The study of air distribution in tunnels and large industrial buildings

Transcription

1 Ventilation, Airflow and Contaminant Transport in Buildings The study of air distribution in tunnels and large industrial buildings 13th January Semester Project Indoor Environmental & Energy Engineering Department of Civil Engineering Aalborg University Group F2P31 Blanka Cabovská Kirstine Meyer Frandsen Omar Benmassaoud Rune Baldur Kessler Andersen

2 1. Semester of Indoor Environmental and Energy Engineering Department of Civil Engineering Thomas Manns Vej Aalborg SV Title: The study of air distribution in tunnels and large industrial buildings Project type: Semester project Project period: September January 2017 Project group: F2P31 Authors: Blanka Cabovská Kirstine Meyer Frandsen Omar Benmassaoud Rune Baldur Kessler Andersen Supervisors: Li Liu Peter V. Nielsen Page nr:63 Appendix:13 Completed: Synopsis: The report works with a continuation of the COBEE paper [Peng et al., 2015], where the CFD predictions will be validated with measurements using experimental methods instead of offering no solution to the case. The first part of the report clarifies theory and methodology used in the following parts, as well as limitations. In the second part of the report the initial 2D CFD predictions are done, which are then compared to the measurements from the laboratory. In these comparisons it was found that the RNG k- was the most accurate turbulence model in predicting the airflow. The RNG k- along with the Realizable k- were then used for 3D predictions and compared to the measurements. Again the RNG k- proved closest in approaching the measurements. In the third part the practical case of air distribution in the room is developed, where heat sources are considered in the simulations. Several simulations with different flow rates were conducted. Velocity profiles and temperature distribution in the room were investigated. Finally the position of the outlet was changed to see the effect on the flow pattern in the room.

3

4 Abstract The aim of this project is to model the air flow in a room and to study the influence of air fluctuations on the ventilation and the quality of the air in the housing. The airconditioning and air-flow processes in buildings form the basis for determining energy consumption, indoor climate and work environment. This study concerns ventilation in large rooms to determine all the desired characteristics in the occupied zone where comfort must be respected. For this, specific calculation models are developed, using CFD software. There are three elements to the project. The first part concerns the theory behind computational fluid dynamics. The second part serves as a continuation of the COBEE case. A model experiment is conducted on a deep room in the laboratory. The measurements are supplied with CFD predictions of the flow for both 2D and 3D models. A comparison will be made between the two methods in order to validate the results. The third part is the practical approach where a case is developed containing heat sources. Variables as velocity decay in the wall jet and Reynolds number effect will be considered. The set-up is also the geometry used in a CFD competition between a number of universities around the world. The aim of this project is to create a benchmark for the study and contribute to the evolution of this engineering field. iii

5

6 Preface This report has been written by group F2P31 from the 1. semester of the Master s Degree in Indoor Environmental and Energy Engineering at Aalborg University. The overall theme of the project is Ventilation, airflow and contaminant transport in buildings with focus on The study of air distribution in tunnels and large industrial buildings. The project period has taken place from September 1st 2016 until January 13th We would like to thank our supervisors Li Liu and Peter V. Nielsen for their guidance throughout the course of the project. Reading guide In this report the references are listed through the Harvard-method. The source is noted in square parentheses, wherein the author s surname and the publication date is listed, e.g. [Hyldgaard et al., 1997]. When the author of a publication is a company and not a person, said company will be listed. The reference is placed before the full stop when it refers to the sentence. If the reference is placed after the full stop, it refers to the paragraph. The bibliography is found in the back of the report along with the sources listed in alphabetical order. In the bibliography the remainder of information about the source is listed, such as whether the source is a book, pdf-file, webpage, etc. The purpose of the bibliography is to examine the critical approach to the sources that has been exercised throughout the course of the project. References to figures and tables occur are made through numerical order in occurrence with the chapter number and placement within the chapter. For example, the first illustration in chapter one is named Figure 1.1, the next illustration Figure 1.2, etc. All figures and tables are provided with explanatory captions; they are placed below the figures and above the tables. This report has been developed and compiled by: Blanka Cabovská Kirstine Meyer Frandsen Omar Benmassaoud Rune Baldur Kessler Andersen v

7

8 Index Abstract iii Chapter 1 Introduction 1 I Methodology 2 Chapter 2 Methodology Theoretical Method Experimental Method Computational Method Chapter 3 Numerical methods Governing equations Methodology Spatial and temporal discretization of equations Chapter 4 Turbulence models 9 Chapter 5 Boundary Conditions 13 Chapter 6 Mesh 16 Chapter 7 Convergence 18 II COBEE Case 20 Chapter 8 Introduction COBEE Case D CFD model Meshing D CFD Model Meshing Chapter 9 CFD Simulations D Case Maximum Velocity in the Occupied Zone D Case Maximum Velocity in the Occupied Zone Chapter 10 Model experiment Methodology Model dimensions vii

9 Group F2P31 Index Equipment Procedure Results Small-Scale to Full-Scale Chapter 11 Comparison of Simulations and the Model Experiment Conclusion III Practical case 47 Chapter 12 Introduction Model Dimensions and Purpose Chapter 13 CFD Simulations Meshing Mesh Independence Test Mesh Quality CFD Simulation Settings Boundary Conditions Variables Simulations Chapter 14 Results Velocity Profiles Temperature distribution Different Outlet Position Simulation without Heat Sources Conclusion IV Conclusion 61 Chapter 15 Conclusion 62 Bibliography 63 Appendix A Inlet velocity calculations 64 Appendix B ANSYS Fluent Input 68 Appendix C Near-Wall Treatment of Simulations 69 Appendix D Other Measurements 70 Appendix E Comparison between Simulations and Measurements 74 Appendix F Mesh for Part III 76 viii

10 1 Introduction The increasing focus on indoor climate in buildings has throughout the years lead to the study of such conditions and through this the development of software and tools to enable it. One of these conditions would be the ventilation in a room, which is required to comply with the comfort criteria set by the Building Regulations. To allow this, the study of fluid dynamics is applied to examine the air distribution within a room. This enables the prediction of the air flow, such as the penetration length and maximum velocities, particularly inside the occupied zone for residential and industrial buildings alike. For the application of fluid dynamics, there are different methodologies available; theoretical, experimental and computational. There are advantages and disadvantages to each. This project aims to apply the knowledge of each of the methods and verify the validity of the different methods when results are compared. In particular the developments within Computational Fluid Dynamics wish to be studied to highlight and errors there may be in the predictions. A comparison is to be made on the effect of Reynolds numbers for the different types of flow; laminar, transitional and turbulent flow. For the following project, the air distribution is examined in a deep room, so as the length in sufficiently long as to not influence the the dimensionless penetration length. Furthemormore the air distribution and veloities are examined for both 2D and 3D cases to examine the effect on the indoor climate in the occupied zones. 1

11 Part I Methodology 2

12 2 Methodology Several methods exist that are able to develop solutions to the analysis of a flow in a given situation. This can be carried out through theoretical, computational and experimental methods. It is therefore dependent upon the individual project and the reason behind said project to determine which solution is optimal. By utilizing several methods, it is furthermore possible to compare the results Theoretical Method The theoretical method, also known as the analytical method, is dependent upon the governing equations. It is a closed problem, in which there are three partial differential equations and three unknowns which will be detailed later. Even for a simple problem with laminar flow and simple geometry, it is not easy to find an analytical solution by working on the three equations since this requires very complex calculations. As this is the case, it can quickly be eliminated as the optimal method Experimental Method The experimental method is the physical and actual approach to a solution. This involves developing the model of the actual case that abides by the similarity principle. So long as the principles of similarity is complied, such as the, the analysis can be transferred to full-scale model through the use of dimensionless numbers. The results are therefore very precise. However, the experimental method is very time-consuming and this serves as the biggest disadvantage. Furthermore it is necessary that the experiment be carried out under very exact circumstances, as there are many risks for errors and uncertainties throughout the procedure of the experiment. As this method is time-costly and difficult to set-up in the case of more complicated geometries, it is not carried out under normal everyday circumstances. However, for the purpose of this project it serves as a validation of the computational method and is therefore relevant for the research Computational Method In many situations the computational method is optimal as it provides many advantages compared to the previously mentioned methods. This especially includes time and money; the computational method is able to give results within a relatively short amount of time, which in turn becomes a cheaper solution for the company employing it. Furthermore it can go beyond relatively simple geometry. While the method may not provide results that are 100% correct as the experimental method would, its results are still relatively accurate and therefore representative for the case. 3

13 Group F2P31 2. Methodology The computational method is carried out using Computational Fluid Dynamics. This utilizes the finite volume method, which calculates approximate solutions to boundary value problems for partial differential equations. It does this using a numerical technique, which acts faster than the previous methods. By using both the experimental and computational method it is possible to make a comparison of the results and therefore evaluate the validity of the computational method. 4

14 3 Numerical methods This section is based on Fluid Dynamics [Michael Brorson, 2008]. In order to apply Computational Fluid Dynamics to a case, it is necessary to understand the equations that describe the motion of a fluid particle. This provides a basic understanding of the different simulation models that are applied throughout the project. Firstly the conditions which enable the validity of the governing equations must be defined; namely the characteristics of the fluid and its environment. There are two descriptions of fluid motion which can be considered: Lagrange description: consists of describing the trajectory of a fluid particle over time. Eulerian description: consists of describing a speed field at a given instant. The fluid is determined to be continuous when all the properties, such as pressure, temperature and density, are defined for every point of space and change progressively from one point to another. As a result the discrete nature of a fluid is unknown. A fluid is said to be compressible when a variation in the density of the fluid has a significant influence on the governing equations; otherwise the fluid is said to be incompressible. A flow is stationary when the velocity and the other variables are no longer dependent upon time. In other words, all the properties of the fluid are constant throughout time. If this is not applicable, the flow is said to be unsteady. The fluid is said to be viscous when the friction created by the fluid influences the solution. In the case where friction can be neglected, the fluid is considered to be non-viscous. The flow of a fluid may be turbulent when it is dominated by eddies and an apparent random appearance. When there is no turbulence, the flow is laminar. Reynolds number makes it possible to determine whether the fluid is laminar or turbulent Governing equations Fluid mechanics seeks to determine precisely the movement of fluid particles within a flow, considering the different forces involved. The objective is therefore to set up an equation that takes the relationship between speed, pressure, volume forces and viscosity friction forces into account. Since the subject of research concerns the movement of air in a large space, all the properties of the air must be taken into account. 5

15 Group F2P31 3. Numerical methods In fluid mechanics there are three main equations which define a flow and describe the motion of a fluid: the continuity equation, the Navier-Stokes equation and the energy equation. All these equations can be gathered into one governing equation as seen if equation div( u )= div( r )+ S (3.1) Density of the fluid [kg/m 3 ] Parameter of the fluid, e.g. temperature, velocity, concentration, etc. [ C, m/s, ppm..] t Time [s] u Velocity of the fluid [m/s] Diffusion coefficient [kg/(m s)] S Source term [ C/m 3,m/(s m 3 ) From the equation it can be seen that choosing the correct parameter, which can be temperature, velocity, concentration, etc., determines the motion of the fluid. For the continuity equation, where = 1, = 1 and S = 0 we find the following + div( u) In fluid mechanics, the principle of conservation of mass within a flow can be described by the continuity equation. The establishment of the local equation is based on the mass balance of the fluid within an element of volume during an elementary time. The following conditions are given for the Navier-Stokes equation. = u, =µ, + xg $ x = v, =µ, + yg $ y = w, =µ, + zg $ z momentum momentum momentum This gives equations 3.2, 3.3 and

16 Aalborg u) v) + div( + div(µru)+ g x (3.2) + div( + div(µrv)+ g y (3.3) + div( + div(µrw)+ g z (3.4) The main objective of this equation is to describe the movement of fluids. Since a fluid can be a liquid or a gas, it can be deduced that the Navier-Stokes equation is concerned with the surrounding conditions. To correctly describe a fluid in motion, its velocity at any point of space must be known. This is called the velocity field. Knowledge of boundary conditions relating to speed and pressure make it possible to solve the equation to obtain the velocity field. However, the analytical solution can be difficult to obtain if not impossible. This is why the use of numerical methods is often necessary for such problems. For the energy equation with the condition that = T, equation 3.5 is obtained. 0 c ˆT @ ˆT (3.5) This equation is determined to describe the temperature distribution within the domain Methodology In general the resolution of a fluid mechanics case numerically involves three major phases: The definition of a geometry A mesh discretizing of the domain The choice of the numerical models Spatial and temporal discretization of equations The spatial discretization consists in replacing the integrals by sums on elements of volume and surface corresponding to the mesh. For each control volume, that is cell, equation 3.6 is applicable. a nb Ø nb + b a p Ø p =0 (3.6) Where 7

17 Group F2P31 3. Numerical methods a nb Ø nb b a p Ø p sum of Diffusion conductance at boundaries sum of fluid parameters at boundary source term diffusion conductance at center of cell Exact solution of the equation The temporal discretization consists in making calculations at determined instants; the result of the simulation at an instant (t i ) becomes the input data of the calculation at time (t i +1). The time step (t i +1-t i ) can be constant or variable. Temporal discretion typically uses the finite difference method. 8

18 4 Turbulence models Turbulence modelling predicts the effects of turbulence on the calculations and therefore analytical solutions of the case. It is based on the Reynolds Averaged Navier-Stokes equations (RANS), that are time-solved equations on motion for fluid flow. They solve transport equations for mean flow quantities and model all scales of turbulence. Reynolds Averaging introduces additional terms, which need to be modelled to ensure closure, as the full Navier-Stokes equation is impractical to compute. This in turn depends on the different RANS models; these may be 1-equation, 2-equation, etc. A 1-equation model could be the Spalart-Allmaras model, whereas the 2-equation models include the more commonly used k- and k-! models. Two equation turbulence models are commonly used. These are industry standard models but are still a very active area of research; the models are constantly being developed to accommodate different types of flow. The two-equations model are almost always based on the transport equation for k, the turbulent kinetic energy, seen in equation 4.1. k = 1 2 (u02 + v 02 + w 02 ) (4.1) The following section is based on the Theory Guide to ANSYS Fluent [ANSYS, 2013] and slides from Chungen Yi [Chungen Yi] and all equation are from the online CFD forum wiki [CFD online, 2017]. For standard cases, the SST k-! and the realizable k- are often recommended. Common for all the utilised model in this project is the use of two-equation models. The k model The k- models are often used in CFD. They are based on a two-equation model, consisting of two transport equations; one for the kinetic energy is derived from k and one for the dissipation rate. Different variations of the k- model exist, as modifications have been made to the original standard k- model. This has lead to the RNG k- model and the realizable k- model. Standard k The standard k- model is one of the most commonly used turbulence models; it is both robust and economically stable, all the while providing reasonable accuracy. This model is able to solve the majority of engineering problems in common practice. The conditions of the standard k- are that there is fully turbulent flow and that the molecular viscosity is negligible. It is suitable for initial iterations/screening of alternative designs and parametric studies. However, it lacks in regards to severe rp, separation and strong streamline curvature. 9

19 Group F2P31 4. Turbulence models The first equation 4.2 handles the turbulent kinetic energy k u i) µ + µ + P k + P b Y M + S k j j The second equation 4.3 handles the dissipation ( u i µ + µ j C 2 2 k j + C 1 k (P k + C 3 P b ) (4.3) As the model we are using may experience separation, we wish to use another model. RNG k The RNG k model is a modification of the standard model with the added benefit of being able to handle laminar flow. It has improved accuracy for rapidly strained flows through the equation, and handles transitional flows better and the different turbulent length scales. Furthermore it is able to handle complex shear flows, which include rapid strain, moderate swirl, vortices, and locally transitional flows. However, the model is still an isotropic eddy-viscosity model. The RNG k model is typically the favoured turbulence model for indoor air. The first equation 4.4 handles the turbulent kinetic energy k u i) µ + µ + P k j j The second equation 4.5 handles the dissipation ( u i µ + µ j j + C 1 k P k C 2 2 k (4.5) Where, C 2 = C 2 + C µ 3 (1 / 0 ) 1+ 3 And, = S k 10

20 Aalborg University S =(2 S ij S ij ) 1/2 Realizable k The realizable k- model on the other hand is very similar to the RNG model. It converges easier and more smoothly than the RNG model. The first equation 4.6 handles the turbulent kinetic energy k u i) µ + µ + P k + P b Y M + S k j j The second equation 4.7 handles the dissipation ( u i µ + µ j C 2 + C 1 j 2 k + p + C 1 k C 3 Pb+ S Where, C 1 = max 0.43,, = S k +5,S = p 2 S ij S ij The k! model Furthermore there is also the k-omega model, which is also from the kinetic energy. The omega is the specific rate of dissipation. As with the k-epsilon, the k-omega model also has a modification in the form of SST k-omega (Shear-Stress Transport). The SST k-omega is based on the two-equation eddy-viscosity model. It combines the benefits of the k-epsilon model with the inner boundary conditions. Standard k! Another type of model is the standard k-! model. It is far superior to the k- in regards to the wall-bounded BL-separation, free shear and low Reynolds number flows. Furthermore it can be used for complex BL flows under adverse opposite delta p and separation. Separation is typically predicted slightly early and at an excessive level. The second equation 4.8 handles the turbulent kinetic + j = i! k ( + j (4.8) The second equation 4.9 handles the dissipation (!). 11

21 Group F2P U j k i! 2 ( + j (4.9) SST k! As with the k- model, there are modifications to the k-! models. Once such modification is the SST(Menter s Shear Stress Transport) k-! model. It is a combination of the k! and k models. The SST k! model is beneficial when dealing with transient simulations. The second equation 4.10 handles the turbulent kinetic + U = P k! k ( + j (4.10) The second equation 4.11 handles the + U = S 2! 2 ( +! j +2 (1 F 1 @x i (4.11) 12

22 5 Boundary Conditions Boundary conditions are necessary parts of the fluid-flow mathematical model as they specify the fluxes coming into and out of the domain. Incorrect specification of boundary conditions will provide incorrect results. Mathematically there are several types of boundary conditions, such as Dirichlet condition, Neumann and mixed boundary condition. Dirichlet boundary condition prescribes the value of a variable at the boundary, whereas the Neumann boundary condition prescribes the gradient of a variable. The mixed boundary condition is a combination of the two mentioned conditions. The following section is based on the slides Boundary conditions by André Bakker [Bakker, 2008]. Flow inlets and outlets A wide range of boundary condition types can be used for flow inlets and outlets. Their use also depends on the properties of the fluid flow. For general flow, pressure inlet and outlet can be used. In case of incompressible flow, it is possible to use the velocity inlet and outflow. For compressible flow, it is required to use mass flow inlet and pressure far field. There are also other special boundary condition types such as inlet vent, outlet vent, intake fan and exhaust fan. Pressure inlet and outlet These conditions are used when velocity and the flow rate are not specified. The absolute pressure is the sum of static gauge pressure and operating pressure. These two values are set separately. Pressure inlet boundary is suitable for both compressible and incompressible flow. Boundary mass flux changes depending on the interior solution and flow direction. The flow direction must be specified. Pressure outlet must always be used together with pressure inlet. Velocity inlets This type of boundary condition is used when the velocity profile at the inlet is known. Velocity vector and scalar properties of the flow are defined. Outflow boundary The outflow boundary condition is used when the details of the flow velocity and pressure are unknown. Outflow cannot be used for compressible flows, for unsteady flows with variable density and together with the pressure inlet boundary condition. Mass flow inlet Mass flow inlet is used for compressible flow. It prescribes mass flow rate at inlet. This means that the mass flow rate remains fixed but total pressure varies. 13

23 Group F2P31 5. Boundary Conditions Pressure far field Pressure far field is used to model compressible free stream flow at infinity. This condition can be used only when the density is calculated using the ideal-gas law. Exhaust fan/outlet vent and inlet vent/intake fan To model external exhaust fan or vent with specified pressure jump or loss coefficient, ambient pressure and temperature. Inlet vent/intake fan conditions are similar, they are only used for inlets. The loss coefficient or pressure jump, flow direction, ambient pressure and temperature are specified. Other boundary conditions Turbulence parameters Definition of turbulence is another boundary condition. Boundary values need to be specified for turbulent kinetic energy k and turbulent dissipation rate. Specification of turbulence parameters can be done by setting k and. Specification of turbulence parameters can be done by setting k and explicitly, or setting turbulence intensity and turbulence length scale, turbulence viscosity ratio or hydraulic diameter. Wall boundaries Wall boundaries determines fluid and solid regions. Thermal boundary conditions, wall roughness and also translational or rotational velocity at the wall boundaries can be specified. Symmetry boundaries Symmetry boundaries are used to reduce the computational time and effort. Flow field and geometry must be symmetric. Periodic boundaries Periodic boundaries can be used when the physical geometry, flow pattern and thermal solution are periodically repeating. This condition helps to save computational time. Axis boundaries This type of boundary condition is used at the centreline of a 2D axisymmetric grid of for 3D O-type grid where multiple grid lines meet at a point. Cell zones - fluid Fluid material needs to be characterized with single species and phase. Some other optional input can be added to allow setting of source terms, such as mass, momentum or energy. Cell zones - solid Solid zone represents the group of cells for which only heat conduction is solved. The type of the material need to be specified. Internal face boundaries Internal face boundaries are used to implement physical models like fans, radiators or interior walls. Material properties 14

24 Aalborg University Relevant material properties need to be specified for material in each zone. Properties like density, viscosity, heat capacity, molecular weight, thermal conductivity and diffusion coefficients need to be defined. Not all the properties are required for all types of models. 15

25 6 Mesh Following text is based on the slides by André Bakker [Bakker, 2008] and online CFD Wiki [CFD online, 2017]. Mesh A mesh (or a grid) represents the geometry of the model for which the simulation is to be carried out on. Mesh generation is the process of splitting the whole object into smaller cells, namely geometric cells. Inside these sub-domains, the discretized governing equations are solved in order to determine the air distribution. The generation of a mesh is an important part of the analysis process as it has a significant impact on convergence, solution accuracy and computational time required to reach a solution. Furthermore the use of a low quality mesh could lead to an inaccurate solution or even lack of convergence and therefore no solution. Figure depicts the basic terminology of grid parts for a 2D mesh. Figure 6.1. Basic grid terminology for a 2D mesh. The geometry of the model can be both simple and very complex. Due of this it is necessary to choose a mesh that is suited to the case. It is possible to divide the mesh types into a few basic categories based on the connectivity of the mesh. A structured mesh is characterized by regular connectivity of the cells; it can be expressed as a 2D or 3D array. The position of all the cells can be described with i, j and k-indexing. The use of this mesh is conditioned to the application of quadrilaterals or hexahedra elements. Structured meshes cannot be used for complicated geometries. An unstructured mesh has irregular connectivity. The cells are arbitrarily arranged in the mesh. It is not possible to describe the position of the cell with i, j and k- indexing; it therefore requires more memory and CPU performance compared to the 16

26 Aalborg University structured meshes. In practice it usually takes more time to reach the converged solution. Unstructured meshes are used for complex geometries. The elements usually used for these type of meshes are triangles for 2D meshes and tetrahedral or square pyramids for 3D meshes. Beyond the structured and unstructured meshes, a category of hybrid meshes exist. This is a combination of an structured and unstructured mesh; it is also the type of mesh that offers the greatest flexibility. The regular and simple components of the geometry consist of a structured mesh, whereas irregular and complex components consist of an unstructured mesh. There are three important measures of mesh quality: skewness, smoothness and aspect ratio. Skewness is one of the most important measures of the mesh quality. It is a comparison of the generated mesh to the ideal mesh, measured on a scale of 0 to 1. The closer the skewness is to 0, the more better the quality of the mesh. Figure 6.2. The principle of an equiangular and skewed quad. Smoothness is another measure of mesh quality. A change in size among the cells should be gradual and smooth. Sudden jumps in the cell sizes should be avoided. This could lead to errors in results at the neighbouring nodes. The aspect ratio is the ratio between the longest and shortest side in a cell. In ideal cases and to ensure the best results the ratio should be equal or close to 1. Mesh independence A mesh independence study is carried out to ensure that the analytical solution of a case is independent of the mesh. It has to be fulfilled separately for each turbulent model. The initial simulation is run on the initial mesh. Convergence must be ensured. If not, it is necessary to refine the mesh and repeat this process. Once the criteria is met, the mesh can be globally refined to finer cells. With this new refined mesh, the simulation is run again. After the simulation, the monitor values from both simulations can be compared. If they are the same, then the first mesh is accurate enough. If there are some differences in a not allowable tolerance, it is not acceptable and the solution is not independent of the mesh. It is necessary to repeat the process again until the solution is independent. 17

27 7 Convergence In finite volumes, for each transport equation and for each control volume an algebraic equation of the type seen in equation 7.1 must be solved. a nb Ø nb + b a p Ø p =0 (7.1) Where a nb Ø nb b a p Ø p sum of Diffusion conductance at boundaries sum of fluid parameters at boundary source term diffusion conductance at center of cell Exact solution of the equation In an iterative calculation, an estimated value for the solution is to be inserted that does not automatically satisfy the equation that is to be solved. By injecting this estimated solution noted Ø, the equation will not be verified and instead of having a zero as a balance, a small value, namely the residue, remains. This can be seen from equation 7.2. a nb Ø 0 nb + b a p Ø 0 p = Res (7.2) If the problem to be solved is well defined, this residue will diminish as the iterations progress. Criteria The problem at hand is how to determine the point at which the iterative calculationss are sufficient to give a realistic solution. One method is to regard the variation of the residue while it is in process. This section is based on [Lutz Angermann, 2010] CFD gives the following guidelines: 10 4 is a sufficient limit for a qualitative analysis and for many engineering applications gives good convergence and is sufficient for the majority of engineering applications gives very good convergence and can be used for fairly complex geometries. When the calculation targets specific physical quantities of the problem such as the kinetic energy k, the dissipation rate or!, velocities, energy, etc., the evolution of 18

28 Aalborg University these quantities should be followed. The calculations should then be stopped after their stabilization. It is also useful to check the global conservation over the entire computational domain e.g. by comparing the incoming flow with the outgoing flow. This information is usually given by the calculation at the end of each simulation. Some commercial codes give access to a variable called convergence rate. This indicator is defined by equation 7.3. Convergence rate = Res(n) Res(n 1) (7.3) In this equation n and n-1 refer to the present and previous iteration respectively. When a value of below 1 is reached through this equation, it indicates the evolution of the calculations has reached convergence of the steady state. Values of the order of 0.95 are usual, whereas smaller values of the order of 0.85 indicate a very good convergence. On the other hand if the values are great than 0.95 it means that convergence is very slow. In such cases it may be necessary to increase the time step or the relaxation coefficients. 19

29 Part II COBEE Case 20

30 8 Introduction In a collaborative study between several universities, 19 teams participated in a workshop entitled "Possible user-dependent CFD predictions of transitional flow in building ventilation" with the purpose of predicting low turbulent flow. The purpose of the workshop was for the different teams to utilize computational fluid dynamics (CFD) software and codes, turbulence models, boundary conditions, numerical schemes and convergence criteria to carry out simulations on low turbulent flow for the same model. Each team therefore carried out simulations according to own experiences, from which a large variety of results evolved. [Peng et al., 2015] This part of the student project serves as an expansion of the study. The study is referred to as the COBEE case throughout this report. Both CFD predictions and a model experiment are carried out. The 2D simulations are based on the same case as in the study. This serves as a direct comparison with results achieved by the remaining 19 teams. Furthermore a model experiment has been conducted to create a benchmark for the study. However, the inlet conditions for the measurements differs to that of the study. Therefore 3D simulations have also been carried out on a model with the exact same dimensions as the model experiment. 8.1 COBEE Case The study concerns ventilation in large rooms. The flow in the room is studied to determine all the desired characteristics such as penetration length and maximum velocities in the occupied zone. For this purpose, a simple model has been defined, which is easily modelled under CFD. The case is a simple problem: a deep room with a slot opening. The principle of the model is illustrated in figure 8.1. Figure 8.1. Geometry of the COBEE case. 21

31 Group F2P31 8. Introduction Criteria set for the geometry is as follows based on the set-up in figure 8.1. Dimensions H, h, l and L are respectively the room height, inlet slot height, length of inlet opening and length of the room and x re is the penetration length. h H = 1 5 l h =4 L should be long enough so it doesn t hit the backwall and effect the prediction. W =2 H Throughout the case, flow is isothermal and flow will be changed in accordance with different Reynolds numbers ranging from 500 to 10,000. The flow between Re 5 to 500, where the flows momentum is too low to be distinguished from the natural air flow. This instability can be explained by the fact that there is no proper model for the transient case in connection with the governing equations, and that existing models are especially dedicated to turbulent regimes. Therefore it is possible to say that this study also serves to predict the errors that may appear during a simulations. The question that arises is how the uncertainty in this range of Reynolds numbers influences the solution for different models and how large the error generated is. The models used for the 2D and 3D simulations respectively will now be defined. To carry out a detailed study on the subject, a numerical solution is necessary in order to simulate the airflow, as the governing equations for airflow has no solution analytically. Based on different models of calculations and on different meshing to ensure the independence mesh, the goal is to determine the penetration lengths in this geometry according to different input parameters. Small-scale modelling allows the study of ventilation in the full-scale large room, based on the similarity principles. The process to realizing the small-scale model is based on making all the parameters dimensionless and utilizing important numbers in the governing equations such as Reynolds number. Reynolds number is constant for both the small-scale and the full-scale one D CFD model The 2D model for which simulations are carried out is based on full-scale dimensions set in accordance with all ratios which define the dimensions mentioned above. The dimensions of the full-scale model are defined as in table D.1. Table 8.1. Dimensions of the 2D full scale model. Parameter [-] Length [m] H 5 h 1 l 4 L 50 22

32 8.3. 3D CFD Model Aalborg University The model dimensions can be seen in figure 8.2 and are of significantly larger scale than the model experiment. 1m 1m 5m 4m Inlet 50m Outlet Slot 4m Figure 8.2. The model used for 2D simulations. The velocities for the different Reynolds numbers for this geometry and their corresponding calculations can be seen in appendix A Meshing With the use of these dimensions, a mesh was developed by Li Liu in order to carry out the simulation. This mesh is illustrated in figure 8.3. It is a triangular type meshing with good growth rate. This is especially necessary close to boundaries, where a large number of iterations have to be done to achieve as exact a result as possible. Figure 8.3. The mesh used for 2D CFD simulations. The mesh independence study, which ensures that the analytical solution of the case is independent of the mesh, has been carried out by Li Liu D CFD Model As with the 2D model it is necessary to define the model used to carry out CFD predictions on a 3D simulation. To deliver a better comparison to the model experiment results, the 3D simulations will be carried out on a model identical to the one utilized for the model experiment. The difference between the models is the additions to the inlet of the 3D model, in accordance with the model experiment. This can be seen in figure 8.4 and

33 Group F2P31 8. Introduction 0.21m 0.20m 0.40m 0.60m Inlet 3.00m Outlet Slot Figure 8.4. The model used for 3D simulations. 0.40m 0.21m Radius 0.92m h = 0.04m H = 0.20m 0.60m Inlet Slot Figure 8.5. The inlet for the model used for 3D simulations. As the boundary condition for the 3D inlet is set at the box with a different height than the slot, the inlet velocity differs from those used for the 2D simulations in order to maintain constant flow rate and Reynolds number. The inlet velocities therefore have to be configured. The velocities and their corresponding calculations can be seen in appendix A Meshing As with the 2D simulation, a mesh for the 3D simulation was developed. This was once again carried out by Li Liu. The inlet was developed according to the dimensions described above. The mesh is once again of the triangular type. Figure 8.6 depicts the whole mesh used, while figure 8.7 shows the specific inlet of the mesh Figure 8.6. The mesh for the 3D simulation. 24

34 8.3. 3D CFD Model Aalborg University Figure 8.7. The mesh for the inlet of the 3D simulation. 25

35 9 CFD Simulations The simulations are carried out on the 2D and 3D models respectively. Through these the penetration lengths can be obtained, which will later be used in connection with the model experiment to predict the expectations. Furthermore the simulations serve as comparison with the COBEE case results. The simulations were carried out in the CFD program ANSYS Fluent D Case For the 2D simulations carried out on the COBEE model, five different turbulence-models were used in order to compare them: RNG k-, standard k-, standard k-!, SST k-! and realizable k-. The remainder of the input can be seen in appendix B. Prediced Penetration Length The predicted penetration length for the different turbulence models by Reynolds number can be seen in table 9.1. Table 9.1. Predicted penetration length for each model and set Reynolds numbers. Reynolds Penetration length [m] number [-] RNG k- std k- std k-! SST k-! Real. k

36 9.1. 2D Case Aalborg University The penetration lengths in table 9.1 are for the model with a length of 50 m. To be able to compare the predictions with the measurements from the model experiment, they will be made dimensionless by dividing the penetration length x re with room height minus the slot height (H-h). A plot of the dimensionless predicted penetration lengths are shown in figure RNG k-0 standard k-0 standard k-! SST k-! Realizable k-0 COBEE predicted 8 x re / (H-h) Re Figure 9.1. Plot of the predicted penetration lengths for the different turbulence models. As shown by the plot, the dimensionless penetration lengths vary greatly dependent on the turbulence model. The variations increase along with the Reynolds numbers. The predictions show that after a certain Reynolds number, the predicted penetration length stop increasing and remain relatively constant ( Re 5000). It is also noticeable that at Reynolds numbers 200, 500, 1000 and 3000 the k-! models deviate from the tendency the models show for the remaining Reynolds numbers. Looking at the flow prediction from the SST k-! model at Reynolds number 3000, an interesting flow pattern is observed, a contour plot of the positive x-velocity [m/s] is shown in figure 9.2. Figure 9.2. Contour plot of the positive x-velocities [m/s] from SST k-! simulation. The flow predicted by the SST k-! model varies from the RNG k- which is normally 27

37 Group F2P31 9. CFD Simulations favoured for indoor air simulation. A contour plot of the positive x-velocities [m/s] for the RNG k- at Reynolds number 3000 is shown in figure 9.3. Figure 9.3. Contour plot of the positive x-velocities [m/s] from RNG k- simulation. As 3D simulations are much more time-consuming than the 2D simulations, two of the five turbulence models will be chosen for the 3D simulations. They will be chosen based on literature and comparisons with the COBEE case. Therefore there will also be focus on the 2D simulations of these two models. The RNG k- model is chosen first, as it is the favoured turbulence model for indoor air simulation. The results from these simulations have been plotted in the graphs containing the results from the COBEE research paper. The results from the 2D RNG k- s comparison to the results from the COBEE paper can be seen in figure 9.4 and figure 9.5. Figure 9.4 is a comparison with the results of all the turbulence models in the COBEE paper. 2D RNG k-epsilon Figure 9.4. Comparison of the 2D RNG k- simulation to the COBEE simulations for all the different turbulence models [Peng et al., 2015][Edited]. Figure 9.5 is a comparison with all the RNG k- simulations in the COBEE paper. 28

38 9.1. 2D Case Aalborg University F2P31-2D-FLUENT Figure 9.5. Comparison of the 2D RNG k- simulation to the RNG k- COBEE simulations [Peng et al., 2015][Edited]. As can be seen in figure 9.5, that the RNG k- predictions carried out are close to being the mean of the predictions from the COBEE paper. The realizable k- model is chosen as the second turbulence model as it is, according to literature, the preferred k- model. As with the RNG k-, the results from the 2D realizable k- are compared with the results from the COBEE paper and can be seen in figure 9.6 and figure 9.7. Figure 9.6 is a comparison with the results of all the turbulence models in the COBEE paper. 29

39 Group F2P31 9. CFD Simulations 2D Realizable k-epsilon Figure 9.6. Comparison of the 2D realizable k- simulation to the COBEE simulations for all the different turbulence models [Peng et al., 2015][Edited]. Figure 9.7 is a comparison with all the realizable k- simulations in the COBEE paper. F2P31-2D-FLUENT Figure 9.7. Comparison of the 2D realizable k- simulation to the realizable k- COBEE simulations [Peng et al., 2015][Edited]. Just as with the RNG k- comparison, it can be seen in figure 9.5, that the RNG k- predictions carried out are close to being the mean of the predictions from the COBEE 30

40 9.2. 3D Case Aalborg University paper Maximum Velocity in the Occupied Zone Other than the dimensionless penetration length, it is possible to find the distance to the maximum velocity by Reynolds number by the CFD predictions. This has been done for the two k- models. Figure 9.8 shows these results for the 2D simulations Distance to Maximum Velocity in the Occupied Zone 2D Realizable k-epsilon 2D RNG k-epsilon Measurements x rm [m] Re Figure 9.8. The distance for the maximum velocity in the occupied zone for 2D simulations. As the figure illustrates, the realizable k- model has a higher distance to the maximum velocity than RNG k-. However, both show the same tendencies with no increase in the distance at Re 5000, as earlier seen with the penetration lengths D Case The 3D case was developed in order to examine the solution to such an analysis. The simulations were carried out on Reynolds numbers ,000, as these are the Reynolds numbers that are used in the model experiment. They will therefore provide results that are comparable in order to determine the validity of the 3D simulations. It was determined to use two turbulence models for the simulations; RNG k- and realizable k-. This enables a comparison between the two models. These models have been chosen because of the results achieved during the 2D CFD simulations, where these models appear to be the optimal choice. 31

41 Group F2P31 9. CFD Simulations As previously mentioned, the inlet boundary condition of the 3D case differs from the 2D case, for which the initial velocity has been adjusted accordingly. This can be seen in appendix A. The remainder of the input can be seen in appendix B. Predicted Penetration Length Through the CFD simulations the penetration lengths at each Reynolds number have been determined. This is determined by the cross-section through the middle of the box, as seen in figure 9.9. Figure 9.9. Cross-section through the 3D model. The penetration lengths from the CFD simulations are shown in table 9.2. Both the penetration lengths and dimensionless penetration lengths are shown for the two turbulence models. Table 9.2. Predicted penetration length for each model and set Reynolds numbers. Dimensionless Penetration length [m] Re [-] penetration length [-] RNG k- Real. k- RNG k- Real. k Figure 9.10 illustrates the plots of the dimensionless penetration lengths for both turbulence models. 32

42 9.2. 3D Case Aalborg University D Realizable k-epsilon 3D RNG k-epsilon 3D Simulations x re / (H-h) Re Figure The predicted dimenionless penetration lengths for the different turbulence models. As shown by the plot, there is very little variation between the RNG k- and the realizable k- models. This was expected, as 2D simulations using the models were also very close. This is further supported by figures 9.11 and extremely similar in them. The air flow and velocities are Figure 9.11 shows the velocity magnitude from the realizable k- model. Figure Contour plot of the velocity magnitude [m/s] from the realizable k- simulation. Figure 9.12 shows the velocity magnitude from the RNG k- model. Figure Contour plot of the velocity magnitude [m/s] from the RNG k- simulation. 33

43 Group F2P31 9. CFD Simulations As previously mentioned, the inlet conditions differ between the 2D and 3D simulation. This does not allow a strict comparison between the two; however, it does enable research into the effect the inlet conditions may have on the flow and thereby penetration length. To be strictly comparable, and 2D and 3D version of the 3D and 2D models respectively should be used. Figure 9.13 displays the 3D RNG k- simulation in comparison with the simulations obtained through the COBEE case. The best comparisons can be made between the other 3D simulations, in particular those carried out in ANSYS Fluent. As illustrated in the graph, the simulations obtained in this report lies within the margin of simulations from other universities. There are in particular similarities with C02 in the region 500 apple Re apple However, from Re > 500, the dimensionless penetration length continues to rise for the simulations obtained in the report, whereas for the majority of COBEE case simulations flatten. The dimensionless penetration length is expected to flatten, as the penetration length becomes independent of the Reynolds number once fully developed turbulent flow has been reached. The continued increase in the dimensionless penetration length of the simulations may be due to the the use of enhanced wall treatment as the near-wall treatment. This is further supported by the simulations seen in appendix C. F2P31-3D-FLUENT Figure Comparison of the 3D RNG k- simulation to the RNG k- COBEE simulations [Peng et al., 2015][Edited]. Figure 9.14 displays the 3D realizable k- simulation in comparison with the simulations obtained through the COBEE case. The predictions fit relatively well with those from the COBEE case. However, in the transient phase (1500appleReapple5000) the simulations give a lower dimensionless penetration length than the COBEE simulations, including the 34

44 9.2. 3D Case Aalborg University 3D COBEE simulations. However, the predictions are in general similar to the COBEE case. Once again, the continued increase of the dimensionless penetration length at fully developed turbulent flow indicates the use of the the enhanced wall-function. F2P31-3D-FLUENT Figure Comparison of the 3D realizable k- simulation to the realizable k- COBEE simulations [Peng et al., 2015][Edited] Maximum Velocity in the Occupied Zone The distance to the maximum velocity has also been found for the 3D simulations. This is especially relevant as it is comparable to the model experiment, since the exact same model dimensions (including the inlet) are used. Figure 9.15 shows these results for the 3D simulations. 35

45 Group F2P31 9. CFD Simulations Distance to Maximum Velocity in the Occupied Zone 3D Realizable k-epsilon 3D RNG k-epsilon Measurements x rm [m] Re Figure The distance for the maximum velocity in the occupied zone for 3D simulations. For the 3D simulations, the RNG and realizable k- models are extremely similar. As previously mentioned, they also show that the distance to maximum velocity continues to increase slightly despite fully developed turbulent flow being reached. The predictions will later be compared to the measurements. 36

46 10 Model experiment The air distribution can, as previously mentioned, be studied through both a computational and experimental approach. This allows for a comparison between theory used for the simulations and reality, which can help evaluate the accuracy of the CFD simulations. The comparison is enabled by performing a model experiment on the COBEE Case in a small 3D scale. Through the model it is possible to evaluate, dimensionless penetration length are achieved. whether the same velocities and 10.1 Methodology The following part explains the procedure and requirements behind the experiment carried out on the model experiment Model dimensions The experiment conducted must have the same ratio of dimensions as the COBEE case, and therefore the 2D and 3D computational simulations. Therefore the following dimensions have been applied. Length L of 3.00 m Width W of 0.40 m Height H of 0.20 m Inlet slot height h of 0.04 m The dimensions are illustrated in figure 10.1 and figure m 0.20m 0.40m 0.60m Inlet 3.00m Outlet Slot Figure Geometry of the model for the model experiment. 37

47 Group F2P Model experiment 0.40m 0.21m Radius 0.92m h = 0.04m H = 0.20m 0.60m Inlet Slot Figure Geometry of the inlet for the model for the model experiment. The 3D simulations were carried out using exactly the same dimensions as the model experiment Equipment Beyond the actual model box, it is necessary to acquire the correct equipment to conduct the experiment. The following equipment has been used: Ducts and fittings connecting the different components Smoke box Orifice plates (flowmeter) Manometer Fan Thermocouples attached to the inlet, outlet and room temperature Laser Software for the laser Arm for the laser Straws The equipment is connected as shown in figure Side: SM Inlet L COBEE box M Above: SM Inlet COBEE box L M SM Smoke machine M Orifice plates and manometer Thermocouples L Laser Fan Figure Setup of the experiment seen from the side and above. 38

48 10.2. Results Aalborg University The inlet is connected to the COBEE box. The inlet has been filled with straws to ensure a uniform flow throughout the box. The fan is connected to the outlet of the box to ensure a smooth flow throughout the system. The criteria to the length of flexible ducts placed before and after the orifice plates are there to ensure reliable measurements of the flow. There is a distance of five times the diameter before the orifice plates and ten times the diameter after the orifice plates. The thermocouples are placed at the inlet, outlet and inside the room to evaluate the thermal, as the experiment has been carried out on isothermal flow. Therefore it is possible to determine potential errors as there is a risk of the smoke machine heating the inlet air. It has been attempted to reduce the number of errors to the extent possible by ensuring stable conditions. This includes leading the outlet after the fan to the outdoors to remove smoke Procedure The laser is placed at the point where the measurement is to be made. The fan is turned on, where-after it runs until steady state is reached. Once steady state has been reached the smoke machine and laser are turned on. The different software is turned on simultaneously; this includes the program BSA Flow Software for the laser to measure the velocity of the air flow and Time Constant to measure the temperatures with the thermocouples. The data is then acquired after each measurement. Measurements are carried out for the following Reynolds numbers; 500, 1000, 1500, 2000, 3000, 4000, 5000, 6000, 7000, 8000, 9000 and This covers both transitional and turbulent flow. The experiment will only be carried down to Re 500, as any values below this will give an uncertainty. With such low flow rates, it cannot be determined whether the velocity measured is caused by the initial velocity or the turbulence generated internally. Therefore any results would be irrelevant. For each Reynolds number, the measurements are carried out to locate the penetration length and the maximum velocity in the occupied zone. This is located in the distance between the inlet and the penetration length Results The results of the measurements can be seen in table

49 Group F2P Model experiment Table COBEE measurement results for penetration length (PL). Reynolds number [-] Measured PL avg. [m] Number of measurements The dimensionless penetration length has been calculated for all the Reynolds numbers. A plot of these can be seen in figure Measurement 1 Measurement 2 Measurement 3 Measurement avg. COBEE measurements 7 6 x re / (H-h) Re Figure Dimensionless penetration length of the model experiment. The graph shows all three measurements of the dimensionless penetration length at every Reynolds number along with the average. As it can be seen from the graph, once fully developed turbulent flow is reached, the dimensionless penetration length stops increasing and remains constant. 40

50 10.3. Small-Scale to Full-Scale Aalborg University Margin of error There are a number of uncertainties and errors that may have been obtained throughout the experiment. They include the following. As with any experiment, human errors could be the source of any major errors or irregularities in the results. This could for example be through the placement of the laser at the wrong point. Furthermore turbulence affects the measurements and gives an uncertainty. This is why Reynolds numbers below 500 have not been examined in the model experiment. The roughness of the box might also affect the turbulence, and thereby alter the Reynolds number. The calibration reports in the lab are 9-10 years old, and more precise equipment for pressure measurement is lacking due to the move. Therefore it is not known whether the correct flow rates were achieved by the manometers is what the reading says, which gives an uncertainty to whether the flow is the correct for each measurement. A calibration report for the laser could not be found and since it is the most precise piece of equipment in the laboratory, it was not possible to calibrate it. An attempt to validate it was attempted with the jet wind tunnel but because of the filters in the jet wind tunnel, the laser could not measure the velocity from the tunnel. The shifting difference between outdoor and indoor pressure, makes it difficult to maintain a set flow rate and this could interfere with the measurements. This also makes it increasingly difficult to set the frequency for the fan, as the manometers readings are fluctuating or reacting slowly, which makes room for more human error. The measurement of the inlet velocity profile gives reason to believe that there might be a fault in one side of the inlet, that causes the lower velocity, making the profile asymmetric. This can be seen in appendix D Small-Scale to Full-Scale The 3D simulations use exactly the same dimensions and results are therefore directly comparable. This is not the case for the 2D simulation. Through the use of the similarity principle, it is possible to convert from one scale to another, usually from small-scale to full-scale. The similarity principle has its foundation in making the governing flow-equations dimensionless, and from this the dimensionless numbers Reynolds, Archimedes, etc., can be derived. As the COBEE case is by default a isotherm case, the Archimedes number is ignored, and the Reynolds number will be worked with. To be able to use the similarity principle the dimensions of the model used in the experiment and the 2D simulations will have be the same. The dimensions of the model is described in section An example of the conversion to full-scale is shown in equation 10.1 for Reynolds number 10,

51 Group F2P Model experiment x re,m H m h m (H fs h fs )=x re,fs (10.1) Where x re,m H m h m H fs h fs x re,fs Measured penetration length in the model [m] Height of the model [m] Height of the model inlet [m] Height of the full-scale model [m] Height of the full-scale inlet [m] Penetration length in full-scale [m] The penetration length for the full-scale model is calculated in equation m (5 m 1 m) = 26.5m (10.2) 0. 2m 0.04 m This can be carried out for all the Reynolds numbers. However, the dimensionless penetration length can be calculated for all the simulations and model experiment and compared. If a full-scale has the same ratio of dimensions as this case, multiplying by (H-h) will give the actual penetration length for said case. 42

52 11 Comparison of Simulations and the Model Experiment Comparisons can be carried out on the results achieved from the 2D and 3D simulations with the measurements from the model experiment. This is used to research the validity of the simulations to reality. However, it should be taken into account that the 2D simulations were carried out on a model with different inlet conditions to the 3D simulations and the model experiment. Therefore it is not strictly comparable. 2D Simulations versus Model Experiment The 2D simulations were carried out on Reynolds numbers 5-10,000. However, the model experiment was only carried out from Reynolds numbers ,000. These then serve as the comparative Reynolds numbers. The dimensionless penetration lengths can be seen on figure D Realizable k-epsilon 2D RNG k-epsilon Average measurements 2D Simulations versus Measurements x re / (H-h) Re Figure The dimensionless penetration lengths of the 2D simulations and the measurements from the model experiment. The graph illustrates how the 2D RNG k- model simulations are very similar to the measurements. The realizable k- model has slightly higher dimensionless penetration lengths for all the Reynolds numbers. 43

53 Group F2P Comparison of Simulations and the Model Experiment However, it is for these simulations that the inlet boundary conditions differ. Therefore it can be seen that the change of inlet does not change the general tendencies of the DPLs as a function of Reynolds number. However, it cannot be determined which of the turbulence models is more accurate, as a model experiment with the same inlet as the 2D simulations would have to be carried out. 3D Simulations versus Model Experiment The 3D simulations, with the exact same dimensions as the model experiment, is also compared to the measurements of the model experiment, especially as these are directly comparable. The dimensionless penetration lengths can be seen in figure D Realizable k-epsilon 3D RNG k-epsilon Average measurements 3D Simulations versus Measurements x re / (H-h) Re Figure The dimensionless penetration lengths of the 3D simulations and the measurements from the model experiment. As can be seen from the graph and as previously established, the RNG k- and realizable k- model simulations are extremely close. Furthermore, they are very similar to the measurements. Throughout the majority of the range of Reynolds numbers, the RNG k- model appears to be slightly closer to the measurement results. The graph clearly shows a deviation in the fully developed turbulent flow region. At Re 5000, the DPL remains fairly constant for the measurements, while it continues to increase for the simulations. This is most likely due to the use of the enhanced wall treatment. However, as the can be seen in appendix C, the enhanced wall treatment decreases the DPL and approaches the measurement results. 44

54 Aalborg University 2D, 3D Simulations and Model Experiment As it was determined to utilize the RNG k- and realizable k- models for the 3D simulations, these will be compared to the 2D simulations using the same models as well as the measurements. This can be seen in the graph illustrated in figure D and 3D Simulations versus Measurements 2D Realizable k-epsilon 3D Realizable k-epsilon 2D RNG k-epsilon 3D RNG k-epsilon Average measurements 7 6 x re / (H-h) Re Figure The dimensionless penetration length of the 2D and 3D simulations and the measurements from the model experiment. In appendix E, the graphs can be seen respectively of the two turbulence models compared to measurement results from the model experiment. From the graph it can be obtained that the 3D simulations are close to the reality of the dimensionless penetration lengths in the transient and turbulent regions up to Reynolds number However, after Re 5000, the DPL keeps rising, albeit at a lower gradient, than the measurements. As previously mentioned, the measurements develop this phenomenon because the penetration length becomes independent of the Reynolds number once fully-developed turbulent flow has been reached. The 2D simulation using the realizable k- model has higher DPLs for the majority of the range of Reynolds numbers. However, both the turbulence models for 2D simulations show the correct tendency to curve around fully developed turbulent flow due to the use of the standard wall function. Despite this, the different inlet for the 2D simulations makes it impossible to compare directly. 45

55 Group F2P Comparison of Simulations and the Model Experiment 11.1 Conclusion It is possible to deduce that the 3D simulations approach the measurements from the model experiment. In particularly the RNG k- model seems optimal to use, as it is very close to the measurements. It has been shown that the enhanced wall treatment gives results that approach the DPL of the model experiment measurements further. Furthermore it can be concluded that while the inlet differs between the 2D simulation and the model experiment, the DPL are still simlar with a similar pattern. Therefore the inlet does not have a huge effect on the flow in the model. 46

56 Part III Practical case 47

57 12 Introduction For this part of the project, a more practical approach is taken. The focus is on the geometry of a large room, more specifically an industrial hall with machinery. A deep room with major heat sources from machinery requires ventilation in order to achieve thermal comfort for the occupants of the room, as well as possibly prevent any impact high temperature may have on the product being developed by the machinery. The velocity and temperature distribution will be investigated with different flow rates in the room. This part is primarily devoted to the process of the complete case from the very beginning, i.e. from defining the case, mesh generating, defining all the conditions, setting the solver and assessing the obtained solution and results Model Dimensions and Purpose The investigated room is a deep room with 50 m in length, 12.5 m in width and 5 m in height. This makes the total volume of the room 3125 m 3. The industrial machinery is situated in the long room. It is considered to be a machine with a significant rate of heat release. Two pieces of the machinery are placed in the room and they are assumed to fill the whole width. As the cross-section is uniform throughout the room, a 2D model is considered. The machinery is represented by a rectangular shape in the simulation model. The dimensions are 1 m in height and 10 m in length. In the model two pieces of machinery are placed. Each of the two industrial machines has a heat flux release of 100 W/m 2. Mixing ventilation is used in this room. The inlet is placed at the wall right under the ceiling. The outlet is placed at the bottom on the opposite wall. The flow rate is used as the variable for further investigation. It is assumed that no other contaminants are released. Figure 12.1 shows the main geometrical characteristics as well as the conditions. The red mark indicates the inlet. 48

58 12.1. Model Dimensions and Purpose Aalborg University Cross-sectional side view: 5.0m 1m 1.0m 100 W/m 2 100W/m m 10m 10m 10m 10m 10m Cross-sectional view from above: 50m 12.5m 100W/m 2 100W/m 2 Figure Geometry and conditions for the model. 49

59 13 CFD Simulations CFD simulations are carried out on the defined model in order to determine the air flow in the room Meshing To describe the geometry of the room for further calculation purposes, the mesh was created. Computer programme ANSYS ICEM 16 was used for creation of the geometry and for generation of the mesh. The mesh is a 2D quadrilateral structured mesh. In the picture 13.1 the detail of the mesh is shown. Figure Detail of the mesh. The full mesh can be seen in appendix F Mesh Independence Test Mesh independence test is a necessary part of any CFD investigation in order to obtain reliable results. On the other hand, it is important to keep in mind that the higher the number of elements in the mesh, the more computational power and time is required to obtain convergence. Therefore it is reasonable to find a compromise between these two criteria and determine the acceptable error in results. Mesh independence for this case was tested, the whole initial mesh was refined several times to obtain meshes with different numbers of elements. All these meshes converged properly without any errors. The penetration length and x-velocities in different distances from inlet were compared to check the mesh independence. The results are shown in table 13.1 and in the

60 13.2. CFD Simulation Settings Aalborg University Table Penetration length obtained during mesh independence test. Number of cells [-] Penetration length [m] It can be seen that the first mesh with the lowest number of elements gave a penetration length that differed a lot from the other meshes Mesh independency 3565 cells cells cells cells cells Velocity [m/s] Distance from inlet [m] Figure Comparison of velocities in different distances from the inlet. The mesh with the lowest number of elements has lower velocities in most of the investigated points compared to the other meshes. Meshes with 57,040 elements and 79,700 cells gave the same x-velocities in 12 of 15 points. In the end the mesh with 57,040 elements was chosen for further simulations Mesh Quality The quality of the chosen mesh was checked. Maximum aspect ratio is 4.13, minimum orthogonal quality is equal to 1 and maximum skewness is CFD Simulation Settings ANSYS Fluent Version 17.1 was used to conduct all the CFD simulations. In all cases, the RNG k- turbulence model was used. This was chosen as a result of the COBEE case 51

61 Group F2P CFD Simulations investigation. The energy equation was allowed as there are several heat sources in the form of machinery. The effect of gravity was considered with gravitational acceleration of 9.81 m/s 2. For air density model the Boussinesq model was considered in the beginning. Since there were problems with obtaining convergence or the calculations of simulations ended up giving different errors, the model had to be disabled and constant density model was used instead. With this density model there were not any convergence problems or errors Boundary Conditions The correct setting of boundary conditions is a challenging part as it can have a significant effect on obtained results. This investigation is considered to be a design stage investigation and it is not possible to obtain any measured data such as surface temperatures. The walls, ceiling and floor are considered to be adiabatic and the temperature of the surfaces was estimated. Ceiling and floor temperature is considered to be 23 C, wall temperature 22 C. Radiation is neglected in the simulations. Therefore the heat flux from all heat sources was lowered to 50% of the considered value (therefore only 50 W/m 2 is used in the simulation). Velocity inlet is characterized with the value of velocity according to the flow rate. Default inlet air temperature is set to 18 C. For outlet, outflow boundary condition is used Variables In the simulations, the flow rate is a variable. Therefore the inlet velocity differs in the simulation settings. In further simulations, the position of the outlet in the room is changed Simulations The simulations were performed with the above mentioned settings. Table 13.2 is giving an overview of conducted simulations. Table Simulations Simulation number [-] Inlet velocity [m/s] Flow rate [m 3 /s] Air change rate [h 1 ]

62 14 Results After conducting the simulations, the results were compared. The main interest was the velocity and temperature in the investigated geometry Velocity Profiles Velocity profiles for several cross-sections were compared. The cross-sections of the investigated room are vertical in five different distances from the inlet wall - 5 m, 15 m, 25 m, 35 m and 45 m. The cross-sections in 15 m and 35 m go through the machinery. Therefore the lines in these graphs for the cross sections start at the height of 1 m. The velocity profiles are shown in the following graphs. The differences in velocity profiles clearly illustrates the different flow rates. 5 Velocity profile for u 0 = 0.14 m/s Height [m] Distance from inlet [m] 5m 15m 25m 35m 45m Figure Velocity profiles in different cross sections for inlet velocity 0.14 m/s It can bee seen that for the lowest inlet velocity, there is not a significant difference in the profiles throughout the whole room. For the second and further cases it can be observed that the jet goes further from the inlet. 53

63 Group F2P Results 5 Velocity profile for u 0 = 0.28 m/s Height [m] Distance from inlet [m] 5m 15m 25m 35m 45m Figure Velocity profiles in different cross sections for inlet velocity 0.28 m/s 5 Velocity profile for u 0 = 0.56 m/s Height [m] Distance from inlet [m] 5m 15m 25m 35m 45m Figure Velocity profiles in different cross sections for inlet velocity 0.56 m/s 54

64 14.1. Velocity Profiles Aalborg University 5 Velocity profile for u 0 = 0.83 m/s Height [m] Distance from inlet [m] 5m 15m 25m 35m 45m Figure Velocity profiles in different cross sections for inlet velocity 0.83 m/s 5 Velocity profile for u 0 = 1.11 m/s Height [m] Distance from inlet [m] 5m 15m 25m 35m 45m Figure Velocity profiles in different cross sections for inlet velocity 1.11 m/s For the higher inlet velocities, higher velocities can be observed in the upper part of the room. 55

65 Group F2P Results 14.2 Temperature distribution The temperature in the room is shown in the following pictures. The temperature is given in Kelvin. The temperature range is limited from the lowest obtained value 291 K to only 305 K to make the temperature difference in clear in the pictures. The black areas within the mesh are areas with temperatures higher than 305 K. Figure Temperature distribution [K] for velocity 0.14 m/s. In the first picture, it can be seen that the temperatures are high in general. The flow rate is low and therefore there are excessive temperatures in the room. In other words, the heat load is high and there is a cooling demand, especially in the right corner near the outlet. Therefore the temperature distribution should be analysed for the other flow rates. Figure 14.7 shows the temperature distribution at an initial velocity of 0.28 m/s. Figure Temperature distribution [K] for velocity 0.28 m/s. Figure 14.8 shows the temperature distribution at an initial velocity of 0.56 m/s. Figure Temperature distribution [K] for velocity 0.56 m/s. Figure 14.9 shows the temperature distribution at an initial velocity of 0.83 m/s. 56

66 14.3. Different Outlet Position Aalborg University Figure Temperature distribution [K] for velocity 0.83 m/s. Figure shows the temperature distribution at an initial velocity of 1.11 m/s. Figure Temperature distribution [K] for velocity 1.11 m/s. It can be seen that higher initial velocities lead to the significantly lower temperature in the room as the heat demand is eliminated due to the high flow rate in the room. However, in the case of higher velocities, it is necessary to check the values of velocity in the occupied zone. If the values of velocity are too high, it can has negative effect on thermal comfort in real case due to occupants experiencing draft. It is necessary to mention that high initial velocities usually require more powerful fans in ventilation system, which usually corresponds with a higher energy consumption. Therefore during the design stage, it is a good idea to investigate the temperature and velocity distribution in the room in order to make the design of the whole system efficient in removing heat demand, meeting the comfort criteria and also lowering the energy consumption of the system Different Outlet Position A small investigation of the outflow position influence was conducted. Two more simulations were carried out with different outlet positions and compared. The same velocity was used for all the simulations m/s. The other settings of the simulation remained the same as for the previous simulations. Table Overview of simulations with different outlet position. Outlet position nr. Description of the position 1 Lower right corner 2 Upper right corner 3 Lower left corner 57

67 Group F2P Results Figure shows the velocity magnitude [m/s] across the room for outlet position 1. Figure Velocity magnitude [m/s] - outlet position nr. 1. Figure shows the velocity magnitude [m/s] across the room for outlet position 2. Figure Velocity magnitude - outlet position nr. 2. Figure shows the velocity magnitude [m/s] across the room for oulet position 3. Figure Velocity magnitude - outlet position nr. 3. For outlet position 1 a short circuit can be observed. In this case, the position is not convenient for obtaining sufficient ventilation in the room. One more simulation was carried out with the outlet in position nr. 3. In this case the higher inlet velocity 1.11 m/s was considered. Figure shows the velocity magnitude with this inlet velocity. Figure Velocity magnitude - outlet position nr. 3 with a higher initial velocity. 58

68 14.3. Different Outlet Position Aalborg University Higher inlet velocity did not result in any change with only a minor difference in the flow pattern. The higher velocity did not solve the problem, as the short circuit in the flow still remains. The problem may be also in the height of the inlet and outlet slots. The situation may be solved by designing slots with smaller height. Furthermore the temperature distribution in the room can be compared for different outlet position. Figure shows the comparison for the same inlet velocity (0.14 m/s) for position 1. Figure Temperature distribution [K] - outlet position nr. 1. Figure shows the comparison for position 2, also with the inlet velocity 0.14 m/s. Figure Temperature distribution - outlet position nr. 2. Comparing these two cross-sections, no significant differences can be seen except near the outlets. With this low inlet velocity, outlet position does not have a major influence on the temperature distribution in the room. Figure and figure show the temperature distribution for outlet in the position nr. 3. The temperature range has been altered as the temperatures far exceed the acceptable range. The temperature range in figure has a full temperature range and figure has a range up to 350 K to clearly illustrate the situation near inlet and outlet. Figure Temperature distribution [K] - outlet position nr

69 Group F2P Results Figure Temperature distribution - outlet position nr. 3, different temeprature range 14.4 Simulation without Heat Sources For the purpose of comparison several simulations were conducted for the same geometry without any heat sources. The settings of the solver remained the same except for the energy equation and gravity effect, which were turned off. However, no significant changes were observed on the results of the velocity between the simulations with and without heat sources. The velocity distribution remained the same and there were only very small (10 9 ) differences in the velocities compared to the case with heat sources. This is an important observation which should be investigated. It may be caused by several problems. Understanding and solving this requires a deeper understanding of the numerical background as well as the computer solver settings. Due to time constraint it was not possible to continue in investigating this in this project as it was discovered at the very end Conclusion In this part the velocities and temperatures in the deep room with heat sources were investigated. The investigation was conducted only for the 2D situation. In real case, the 3D would be preferred. Velocity profiles and temperature distribution in the room were shown for several different inlet velocities. Furthermore the flow with different outlet position was investigated. The results showed that there is a risk of short circuit if the outlet is placed in an inconvenient place. However, it has shown that there is a potential error in the results, as there were problems with correct modelling of the convection. There is no significant difference in values of velocities between simulations with heat sources and without heat sources. This is an important finding which need to be analysed by further investigation. In the beginning of developing the problem, the expectations were much higher. However, during the process several problems appeared - for example, problems with mesh generation or errors in solver caused probably due to some insufficient or incorrect settings. Due to the available time the problem for this part had to be reformulated with comparison of the initial expectations and plans. It has shown that further study of CFD theory and more experience with the solving programmes are necessary abilities for being able to conduct high quality and reliable simulations. 60

70 Part IV Conclusion 61

71 15 Conclusion CFD predictions were made for a deep room, following the guidelines of the COBEE case [Peng et al., 2015], but in this report the predictions were validated with measurements on a box that is manufactured according the similarity principle for the case. For the CFD predictions five different turbulence models were used, the models were as follows: Standard k-, RNG k-, Realizable k-, Standard k-! and SST k-!. The results from the different models varied a lot, in a similar fashion to the results of the COBEE case [Peng et al., 2015]. The measurements were conducted on a box with a different inlet than described in the COBEE case, but it did not make a notable difference according to predictions. Comparing the predictions to the measurements, it was found that RNG k- and had the most accurate predictions. When the most accurate turbulence model had been found, it was used for 3D simulations of the case. Other than the RNG k- model, it was decided to conduct 3D simulations with the Realizable k-, as it according to theory is the best k- model. The RNG k- was again proven the model that best approached the model experiment measurements. In the practical case, the whole process from the develeopment of the case to the evaluation of results was followed. CFD simulations were carried out for a 2D case where heat flux from machinery was included. The main variable was the flow rate. Furthermore the influence of different outlet position on both velocity and temperature distribution was investigated. In the end, a few simulations without any heat sources for the same geometry and conditions were conducted. All the results were compared. It showed a problem with simulation settings. In several cases, there were problems with obtaining convergence and correct setting of the solver. All the results were not satisfying as there was not any significant difference between the simulation with and without heat source. This problem will remain for further investigation. 62

72 Bibliography ANSYS, November Inc. ANSYS. ANSYS Fluent Theory Guide, release 15.0 edition, Bakker, André Bakker. Applied Computational Fluid Dynamics, URL CFD online, CFD online. Online CFD wiki, URL Chungen Yi. Chungen Yi. Introduction to RANS turbulence modeling. Hyldgaard et al., Carl Erik Hyldgaard, M. Steen-Thøde og E.J. Funch. Grundlæggende Klimateknik og Bygningsfysik. Aalborg Universitet, Lutz Angermann, editor. Numerical Simulations - Examples and Applications in Computational Fluid Dynamics. InTech, Michael Brorson, Michael Brorson. Fluid Dynamics Peng et al., November Lei Peng, Peter V. Nielsen, Xiaoxue Wang, Sasan Sadrizadeh, Li Liu og Yuguo Li. Possible user-dependent CFD predictions of transitional flow in building ventilation Trafik- og Byggestyrelsen, Trafik- og Byggestyrelsen. Bygningsreglementet,

73 A Inlet velocity calculations The initial velocities at the inlet serve as the boundary conditions for the 2D and 3D simulations. 2D Model Inlet Velocity The initial x-velocities for the 2D simulations are calculated first. This is done by the use of Reynolds number. The simulations are carried out on Reynolds numbers 5-10,000. Equation A.1 is used. Re = u 0 l (A.1) Where Re Reynolds number [-] u 0 Initial velocity [m/s] l Characteristic length, h or p A i [m] Kinematic viscosity [m 2 /s] An example of how the initial velocity for the 2D simulation is calculated for Reynolds number 10,000 is shown. The characteristic length is the slot height h of 1 m and the kinematic viscosity is m 2 /s = m u 0 1m m 2 /s u 0 =0.151 m/s 64

74 Aalborg University This is repeated for all the Reynolds numbers and gives the results seen in table A.1. Table A.1. The initial x-velocities for the 2D simulations in Fluent dependent upon the Reynolds number with h=1 m. Re [-] u 0 [m/s] e e e e e e e e e e e e e e e e e e-01 These are the inlet velocities used in the 2D simulations. 3D Model Inlet Velocities In order to make a comparison between the 2D and 3D simulations, it is necessary to use the same Reynolds numbers, calculated using the same characteristic length, slot height h. This is a criteria based on the similarity principle. However, as the boundary conditions for the inlet differs between the two models, as described in chapter 8, the x-velocity inserted into ANSYS Fluent must be adjusted according to the model. The object of each 2D and 3D simulation is to maintain the same Reynolds number and the same velocity in the slot. Therefore the flow rate through the model must be identical. The initial velocity of the 2D simulations with the slot as the inlet is known through the equation A.1 for Reynolds number as previously calculated. However, as the 2D model uses different dimensions than the 3D model, the velocities must be adjusted according to a new characteristic length of slot height h to 0.04 m. The velocities with the new characteristic length can be seen in table A.2. 65

75 Group F2P31 A. Inlet velocity calculations Table A.2. The initial x-velocities for the 2D simulations in Fluent dependent upon the Reynolds number with h=0.04 m. Re [-] u 0 [m/s] This enables the calculation of the initial x-velocity in the inlet of the box (3D simulations) through equation A.2. q = u 0 A i (A.2) Where q Flow rate [m 3 /s] u 0 Initial velocity [m/s] A i Inlet area [m 2 ] An example of how the initial velocity is calculated for Reynolds number 10,000 will be shown. First the flow rate is calculated. The initial velocity used for 2D simulations at this Re is m/s. The slot height is 0.04 m and the width of the box is 0.40 m. q =3.778 m/s (0.04 m 0.40 m) = m 3 /s The initial velocity can then be calculated for the 3D simulation when the inlet is set to the box. The height of the box is m. u 0,box = m3 /s m 0.40 m = m/s 66

76 Aalborg University Therefore the initial x-velocity used for the 3D simulations in ANSYS Fluent is m/s. This is repeated for all the Reynolds numbers. The initial velocities used for the boundary conditions for the 3D simulations can be seen in table A.3. Table A.3. The initial x-velocities for the 3D simulations in Fluent dependent upon the Reynolds number. Re [-] u 0 [m/s] However, the initial velocity will not be uniformly distributed throughout the slot for the 3D simulations as it does in the 2D simulations as they have two different inlets. The velocity in the slot for the 3D simulations will be distributed in accordance to the frictional forces alongside the walls. This can be seen in the cross-section of the inlet for the 3D simulation of Re=3000 in figure A.1. The initial velocity at the inlet for the 3D simulation is m/s. Figure A.1. The cross-section of the slot in the 3D simulation of Re=3000. As it can be seen from figure A.1, the maximum velocity in the slot is m/s. This is higher than the initial velocity of m/s for the 2D simulation. However, Reynolds number is based upon the average initial velocity in the profile, and as the flow rate is identical, it is assumed that the average velocity in the slot for the 3D simulations is m/s. Identical Reynolds numbers are therefore ensured throughout the simulations. 67

77 B ANSYS Fluent Input Table B.1 shows the input used in ANSYS Fluent for the 2D and 3D simulations respectively. Table B.1. ANSYS Fluent input for the 2D and 3D simulations. 2D 3D Models std k-, RNGk-, Realizable k-, RNG k- and Realizable k- std k-! and SST k-! Near wall-treatment Standard wall function Enhanced wall treatment Velocity inlet Velocity inlet Inlet Boundary conditions Turbulent intensity 10% Turbulent intensity 10% Outlet Outflow Outflow Walls Walls Walls Scheme Simple Simple Accuracy Second-order Second-order Momentum step 0.3, ,

78 C Near-Wall Treatment of Simulations In order to determine which near-wall treatment to use, simulations were carried out using two different treatments. Here the realizable k- turbulence model was used. The simulations were carried out on the 3D model, as this has the same inlet boundary conditions as the model experiment. Thereby the results are directly comparable. Figure C.1 depicts the dimensionless penetration lengths obtained through the simulations and the model experiment Near-wall Treatment versus Measurements Standard wall function Enhanced wall treatment Measurements x re / (H-h) Re Figure C.1. Expected dimensionless penetration lengths of the simulations using different nearwall treatments compared to the measurements. As illustrated on the figure, the enhanced wall treatment approximates the measurements from the model experiment more so than the standard wall function, in particular in the region 500 < Re < 4, 000. However, the curvature pattern from the standard wall function has a better fit with the measurement. Still, the enhanced wall function is chosen as the best fit for the remaining 3D simulations. It should be taken into account when comparing the simulations with the model experiment, that the dimensionless penetration lengths seem to be estimated higher for Re 5, 000 when using the enhanced wall treatment. 69

79 D Other Measurements Other measurements were conducted to ensure the best set-up and most correct result of the model experiment. This included the investigation of the equipment used. Alternative Set-up A set-up was conducted where a duct connected the smoke machine directly to the inlet box. This was carried out for some of the Reynolds numbers. Results The results from the measurements can be seen in table D.1. Table D.1. COBEE measurement results for penetration length (PL). Reynolds number [-] Measured PL avg. [m] No. of measurements The results from table D.1 vary greatly from the results in table This prompted an investigation of the flow in the two different set-ups. Investigation of Flow in the Box The velocity profile of the inlet was looked into. This was done by measuring the velocity at the inlet where the inlet box is connected to the main box (by the slot), across the width of the box. The velocity profile of the set-up with the smoke machine connected to the inlet box, can be seen in figure D.1. 70

80 Aalborg University Velocity profile for model experiment BW 1.2 BW 4.0 Uniform velocity goal Velocity [m/s] Distance from sidewall [cm] Figure D.1. Velocity profile of the model with the smoke machine connected to inlet box. Figure D.1 shows that the velocity profile is a top hat profile. The velocity also drops at the wall furthest from the laser. The velocity profile at the inlet for the set-up where the smokemachine is not connected directly to the inlet box, as shown in figure D.2, is then investigated. Figure D.2. Model with the back wall of the pressure box removed. The velocity profile of the inlet was measured as previously done. measurements can be seen in figure D.3. The results of the 71

81 Group F2P31 D. Other Measurements Velocity profile for model experiment, open channel with straws Open channel velocity profile Uniform velocity goal Velocity [m/s] Distance from sidewall [cm] Figure D.3. Velocity profile of the model with the inlet box free of the smoke machine. Figure D.3 shows that the velocity profile is very close to be uniform. However it seems that as with the previous measurement, that the velocity dives at a distance of 36 cm which is close to the opposing side wall. This could be because there is a problem with the inlet and can be added to the margin of error. Investigation of Equipment To clarify the margin of error, the equipment is investigated. The first piece of equipment that is investigated is the digital and the analogue manometer. The investigation is conducted using the jet wind tunnel, as shown in figure D.4, as it is not influenced by the outdoor pressure, which causes the flow to fluctuate and makes it difficult to determine the flow with the digital manometer. 72

82 Aalborg University Figure D.4. The jet wind tunnel. The results of the investigation can be seen in table D.2. From the table it can be seen that there is a deviance between the 2 manometers of about 15 %. It was not possible to determine which of the manometers was measuring correctly, as the more precise equipment could not be found due to the lack of paperwork (because of the move of the laboratory). Therefore it was decided to use the analogue manometer because its readings did not fluctuate as much as the digital manometer. Table D.2. Investigation of digital and analogue manometer. Digital manometer [Pa] Analogue manometer [Pa] Deviation [%] An investigation of the lasers validity was attempted but due to filters in the jet wind tunnel, it was not possible to get readings from the jet wind tunnel and the investigation was cancelled. 73