, it was found that, in both the model room and ward cases, the numerical results of LBM generally agreed well with those of the traditional CFD method with the turbulence model used. However, in the model room case, the LBM predicted better than the traditional CFD method, particularly in the region of velocity drop along the vertical inlet jet. The LBM was also able to capture the vortical structure as the air flowed over the partition.
For steady flows in both the model room and ward cases, the traditional CFD approach predicted relatively smoother flow patterns and velocity profiles, while LBM was able to resolve some detailed flow structures, such as vortices in the computational domain, which cannot be resolved by the traditional CFD method. This resolution gain by LBM was offset only moderately by the increase of the computing time.
The research in this paper, although limited to some extent as the first work, has demonstrated that LBM has the potential to become an effective alternative computational tool for indoor airflow simulation.
As an emerging computational method, LBM's full benefits in indoor airflow simulation can only be fully realized through additional research. Future research needs include additional validation studies and nonisothermal flow simulation of indoor airflows at different conditions.
A = control surface
[c.sub.i] = particle discrete velocity
[c.sub.s] = speed of sound
[[florin].sub.i] = distribution function
[[florin].sub.i.sup.eq] = equilibrium distribution
k = turbulent kinetic energy
n = normal vector
p = pressure
u = velocity vector of fluid parcel
S = source term
V = control volume
x = Cartesian coordinate
[DELTA]t = step size in time
[DELTA]x = lattice spacing
[epsilon] = dissipation rate of turbulent kinetic energy
[empty set] = variables in transport equation
[GAMMA] = diffusion coefficient
v = kinematic velocity
v* = lattice kinematic velocity
[rho] = fluid density
[tau] = relaxation time
[[omega].sub.i] = weight
Abdilghanie, A.M., L.R. Collins, A. David, and D.A. Caughey. 2009. Comparison of turbulence modeling strategies for Indoor flows. Journal of Fluids Engineering 131(5):051402-1-18.
Andreas, G.Y., P. John, E.K. Michael, P. Aggelos, and K.S. Athanassios. 2007. A lattice Boltzmann study of viscous coupling effects in immiscible two-phase flow in porous media. Colloids and Surfaces A: Physicochemical Engineering Aspects 300:35-49.
ASHRAE. 1996. ASHRAE Handbook--HVAC Systems and Equipment. American Society of Heating, Refrigerating and Air-Conditioning Engineers, Atlanta.
Chen, Q. 1995. Comparison of different k-[epsilon] models for indoor air flow computations. Numerical Heat Transfer, Part B 28:353-69.
Chen, Q. 2009. Ventilation performance prediction for buildings: A method overview and recent applications. Building and Environment, 44(4):848-58.
Chen, S. and G. Doolen. 1998. Lattice Boltzmann method for fluid flows. Annual Review of Fluid Mechanics 161:329-64.
Chen, H. and W. Matthaeus. 1992. Recovery of Navier-Stokes equations using a lattice-gas Boltzmann method. Physics Review A 45:5339-42.
Chen, Q., K. Lee, K. Mazumdar, S. Poussou, L. Wang, M. Wang, and Z. Zhang. 2010. Ventilation performance prediction for buildings: Model assessment. Building and Environment 45(2):295-303.
Crouse, B., M. Krafczyk, S. Kuhner, E. Rank, and C. Treeck. 2002. Indoor air flow analysis based on lattice Boltzmann methods. Energy and Buildings 34:941-49.
D'Humiere, D., I. Ginzburg, Y. Krafczyk, P. Lallemand, and L. Luo. 2002. Multiple relaxation time lattice Boltzmann models in three dimensions. Philosophical Transactions of the Royal Society of London A 360:437-51.
Ezzat, K.H., B. Elhadidi, and J.E. Dannenhoffer III. 2008. Efficient coupling of multizone and CFD indoor flow models through proper orthogonal decomposition. ASHRAE Transactions 113(2):282-89.
Frisch, U., B. Hasslacher, and Y. Pomeau. 1986. Lattice gas automata for the Navier-Stokes equation. Physical Review Letters 56(14):1505-08.
Geller, S., M. Krafczyk, J. Tolke, S. Turek, and J. Hron. 2006. Benchmark computations based on lattice-Boltzmann, finite element and finite volume methods for laminar flows. Computers & Fluids 35:888-97.
Grouse, B., M. Krafczyk, S. Kuhner, E. Rank, and C. van Treeck. 2002. Indoor air flow analysis based on lattice Boltzmann methods. Energy and Building 34:941-49.
He, X., Z. Zou, L.S. Luo, and M. Dembo. 1997. Analytic solutions of simple flows and analysis of nonslip boundary conditions for the lattice Boltzmann BGK model. Journal of Statistical Physics 87:115-36.
Hsu, T.H., P.T. Hsu, and S.P. How. 1997. Mixed convection in a partially divided rectangular enclosure. Numerical Heat Transfer, Part A 31:655-83.
Jiang, J.B, X.L. Wang, Y.Z. Sun, and Y.H. Zhang. 2009. Experimental and numerical study of airflows in a full-scale room. ASHRAE Transactions 115(2):867-86.
Karimipanah, T., H.B. Awbi, M. Sandberg, and C. Blomqvist. 2007. Investigation of air quality, comfort parameters and effectiveness for two floor-level air supply systems in classrooms. Building and Environment 42(2):647-55.
Kono, K., T. Ishizuka, H. Tsuda, and A. Kurosawa. 2000. Application of lattice Boltzmann model to multiphase flows with phase transition. Computer Physics Communications 129:110-20.
Lee, H. and H.B. Awbi. 2004. Effect of internal partitioning on indoor air quality of rooms with mixing ventilation--basic study. Building and Environment. 39:127-141.
Lee, T. and C.L. Lin. 2005. A stable discretization of the lattice Boltzmann equation for simulation of incompressible two-phase flows at high density ratio. Journal of Computational Physics, 206:16-47.
Li, Q., Y. Hiroshi, M. Akashi, B. Lei, Q. Meng, and L. Zhao. 2009. CFD study of the thermal environment in an air-conditioned train station building. Building and Environment 44(7):1452-65.
Lin, C.H., R.H. Horstman, M.F. Ahlers, L.M. Sedgwick, K.H. Dunn, J.L. Topmiller, J.S. Bennett, and S. Wirogo. 2005. Numerical simulation of airflow and airborne pathogen transport in aircraft cabins--Part I: Numerical simulation of the flow field. ASHRAE Transactions 111(1):755-63.
Meinhart, C.D., S.T. Wereley, and J.G. Santiago. 1999. PIV measurements of a microchannel flow. Experiments in Fluids 27:414-19.
Patankar, S.V. 1980. Numerical heat transfer and fluid flow. Taylor & Francis.
Posner, J.D., C.R. Buchanan, and D. Dunn-Rakin. 2003. Measurement and prediction of indoor air flow in a model room. Energy and Buildings 35:515-26.
Rey, F.J. and E. Velasco. 2000. Experimental study of indoor air quality, energy saving and analysis of ventilation norms in climatised areas. Energy and Buildings 33:57-67.
Seta, T., E. Takegoshi, and K. Okui. 2006. Lattice Boltzmann simulation of natural convection in porous media. Mathematics and Computers in Simulation 72:195-200.
Sorensen, D.N. and P.V. Nielsen. 2003. Quality control of computational fluid dynamics in indoor environments. Indoor Air 13:2-17.
Srebric, J., V. Vukovic, G. He, and X. Yang. 2008. CFD boundary conditions for contaminant dispersion, heat transfer and airflow simulations around human occupants in indoor environments. Building and Environment 43(3):294-303.
Stamou, A. and I. Katsiris. 2006. Verification of a CFD model for indoor airflow and heat transfer. Building and Environment 41:1171-81.
Succi, S. 2001.The lattice Boltzmann equation for fluid dynamics and beyond. Oxford University Press.
Sukop, M. and D. Thorne. 2005. Lattice Boltzmann modeling, an introduction for geoscientists and engineers. Springer, Berlin.
Tsutahara, M., T. Kataoka, K. Shikata, and N. Takada. 2008. New model and scheme for compressible fluids of the finite difference lattice Boltzmann method and direct simulations of aerodynamic sound. Computers & Fluids 37:79-89.
Turiel, I., C.D. Hollowella, R.R. Mikscha, J.V. Rudya, R.A. Younga, and M.J. Coyeb.1983. The effects of reduced ventilation on indoor air quality in an office building. Atmospheric Environment 17:51-64.
Wolf-Gladrow, D.A. 2000. Lattice-gas cellular automata and lattice Boltzmann models--An introduction. Springer, Berlin.
Yakhot, V. and S.A. Orszag.1986, Renormalization group analysis of turbulence: I. Basic theory. Journal of Scientific Computing 1:1-51.
Yan, W., Y. Zhang, Y. Sun, and D. Li. 2009. Experimental and CFD study of unsteady airborne pollutant transport within an aircraft cabin mock-up. Building and Environment 44(1):34-43.
Yang, X., J. Srebric, X. Li, and G. He. 2004. Performance of three air distribution systems in VOC removal from an area source. Building and Environment 39(11):1289-99.
Zhai, Z. 2006. Application of computational fluid dynamics in building design: aspects and trends. Indoor and Built Environment 15(4):305-13.
Zhang, J.S. 2005. Combined heat, air, moisture, and pollutants transport in building environmental systems. JSME International Journal, Series B 48(2):182-90.
Received May 3, 2010; accepted August 18, 2010
S.J. Zhang is an associate professor at the Center of Fluid Mechanics,, College of Environmental Science and Engineering, Hohai University, Nanjing, China. C.X. Lin is an associate professor in the Department of Mechanical, Aerospace, and Biomedical Engineering at the University of Tennessee, Knoxville, TN.
S.J. Zhang, PhD
C.X. Lin, PhD
|Printer friendly Cite/link Email Feedback|
|Author:||Zhang, S.J.; Lin, C.X.|
|Publication:||HVAC & R Research|
|Date:||Nov 1, 2010|
|Previous Article:||Research on flow resistance characteristics with different window/door opening angles.|
|Next Article:||Indoor air quality, ventilation, and energy conservation in buildings: innovation and integration (part 1).|