Development of New Method for Flow Computations in Vehicle Ventilation

Transcription

1 2005:110 CIV MASTER S THESIS Development of New Method for Flow Computations in Vehicle Ventilation FRIDA NORDIN MASTER OF SCIENCE PROGRAMME Luleå University of Technology Department of Applied Physics and Mechanical Engineering Division of Fluid Mechanics 2005:110 CIV ISSN: ISRN: LTU - EX / SE

2 Abstract It is desired by the CFD-engineers of the Climate team at Volvo Cars to be able to estimate the accuracy of the computed pressure drop over ventilation ducts in cars. It is also of interest to be able to accurately predict the velocity distribution in the ducts for a better prediction of the distribution in the car compartment. The present method of creating computational models of the ducts involves the use of Wall Functions in order to model the near wall region. An alternative method has been developed in this thesis work in which the boundary layer is fully resolved. This implies a different grid in the computational domain, different turbulence models have also been tested with the alternative method. The ventilation duct chosen for this study is the B-pillar duct. Unfortunately no test data are available for this duct and an academic experimental case has been used in order to investigate the impacts of the alternative method and also to investigate the accuracy of the present method. The results from the academic case study were used as input when models of the B-pillar duct were created. From the study of the academic case it was shown that the grid resolution of a model is of great importance in order to accurately predict the velocity distribution. A much higher grid resolution than what is generally obtained in the B-pillar duct models when using the present method must be achieved if it is desired to predict the velocity field in the ducts. Due to differences between the academic case and the B-pillar duct case and since no test data are available for the B-pillar duct, the accuracy of the computed pressure drop over the ventilation duct is difficult to estimate. Commonly for both cases were however that simulations with models created according to the alternative method resulted in a higher pressure drop than simulations with models created according to the present method.

3

4 Acknowledgements I would like to express my sincere gratitude towards all the people who supported me during the work of this thesis. Firstly, I would like to thank my supervisor at Volvo Car Corporation, Ph.D Åsa Adamsson for her guidance and continuous support throughout the work. I also would like to thank Ph.D Andreas Borg at Volvo Car Corporation, for always finding time to discuss my work and for many unvaluable advices. My examiner at Luleå University of Technology, Prof. Rikard Gebart, is gratefully acknowledged for providing me with fast and full answers and for his interest and support. Finally, I would like to thank the whole CFD-group for always making me feel part of the group and for a great atmosphere.

5 Contents 1 Introduction Current Situation Description of the Project Outline of Thesis Work Theory Governing Equations Computational Methods Numerical Grid Finite Volume Method Errors and Accuracy Turbulent Flow Reynolds-Averaged Method Turbulence Models Near Wall Treatment The Wall Function Approach The Resolving the Near-Wall Region Approach Grid Considerations Academic Case Description of the Experiment Models Created According to the Present Method Development of an Alternative Method Grid Dependency Study Influence of Turbulence Models Results from the Academic Case Study Model Criteria Pressure Distribution Velocity Distribution Turbulent Kinetic Energy Pressure Drop

6 4 B-pillar Duct Grid Considerations Compromised Mesh Ideal Mesh Models Generated According to the Present Method Results from the B-pillar Duct Study Model Criteria Pressure Drop Solution Stability and Convergence Conclusions and Recommendations Future Work A Suggestion of Computational Method 75 B Model Settings 84 C Grid Settings for the Grid Dependency Study 87

7 Chapter 1 Introduction 1.1 Current Situation At the climate team of the Volvo CFD group, numerical methods are used to develop ventilation-system ducts and nozzles. Until now, the computations of the ducts have mainly been done in order to investigate the impact of different duct designs and not to predict absolute values. The latter has however become more important. In order to fulfil requirement specifications for the ventilation ducts and to give input to the development of the ventilation-air heater (HVAC), absolute values of the pressure drop are required. It is also desired to achieve accurate prediction of the velocity distribution in the ducts and nozzles in order to better predict the distribution of the ventilation air in the compartment. The current method used to predict the air distribution and pressure drop in the ducts and channels is a so called high-reynolds number formulation. This method implies a rather rough approximation of the boundary layer of the flow, which is not an optimum approach for predicting internal flows, which are highly affected by the surrounding walls. Another characteristic of the duct flows of interest that makes the current approach less appropriate is the relatively low mass flow in the ventilation ducts, which increases the impact of viscous effects. 1.2 Description of the Project The goal of this thesis work is to investigate different approaches in generating the computational grid, the impact of different turbulence models and to give an input to a new computational method for simulating flow through a B-pillar duct. The B-pillar duct, also called rear ventilation duct, is illustrated in Figure 1.1 and is one of the longest and geometrically most complex of the ventilation ducts in a car. Unfortunately, there are no test results available for the B-pillar duct making it 6

8 1.3. OUTLINE OF THESIS WORK 7 Figure 1.1: The B-pillar duct in Volvo cars. difficult to validate the computational results. To be able to compare the impacts of different configurations of grid design and turbulence models, and also to make a grid dependency study, an academic case with experimental data has been used. 1.3 Outline of Thesis Work This approach has divided the project work as well as this report into two parts. The first part treating the investigation of mesh generation, choice of turbulence model and grid dependency study for the duct corresponding to the academic experimental case. The second part of the report describes the work how to translate the results from the academic case study into a computational model for the B-pillar duct. A goal of the thesis work was also to give input to a new computational method for ventilation ducts and this will be found in Appendix A. The commercial softwares used in this project are ANSA , TGrid and FLU- ENT 6.1.

9 Chapter 2 Theory 2.1 Governing Equations Fluid flow obeys conservation laws for mass, momentum, and energy [1]. Since no heat transfer occurs in the problems in this thesis work, only mass and momentum will be considered. The set of equations used in order to describe the motion of a fluid flow consists of the continuity and momentum equations and are generally called the Navier-Stokes equations. The principle of conservation of mass can be expressed on a differential form [2] ρ t + (ρu i) = 0, (2.1) x i where u i (i=1,2,3) or (x, y, z) are the velocity components in the direction of the coordinates x i and ρ is the density of the fluid and t is time. This equation is known as the continuity equation. The differential form of the conservation of momentum expressed by Newton s second law, can be written as [2] ρu i t + ρu iu j x j = ρg i + τ ij x j, (2.2) where g i is the component of the gravitational acceleration in the direction of the Cartesian coordinate x i and τ ij is the stress tensor. τ ij can be expressed as [2] ( τ ij = p + 2 ) 3 µ u i δ ij + 2µe ij, (2.3) x i 8

10 2.1. GOVERNING EQUATIONS 9 where µ is the dynamic viscosity, p is the static pressure, δ ij is the Kronecker delta and e ij is the strain rate tensor [2], e ij = 1 2 ( ui + u ) j. (2.4) x j x i If the fluid is assumed to be incompressible (density does not change with pressure) the continuity equation (Eq. 2.1) reduces to u i x i = 0, (2.5) and the stress tensor in the equation of momentum conservation (Eq. 2.3) reduces to τ ij = pδ ij + 2µe ij. (2.6) Assuming the flow to consist of an incompressible newtonian fluid, in which the temperature differences are small allowing the viscosity to be regarded as a constant (and noting that ( p/ x j )δ ij = p/ x i ) [1], the Navier-Stokes equation can be expressed as u i t + u iu j x j = 1 p + g i + µ ρ x i ρ x j ( ui + u ) j. (2.7) x j x i

11 10 CHAPTER 2. THEORY 2.2 Computational Methods The partial differential equations (PDEs), referred to as the Navier-Stokes equations (Eq.2.7) that describes the motion of a fluid can only be solved analytically for a few special cases [2]. In order to be able to solve a wider range of problems, discretization methods that approximates the PDEs with a system of algebraic equations are used and can be solved numerically with the help of computers [2]. This approach of describing and solving flow-related problems is generally called CFD, Computational Fluid Dynamics Numerical Grid The discretized equations are solved at discrete positions in a computational domain. A numerical grid defines these positions which are called nodes. The grid also describes the geometry of the computational domain. An unstructured grid is used in this project, which is a type of grid well suited when the geometry of the domain is complex, since the cells may have any shape[2]. Only tetrahedraland prismatic-shaped cells are however used in this project Finite Volume Method The discretization method used in this project (by the FLUENT 6.1 Solver), and in most codes used for industrial purposes is the Finite Volume Method (FVM). In this method, the computational domain is subdivided into a finite number of control volumes (cells) that are in direct contact to each other. An integral form of the conservation equations is used and applied to all the control volumes, and the variable values are calculated at a computational node at the center of the control volume [2]. Variable values at locations other than the computational node are interpolated from the nodal values. This is normally done by a series expansion about a single point and referred to as the differencing scheme of the approximation. The order of the scheme is the same as the highest order term included in the series expansion. The FVM is conservative as long as the surface integrals are the same for all control volumes that share a boundary, and it is possible to use any type of grid [2] Errors and Accuracy The accuracy of the numerical solutions depends on the quality of the discretisation, i.e. the quality of the discretization method and the quality of the numerical grid [2]. However, numerical results are always approximate. Errors arise from each part of the process in achieving numerical solutions. Three kinds of systematic errors are however always included in a numerical solution[2]: - Modelling errors - Discretization errors

12 2.2. COMPUTATIONAL METHODS 11 - Iteration errors The modelling errors are defined as the difference between the actual flow (reality) and the exact solution of the mathematical model, and depend on the assumptions made in deriving the transport equations for the variables [2]. An important source of model errors is the use of turbulence models when describing a turbulent flow [3]. The discretization errors are defined as the difference between the exact solution of the conservation equations and the exact solution of these equations when discretized, these types of errors should become small as the grid spacing goes to zero[2]. The iteration errors are defined as the difference between the iterative and exact solution of the discretized equations and decreases as the number of iterations increases[2]. Both the discretization- and iteration errors are time-dependent since a higher grid-density increases the computational time required as do an increased number of iterations. The modelling errors can only be known by comparing solutions with accurate experimental data or with data obtained from more accurate models if the iteration- and discretization errors are negligible [2]. Errors of different types may cancel each other out, so that numerical solutions from a coarse grid might agree better with corresponding experimental data than solutions obtained from a finer grid [2].

13 12 CHAPTER 2. THEORY 2.3 Turbulent Flow Turbulent flow is characterized by irregular, non-linear and three dimensional motions, a high diffusivity, high levels of fluctuating vorticity and large viscous losses [1]. Since these characteristics can be of small scale and high frequency, they are in most cases too computationally demanding to be simulated directly [4] Reynolds-Averaged Method Instead of solving the exact governing equations for the turbulent flow, they can be time averaged to remove the small scales. In the Reynolds-averaged approach the variables are decomposed into a timeaveraged and a fluctuating term [2] where φ(x i, t) = φ(x i ) + φ (x i, t), (2.8) 1 T φ(x i ) = lim φ(x i, t) dt. (2.9) T T 0 The variable t is time and T is the averaged interval and φ is the flow variable. If T is large enough, φ does not depend on the time at which the averaging started [2]. Applying the Reynolds-averaging method (2.9) to the Continuity-(Eq. 2.1) and Momentum-(Eq. 2.2) equations and assuming that the fluid is incompressible, yields the Reynolds-averaged Navier-Stokes (RANS) equations [2], and x i (ρū i ) = 0 (2.10) t (ρū i) + (ρū i ū j + ρu i u j ) = p + τ ij, (2.11) x j x i x j where τ ij are the mean viscous stress tensor components

14 2.3. TURBULENT FLOW 13 ( ūi τ ij = µ + ū ) j. (2.12) x j x i Averaging any linear term in the conservation equations simply gives the identical term for the averaged quantity, since φ = 0 according to (Eq. 2.9). However, averaging the nonlinear terms leads to terms such as the Reynolds stresses, ρu i u j, which must be modelled [2]. There are different approaches in how to approximate these terms in order to achieve closure and these approximations are called turbulence models Turbulence Models Eddy-Viscosity Hypothesis A common method to model the Reynolds stresses is to employ an eddy-viscosity hypothesis [2] according to ( ūi ρu i u j = µ t + ū ) j 2 x j x i 3 ρδ ijk. (2.13) In Eq. 2.13, k is the turbulent kinetic energy, defined as k = 1 2 (u x u x + u y u y + u z u z ). (2.14) The last term in Eq is included in order to make sure that the equation always is valid. Some of the commonly used turbulence models that apply the eddy-viscosity hypothesis are shortly mentioned in the following sections. The Standard k-ε Model The Standard k-ε model is based on transport equations of the turbulent kinetic energy, k, and its dissipation rate, ε. In FLUENT 6.1 [4] the transport equations for these quantities are as follows; t (ρk) + (ρku i ) = x i t (ρε) + (ρεu i ) = x i x j x j [( µ + µ ) ] t k + G k + G b ρε Y M + S k, (2.15) σ k x j [( µ + µ ) ] t ε ε + C 1ε σ ε x j k (G k + C 3εGb ) C 2ε ρ ε2 k + S ε, (2.16)

15 14 CHAPTER 2. THEORY where G k represents the generation of turbulent kinetic energy due to the mean velocity gradients, G b is the generation of turbulent kinetic energy due to buoyancy, Y M is the contribution of the fluctuating dilatation in compressible turbulence to the overall dissipation rate [4]. C 1 ε, C 2 ε and C 3 ε are constants and σ k and σ ε are the Prandtl numbers for k and ε. S k and S ε are user-defined source terms[4]. The default values of the model constants in FLUENT 6.1 are C 1ε = 1.44, C 2ε = 1.92, σ k = 1.0, σ ε = 1.3 The RNG k-ε Model The RNG k-ε model is derived from the instantaneous Navier-Stokes equations, using a technique called Renormalisation Group (RNG) methods [4]. The transport equations for k and ε are [4] t (ρk) + (ρku i ) = x i t (ρε) + (ρεu i ) = x i x j x j ( ) k α k µ eff + G k + G b ρε Y M + S k (2.17) x j ( ) ε ε α ε µ eff + C 1ε x j k (G k + C 3εGb ) C 2ε ρ ε2 k R ε + S ε (2.18) where G k, G b, Y M, S k and S ε represents the same phenomenon as described above for the Standard k-ε model [4]. The default values of the model constants in FLUENT 6.1 are C 1ε=1.42, C 2ε = The Realizable k-ε Model The modelled transport equation for k is the same for the Realizable k-ε model as for the Standard k-ε model (Eq. 2.15). The modelled transport equation for ε differ however from the Standard and RNG k-ε models t (ρε)+ (ρεu i ) = x i where x j [( µ + µ ) t ε ε ]+ρc 2 1 S ε ρc 2 σ ε x j k + νε +C ε 1ε k C 3εG b +S ε (2.19) C 1 = max[0.43, η η + 5 ] (2.20)

16 2.3. TURBULENT FLOW 15 and η = S k ε (2.21) G k represents the generation of turbulent kinetic energy due to the mean velocity gradients. G b is the generation of turbulent kinetic energy due to bouncy [4]. Y M represents the contribution of the fluctuating dilatation in compressible turbulence to the overall dissipation rate [4]. C 2 and C 1ε are constants, σ k and σ ε are the Prandtl numbers for k and ε and S k and S ε are user-defined source terms [4]. The default values of the model constants are C 1ε=1.44, C 2 = 1.9, σ k = 1.0, σ ε = 1.2. The Shear Stress Transport (SST) k-ω Model The SST k-ω model is a k-ω model in which the definition of the turbulent viscosity is modified to account for the turbulent shear stress [4]. The turbulent kinetic energy, k, and the specific dissipation rate, ω, are modelled in FLUENT 6.1 according to the following transport equations and t (ρk) + (ρku i ) = x i x j ( ) k Γ k + G k Y k + S k (2.22) x j t (ρω) + (ρωu i ) = x i x j ( ) ω Γ ω + G ω Y ω + D ω + S ω. (2.23) x j In these equations, G k represent the generation of turbulent kinetic energy due to mean velocity gradients. G ω represents the generation of ω. Γ k and Γ ω represent the effective diffusivity of k and ω, respectively. Y k Y ω represent the dissipation of k and ω due to turbulence. D ω represents the cross-diffusion term. S k and S ω are user-defined source terms. The effective diffusivities for the SST k ω model are given by Γ k = µ + µ t σ k, (2.24) Γ ω = µ + µ t σ ω, (2.25) where σ k and σ ω are the turbulent Prantl numbers for k and ω, respectively. The model constants in FLUENT 6.1 are σ k = 2.0, σ ω = 2.0.

17 16 CHAPTER 2. THEORY 2.4 Near Wall Treatment Turbulent flow is highly affected by bounding walls. In the region close to the wall, quantities, like mean velocity and turbulent kinetic energy, changes rapidly involving large gradients. Also the momentum and other scalar transports are most powerful in this region.[4] Generally, the near-wall region is subdivided into three regions, where the outermost is called the fully turbulent region, the innermost (closest to the wall) is called the viscous sublayer and the third, buffer region is in between the two others [4]. In the fully turbulent region, logically, it is turbulence that mainly affects the flow behavior. In the viscous sublayer, molecular viscosity-effects are very important and the flow is almost laminar. The buffer region is in-between in duplicate ways as the effects of molecular viscosity and turbulence are regarded as equally important here. The demarcation between these three regions is usually defined by a wall unit called y + [4]. y + is defined as y + ρu τ y µ, (2.26) where y is the normal distance from a node, at the cell center, to the wall, ρ is the fluid density, µ is the dynamic viscosity of the fluid and u τ is the friction velocity at the wall and will be described later. The viscous sublayer is generally assumed to extend from the wall to y + 5 and the buffer region from the upper limit of the sublayer to y + 60 and the fully turbulent region (also called the log-law region) from the upper limit of the buffer region to about y [4], depending on the Reynolds number of the flow. The Reynolds number, Re, is a non dimensional quantity, given by Re = UL c ν, (2.27) where U is the mean velocity of the flow, L c is a characteristic length of the computational domain and ν is the kinematic viscosity of the fluid. The Reynolds number is a frequently used measure for describing whether a fluid flow is laminar or turbulent. Turbulence models must be modified in order to include the wall-effects of the turbulent flow [4]. This is mostly done in two different ways which are to be treated in the two following sections.

18 2.4. NEAR WALL TREATMENT The Wall Function Approach A wall function contains a logarithmic law for the mean velocity in the fully turbulent region and formulas for turbulent quantities near the wall. The viscous sublayer and the buffer region are not resolved since the wall function is used as a bridge over this region. Models that applies the wall function approach is often referred to as high-reynolds number models, since the wall function approach is best suited for high Reynolds number flows which aren t too affected by viscosityeffects. The law-of-the-wall for mean velocity in the standard wall function, accessible in FLUENT 6.1, can be expressed as where U = 1 κ ln (Ey ) (2.28) U U P Cµ 1/4 k 1/2 P τ w /ρ (2.29) y ρc1/4 µ µ k 1/2 P y P (2.30) and κ = von Kármán constant (=0.42) E = empirical constant (=9.81) U P = mean velocity of the fluid at a point P k P = turbulent kinetic energy a at point P y P = normal distance from the wall to the point P µ = dynamic viscosity of the fluid ρ = density of the fluid τ w = shear stress at the wall The value of C µ depends on how it is treated in each turbulence model [4]. It is recommended that the distance to the first node adjacent to the wall (y P )

19 18 CHAPTER 2. THEORY correspond to a value of y above 30 for the law of the mean velocity to be valid [3][4]. In FLUENT 6.1 [4], this law is employed when y is greater than If it is assumed that the flow is in local equilibrium, which means that the production and dissipation of turbulence are nearly equal [2], the friction velocity, u τ, can be expressed by u τ = C 1/4 µ k 1/2, (2.31) and the wall unit y (Eq. 2.30) equals y + (Eq. 2.26). The friction velocity is also given by [2] u τ = τ w ρ, (2.32) where τ w is the shear stress at the wall. If the mesh is such that y < at the first node, a laminar stress-strain relationship that can be written is applied [4]. U = y (2.33) The diffusive flux of the turbulent kinetic energy through the wall is usually taken to zero [2], which yields the boundary condition that the normal derivative of the turbulent kinetic energy is zero [2][4], where n is the local coordinate normal to the wall. k = 0, (2.34) n The production of k at the wall-adjacent cell is computed from and ε is computed from G k τ w U y, (2.35)

20 2.4. NEAR WALL TREATMENT 19 ε P = C1/4 µ k 1/2 P. (2.36) κy P ε is computed from Equation 2.36 at the wall-adjacent cell [4]. The wall function approach is very common in industrial applications because of its economical and robust nature, and for many cases it is a reasonably accuracy of the results [4]. However, in some cases it is not a good choice. For instance when near-wall effects are important such as flow through narrow passages or lowvelocity fluid flow. In such cases another approach which fully resolves the near wall region is preferable The Resolving the Near-Wall Region Approach In this approach, the turbulence model is modified in order to enable a resolution of all three parts of the near-wall region [4]. This requires a highly dense grid in the near-wall region of the domain in order to capture the gradients, which significantly increases the number of cells in the computational domain. Models that applies this approach to the near-wall region is often referred to as low-reynolds number models. It is important to note that this is because of a local turbulent Reynolds number which is low in the viscous-affected region and signifies that viscosity effects are important [4]. In order to come around the restriction of a very fine grid in the whole domain, which requires an increase of the computational time, a near-wall modeling method has been developed that has the ability to blend between the wall function - and fully resolving the near wall region - approaches. This is done by combining a two-layer model and enhanced wall functions and is called Enhanced Wall Treatment[4]. This method is available in FLUENT 6.1 for the three k-ε models, described in Section 2.3.2, and the Reynolds Stress Model(RSM) [4]. Enhanced Wall Treatment The two-layer model is an integral part of the Enhanced Wall Treatment and is used to specify ε and the turbulent viscosity in the near-wall cells [4]. When using the two-layer model, the whole domain is subdivided into two regions, a viscosity affected region close to walls and a fully turbulent region. The regions are defined by a wall-distance-based turbulent Reynolds number [4], Re y ρy k µ, (2.37)

21 20 CHAPTER 2. THEORY where y is the normal distance from the wall to the node and the two regions are separated at Re y = 200 [4]. In the fully turbulent region, where Re y > 200, the k-ε models or the RSM are used. In the viscosity-affected region (Re y < 200), the turbulent viscosity for the Enhanced Wall Treatment is defined as a combination of the turbulent viscosity expressed by the two-layer formulation and the turbulent viscosity expressed by the currently used turbulence model [4]. It can be written as µ t,enh = λ εµ t + (1 λ ε ) µ t,2layer (2.38) where µ t is the turbulent viscosity defined according to the current turbulence model. The turbulent viscosity for the two-layer model is computed from and the length scale, l µ, is computed from µ t,2layer = ρc µl µ k, (2.39) l µ = yc l ( 1 exp Rey/Aµ ). (2.40) c l and A µ are constants with the following values; c l = κc 3/4 µ, A µ = 70. The blending factor, λ ε, is defined in such a way that it is equal to unity far from walls and is zero close to walls [4]. The ε field in the viscosity-affected region is computed from and the length scale, l ε, is computed from ε = k3/2 l ε, (2.41) l ε = yc l ( 1 exp Rey/Aε ). (2.42)

22 2.4. NEAR WALL TREATMENT 21 The constant A ε = 2c l. A similar blending procedure as the one for the turbulent viscosity is used in FLUENT 6.1 for the specification of ε, in order to achieve a smooth transition between the algebraically specified ε in the inner region (Eq. 2.41) and ε obtained from solution of the transport equation in the outer region [4]. The enhanced wall function is a law-of-the-wall that is applicable in all three parts of the near-wall region. This is made possible by blending linear(laminar) and logarithmic(turbulent) laws-of-the-wall in the following manner, The general equation for the derivative du+ dy + u + = exp Γ u + lam + exp 1 Γ u + turb, (2.43) is + du + du = lam expγ dy + dy + + exp 1 Γ du + turb dy +. (2.44) This formulation guarantees the correct asymptotic behaviour for large and small values of y + and a reasonable representation of velocity profiles in the case where y + falls inside the buffer region (3 < y + < 10) [4]. It is however recommended that the mesh is generated according to either the wall function approach or the near-wall approach. The enhanced turbulent law-of-the-wall can be modified and extended to take into account other effects such as pressure gradients [4]. Near Wall Treatment for the SST k-ω Model In FLUENT 6.1, the wall boundary conditions for the k equation in the k-ω models are treated in the same way as the k equation is treated when Enhanced Wall Treatment is used with the k-ε models [4]. In FLUENT 6.1 the value of ω at the wall is specified as ω w = ρ(u τ ) 2 µ ω+. (2.45) The asymptotic value of ω + in the laminar sublayer is given by ( ) ω + = min ω w + 6, β (y + ) 2, (2.46)

23 22 CHAPTER 2. THEORY where where ω w + = ( 50 k + s 100 k + s ) 2 k + s < 25 k + s 25 k + s and k s is the roughness height. = max (1.0, ρk su ) µ (2.47) In the turbulent region, the value of ω + is ω + = 1 β du + turb dy +, (2.48) which lead to the value of ω in the cell adjacent to the wall as ω = u β κy, (2.49) where β = If the wall adjacent cell is being placed in the buffer region, FLUENT 6.1 will blend ω + between the logarithmic and laminar sublayer values [4]. If the Transitional Flows option is enabled for the SST k-ω model, a low- Reynolds number variant is used Grid Considerations Resolving the Near Wall Region If choosing a turbulence model which is modified in order to resolve the near wall region a sufficient number of cells must be generated into a very small region adjacent to the wall, in order to capture the variations of the flow variables [4][3]. y + (Eq. 2.26),the non dimensional wall distance is commonly used as a measure to determine if the near wall region is sufficiently resolved. The mesh guidelines available in [4] for the Enhanced Wall Treatment option, when using any of the three k-ε models or the RSM, and for the Transient Flow option, when using any of the k-ω models, are as follows

24 2.4. NEAR WALL TREATMENT 23 - y + at the wall-adjacent node should be on the order of y + 1. A higher y + value is acceptable as long as it is well inside the viscous sublayer (y + < 4 to 5). - There should be at least 10 cells within the viscosity-affected near wall region (Re y < 200) in order to solve the mean velocity and turbulent quantities in that region. Some other general guidelines [3] for the near wall mesh are - Depending on the Reynolds number, ensure that there are 5-10 nodes between the wall and y + = 20 for adequate boundary layer resolution. - Avoid the use of tetrahedral elements in the boundary layer. Another consideration when generating a grid with different types of cells in different regions of the computational domain is to keep the distance between the nodes as homogeneous as possible in order to make the transition between the different cell-types as smooth as possible. This is of course important for the whole mesh [3]. Figure 2.1 is an illustration of the transition between a prism cell and a tetrahedral cell. Figure 2.1: The distance between the nodes in the interface between different cell types should be kept as homogeneous as possible. Wall Function If the Wall Function approach is applied, the mesh guidelines are different. In [4] the following advices are given - It is important that the first node adjacent to the wall is positioned in the region where the log-law is valid. - The log-law is known to be valid for y + > 30 to 60, and a y + value close to the lower bound is most desirable.

25 24 CHAPTER 2. THEORY - FLUENT employs the log-law when y + > The upper bound of the log-law depends on, among others, pressure gradients and Reynolds number. As the Reynolds number increases, the upper bound tends to also increase. - It is important to have at least a few cells inside the boundary layer. For the upper limit of the distance between the first node adjacent to the wall and the wall, when using wall functions, the recommendations depend on the Reynolds number of the flow. In the case of moderate Reynolds numbers, a distance corresponding to y + < 100 is required if the boundary layer is to be solved accurately[3].

26 Chapter 3 Academic Case When investigating impacts of different parameters in a computational model it is favourable to have access to an experiment or a test corresponding to the model in order to compare and validate the computational results with the experimental ones. Unfortunately, no test data are available for the B-pillar duct used in this project, so computational models based on an academic experimental case has therefore been created. The academic case is found in a database linked to the ERCOFTAC (European Research Community On Flow, Turbulence And Combustion) homepage[6]. The geometry of the experimental duct is less complicated than the geometry of the B-pillar duct, and the flow characteristics are to some extent different from those that usually are applied in the ventilation ducts. However, the ability to compare simulated results to experimental ones was considered to be more important than the differences between the ducts. Today, a method based on the Wall Function approach is employed, by the CFD-engineers at the Volvo Climate team, when modelling ventilation ducts in cars. These ducts are generally quite narrow and the flow rate of the ventilationair is normally low which makes this approach inconvenient. The model criteria when using Wall Functions (Sec ) implies a coarse grid close to walls and since the ducts are narrow the grid will be coarse in the whole domain. With the academic experimental case as basis, an alternative method to generate computational models has been developed and investigated in terms of mesh generation and turbulence modelling. Computational models of the academic experimental duct have also been generated according to the present method in order to investigate the accuracy of this method and in order to compare these results to the results when using the alternative method. 25

27 26 CHAPTER 3. ACADEMIC CASE 3.1 Description of the Experiment The experiment [6] is performed with a circular cross section pipe made of two long straight inlet and outlet parts, connected by a 180 bend, illustrated in Figure 3.1. In the figure, the coordinate s describes the position along the pipe downstream the bend, and -s the position upstream the bend. The relationship s/d, where D is the inner diameter of the pipe given in Table 3.1, is frequently used to describe a specific location of the pipe. This duct will henceforth be referred to as the A-duct. Figure 3.1: The geometry of the duct used in the experimental case. Geometric properties and flow characteristics for the experimental case are given in Table 3.1 and Table 3.2, respectively. Geometric properties Pipe diameter, D [mm] 76.2 Straight pipe length [mm] 7300 Total length [mm] Mean radius of the bend curvature, R [mm] Table 3.1: Geometric properties of the academic case. The experiment is performed using a centrifugal blower placed at one end of the pipe in order to draw airflow through the test rig [6]. Measurements are performed at several positions along the pipe and at four different angular positions along the bend. These angular positions are illustrated in Figure 3.2, where θ is the angular coordinate. Available measurements are mean- and fluctuating velocity components, turbulent

28 3.1. DESCRIPTION OF THE EXPERIMENT 27 Flow characteristics Air with kinematic viscosity, ν [m 2 /s] Bulk axial velocity in inlet straight pipe, U 0 [m/s] 10.4 Reynolds number, Re Wall friction velocity (at s/d=-18), u τ [m/s] Table 3.2: Inflow parameters for the academic case. Figure 3.2: Pipe bend with angular positions. kinetic energy (deduced from the fluctuating velocity components) and distribution of the static pressure coefficient, C p. C p is given by [6] C p = p p ρu 0 2, (3.1) where p is the static pressure at a given point, p 0 is the reference static pressure (taken at s/d=-18), ρ is the air density and U 0 is the mean bulk axial velocity in the pipe. The mean bulk velocity is given in Table 3.2.

29 28 CHAPTER 3. ACADEMIC CASE The velocity measurements are performed using a miniature hot-wire probe, and the static pressure is obtained using wall tappings [6]. The pressure measurements where performed along the inner and outer bend of the pipe. The velocity measurements where performed along the pipe-diameter parallel to the plane of the bend, and profiles are available for 0.47 r/d 0.47, where r is the inner radius and D the inner diameter of the pipe. In Figure 3.3 the diameter at which the velocity measurements are performed is represented by the horizontal diameter. Figure 3.3: Cross-section of in- and outlet part of the A-duct.

30 3.2. MODELS CREATED ACCORDING TO THE PRESENT METHOD Models Created According to the Present Method The present computational method, used by the Climate team for predicting the flow in ventilation ducts, consists of directions of how to generate the surfaceand volume-mesh, which turbulence model to use and settings for the boundary conditions of the computational domain. These directions have been followed in order to generate computational A-duct models that correspond to the present method of creating ventilation duct models. A short sum up of the recommended settings when modelling a ventilation duct according to this method is given in Table 3.3. Settings according to current procedure Edge length of surface-element Element-type of surface mesh Element-type of volume mesh Turbulence model Near wall treatment 1-6 mm Triangles Tetrahedrons Realizable k-ε Standard wall function Table 3.3: Some of the used settings when creating a model according to the present computational method. In order to investigate the present computational method and to get an estimation of its accuracy when simulating flow through the B-pillar duct, three models of the A-duct have been created with different edge lengths of the surface elements. 3, 6 and 12 mm are the chosen lengths. Examples of the mesh resolution at a cross section, for each model is illustrated in Figure 3.4. The reason for choosing the third length to 12 mm, even though that is twice the maximum length according to the procedure (see Table 3.3), is the difference in hydraulic diameter, D h, between the A-duct and the B-pillar duct. D h is given by [7] D h = 4A P, (3.2) where A is the cross sectional surface of the fluid domain and P is the circumference of the domain. (For the circular A-duct, the hydraulic diameter is the diameter.) The grid resolution obtained for a A-duct model using surface-elements with 12 mm edges approximately corresponds to the obtained resolution in B-pillar duct model using surface-elements with 6 mm edge lengths. Following the same line of arguments, the A-duct models with edge lengths of 3- and 6 mm would correspond to B-duct models having surface elements with 1- and 3 mm edge lengths.

31 30 CHAPTER 3. ACADEMIC CASE (a) 3 mm element edge. (b) 6 mm element edge. (c) 12 mm element edge. Figure 3.4: Grids with three different edge lengths of the surface mesh at a crosssection of the A-duct.

32 3.3. DEVELOPMENT OF AN ALTERNATIVE METHOD Development of an Alternative Method The y + -criteria connected to the two different approaches of modelling the near wall region (Sec ) greatly affects the resulting mesh. By it s definition (Eq. 2.26), y + at the first node adjacent to the wall depend on the normal distance to the wall from the node and the friction velocity, u τ, at the wall. When creating computational models for ventilation ducts (designed for cars), which have a narrow geometry and in most cases a quite low Reynolds number of the flow, it can be difficult to create a mesh that both fulfills the y + -criteria and yet is sufficiently dense in order to resolve the flow variations. Since the size of the elements is the only parameter that is independent of the flow characteristics, an adjustment of the mesh is the only mean for accomplishing an accurate y + -value for the model, which results in a very coarse grid for the models that employ the Wall Function approach. Following this line of arguments, the only way to increase the gridresolution and thereby also the accuracy of the duct models is to fully resolve the near wall region of the flow, allowing (implying) a large amount of cells in the model. The theoretical basics of this approach are described in Sec Of course there are drawbacks using this approach as well, for instance the large amount of cells that is required, which increases the computational time and also the fact that more work will be needed in order to generate a high-quality mesh. Time is as always a restricting factor when effectiveness is a commandment, which will result in a mix between the two approaches (fully resolving the near wall region vs. wall functions) for the B-pillar duct. It is however possible to create a complete low-reynolds number model for the A-duct. Grid Considerations In order to fulfil the mesh-criteria for a model that fully resolves the near wall region, described in Sec , layers of prismatic cells are generated from the duct-wall into the domain. The prismatic cells are generated with a quite large aspect ratio in order to save the number of cells and thereby also computational time. The layers are created with a specified growth rate greater than 1, so that the node distribution in the near wall region is more dense close to the wall. This limits the obtained number of cells and it also makes it possible to avoid large variations of the distance between the nodes in the interface where prismatic cells are in contact to the tetrahedral cells, which are generated in the middle of the duct. Some other considerations when generating a mesh of this type are for instance how deep the prismatic region should be and how many layers (nodes perpendicular to the wall) it should contain. Several grids have been created in order to investigate the differences between different settings but also in order to develop a method for generating these types of grids that is as straight forward and user friendly as possible.

33 32 CHAPTER 3. ACADEMIC CASE Grid Dependency Study Since the governing equations are discretized (according to the Finite Volume Method (FVM), see Sec 2.2.2) the solution of a simulation will be an approximation of the exact mathematical solution. The difference between the exact and simulated solution is called the numerical- or discretisation error of a simulation [2], Φ φ h = ɛ, (3.3) where Φ represent the exact solution, φ h represents the simulated solution and ɛ the numerical error. This error may be approximated by a Taylor series expansion [2] ɛ = k 1 h + k 2 h 2 + O(h) 3, (3.4) where k 1 and k 2 are constants, h representing the edge length of a volume element, and O represents higher order terms. The order of the terms depends on the order of the advection scheme [2]. To give an estimate of the numerical error in a simulation, a grid dependency study should be performed. Strictly, the grid should be doubled twice in each direction for the most accurate result [3], but that is only possible when the grid is structured. Since the use of tetrahedral-cells when generating the volume mesh implies an unstructured grid, the refinement is done by changing the edge length of the surface elements. When a change of a factor 2 resulted in either a very coarse grid when enlarged or a very fine grid with a very large amount of cells when diminished, a factor 1.5 has been used instead for the refinement of the grid. Meaning that the element length of the surface mesh (which controls the size of the tetrahedral volume cells) has been refined twice by a factor of 1.5. The three edge lengths for the surface mesh are chosen to 3, 4.5 and 6.75 mm, respectively. The refinement of the prismatic cells is done by keeping the same height of the prismatic-cell region in all three cases but adjusting the number of layers so that the height of the prismatic cell closest to the tetrahedral-cell region is about 2 3 of the adjacent tetrahedral cell-height. A case is set up and runned for the A-duct with each grid and a resulting quantity is chosen for the study. The parameter to be compared, φ h, is the difference in C p (3.1), C p, over an interval of the pipe. The interval is illustrated in Figure 3.5, and stretches from one diameter upstream the bend to 14 diameters downstream the bend. The resulting difference of C p over the specified interval from the three simulations is presented in Table 3.4.

34 3.3. DEVELOPMENT OF AN ALTERNATIVE METHOD 33 Figure 3.5: The interval of which the pressure-difference has been studied is located between s/d=-1 and s/d=14. Difference in C p between s/d=-1 and s/d=-14 Edge length [mm] C p Table 3.4: Difference in C p at one interval of the A-duct from simulations with the three different grids. The exact solution of the simulation is described by the sum of the simulated solution and the numerical error according to (Eq. 3.3). The exact solution expressed by the three different simulations is given in (Eq. 3.5), where h is the edge length of the surface-element of the finest grid. Φ = φ 2.25h + k 1 (2.25h) + k 2 (2.25h) 2 Φ = φ 1.5h + k 1 (1.5h) + k 2 (1.5h) 2 (3.5) Φ = φ h + k 1 h + k 2 h 2 The three unknowns and equations give the following solution; Φ = k 1 = k 2 = (3.6) From this result, the numerical error in each one of the three simulations may be estimated, as an absolute value in terms of C p as well as a relative numerical

35 34 CHAPTER 3. ACADEMIC CASE error of the simulation. For the three different cases, following relative error is computed. ɛ 2.25h /Φ 9% ɛ 1.5h /Φ 2% ɛ h /Φ 0.5% (3.7) To make sure that the assumption to evaluate the numerical error by a Taylor series is valid for the simulations, same computations were performed letting the result of the model with an edge length of 3 mm (h) be the exact solution since the relative error for this model was estimated to only 0.5%. This resulted in about the same error for the two other models, which indicates that the assumption is valid. Based on the results of this study, only the model with 3 mm edge length is close to be grid independent. However the mesh with an edge length of 4.5 mm (1.5h) is chosen as the mesh to be used for studying the influence of different turbulence models and from which a model for the B-pillar duct should be developed. The reason for this choice is that the amount of cells that can be generated in a model of the B-pillar duct is restricted if the model is to be used in a project, and a mesh for the B-pillar duct corresponding to the grid with a 3 mm edge in the A- duct would not be realizable. So the numerical error for the following simulations based on the grid with a 4.5 mm edge is estimated to be ±2% of the exact solution. An illustration of the chosen grid at a cross-section of the A-duct is shown in Figure 3.6 Figure 3.6: Cross section of the A-duct with a 4.5mm edge length and 18 prism-cell layers adjacent to the wall.

36 3.3. DEVELOPMENT OF AN ALTERNATIVE METHOD 35 Some of the settings for the chosen grid are presented in Table 3.5. Properties of the chosen mesh Edge length of surface element 4.5 mm First prism height 0.1 mm Growth rate 1.2 Number of prism layers 18 Height of last layer 2.2 mm 2 3 of tet-cell height 2.6 mm y + at first node 1.8 y + at last prism layer 260 nodes within y + = 20 6 nodes within y + = Table 3.5: Mesh generation settings and resulting properties of the model with a 4.5 mm edge length of the surface elements. More details of the settings for the three models, with differing surface mesh, used in this study can be found in Appendix C Influence of Turbulence Models In the work of developing a new method for predicting the flow in a ventilation duct, five different turbulence models have been tested. Since the situation is, as already mentioned, such that a low-reynolds number model would be preferable but the restriction in computational time leading to a restriction of the amount of cells makes it difficult to realize a complete low-reynolds model in the B-pillar duct, the choice of turbulence models is also restricted. In FLUENT 6.1, which is the currently used solver, an approach of modelling the near-wall-region that makes it possible to vary between fully resolving the boundary layer and applying a wall function to describe it, the so called Enhanced Wall Treatment [4], is accessible for four turbulence models. These are the three variations of the k- ε model (see Sec ) and also the Reynolds Stress Model (RSM) [4]. The Enhanced Wall Treatment approach is described in Section These four models and one k-ω model, the SST k-ω model (see Sec ) with Transitional Flows option (Sec ), are chosen for this investigation of the turbulence model influence. The models are listed below. - The Standard k-ε model with Enhanced Wall Treatment option. - The RNG k-ε model with Enhanced Wall Treatment option. - The Realizable k-ε model with Enhanced Wall Treatment option.

37 36 CHAPTER 3. ACADEMIC CASE - The SST k-ω model with Transitional Flow option. - The Reynolds Stress Model model with Enhanced Wall Treatment option. Unfortunately, the computations with the Reynolds Stress model (RSM) never converged to an acceptable level in spite of several essays. Since the A-duct has a quite simple geometry compared to the B-pillar duct, these results indicated that the RSM model would never (at least not for a long time) be considered for the B-pillar duct in a real project and were not further investigated because of this reason. In order to investigate the effects of the different turbulence models, the behaviour of several parameters are studied. The pressure distribution in terms of C p (Eq. 3.1), the axial velocity distribution at a number of cross-sections along the pipe and the turbulent kinetic energy at the same cross-sections. Since it is the bended part of the A-duct that is most similar to the B-pillar duct, the behaviour of different parameters in this region seemed to be the most interesting to study. The results from computations with different turbulence models are compared to each other and to the corresponding results from the experiment.

38 3.4. RESULTS FROM THE ACADEMIC CASE STUDY Results from the Academic Case Study With the experiment described in Section 3.1 as basis, several simulations have been performed with different computational models of the A-duct. To start with, three models were generated according to the present method (for duct flow computations at Volvo), in order to give an estimate of the accuracy of this approach. Then an alternative method of generating the computational grid was developed and a model with the resulting grid was simulated with four different turbulence models (still with the characteristics of the experiment as basis). In this section, the results from the above mentioned simulations will be presented. For the present method models, quantities as pressure- and velocity distribution are presented for the different grid-resolutions and compared to the corresponding experimental values. For the alternative method model, the influence of four different turbulence models is studied for resulting quantities as pressure, velocity and turbulent kinetic energy and compared to the corresponding experimental values. The results from the two different methods are presented separately for each quantity. Since a fulfilment of the grid criteria connected to the chosen near wall modelling approach is of great importance in this project, these results are presented first Model Criteria Results using the Present Method The resulting average y + -value at the first node adjacent to the wall for the three models generated according to the present method are given in Table 3.6. Element length y + (area-weighted average) 3 mm 22 6 mm mm 87 Table 3.6: Area-weighted average values of y + for the three present method models. Of the three models it is the one with an edge length of 6 mm that has the most appropriate result of y + at the first node adjacent to the duct wall according to the model criteria for Standard Wall Functions, described in Section The resulting y + value for the model with 3 mm edge length is below the recommended value for the model to be valid, even though the log-law theoretically is employed as long as y + > [4], and the model with the 12 mm edge length is quite close to the upper limit of the recommended interval since the Reynolds number in the academic case is of moderate size (See Table 3.2 and Sec ). It can be mentioned that corresponding grid-density in B-pillar duct models would result

39 38 CHAPTER 3. ACADEMIC CASE in much lower y + -values due to a generally much lower Reynolds number of the ventilation air. Results using the Alternative Method The development of a new model, in terms of mesh structure and approach of describing the boundary layer, has resulted in a mesh with prismatic-cell layers in the near wall region of the duct and a grid resolution that implies a numerical error of ±2%. The resulting average y + -value at the first node adjacent to the wall is < 2 and there are at least 10 nodes inside the viscosity-affected near wall region (Re y < 200). These results fulfils the mesh guidelines for the Enhanced Wall Treatment approach when using any of the three k-ε models and the Transitional Flows option when using the SST k-ω model [4](Sec ) Pressure Distribution The available pressure measurements from the experiment are in terms of the static pressure coefficient, C p (Eq. 3.1). To compare the simulated results with the experimental measurements the difference between C p at different locations along the A-duct, C p, has been computed for three different intervals. These intervals are illustrated in Figure 3.7 as Int 1, Int 2 and the sum of Int 1 and Int 2. The comparison to the experimental results is presented as the difference between the computed C p and the experimental value of C p for the specified intervals. Figure 3.7: Intervals along the A-duct for which the pressure distribution is investigated.

40 3.4. RESULTS FROM THE ACADEMIC CASE STUDY 39 Results using the Present Method In Figure 3.8 the difference between the simulated values of C p and the experimental measurements (computed C p experimental C p ), for the three models generated according to the present method, are given. The numbers on the x- axis in the diagrams of Figure 3.8 corresponds to the intervals of the duct (with corresponding numbers) illustrated in Figure 3.7, where Int 1 and Int 2 are represented by number 1 and 2, respectively. Number 3 on the x-axis of the diagrams represent the sum of Int 1 and Int 2 (this interval is the same as in the grid dependency study). Results from measurements performed at the inner bend of the duct are presented in Figure 3.8(a) and from the outer bend in Figure 3.8(b). In Figure 3.8, the experimental values are represented by y = 0. It is only the point-values that are of interest, the curves connecting the points are only included for clarity reasons The difference form the experimental C p value at the last interval (nr 3) in Figure 3.8(b) is also presented in Table 3.7 as the percentage deviation from the experimental values. Deviation from the experimental value of C p Model (edge length) Deviation [%] 3 mm -3 6 mm mm -9 Table 3.7: Percentage deviation of the computed value of C p from the corresponding experimental value for the three present method models at the interval between s/d=-1 and 14. The difference in C p, C p, can be regarded as the static pressure drop over the specified interval in relation to the dynamic pressure ( 1 2 ρu 0 2 ), (see Eq. 3.1) since the reference pressure (p 0 ) is the same at both end-points of the interval. Then the results in Figure 3.8 and Table 3.7 can be regarded as the deviation from the experimental pressure drop (since the dynamic pressure is the same for all A-duct models) for the specified intervals. Of the three present method models, the model with 3 mm edge length of the surface elements corresponded best to the experimental values of C p at the third interval with a deviation of 3%. Since this model has the highest grid density this result is logical. The results of the other two models are not consistent to the grid density since the model with an edge length of 12 mm deviates less from the experimental values than the model with an edge length of 6 mm. It is worth mentioning that a corresponding grid density as in the 3 mm model of the A-duct is not realizable for a B-pillar duct model in a real project. Common for all three models is that they all underestimated the pressure drop in comparison to the experimental results.

41 40 CHAPTER 3. ACADEMIC CASE (a) Measurements from the inner bend of the duct. (b) Measurements from the outer bend of the duct. Figure 3.8: Difference from experimental values of C p at three different intervals along the A-duct.

42 3.4. RESULTS FROM THE ACADEMIC CASE STUDY 41 Results Using the Alternative Method For the developed grid, described in Section 3.3, the difference between computed results of C p using different turbulence models and the corresponding experimental results are presented in Figure 3.9. The numbers on the x-axis correspond to the intervals in Figure 3.7 in the same way as described for the models created according to the present method. Results from measurements performed at the inner bend of the duct are presented in Figure 3.9(a) and from the outer bend in Figure 3.9(b). In Table 3.8 the percentage deviation from the experimental value of C p for the third interval (number 3 in Fig. 3.9) is presented for each turbulence model with the new grid. Deviation from the experimental value of C p Model Deviation [%] Standard k-ε 20 RNG k-ε 20 Realizable k-ε 20 SST k-ω 10 Table 3.8: Percentage deviation from experimental value of C p between s/d=-1 and 14 for the new grid with different turbulence models. Regarding C p to be the pressure drop over a specified interval in relation to the dynamic pressure, as was done for the present method models, the three k-ε models over-estimated the pressure drop with 20% and the SST k-ω model overestimated the pressure drop with 10% in comparison to the experimental result. From these results and the results in Figure 3.9 one can see that the three k-ε models are very similar to each other and even though the absolute values of the results from the SST k-ω model differ from the k-ε models the same behaviour of the results can be distinguished. The results from the computations with the alternative method models deviates more from the experimental values of C p than the present method models. The behaviour of the alternative method models is however consistent. Of the different turbulence models, the SST k- ω model agrees best to the experimental values of C p. All turbulence models over-estimated the pressure drop in comparison to the experimental results.

43 42 CHAPTER 3. ACADEMIC CASE (a) Measurements at the inner bend. (b) Measurements at the outer bend. Figure 3.9: Difference from experimental results of C p for two intervals and the sum of these intervals along the A-duct.

44 3.4. RESULTS FROM THE ACADEMIC CASE STUDY Velocity Distribution Results Using the Present Method Profiles of the axial velocity, normalized by the mean bulk velocity U 0 (See Tab. 3.2), for the three present method models as well as for the experiment are given in Figure The profiles are taken one diameter upstream (s/d=-1) and downstream (s/d=1) the bend, along the horizontal diameter in Figure 3.3. x = 0 represents the middle of the duct diameter and x = 1 is located at the outer bend of the A-duct (the left end of the horizontal diameter in Figure 3.3). It is noted in Figure 3.10 that the model with 3 mm edge length agrees best to the experimental profiles at both cross sections (at S/D=-1 and s/d=1) and that the 6 mm model corresponds quite well at one diameter upstream the bend, however, less well at one diameter downstream the bend. The 12 mm model agrees poorly at both cross sections, the profile at s/d=-1 is practically a plug-profile and does not change much to s/d=1. From these velocity results it is clear that a higher grid density results in a more accurate prediction of the velocity-field. Once again it can be mentioned that the grid resolution of the model with an edge length of 12 mm best agrees with the grid resolution of the B-pillar duct models today. Another thing that can be considered when studying Figure 3.10(a) is that it has been shown by Sassan Etemad [8], who is a PhD student at Volvo Cars, that the inlet flow-conditions upstream a bend, similar to the A-duct bend, have significant impact on the behaviour of the predicted flow in and after the bend.

45 44 CHAPTER 3. ACADEMIC CASE (a) U/U 0 at s/d=-1 (b) U/U 0 at s/d=1 Figure 3.10: Normalized axial velocity before and after the bend.

46 3.4. RESULTS FROM THE ACADEMIC CASE STUDY 45 Results Using the Alternative Method In the Figures 3.11 to 3.14, velocity profiles at four different cross-sections of the A-duct from simulations with the different turbulence models and from the experiment are presented. Two of the cross-sections are in the duct bend and the positions of these cross-sections are illustrated in Figure 3.3. The measured velocity is normalized with the mean bulk velocity, U 0, given in Table 3.2. For cross-sections at one diameter up- and down-stream the bend, the axial velocity (U) is measured and for the cross-sections in the bend it is the velocity magnitude (VelMag) that is presented. x = 0 represent the middle of the duct diameter and x = 1 represent the outer bend as described for the present method models. No significant differences can be distinguished between the resulting velocity profiles for the different turbulence models. In comparison to the experimental results, all models differ a little bit. At s/d=-1 (Fig. 3.11) there is a discontinuity at the middle of the duct-diameter (x = 0) for the experimental values, which is not captured by the simulations. This discontinuity of the velocity profile might be a result of the bend but could also be a measurement error. For the velocity profiles in the bend (at θ = 67.5 and θ = ) and at one diameter downstream the bend (s/d=1), the simulated results does not capture the flow variations completely but shows similar behaviour to the experimental values. Simulations with all turbulence models tested results in a better agreement to the experimental values than simulations with the present method models.

47 46 CHAPTER 3. ACADEMIC CASE Figure 3.11: Normalized axial velocity, U/U 0, at s/d=-1. Figure 3.12: Normalized velocity magnitude, (Velmag)/U 0, at θ = 67.5.

48 3.4. RESULTS FROM THE ACADEMIC CASE STUDY 47 Figure 3.13: Normalized velocity magnitude, (Velmag)/U 0, at θ = Figure 3.14: Normalized axial velocity, U/U 0, at s/d=1.

49 48 CHAPTER 3. ACADEMIC CASE Turbulent Kinetic Energy Only the model created according to the method developed in this thesis work, have been investigated in terms of turbulent kinetic energy for the different turbulence models. Profiles of turbulent kinetic energy, k, at the same four cross-sections of the A- duct as for the velocity profiles are given in Figure 3.15 to It can be seen in Figure 3.15 that simulations with all the different turbulence models over predicts the turbulent kinetic energy, k, at one diameter upstream the bend (s/d=-1). The long inlet part of the A-duct might be a reason why k becomes over predicted here, since the simulated results agrees better to the experimental ones at cross-sections in- and right after the duct bend. Since the B- pillar duct doesn t have any long straight parts similar to the in- and outlet-parts of the A-duct, the simulated behaviour of the flow is most interesting in- and right after the bend. Another parameter that might contribute to an over-prediction of k is the inlet boundary conditions, where the turbulent quantities are set to quite low values (see Appendix B). This corresponds well to the physics at the inlet but since the turbulence models are developed for a fully turbulent flow [4] it is uncertain how they behave if the flow is laminar or in the transition between laminar and turbulent. These settings are however kept since it is difficult to predict the turbulent inlet profile for the applications of the B-pillar duct, and the inlet boundary conditions used are recommended by the FLUENT support when performing duct flow calculations. For the different turbulence models, simulations with SST k-ω shows a slightly better agreement to the experimental values and simulations with the Standard k-ε model seems to agree the least, but there are no big differences between the models.

50 3.4. RESULTS FROM THE ACADEMIC CASE STUDY 49 Figure 3.15: Turbulent kinetic energy, k, at s/d=-1. Figure 3.16: Turbulent kinetic energy, k, at θ = 67.5.

51 50 CHAPTER 3. ACADEMIC CASE Figure 3.17: Turbulent kinetic energy, k, at θ = Figure 3.18: Turbulent kinetic energy, k, at s/d=1.

52 3.4. RESULTS FROM THE ACADEMIC CASE STUDY Pressure Drop No experimental data for the total pressure drop of the A-duct are available for comparison with the computed results from the different models. The pressure drop over ducts is, however, one of the most interesting parameters for the Climate team, so the computed results for the different models are presented in Table3.9. PM and AM stands for Present Method and Alternative Method, respectively. Total Pressure Drop over the A-Duct Model Pressure drop [Pa] PM model with 3 mm edge 254 PM model with 6 mm edge 259 PM model with 12 mm edge 256 AM model with Standard k-ε 335 AM model with Realizable k-ε 330 AM model with RNG k-ε 330 AM model with SST k-ω 298 Table 3.9: Resulting total pressure drop from simulations with the different A-duct models. The computed value of the pressure drop between the in- and outlet of the A-duct, differs a lot between the models. Again, the three PM models shows inconsistency in the results as the grid is refined since the value of the pressure drop for the 12 mm model is in between the results from the two models with higher grid-density. Also the values of the results are inconsistent to the previous results, since the pressure drop at the third interval in Figure 3.8 was higher for the 3 mm model than for the two other PM models, a result which is now reversed. For the models that resolves the near wall region ( AM models), the one with SST k-ω as turbulence model gives a lower result than the ones with the different types of the k-ε model. Since no experimental results are available for comparison for this quantity the accuracy of the computed results can not be estimated, but from the previous pressure results presented it is likely that the SST k-ω model agrees better to the experiment than the k-ε models. Apart from the fact that the Standard k-ε model gives a higher pressure drop than the other k-ε models the results from the AM models are consistent to the previous pressure results at different intervals along the A-duct.

53 Chapter 4 B-pillar Duct The B-pillar duct provides the back passenger seat with ventilation air and the side rear windows with a defrosting effect. In Figure 4.1(a) the whole ventilation system of a Volvo S80 is illustrated, where the B-pillar ducts are coloured red, and the position of the B-pillar duct in the car is described by Figure 4.1(b). (a) Ventilation system. (b) Position of the B-pillar duct in the compartment. Figure 4.1: The position of the B-pillar ducts, that are coloured red, in the ventilation system and the compartment. As can be seen, the B-pillar duct stretches from the HVAC by the instrument panel, under the front seat and half way up in the B-pillar. The duct is bended at several locations and the shape of the cross-section is highly varying. Depending on the desired effect of the air distribution from the ventilation duct, air with different flow-rate will be transported through it. The interval of different 52

54 4.1. GRID CONSIDERATIONS 53 mass flows is large and this poses some problems when creating the computational models since they should be valid for the whole range. Here, valid means that the model should fulfil the criterias given in Section In this project, two different mass flows have been used, one in the lower part of the interval with 5 l/s and the other in the higher part with 15 l/s. With the mean hydraulic diameter (Eq. 3.2), D h = 50 mm, as the characteristic length of the B-pillar duct, these two flow rates results in a Reynolds number (Eq. 2.27) of about 6000 and Even for the higher flow rate of 15 l/s the Reynolds number is much less than in the experiment used in the Academic Case study (see Tab. 3.2). Since no test data are available for the B-pillar duct, the results from the Academic Case, described in Chapter 3, are used as input when creating models according to the alternative method. No major advantage of the alternative method could be distinguished from the results of the pressure distribution compared to the results from the present method models. It was however still interesting to continue the study of the alternative method models considering the results of the velocity profiles for the present method and the fact that the results of the model with 12 mm edge length were of highest interest for the B-pillar duct study. The study of the influence from the turbulence models didn t prove any model superior for all quantities tested. The SST k-ω model did however agree best to the experimental pressure results of the alternative method models and is therefore chosen to be further investigated with the B-pillar duct models. Because of the big geometrical differences between the B-pillar duct and the A-duct and because the B-pillar duct models should be valid for a large range of mass flows, it was considered interesting to also try a turbulence model which had the Enhanced Wall Treatment option. The Realizable k-ε model was therefore also chosen for the B-pillar duct study. The reason for choosing the Realizable k-ε model instead of any of the other two k-ε models is because this is the model used in the present method for duct calculations and since no significant differences could be distinguished between the models it didn t seem to be any reason for changing. 4.1 Grid Considerations In order to translate the mesh settings from the A-duct model into a model of the B-pillar duct, two dimensionless quantity s have been used; y + as a guideline of how to resolve the boundary layer and the relation between the hydraulic diameter l e D h, (Eq. 3.2), D h, of the ducts and the edge length of the surface element, l e ; as a measure of the grid-density. The same amount of nodes should be included inside a specific y + - value for the mesh in both ducts and the relation between the hydraulic diameter and the edge length of the surface elements should be the same. Unfortunately, it was not possible to make a complete translation from the developed mesh for the A-duct to a mesh for the B-pillar duct if the B-pillar duct

55 54 CHAPTER 4. B-PILLAR DUCT model was to be used in a real project today. Mainly due to the restriction in run time and as a consequence the amount of cells in the model, and compromises were required. The approach of mesh generation in the B-pillar duct is a bit different from how it was performed in the A-duct. Due to a more complex geometry in the B-pillar duct it is not possible to generate prismatic cells near the duct wall in the whole region. In these passages, only tetrahedral cells can be generated with TGrid. In order to still fulfil the requirements in terms of y + in the whole domain, the surface mesh must be greatly refined in these regions. Such refinement of the surface mesh results in a large amount of cells, which becomes restricting since the B-pillar duct models should be realizable in projects today. In Figure 4.2, the resulting distribution of y + at the first node adjacent to the wall, when using the compromised mesh (which will be described in Sec ), is illustrated. The areas with significantly higher values are the areas where a complicated geometry implies the use of tetrahedral cells all the way down to the wall. The end-part of the duct where y + values are high is the duct nozzle and because of many small details in this region, a separate study would be required to resolve this area correctly. The other region with high y + values however, could be resolved with a few layers of prismatic cells if generated with the another software instead of TGrid, for instance ICEM-CFD. Figure 4.2: The regions with only tetrahedral-cells are the ones with significantly higher y + -value. Since the alternative approach in creating the computational grid involves fully resolving the near wall region, the high flow rate is now the restricting flow. This is due to the fact that the friction velocity, u τ, generally increases with increasing velocity (because of increased shear stress at the wall) which implies that y + increases for a position at a constant distance from the wall (See Eq and

56 4.1. GRID CONSIDERATIONS ), and more nodes are required inside the specific distance. The value of y + at the first node adjacent to the wall is not known a priori, which means that when the mesh is generated it is not possible to know the required positions of the nodes in order to fulfil the model criteria. In order to still be able to estimate the value of y + at the first node an iterative estimation of the friction velocity, u τ, is done from the law of the wall (Eq. 2.29), assuming flow equilibrium (See Sec ) Compromised Mesh In order to reduce the number of cells to a realizable amount for a computational model of the B-pillar duct in a real project, a number of compromises are performed. The edge length of the surface elements is larger than required in order to achieve the desired relationship to the hydraulic diameter and the number of prismatic-cell layers is diminished. The criteria of a low-reynolds number model in terms of y + is also compromised, when the high flow rate is used, in the regions where only tetrahedral cells could be generated. In table 4.1 the resulting settings for the compromised grid are presented. In Table 4.2 the translation quantities between the two grids are presented. D h stands for hydraulic diameter and l e is the edge length of the surface elements. It is not only the restriction in amount of cells that implies the compromise of the number of prismatic-cell layers, also the generally more complicated geometry of the B-pillar duct compared to the A-duct makes it difficult to generate as many layers. Property Value First prism height 0.15 mm Growth rate 1.2 Number of layers 12 l e in prism-cell region 3.5 mm l e in tetrahedral-cell region 1.2 mm Total number of cells Table 4.1: Mesh properties for the compromised mesh in the B-pillar duct. Quantity A-duct B-pillar duct l e /D h Estimated number of nodes inside y + = y + = Table 4.2: Quantities for translation between the two ducts.

57 56 CHAPTER 4. B-PILLAR DUCT The grid resolution of the compromised mesh is illustrated at a cross-section of the B-pillar duct in Figure 4.3. Figure 4.3: Grid resolution of compromised mesh at a cross-section of the B-pillar duct. Investigation of the impact of the number of prism layers A higher number of prismatic-cell layers increase the number of cells in the domain since the expansion-rate for the tetrahedral cells is higher than for the prismatic cells. The amount of cells is, as mentioned several times, a major restriction when creating the models so an investigation of the impact of diminishing the number of layers would be interesting. The most important drawback of doing so is that the control over the node distribution in the boundary layer decreases since it is more difficult to predict the distribution of the tetrahedral cells. Also the relationship between the heights of the cells (see Sec ) at the interface between prismatic and tetrahedral cells deteriorates. This investigation is also of interest if it is desired to change the mesh generation program to ICEM-CFD where it might be complicated to generate as many layers, but where on the other hand it is possible to create prism-cell layers near walls in the whole duct region (except in the nozzle). The difference in resulting pressure drop for a case with 9 prismatic-cell layers instead of 12 can be deduced from the results in Table 4.3. The flow rate is 5l/s and the turbulence model used is the SST k-ω model. Number of prism-layers Total number of cells Pressure drop [Pa] Table 4.3: Resulting pressure drop with different numbers of prism layers.

58 4.1. GRID CONSIDERATIONS 57 As can be read in Table 4.3 no mentionable difference can be distinguished between the two cases. The difference in number of cells is however not large enough to significantly decrease the computational time and the control over the node distribution was considered more important so the model with 9 layers will not be further investigated. This still indicates that diminishing the number of prism-cell layers from 12 to 9 does not affect the result of the pressure drop for the B-pillar duct when simulated with a flow rate of 5 l/s Ideal Mesh It has been concluded that a complete translation of the mesh settings developed for the A-duct model to a model of the B-pillar duct could not be performed if the B-pillar duct model was to be used in real projects. This does not mean that it is not possible. In order to investigate the impact of the compromises done in the Compromised Mesh, a grid, which to a higher degree corresponds to the translation parameters, is generated. The number of prismatic-cell layers is still kept to 12, but the surface mesh is refined in order to accomplish the right relationship between the hydraulic diameter and the edge length, and the regions with only tetrahedral cells is refined in order to fulfil the y + criteria also for the high flow rate (15 l/s). The mesh properties and the resulting translation parameters for the ideal mesh are given in Table 4.4 and 4.5, respectively. Property Value First prism height 0.08 mm Growth rate 1.2 Number of layers 12 l e in prism-cell region 2.2 mm l e in tetrahedral-cell region 0.5 mm Total number of cells Table 4.4: Mesh properties for the ideal mesh in the B-pillar duct. Quantity A-duct B-pillar duct l e /D h Estimated number of nodes inside y + = y + = Table 4.5: Quantities for translation between the A- and B-duct models. In Figure 4.4 the mesh resolution for the ideal mesh at a cross section of the B-pillar duct is illustrated.

59 58 CHAPTER 4. B-PILLAR DUCT Figure 4.4: Element resolution of ideal mesh at a cross-section of the B-pillar duct. 4.2 Models Generated According to the Present Method Two models of the B-pillar duct, with differing edge lengths of the surface mesh, have been created according to the present method used when simulating flow through ventilation ducts. The model settings are the same as when corresponding models were created for the A-duct according to the present method, described in Section 3.2. This implies the Wall Function approach of modelling the near wall region and the Realizable k-ε model as chosen turbulence model. Only tetrahedral cells are generated in the computational domain. The edge lengths of the surface mesh for these two models are 3 and 6 mm which is inside the recommended interval (see Tab. 3.3). In Figure 4.5 the grid resolution at a cross section of the B-pillar duct is illustrated for the two models. It should be noted here that the grid resolution of these two models does not correspond to the grid resolution of the A-duct models with the same edge lengths, rather to the two coarser A-duct models (with 6 and 12 mm edge lengths). The resulting number of cells in these two models is presented in Table 4.6. Edge length Total number of cells 3mm mm Table 4.6: Amount of cells for the two grids generated according to the present method.

60 4.2. MODELS GENERATED ACCORDING TO THE PRESENT METHOD59 (a) Grid resolution with 3 mm edge length. (b) Grid resolution with 6 mm edge length. Figure 4.5: Grid resolution at a cross section surface of the B-pillar duct with different edge length of the surface elements.

61 60 CHAPTER 4. B-PILLAR DUCT 4.3 Results from the B-pillar Duct Study All the models of the B-pillar duct are simulated with two different flow rates, 5 and 15 l/s. The models that are created according to the alternative method, described in Section 3.3, are also simulated with two different turbulence models, the Realizable k-ε model and the SST k-ω model, both with the approach of fully resolving the near wall region ( Enhanced Wall Treatment - and Transitional Flows -option). The two models created according to the present method are simulated with the Realizable k-ε model with the Wall Function approach. When investigating the results of the different simulations it is the total pressure drop over the duct that has been the main quantity of interest. The resulting average y + value at the first node adjacent to the duct wall have been considered as a measure of the validity of the models and the residuals have been studied in order to compare the stability and degree of convergence for the different turbulence models Model Criteria In Table 4.7 the resulting average y + value at the first node adjacent to the duct wall for the different B-pillar duct models are presented, for each flow rate. Resulting y + at the first node adjacent to the duct wall Model y + at prism wall-cell y + tet wall-cell 5 l/s PM model, l e =6 mm PM model, l e =3 mm CM with Realizable k-ε IM with Realizable k-ε CM with SST k-ω IM with SST k-ω l/s PM model, l e =6 mm PM model, l e =3 mm CM with Realizable k-ε IM with Realizable k-ε CM with SST k-ω IM with SST k-ω Table 4.7: Resulting average y + for the different B-pillar models when simulated with flow-rates of 5 and 15 l/s. PM stands for present method, CM stands for Compromised Mesh and IM stands for Ideal Mesh in Table 4.7. Of the two columns with y + values, the one

62 4.3. RESULTS FROM THE B-PILLAR DUCT STUDY 61 called y + at prism wall-cell represents the values in the regions where prismatic cells could be generated close to the wall and the results in the other column represents the regions where only tetrahedral cells were generated. For the PM models at the lower flow rate (5 l/s), the resulting y + value is far below the recommended values when using the Wall Function approach (see Sec ) indicating that these models are not valid. The PM model with an edge length of 6 mm is close to the theoretical limit (at y + = ) above which the law-of-thewall is applied by the turbulence model [4] but the other PM model with 3 mm edge length is inside the laminar region [4](Sec ). For the Compromised and Ideal Mesh, practically the same results are achieved with the different turbulence models. For the low flow rate of 5 l/s, the models with both the Compromised and Ideal Mesh fulfils the y + criteria at all regions. However, for the high flow rate of 15 l/s only the models with the Ideal Mesh fulfils the criteria in the whole duct domain when fully resolving the near wall region. Both the PM models are above the theoretical limit (though still below the recommended value) when applying the Wall Function approach, for the higher flow rate Pressure Drop The total pressure drop from the inlet of the B-pillar duct to the outlet surface, computed with the flow rate of 5 l/s for the different B-pillar duct models are presented in Figure 4.6. In the figure, 3 mm and 6 mm stands for the PM models with the corresponding edge lengths, CM and IM stands for Compromised and Ideal Mesh and Rea and SST stands for Realizable k-ε and SST k-ω, respectively. Figure 4.6: Total pressure drop for the B-pillar duct models when simulated with 5 l/s.

63 62 CHAPTER 4. B-PILLAR DUCT When studying Figure 4.6 it can be seen that the difference in pressure drop is greater between the two PM models than between the models created according to the alternative method ( AM models). The pressure drop for the 6 mm model is about 9% less than for the 3 mm model compared to 6% difference between the IM Rea and the CM SST models. Since no test data are available for the B-pillar duct it is difficult to draw conclusions from the computed results. It seems however likely that the results from the 3 mm model and the AM models are more accurate than the results from the 6 mm model. If this is the case, it seems more important to have a high density grid than to fulfil the model criterias for the PM models (even though none of the PM models fulfils the criterias) when simulated with the low flow rate. Another result which can be seen is that the highest pressure drop was computed with the AM model when using SST k-ω as turbulence model. This is (unfortunately) inconsistent with the results of the Academic Case study, where simulations with the SST k-ω model resulted in a lower pressure drop than when the Realizable k-ε model was used. The difference between the PM and AM models is however consistent with the results from the Academic Case since the resulting pressure drop is lower for the PM models. The resulting pressure drop for the different mesh-types (CM and IM) was consistently lower for the Ideal Mesh, independent of turbulence model. The outlet surface, which is used when computing the total pressure drop, is situated at a certain distance from the duct nozzle where the static pressure is assumed to be zero. It was considered interesting to also study how the pressure drop varies at different parts of the B-pillar duct. In Figure 4.7 the pressure drop between the inlet and two different cross-section surfaces and the total pressure drop are presented for the AM models. The first section stretches from the inlet until the first region where only tetrahedral cells could be generated. The second section also starts at the inlet but stretches to a cross-section surface right before the nozzle and the third section is the same as in Figure 4.6 (from in- to outlet surface). An interesting discovery when studying Figure 4.7 is that the difference between the Compromised and Ideal Mesh is less at the two sections inside the duct for both turbulence models compared to the total pressure drop. This indicates that the grid dependency is less in the duct than in the nozzle and outlet box. It is common for both turbulence models that the pressure drop is less for the Compromised Mesh than for the Ideal Mesh in the first section and that the difference is very small at the second section and reversed when the nozzle and outlet box are included in the third section.

64 4.3. RESULTS FROM THE B-PILLAR DUCT STUDY 63 Figure 4.7: Pressure drop at different sections of the B-pillar duct for the alternative method models. The resulting total pressure drop when simulating the B-pillar duct models with the higher flow rate of 15 l/s are presented in Figure 4.8 Figure 4.8: Total pressure drop for the B-pillar duct models when simulated with 15 l/s.

65 64 CHAPTER 4. B-PILLAR DUCT The resulting pressure drop from the simulations with a higher flow rate (15 l/s) are quite different from the previous results with 5 l/s. One important change is that this time the PM models show less difference than the AM models. This could indicate that the grid resolution becomes less important than for the low flow rate. The pressure drop result for the PM models is however still lower than for the AM models. Another change in the results compared to simulations with the lower flow rate is that there is now a little less difference between the mesh types (CM and IM) when the Realizable k-ε model is used than with the SST k-ω model. The same study of the pressure drop at different sections for the AM models was performed also with 15 l/s, and the results are given in Figure 4.9. Figure 4.9: Pressure drop at different sections of the B-pillar duct for the alternative method models, simulated with 15 l/s. These results were even more interesting than the results with the lower flow rate. It should be remembered that the Compromised Mesh did not fulfil the y + criteria in the regions with only tetrahedral cells for the high flow rate. The fact that no big differences are observed between the mesh types when using the Realizable k-ε model indicates that the Enhanced Wall Treatment function manages to accurately model the regions where the y + criteria for a low-reynolds number model are not fulfilled. The SST k-ω model on the other hand does not seem to be able to do that. The results for the Compromised Mesh differs a lot from the results using the Ideal Mesh with the SST k-ω model. A large change of the results between the second and third section is observed also for the higher flow rate which indicates that the quality of the mesh in the nozzle and the outlet box is of great importance for the results, and not high enough in the Compromised

66 4.3. RESULTS FROM THE B-PILLAR DUCT STUDY 65 Mesh Solution Stability and Convergence In Figure 4.10 the solution residuals for simulations with SST k-ω and Realizable k-ε models, at in inflow rate of 5 l/s, are presented. (a) SST k-ω, 5 l/s. (b) Realizable k-ε, 5 l/s. Figure 4.10: Solution residuals from simulations with two different turbulence models at a flow rate of 5 l/s. As can be seen, the solution residuals for the Realizable k-ε model goes down more than 6-7 orders, except for the continuity residual (which is scaled differently according to FLUENT support). The solution residuals for the simulation with the SST k-ω model on the other hand, does not reach the same level of convergence

67 66 CHAPTER 4. B-PILLAR DUCT at all. The residuals go down only 3-4 orders and they fluctuates more than the residuals for the Realizable k-ε model.

68 Chapter 5 Conclusions and Recommendations It would be of great importance for the CFD-engineers at the Climate team if the accuracy of the computed results using the present method (PM) could be estimated. In the Academic Case it was shown that the PM model with an edge length of 3 mm of the surface mesh agreed best to the experimentally determined pressure results of all models tested. Simulations with this model also resulted in a velocity prediction which agreed almost just as well to the experimental results as the alternative method (AM) models. These results indicates that the 3 mm present method model is highly accurate. The conditions in the Academic Case can however not be achieved for any ventilation duct. A similar grid-resolution could not be obtained if the model criterias of a high-reynolds number model should be fulfilled due to a much lower Reynolds number and a more narrow duct geometry. As already described, the grid resolution which permits the model criteria to be fulfilled in a B-pillar duct model, if simulated with the higher flow rate of 15 l/s, corresponds to the grid resolution of the A-duct model with an edge length of 12 mm. If the B-pillar duct model is simulated with a lower flow rate, such as 5 l/s, an even coarser grid is required for the model to be valid. The accuracy of the A-duct model with an edge length of 12 mm is however difficult to estimate since the results of the pressure distribution were inconsistent with the grid refinement, indicating that the model is highly grid-dependent. The result deviated however less from the experimental values than the results from the models created according to the alternative method that were simulated with the three k-ε models. From the velocity results of the 12 mm present method model, it is however clear that a higher grid resolution is required in order to accurately predict the velocity distribution. The accuracy of the computed results when using models created according to the alternative method is also difficult to estimate. The need of compromises when creating the grid for the B-pillar duct models that should correspond to 67

69 68 CHAPTER 5. CONCLUSIONS AND RECOMMENDATIONS the developed grid in the Academic Case and the geometrical differences between the two ducts implies that the numerical error of the Compromised Mesh in the B-pillar duct is different from the estimated error in the developed grid. However, when using the Realizable k-ε model with the Enhanced Wall Treatment option there seemed to be little difference between the results of the Compromised and Ideal Mesh, when looking at the pressure distribution inside the B-pillar duct, for both the high and low flow rate. This indicates that the grid dependency is quite low for the mesh in the duct-part of the B-pillar duct. The large effect of the results for the Compromised Mesh when the nozzle and outlet box were included in the total pressure drop indicates that this part of the B-pillar duct needs more work. If only the pressure drop over the ventilation ducts is of interest to predict, no major advantages of the alternative method have been discovered in this study. For the low flow rate in the B-pillar duct case, the biggest difference in the computed result of the total pressure drop was however between the two models created according to the present method. But for the high flow rate, the difference between these models was very small and the results from the alternative method models differed more. The overall difference between the resulting pressure drop from the different models was quite small for the high flow rate indicating that the method used was of less importance at higher flow rates. Something that could be an advantage for the alternative method is the fact that models created according to this method seems to somewhat over estimate the pressure drop in difference to the models created according to the present method that rather seems to under estimate the pressure drop. Since the computed pressure drop over the ventilation ducts is used as input to the development of the HVAC a little too high value should be preferred instead of a too low. If other quantities, such as velocity, are of interest or if it is desired to use models which fulfils the model criteria and doesn t have a highly grid-dependent mesh, a method similar to the alternative method must be applied. The biggest drawback of the alternative method is the increase of computational time which is required due to a higher number of cells. As computer resources are likely to increase with time, the amount of cells in a model will become less restricting and models of the B-pillar duct which are complete low-reynolds number models will be possible to generate. For the models created according to the present method on the other hand, the limit seems to have already been reached. If the near wall region is to be modelled by a Wall Function approach, the possibilities of grid refinement are highly restricted if the model should fulfil any model criteria. In the Academic Case study the use of SST k-ω gave the best agreement to the experimental pressure results of the alternative method models, which was the

70 5.1. FUTURE WORK 69 only quantity where any differences could be distinguished between the different turbulence models. For the B-pillar duct, the Realizable k-ε model proved however superior in both stability and degree of convergence of the solution residuals and also in stability of the results when simulating air flow with the higher flow rate. These results indicated that the Enhanced Wall Treatment function accurately managed to model the regions in the B-pillar duct were the y + criteria of a low-reynolds number model were not fulfilled. A sum up of the most important conclusions from this thesis work are listed below. - Simulations with models created according to the alternative method results in a higher pressure drop than simulations with models created according to the present method and it is likely that the true value is in between these results. - If the velocity distribution in the ventilation ducts should be accurately predicted, the alternative method should be used. If a method like the alternative method is to be used, the following settings can be recommended from the results of this study. - Use Realizable k-ε as turbulence model and Enhanced Wall Treatment as near wall modelling approach. - Use a mesh generated as the Compromised Mesh (Sec ) with prismatic cells close to the duct wall if possible. A more detailed description of the mesh generation procedure is presented in Appendix A. 5.1 Future Work In order to be able to validate the computed results for the B-pillar duct models and to some extent estimate the accuracy, test data are required. A realization of B-pillar duct tests would therefore be highly interesting. A study of the possibilities of the mesh resolution in the nozzle and the outlet-box would be preferable since these parts of the model seemed to highly affect the results of the Compromised Mesh. It would also be interesting to further investigate the possibilities with another mesh generation software, for instance ICEM-CFD, which proved to be able to generate layers of prismatic cells in more parts of the B-pillar duct than what was possible with TGrid. If prismatic cells could be generated in the near wall region of the whole duct, the required amount of cells in the model would decrease and it

71 70 CHAPTER 5. CONCLUSIONS AND RECOMMENDATIONS would be more likely that the model criterias could be fulfilled also for the higher flow rate.

72 Bibliography [1] Kundu P.K. (1990), Fluid Mechanics, 1st edition, San Diego; Academic Press, ISBN [2] Ferziger J.H., Peric M.(2002), Computational Methods for Fluid Dynamics, 3rd edition, Berlin; Springer-Verlag Berlin Heidelberg New York, ISBN [3] Casey M., Wintergerste T. (2000), Best Practice Guidelines, 1st version, Sulzer Innotec; European Research Community On Flow, Turbulence And Combustion (ERCOFTAC) [4] Fluent(2001), FLUENT 6 User s Guide, Cavendish Court; Fluent Inc [5] Pope S.B. (2000), Turbulent Flows, 1st edition, Cambridge; Cambridge University Press, ISBN [6] Anwer M. Swirling and non-swirling flows in curved pipe, ERCOFTAC Classic database, Case04, ( ) URL: [7] Lunds Institute of Technology, Course material MMV016 ( ), URL: ht/courses/mmv/mmv016/stromningslara/lecture %20K8.pdf [8] Etemad S., Sundén B.(2004) Prediciton of developing turbulent flow in a rectangular-sctioned curved duct, Gothenburg, Volvo Car Corporation, Lund, Lund Institute of Technology 71

73 72

74 Appendix 73

75

76 Appendix A Suggestion of Computational Method The alternative way of generating computational grids in ventilation duct models, introduced in this thesis work, is based on the approach where the near wall region is fully resolved. This implies a very fine grid in the near wall region and the wall unit y + is commonly used as a measure if the mesh is fine enough. y + is computed from y + = u τ y ν, (A.1) where y is the normal distance from the wall to the first node, u τ is the friction velocity and ν is the kinematic viscosity of the fluid. y + is not known in advance but can be estimated with the help of a matlab program in which the friction velocity, u τ, is iteratively estimated from the loglaw (Eq. 2.28) assuming the flow to be in local equilibrium (See Sec ). It is a good idea to make such an estimation since it saves a lot of work if the estimation is close enough to the computed value of y +. In order to use this program, for estimating the friction velocity, the radius of the duct and the flow velocity parallel to the wall at a radial distance from the duct wall must be known. Since most ducts have inhomogeneous cross-section surfaces, a mean radius for the duct and a corresponding mean velocity of the fluid can be used. When using the above mentioned matlab program it can be considered that a too low value of the friction velocity would allow a too high value of the distance from the wall to the first node and imply a too large value of y +. For this reason it might be good to somewhat over estimate the friction velocity. The approach to generate the volume mesh is to create layers of prism cells close to the duct wall and to generate tetrahedral cells in the middle of the duct. If it is 75

77 76 APPENDIX A. SUGGESTION OF COMPUTATIONAL METHOD possible to generate prism cell layers close to the wall in the whole duct domain, an estimation of u τ and y + can be done after the surface mesh is generated but if there are regions in the duct where only tetrahedral cells can be generated, the y + criteria must be considered before generating the surface mesh. If the grid in the ventilation ducts is to be used for different mass flows, it should be dimensioned according to the highest mass flow since a higher flow velocity will increase the value of y + at a constant distance from the wall. This can be applied for the prism cells, but when dimensioning the surface mesh in regions which are too complex to be able to have prism cells, a low mass flow ( 5l/s) should be used. This is due to the restriction in the amount of cells in the domain. It is not possible to fulfil the y + criteria for a high flow rate ( 15l/s) in these regions but it should be possible for a low. When estimating the distance from the wall to the first node for a tetrahedral cell the following assumptions are made. The tetrahedral cell is approximated as an equilateral triangle and the node is assumed to be placed at 1 3 of the triangle height. From these assumptions the distance from the wall to the first node can be estimated as an interval from ( a 3 sin π ) ( 3 to 2a 3 sin π ) 3, if a is the edge length of the tetrahedral cell. It is however safer to use the smallest distance. In the following sections, each step in creating the computational model is described, distributed among the used software. After each section, a table of the corresponding settings for the compromised mesh in the case with the B-pillar duct will be presented. (See Sec ) The resulting y + value when a grid with these settings are run with two different flow rates (5 and 15 l/s) are presented in Section When something is written inside [ ] it means that it is an available option in the described program. ANSA If the geometry of the duct is complicated and there is a possibility that TGRID will fail to generate prism cells in some regions implying the use of tetrahedral cells, fan-surfaces should be created in order to define these regions. To have several fan-surfaces along the duct is also good in order to estimate the mean crosssection area of the duct and for investigating different variables in post processing. When creating the surface mesh in regions of the duct where prism cells are to be generated, the element edge length should be estimated from a relationship to the hydraulic diameter of the duct in order to ensure a sufficient resolution of the tetrahedral cells. The hydraulic diameter, D h, at a specific cross section is

78 77 computed from D h = 4A P (A.2) where A is the area of the cross-section surface and P is the circumference of the cross-section surface. If the duct has an inhomogeneous cross-section, compute an average hydraulic diameter. The optimal relation-ship is l e D h = 0.06, (A.3) where l e is the edge length of a surface element. The surface mesh is generated using [FREE] and [TRIA]. It is recommended to use [RECONS] after using [FREE]. This command reconstructs the mesh and improves the quality of the surface mesh, which will decrease the number of volume cells with bad quality. Since the surface mesh must be refined in regions where only tetrahedral cells are to be generated in the volume mesh, it can be good to use the command [SPACING] on the surface mesh next to these regions in order to create a smooth transition between the regions. When the volume mesh is generated in TGRID, pyramids will be created on the fan-surface between a region with prism cells and a region of tetrahedral cells. There is a risk that these pyramid cells will have a very bad quality and also be difficult to manually improve. In these cases it is favourable to create interface surfaces on these fan-surfaces. This implies a need to create surfaces with quadrilateral elements in ANSA and the number of the layers of quad-elements must match the number of prism layers generated in TGRID. It is difficult to know how many prism layers it will be possible to generate in TGRID the first time the grid is created, so for this reason it might be time saving to investigate this first and then return to ANSA to create the surfaces with quadrilateral elements if needed. If this is the case, the surfaces with quadrilateral elements should be generated where the prism cells will be connected to the tetrahedral cells. A suggestion of how to create these surfaces is presented below; - Pick one of the fan-surfaces that defines the region with tetrahedral cells and delete this surface and then recreate it with the command [NEW] and select [AUTO] in order to make the new surface completely flat.

79 78 APPENDIX A. SUGGESTION OF COMPUTATIONAL METHOD - Use the command [SHRINK] to define the region where the quadrilateral elements are to be generated. When using [SHRINK], make sure that no surfaces in contact to the surface to be shrunk are in visible mode. Shrink the surface the same distance (in mm) as the estimated total height of the prism layers (from TGRID). Have [Curve s] in visible mode when using shrink. If the obtained surface does not match the curves, use [FINE] to smooth the surface. Delete the curves. - Use [PROJECT] to link the two surfaces together and delete the single surface. - Set new PID:s of the new surfaces. - [CUT] the corners of the surface where the quad-elements are to be generated so that this generation is possible. - Use [NUMBER] (in Mesh mode) in order to create the same amount of nodes on the surface edges defining the quad-element surface, so that the same amount of quad-elements will be generated in every layer. - Use [SPACING] on the corner edges in order to place the nodes so that the quad-elements will increase in height corresponding to the expansion rate of the prism cells. Use the [Geometric] option with a [factor] of 1.2. Remember that the elements should be lowest close to the wall. In Figure A.1 the effect of the [SPACING] command is illustrated. Figure A.1: Illustration of the [SPACING] command at the corner edges. - Use [MAP] and [QUAD] to generate the quadrilateral elements. In order to avoid too bad quality of the tetrahedral cells connected to the interface surface try to keep the aspect ratio of the quadrilateral elements closest to the duct wall below 10. This is adjusted with the element length on the outer edge of the surface with quadrilateral elements.

80 79 Outlet Box When simulating flow through the ventilation ducts, an outlet box is used as an approximation of the car compartment. If this box is too large or too well resolved a huge amount of cells will be concentrated here. In this thesis work another type of outlet box is used. Instead of only one box, two boxes are created where one is inside the other. The outer box is large and has a very coarse grid while the inner box is a lot smaller and has a less coarse grid. The inner box is situated at the nozzle in order to resolve the flow variables at the outlet from the duct. Approximate measures of the used box are given in Table A.1. Dimensions of outlet box for the B-pillar duct Outer Box Width (side wise perpendicular to the outlet) 890 mm Height (height wise perpendicular to the outlet) 650 mm Depth (in the outlet flow direction) 720 mm Inner Box Width (side-wise perpendicular to the outlet) 560 mm Height (height-wise perpendicular to the outlet) 410 mm Depth (in the outlet flow direction) 335 mm Table A.1: Dimensions of the outlet box used for the B-pillar duct. In Figure A.2 the outlet box described above is illustrated. Figure A.2: The outlet box, consisting of an inner and outer part. The element lengths of the surface mesh at different parts of the outlet box are listed below. - Inner box - 20 mm. - Edges close to the nozzle - 15 mm, use [SPACING].

81 80 APPENDIX A. SUGGESTION OF COMPUTATIONAL METHOD - Edges on the outer box close to the nozzle mm. - Outer part of the outer box - 70 mm. - Between outer part and surfaces close to the nozzle mm. ANSA Settings for the B-pillar duct The settings in ANSA for the compromised grid in the B-pillar duct are given in Table A.2. ANSA Settings for the surface mesh in the B-pillar duct Element edge length in prism regions 3.5 mm Element edge length in tetrahedral regions 1.2 mm Element length on the edge of one of the quad-surfaces 1.4 mm Distance of shrunk surface 6 mm Number of nodes on corner edges 11 D h /l e 0.07 Table A.2: Settings when creating the surface mesh in the B-pillar duct. TGRID When generating the volume mesh, begin with the prism cells. Prism Cells Use the above mentioned matlab program in order to estimate the required normal distance from the wall to the first node, in order to fulfil the y + criteria of the model. When using any of the k-ε models with the Enhanced Wall Treatment option the first node adjacent to the wall should be placed at a distance from the wall corresponding to y + 1 and at least y + < 4 5 (See Sec ). Use the highest flow rate that will be modelled in the duct. The height of the first prism layer can be twice the distance to the first node from the wall, since the node is situated at the cell center. Before deciding the growth rate and the number of prism layers some things should be considered. For instance that at least 10 nodes should be inside Re y = 200 and the aspect ratio of the prism cells that are connected to the tetrahedral cells should not be too large, in order to keep a homogeneous distance between the nodes. Since the turbulent Reynolds number is difficult to estimate in advance, one could use y + as a measure also here. According to [5] the viscous region stretches to about y + = 50 and Re y < 200 is a measure for the viscosity affected region applied when using the Enhanced Wall Treatment option [4]. The aspect ratio of the prism cells can be adjusted with

82 81 both the growth rate and the number of cells. Depending on the geometry of the duct of interest, it might not be possible to generate as many layers as desired. In this case, generate as many as possible. The region of prism cells should not be to large either since the ducts generally are quite narrow and the large aspect ratio of the prism cells only is acceptable in the near wall region where the gradients are most important normal to the wall [3]. Remember to set the prism-cap surface as interior type in [Boundary][Zones]. Interface Surface If TGRID managed to generate prism cells in the whole domain this section can be ignored. The first time a mesh is generated one could try to create the tetrahedral cells directly but if the pyramid cells, which will be generated at the fan-surface connected to both a prism- and a tetrahedral cell region, are of very bad quality it can be worth to return to ANSA and create surfaces with quadrilateral elements. (Described above) If this has been done, continue to read this section. The following procedure describes how to create the interface surfaces - Select the [Boundary][Zones] menu. Make a copy of the surfaces with quadrilateral elements and rename the copied surface to an appropriate name. - Open the \boundary directory and choose create-tri-surface. Select the copied surfaces and press y (yes). - Select the [Boundary][Nodes] menu. Deselect the only free nodes option. Select the surfaces to be connected (the triangulated copied surface and the corresponding original surface with the quad-elements), one surface at the Compare.. and the other at the With.. side. Merge only one pair of surfaces at the time. Remember to change the tolerance to about in order to avoid that some nodes are too far apart from each other to be merged. [Merge] the surfaces. Remember to set the created interface surfaces as interface type in [Boundary][Zones]. In Figure A.3, a surface in the B-pillar duct with quadrilateral elements is presented. Tetrahedral Cells Define domains for the tetrahedral cells. Create the domains so that the cell size should be about the same in the whole domain. The outlet box for instance,

83 82 APPENDIX A. SUGGESTION OF COMPUTATIONAL METHOD (a) The shrunk, projected and cut surface. (b) The quad-elements. Figure A.3: One of the surfaces in the B-pillar duct where quadrilateral elements are created. should probably be defined as a separate domain. Generate the tetrahedral cells according to the current procedure. TGRID Settings for the B-pillar duct The used TGRID settings for the B-pillar duct are given in Table A.3. TGRID Settings for the volume mesh in the B-pillar duct Prism Settings Method Geometric First prism height 0.15 mm Rate 1.2 Number of layers 12 Tetrahedral Settings [Init/Mesh] Add Interior Nodes selected Perturb Nodes selected Node Perturbation 0.1% Max Cell Size in outer outlet box Max Cell Size in inner outlet box 2000 Max Cell Size inside the duct 200 Max Cell Skew 0.95 Table A.3: Settings when creating the volume mesh in the B-pillar duct.