Modelization on a ventilated heat exchanger using Computational Fluid Dynamics

Treball de Fi de Grau Grau en Enginyeria de l’Energia Modelization on a ventilated heat exchanger using Computational Fluid Dynamics Memòria Autor: Ferran Castel Turégano Director: Raul Benítez Iglesias Departament ESAII Ponent: Riccardo Mereu (Politecnico di Milano) Convocatòria: Juliol 2022 2 3 Index Abstract ..................................................................................................................................................................... 6 Introduction ............................................................................................................................................................ 7 1. Case study....................................................................................................................................................... 8 1.1 The Heat exchanger ................................................................................................................................. 8 1.1.1 Drawings of the machine ............................................................................................................ 10 2. CFD Model .................................................................................................................................................... 12 2.1 Description of the problem................................................................................................................ 12 2.1.1 Navier-Stokes equations ............................................................................................................. 12 2.2.1 Turbulence model .......................................................................................................................... 13 2.3 Finite Volume Method .......................................................................................................................... 15 2.4 Numerical solution of the system .................................................................................................... 17 2.4.1 Pressure-Based Solver ................................................................................................................. 18 2.4.2 Residuals ............................................................................................................................................ 18 2.5 Mesh ............................................................................................................................................................. 20 2.5.1 Type of meshing.............................................................................................................................. 21 2.5.2 Calculus domain .............................................................................................................................. 22 2.5.3 Mesh Geometry ............................................................................................................................... 22 2.5.4 Moving mesh approaches............................................................................................................ 27 2.5.6 Building of the mesh ..................................................................................................................... 31 2.5.7 Mesh refinement............................................................................................................................. 37 2.5.8 Number of iterations per simulations ................................................................................... 38 2.6 Setup conditions ..................................................................................................................................... 39 2.6.1 Overall boundary conditions ..................................................................................................... 40 2.6.1.1 Fan approaches ........................................................................................................................... 42 3. Results ............................................................................................................................................................ 46 3.1 Fan model results ................................................................................................................................... 47 3.2 Results of Rotational Reference Frame Approach .................................................................... 51 3.4 Moving mesh ............................................................................................................................................ 54 4. Conclusions .................................................................................................................................................. 57 References ............................................................................................................................................................. 59 4 Figure Index Figure 1. Luve’s Heat Exchanger modulus ..................................................................................................................... 9 Figure 2. Draw of a one singular module ........................................................................................................................ 9 Figure 3. Schematic representation of the air flow in the heat exchanger. .................................................. 10 Figure 4. Finned pack profile............................................................................................................................................. 10 Figure 5. Drawings of the machine ................................................................................................................................. 11 Figure 6. Two plots of residuals values during a simulation............................................................................... 19 Figure 7. Residuals of the simulation ............................................................................................................................ 20 Figure 8. Scheme of a 3D mesh. Source: manchestercfd.uk ................................................................................ 21 Figure 9. Different cell types.............................................................................................................................................. 21 Figure 10. Structured mesh vs unstructured mesh................................................................................................. 22 Figure 11. LuVe’s CAD model of the fan used in the heat exchanger. ............................................................. 23 Figure 12. Cross section view of the fan...................................................................................................................... 23 Figure 13. On the left, the CAD model. On the right, the simplificated geometry ...................................... 24 Figure 14. Geometry shaded representation of the heat exchanger with the fan blades. ..................... 25 Figure 15. Fan model approach geometry. ................................................................................................................. 25 Figure 16. Geometry with inlet and outlet volumes(Fan Model) ...................................................................... 26 Figure 17. Stationary and Rotating Reference Frames .......................................................................................... 27 Figure 18. Drawing of the moving domain in the fan motion ............................................................................. 30 Figure 19. Calculating the Aspect Ratio for a Unit Cube ....................................................................................... 30 Figure 20. Equilateral Triangle (A) and a highly skewed Triangle (B) .......................................................... 31 Figure 21. Vectors used on the calculation for orthogonal quality. ................................................................. 31 Figure 22. Isometric and section view of the mesh ................................................................................................. 32 Figure 23. Cross section view of the fan shroud - Fan model mesh................................................................. 32 Figure 24. The exterior volume and the two bodies of the fan shroud. ......................................................... 33 Figure 25. Shaded elements on the fan blades .......................................................................................................... 34 Figure 26. Borderline of the moving blades and static blades ........................................................................... 34 Figure 27. Cross section of the lower body mesh .................................................................................................... 35 Figure 28. 3D Display of the final mesh ........................................................................................................................ 36 Figure 29. Front view of the mesh. ................................................................................................................................. 37 Figure 30. Plot of mass flow rate vs number of iterations ................................................................................... 39 Figure 31. Inlet surface ........................................................................................................................................................ 40 Figure 32. Outlet Surface..................................................................................................................................................... 41 Figure 33. Fan Curve ............................................................................................................................................................. 43 Figurí 34. Interior wall defined as the Fan Model .................................................................................................... 44 Figure 35. Mesh motion ....................................................................................................................................................... 44 Figure 36. Mesh volume that rotates in the sliding plan simulation ............................................................... 45 Figure 37. Experimental velocity map of the outlet of the heat exchanger. ................................................ 46 Figure 38. Velocity contour on the YX and ZX planes – Fan Model aproach ................................................ 47 Figure 39. Pressure contours on the YX and ZX planes – Fan Model aproach ............................................ 47 Figure 40. Velocity streamlines on the XY plane – Fan model approach....................................................... 48 Figure 41. Velocity contour at the outlet - Fan model approach ....................................................................... 48 Figure 42. Velocity contour on the YX and ZX planes – Rotating Reference Plane approach............... 51 Figure 43. Pressure contours on the YX and ZX planes – Rotating Reference Plane approach ........... 51 Figure 44. Velocity streamlines on the XY plane – Rotational Reference Frame approach .................. 52 Figure 45. Velocity contour at the outlet (465 rpm) – Rotational Reference Frame approach .......... 52 Figure 46. Velocity contour on the YX and ZX planes – Moving mesh approach ....................................... 54 Figure 47. Pressure contours on the YX and ZX planes – Moving Mesh approach ................................... 54 Figure 48. Velocity streamlines on the XY plane – Moving Mesh approach ................................................. 55 Figure 49. Velocity contour at the outlet (465 rpm) – Moving Mesh approach ......................................... 55 5 Table Index Table 1. Explanation of different bodies in the geometry. ................................................................................... 26 Table 2. Mesh quality feature - Fan Model .................................................................................................................. 32 Table 3. Meshing properties of the upper body ........................................................................................................ 35 Table 4. Meshing properties of the upper body ........................................................................................................ 36 Table 5. Final number of nodes and elements in the mesh ................................................................................. 36 Table 6. Mesh Refinement for moving mesh approaches ..................................................................................... 38 Table 7. Values of mass flow rate for increasing values of iterations ............................................................. 39 Table 8. Configuration of the simulation – Rotating Reference plane approach........................................ 44 Table 9. Configuration of the simulation – Sliding plane approach ................................................................. 45 Table 10. Experimental results of the heat exchanger .......................................................................................... 46 Table 11. Resuls of Fan Model .......................................................................................................................................... 49 Table 12. Results of Rotational Reference Frame approach at 850 rpms. .................................................... 53 Table 13. Results of Moving Mesh approach at 850 rpms ................................................................................... 56 Table 14. Results at 850 rpm ............................................................................................................................................ 57 Table 15. Results at 465 rpm ............................................................................................................................................ 57 6 Abstract This work presents the 3D modelization of a finned tube heat exchanger for civil and industrial applications using CFD software ANSYS Fluent 15.0. The analysed heat exchanger is manufactured and distributed by the LuVe group. The work aims to develop a numerical model that can simulate the real behaviour of a real heat exchanger. Consequently, the simulation will be compared with the provided experimental data to verify the correct function of the model. The simulations will be performed using two different approaches; the first will be executed using the fan model feature and the second one using two different moving mesh method. This numerical model will subsequently be used to study and improve and optimize the performance of the machine, evaluate different plenum geometries, analyse the levels of sound and vibrations, and plenty of valuable parameters. Key words: Ansys Fluent, numerical modelization, fan model, moving mesh 7 Introduction This work aims to study and define the fluid Dynamics of a heat Exchanger provided by LuVe group, a top-ranked Italian enterprise that produces heat exchangers for both residential and industrial purposes. The analysis will be carried out through Computational Fluid Dynamics (CFD). Computational science is a multidisciplinary domain, based on the idea of computational thinking which allows to create a simplified abstraction of reality and to describe and understand it better, by representing a phenomenon in a computer-based mathematical language. A model describes, classifies, but mostly understands, predicts, and controls the understudied phenomena. Once it is specified, one needs to program it, run it and study the results. These simulation technics have deepened our understanding of fluid behaviour. Applied to heat exchangers, simulations can be obtained to evaluate the performance of the machines without needing to execute time and money-consuming tests. In fact, with CFD analysis, valuable data such as volume flow, pressure drops in critical areas and amount of energy exchanged between the two mediums, can be collected with tremendous accuracy. Moreover, when a reliable model is achieved it permits to conduct of optimization features, for instance, modification the geometric parts of the machine to reduce pressure drop while increasing heat capacity without decreasing efficiency. In this case study, the setting of the model, simulation and analysis will be made with the commercial software ANSYS Fluent 15.0. Given a LuVe manufactured axial heat exchanger, the scope of the work is to build a numerical number that emulates its physical properties. The validation of the model will be done by comparing the results with experimental data provided by the producer. Regarding the simulation, there will be two different approaches: one using the Fan Model Ansys-Fluent feature and the other one using the moving mesh method. 8 1. Case study A heat exchanger is an equipment in which the exchange of thermal energy is carried out between two fluids. By virtue of the first principle of thermodynamics, the bodies must be at different temperatures in order for there to be transfer of thermal energy from one of these compartments to the other, for which they are defined as a hot side (where the fluid having a higher temperature flow, to be cooled) and a cold side (where the fluid having a lower temperature flow, to be heated). The studied machines can be classified as indirect contact surface exchangers: the fluids do not come into direct contact with each other but are separated by a surface which is crossed by the thermal flow. The way of exchanging energy varies on each technology. There are many typologies of heat exchangers available in the market for different purposes; they are used both in industrial and commercial refrigeration as well as for civil applications such as air conditioning. In the case study, the two mediums exchanged are gas and liquid, accordingly, the best technological solution is the finned tube heat exchanger. It operates with air and a refrigerant that easily shifts to liquid and gas. Thanks to this principle heat exchange can occur and it is able to move heat from some place to another, as the refrigerant transmutes from liquid to gas and back. The work is dedicated to the study of the service fluid, therefore to the modelization of the motion of the air inside the machine and its improvement. A greater flow of air in contact with pipes means a great thermal power exchanged between. Although work studies a machine for air-cooling applications, the effect of heat exchange will not be considered because the heat effect on the behaviour of the air within can be neglected because does not have a meaningful effect on the air dynamic. 1.1 The Heat exchanger The studied exchanger has an axial fan and are commercialised in packed modules, depending on the total cooling power required, as shown in Figure 1. Yet, the study will be done on a singular one. The schematics of the singular module are shown in Figure 2. 9 Figure 1. Luve’s Heat Exchanger modulus Figure 2. Draw of a one singular module The functioning of the system is very simple: a fan absorbs outer air and pulls it towards the coil where the liquid refrigerant is circulating and passes through the machine until exiting through the outlet. The heat exchange keeps occurring while the airflow is kept. The refrigerant circulates within the tubes in the coil, is cooled by the air and heads back to the expansion valve to restart the thermodynamical cycle. This process is schematically described in Figure 3. 16 get all the accurate results. In fluid dynamics, one of the most used methods is the Finite Volume Element. With this method, the system is discretised and subdivided in small volumes(control volumes or cells); therefore the equations of motion and continuity are applied in integral form to each of them, obtaining as much equations as volumes are in the system. In that way, the program will not treat the heat exchanger, but instead, as a mesh of small volumes mounted together that emulate its shape. The following differential equations, written in a general way where 𝜙 is a general scalar magnitude, such as velocity or pressure, are presented to illustrate this method: 𝜕(𝜌𝜙) 𝜕𝑡 +∇·(𝜌𝒖𝜙)=∇·(Γ∇𝜙)+𝑠 (15) Where Γ is the transported property and s is the source term. This happens at any point of the fluid, but as said before, it is needed to translate equation 15 into the integral form for a generic control volume V: ∫[𝜕(𝜌𝜙) 𝜕𝑡 +∇·(𝜌𝒖𝜙)−∇·(Γ∇𝜙)−𝑠 𝑉] 𝑑𝑉=0 (16) Then, as every cell is touching with another, the Gauss theorem is applied with the A surface of the volume V, to take into account the influence of every adjacent cell: ∫𝜕(𝜌𝜙) 𝜕𝑡 +∫𝜌𝒖𝜙·𝑛 𝑑𝐴=∫Γ∇𝜙·𝑛𝑑𝐴 𝐴 𝐴𝑉 =∫𝑠 𝑑𝑉 𝑉 (17) Approximating the integral calculus to a numerical approach, the equations follow as: 𝜕(𝜌𝜙) 𝜕𝑡 𝑉+∑𝑝𝑓𝑢𝑓·𝑛𝑓𝜙𝑓𝑠𝑓 𝑛𝑓 𝑓=1 =∑𝜇𝑓(∇𝜙)𝑓·𝒏𝑓𝑠𝑓 𝑛𝑓 𝑓=1 +𝑠𝑉 (18) Equation 18 refers to the unknowns’ magnitudes 𝜙 at the center of each cell. But are the scalar value variables 𝜙𝑓 the unknowns to be evaluated in each face of the volume in order to get the final magnitude for the cell. For doing this, it has been used the second order upwind procedure that goes as follows; the value of 𝜙𝑓 is derived in the normal direction of the velocity. Then the quantity 𝜙𝑓 is 17 calculated through a Taylor development of the general magnitude 𝜙 around the center of the cell. 𝜙𝑓,𝑈𝑃𝑆= 𝜙+∇𝜙·𝒓 (19) Where 𝜙 is the magnitude value at the centre of the cell and r is the vector referred to the centre of the cell and points upwind to the centre of the face. The gradient is made by Green-Gauss Theorem, hence approaching the gradient of the cell with the midpoint rule: (∇𝜙)0≅1 𝑉∫∇𝜙𝑑𝑉 𝑉=1 𝑉∫𝜙𝒏𝒇𝑑𝑆𝑓 𝑆𝑓=1 𝑉∑ϕ  𝑛𝑓 𝑓=1 ·𝑛𝑓𝑆𝑓 (20) where (∇𝜙)0 is the gradient at the center of the cell, while 𝜙 is the value of 𝜙 at the center of the cell calculated by the Green-Gauss Node-Based method. The magnitude 𝜙is calculated as the average mean of the node components of the face and the node values 𝜙𝑛are build through the average of the values in the center point of the cell around the node: 𝜙=1 𝑁∑𝜙𝑛 𝑛 (21) The construction of the gradient is necessary not only to get the value in the centre of the face 𝜙𝑓, but also to calculate the diffusion terms in the equation of conservation of motion, typically in the pressure gradient. 2.4 Numerical solution of the system The algorithm of resolution of the Navier-Stokes discretised equations are solved by a segregated approach. The functioning of this solver is sequential; it solves all the motion equations separately in an iterative way to reach a converged solution. The convergence is reached when the changes in solution variables from one iteration to the next are negligible and overall property conservation is achieved. In CFD software the resolution process carries out the following steps [2]: 1- Update the fluid properties depending on the results of the current iteration. For the first iteration, the initial conditions are used and an approximate initial guess is made 18 2- Solving of the motion equations using the current pressure values. 3- If step number 2 does not satisfy continuity, the pressure is rectified with a formula. 4- Recalculate velocity using the corrected pressure value. 5- Solve the equations for the scalar quantities such as turbulence motion using the actual values of the variables. 6- Verify convergence; if reached follow to next step, if not, rectify pressure values again until reached. 7- Advance to the next time. These steps are repeated until satisfying convergence criteria of the solution. 2.4.1 Pressure-Based Solver There are to main different approaches available to solve and operate flow conditions, the pressure-based approach, which was developed for low-speed incompressible flows and the density-based approach which is mainly used for high-speed compressible flows. In the case study the pressure-based solver will be used as the model is accurate enough even though the air is treated as incompressible. In the pressure field is extracted by solving a pressure or a pressure correction equation which is obtained by manipulating continuity and momentum equations. This solver employs an algorithm which belongs to a general class of methods called the projection method. In the projection method, the constraint of mass conservation (continuity) of the velocity field is achieved by solving a pressure (or pressure correction) equation. The pressure equation is derived from the continuity and the momentum equations in such a way that the velocity field, corrected by the pressure, satisfies the continuity. Since the governing equations are nonlinear and coupled to one another, the solution process involves iterations where in the entire set of governing equations is solved repeatedly until the solution converges. 2.4.2 Residuals The residual is one of the most fundamental measures of an iterative solution’s convergence, as it directly quantifies the error in the solution of the system of equations. 19 In a CFD analysis, the residual measures the local imbalance of a conserved variable in each control volume. Therefore, every cell in your model will have its own residual value for each of the equations being solved. In an iterative numerical solution, the residual will never be exactly zero. However, the lower the residual value is, the more numerically accurate the solution. For CFD, RMS residual levels of 1E-4 are considered to be loosely converged, levels of 1E-5 are considered to be well converged, and levels of 1E-6 are considered to be tightly converged. For complicated problems, however, it's not always possible to achieve residual levels as low as 1E-6 or even 1E-5. [3] In an iterative numerical solution, the residual will never be exactly zero. However, the lower the residual value is, the more numerically accurate the solution. Since they don’t have physical meaning, the only thing it is wanted from them is to be steady. When a simulation starts diverging, so do the residuals too. This phenomena can be seen in the figure 6 below: Figure 6. Two plots of residuals values during a simulation. The oscillations on the graphic on the left indicate that the variables on the simulation have a high variability, therefore this simulation will unavoidably result in false solution, nonetheless, the right-hand graph does converge as the residual values decrease at every iteration. The residuals that are to be studied in the simulation are the velocity components, the mass flow continuity and k and epsilon values. 20 Figure 7. Residuals of the simulation 2.5 Mesh As explained in the chapter 4.2, a mesh which splits the domain into a discrete number of elements is create for which the solution can be calculated. This process is very important in CFD analysis because the accuracy and stability of the calculus are highly dependent on the quality of the mesh, its density, distribution and order will have a significant influence on the degree of precision of the solution. By understanding the physics of the system that is to be analysed, it can be decided whether some features and details of the geometry can be removed or simplified prior to meshing because the more complex the model is, more elements and more nodes will be analysed, increasing the computational weight required to do so. This is one of the most complex procedures of CFD software and it is one of the most timeconsuming phases of the modelization. Due to the two different ways to simulate a fan done in this work, there will be two different meshes. As mentioned before the mesh divides a geometry into many elements which are used by the solver to construct volumes. The cell is the control volume into which the domain is broken up. Each cell edge is jointed to another by nodes and the outer faces of the mesh are called boundaries. 21 Figure 8. Scheme of a 3D mesh. Source: manchestercfd.uk 2.5.1 Type of meshing There are different control volumes that can be used to build a mesh, depending on the geometry. Due to the different shapes, two big groups can be identified, the structured and unstructured mesh. Figure 9. Different cell types. In Figure 7 are depicted the different volumes used in meshing techniques. Structured meshing uses hexahedron volumes that allow easy nodal neighbour connectivity, which simplifies computational operations, converge well and give accurate results. Alas, they cannot be used in complex geometries, whereas unstructured meshing uses tetrahedral, hexahedral and polyhedral volumes and can accommodate completely to arbitrary geometries. However, the generation of such mesh are very complex and so is the computational effort required to solve them due to the large number of operations per node. 22 Figure 10. Structured mesh vs unstructured mesh The choice of whether to use structured or an structured meh is very problem specific. Depending on the shape of each body belonging to the geometry it will be used on or another. 2.5.2 Calculus domain The domain is composed by the physical volume of the heat exchanger and external ensembled parts at the enter and exit of the machine to simulate the environment. These extra extensions are important in order to study the air behaviour. These regions will be treated with atmospheric pressure conditions. In CFD, meshes have cells anywhere the studied fluid is passing through. Keeping that in mind, those zones where there is a physical object will in fact be a void in the mesh. The walls of the machine will also be treated specially, but this will be explained on the setup of the simulation. 2.5.3 Mesh Geometry To build a mesh first it is needed build a geometry which Ansys Fluent can read and process. The file type is called STEP and will be done with SolidWorks. This file will be a faithful representation of the geometry of the exchanger. The drawings of the machine are shown in Figure 5, back in chapter 1.1.1 of this work. The geometry will be traced upon these dimensions and a CAD model of the ventilator provided by LuVe using Solidworks features and 3D modelling techniques. The finned tubes will be simplified and treated as solid block that comes after the plenum because in the simulation there is no going to be heat exchange plus it would add an extra complexity to the geometry. In order to simulate the coil, in the simulation this zone will be treated as a porous zone, which will create an equivalent air resistance as the coil. 23 Figure 11. LuVe’s CAD model of the fan used in the heat exchanger. In the figure 9 is shown the CAD model. As it can be seen, there are things that can be erased and simplified because they have no relevance in the air behaviour, such as the corporative letters on the outer part of the fan or the nail holes. In addition, the small metallic net at the inlet has no other but a protective purpose of the fan, so not putting it does not have big effect on the air dynamics. Figure 12. Cross section view of the fan 24 The procedure to generate the geometry has been the following: 1. Open the CAD model in SolidWorks. Draw the profile of the fan seen in Figure 8 and revolve it 360º upon the axis to get a body that fits and overlaps the fan shroud shape. 2. Subtract the static and moving blades to the previous body in order to create the surfaces of the blades. 3. Completely eliminate the previous CAD file parts so that the . 4. Divide the fan shroud in two bodies because that the upper part is the one that will be moving by creating a plane between them . 5. Extrude a prism shaped form that resembles the plenum and the coil using the dimensions on the drawings, edges included. 6. Differentiate the different parts of the rectangular body, having the plenum, the porous zone and exit part, using planes and splitting the before mentioned bodies. 7. Add an extra volume on the enter and the exit part of the air to see the behaviour of the air while entering and exiting the machine. For the fan model approach, step 2 is skipped, and a void cylinder is created in the middle of the fan shroud to emulate the fan, the reason of this step is because the fan model approach in Ansys creates a homogeneous velocity profile that is not realistic. This will be further explained in the next chapter. The result of the fan shroud geometry can be seen in Figure 9. Even though in the figure the fan can be seen, notice that the fan shroud is solid volume with blade-shaped voids where the air cannot pass that represent the fan. Figure 13. On the left, the CAD model. On the right, the simplificated geometry 25 The whole heat exchanger’s geometry is presented below: Figure 14. Geometry shaded representation of the heat exchanger with the fan blades. Figure 15. Fan model approach geometry. Figure 14 is the geometry used in the moving mesh approach and Figure 15 will be used in the Fan Model approach. Colours are used in Figure 15 to differentiate the parts on the machine: blue and brown are the fan shroud, pink is the plenum, green is the coil with the tubes, and purple is the exit part. 32 As the geometry is continuous and mostly rectangular, structure mesh can be done in all the bodies that form it. Consequently, the meshing will be consistent of hexahedrons of different element size. Figure 22. Isometric and section view of the mesh Even though the curves and shape of the cylinder might have resulted in unstructured mesh, Fluent software manages to do it in a structurally way as seen in the Figure bellow. Figure 23. Cross section view of the fan shroud - Fan model mesh Table 2. Mesh quality feature - Fan Model Mesh Quality – Fan Model Number of elements 463.768 Average Skewness 0,0882 Orthogonal Quality 0,9177 33 Moving mesh approaches – Upper part For the two moving mesh approaches it is need to develop a thinner mesh. The upper part of the heat exchanger is conformed by 3 bodies. These bodies have curves and circular parts which are difficult to geometrise with hexahedrons. Besides, it has the fan and the stator blades. The curvature and profile of the blades make it impossible to create a structured mesh. When dealing with such shapes, a high number of elements is required, hence the density of elements in these areas is much higher than others to fit the curvature while accomplishing the minimum mesh quality requirements. Figure 24. The exterior volume and the two bodies of the fan shroud. The before-mentioned phenomena can be seen in the shaded parts of Figure 18. In this figure are the 3 bodies displayed in different colours; green is the exterior volume, grey the moving blades and brown the static blades. The dark zones have a high density of tetrahedrons to fit the blades of the fan and the outer volume. Note the definition difference between the outer volume and the fan shroud occurs because the entering air does not have as much importance as than the fan itself. That is caused by the element size chosen in each body A shaded vision of the meshed blades is presented below. 34 Figure 25. Shaded elements on the fan blades Meshing the blades has been the most difficult and laborious part to mesh by far and it has required a lot of computational power and time because in this body there are 467.636 elements. Figure 26. Borderline of the moving blades and static blades In Figure 26 there is a change in the element body, being grey the moving blades and brown the static blades, both belonging to the fan shroud. 35 Table 3. Meshing properties of the upper body Exterior volume Fan shroud – moving blades Fan shroud – static blades Typology Tetrahedrons and prisms Tetrahedrons Tetrahedrons Element size 60 mm 35 mm 50 mm Curve element size 5 mm 5 mm 5 mm Number of elements 173.624 467.636 756.449 Number of nodes 33.378 89.656 143.680 Building of the mesh– Lower part The lower part of the machine is also composed by three bodies: the plenum, the coil and the exterior volume. Even though the plenum has a chamfer, the overall regular prismatic geometry shape allows us to develop structured meshing in these zones. Subsequently, the following mesh will mostly be formed by hexahedrons. Figure 27. Cross section of the lower body mesh The difference between the two parts is remarkable as the meshing process has managed to do structured and regular cells. In Figure 21 the bodies are depicted with different colours; yellow is the plenum, light green is the coil and blue is the outlet external volume. 36 Table 4. Meshing properties of the upper body Plenum Coil Outlet exterior volume Typology Hexahedrons and Tetrahedrons Tetrahedrons Element size 60 mm 35 mm 50 mm Number of elements 89.352 16.992 24.300 Number of nodes 97.850 19.800 25.949 Final mesh Table 5. Final number of nodes and elements in the mesh Number of nodes Number of elements Upper body – unstructured mesh 266.714 1.397.709 Lower body – structured mesh 143.599 130.064 Total 410.313 1.528.353 By looking at table 4 it is seen that the unstructured mesh has far more elements because the non-homogeneous form and complex shapes. Figure 28. 3D Display of the final mesh 37 Figure 29. Front view of the mesh. This mesh has the quality requirements and can be used in fluent simulations. 2.5.7 Mesh refinement To make sure that the definition of the mesh is accurate enough in a CFD simulation it is necessary perform a sensitivity analysis so that it makes sure that the generated mesh is not getting a false solution but that is near to the true one. One would say that a fine grid would give always more accurate results than a coarse grid. Nevertheless, this comes at the cost of larger grid generation and computing time, as well as an increasing cost of computational requirements. Therefore, it is needed to understand to what extent does an improvement of the resolution of the mesh imply an improvement of the result and if it is worth the beforementioned computational cost. To know where the break-even point where the mesh is sufficiently fine enough to be optimal in terms of computational resources and precision a Grid Convergence Study (GDC). This study conducts a systematic meshing exercise where a series of grids are generated within different criteria of resolution, at least at three different levelscoarse, medium, and fine. GCS is based on the fundamental principle that with the increase in fineness of grids, the spatial discretization errors will asymptotically approach to zero and thereby helping to 38 achieve a grid-independent solution. What this means is that the solution is independent of the mesh resolution and any further refinement is not going to improve the solution. A widely used method is the Roache method where meshes with different resolutions are generated for the study and simulations are done on each one. The parameters of interest are plotted against the grid size and when the delta change in the solution come small, one can pick the smallest mesh which gives a grid-independent solution for routine production runs. Below are the results of the refinement for the two different meshes. In this study, 4 different meshes has been used to determine the final mesh to be used. Table 6. Mesh Refinement for moving mesh approaches Mesh elements Mass Flow inlet (kg/s) Mass flow outlet (kg/s) Average mass flow (kg/s) Mass flow difference(%) 1.094.817 8,8411 8,8410 8,8411 1.397.309 8,7494 8,7492 8,7493 -1,05 1.633.055 8,7688 8,7688 8,7688 0,22 2.006.589 8,7527 8,7525 8,7526 -0,19 Upon the results it is decided to use the 1.3 M elements mesh because it Is considered to give the best ratio between computational time and the error in the mass flow rate. 2.5.8 Number of iterations per simulations In the same way that happens with the mesh, in steady-state simulations, an study is carried to know when the simulation converges because at some point, the error in the simulation will decrease and will no longer depend on the number of iterations. Hence, knowing at which number of iterations the simulation converges will result in a quicker simulation time and a diminution of the computational resources required for compiling the program. This study is conducted for the Rotational Reference Frame Approach with the previous mesh. 39 Table 7. Values of mass flow rate for increasing values of iterations Figure 30. Plot of mass flow rate vs number of iterations From the figure 30 it can be observed that at 1500 iterations the mass flow rate starts fluctuating 2.6 Setup conditions Tt has been used the commercial software ANSYS Fluent 15.0 to conduct the simulations. In this chapter the configuration of the simulation is described and explained. The problem has been considered in steady state for the fan model approach and as a timedependent state for the moving mesh approach. Nevertheless, they have both configured as a 𝑘−𝜀 RNG model which is suitable to work with flows with big pressure gradients, bends, and rotations. 40 2.6.1 Overall boundary conditions Every problem in fluid dynamics must be solved by imposing initial and boundary conditions. Those are the values of the variables such as pressure and velocity of the air that are specified for the simulation. Is from this conditions that the software can then calculate how the variables are developed inside our system. The boundary conditions will be specified for each approach are presented in the following chapter. The only things that change between approaches is how the fan is tr Flow Inlet and intake Fan The inlet of the fan will be defined as a Pressure Inlet which demands for a specification of static pressure. This value is set to 0 Pa to have an effective difference in pressure between the inlet and the outlet and to simulate an air inlet at atmospheric pressure that does not create any velocity on the fluid. The inlet surface will be the disk on the fan shroud as shown below: Figure 31. Inlet surface Flow Outlet The oulet will be defined as a Pressure Outlet and set to 0 Pa for the same reason as before, it is wanted to create an atmospheric boundary condition so air passes through the machine thanks to de depression created by the fan. 41 Figure 32. Outlet Surface Wall Due to the relative viscosity between the fluid and the solid wall is zero; no-slip condition is considered for viscous fluids: 𝑢|𝑤𝑎𝑙𝑙=𝑉𝑤=0 (30) where 𝑉𝑤 is the wall’s velocity. If the walls are not moving then the fluid velocity is zero. Modelization of the coil In the same way as done with the fan, the simulation of the coil and the tubs with the aluminium finned profile adds too much complexity to the simulation and it is out the main scope of the work which is to study the air dynamics. What it has been done to maintain the coil effect is to treat this zone as a porous zone, so that, in the volume part where exists the coil, the fluid will suffer the equivalent resistance and therefore a diminution on its motion. In the body where resides the battery, a condition of Porous media zone is applied. Since the physical volume that blocks the fluid is not present in the model, by default Fluent uses a superficial velocity inside the porous medium, based on the flow rate, to ensure continuity to the velocity vectors on the interface of the porous. The porous medium is modelled by adding a source term to the equations of motion: 𝑆𝑖=−(−𝜇 𝛼𝑣𝑖+𝐶21 2𝜌|𝑣|𝑣𝑖) (31) Where 𝑆𝑖 is the source term for any direction. The first term with the coefficient 1/𝛼 represents the viscous loses while the second coefficient indicates 𝐶2 the inertial loses. 48 Figure 40. Velociy streamlines on the XY plane – Fan model approach Figure 41. Velocity contour at the outlet - Fan model approach 49 Table 11. Resuls of Fan Model As this approach is based on the pressure vs velocity curves, it is only possible to obtain the equivalent values for a rotation velocity of 850 rpms, we would otherwise need to conduce a fan study at the desired rpms to get them. It can be said that given the fan curve, the fan model has managed to find the equivalent working point of the system as the mass flow rate is very accurate. The fan pressure jump can be seen on Figure 37 right after the inlet, that is where the fan surface is imposed. It can be seen how the fan model operates; it generates a pressure jump in the fan shroud that creates the motion. Watch that the depression generated by the fan is depicted in blue and then the pressure raises again in yellow right after the surface. By looking at the table values, this pressure jump is of 110 Pa. It can also be seen how the pressure raises when the air collides with the battery that it has been treated as a porous media that creates resistance to the airflow. By looking at Figure 36 and the streamlines on the right picture of Figure 38 it can be seen how the air develops in this approach; it enters the inlet with high velocity and linearity and slows downs as he travels through the plenum. Note that some turbulence happens in the centre of the plenum because the surface simulating the fan is empty at the centre, so there is no velocity input there and the air is dragged towards it because the depression generated at the plenum. Geometry Fan model Mass Flow rate (kg/s) 8,54 Entrata mezzo [Pa] 73.2 Entrata Plenum [Pa] 39.02 Before Fan [Pa] -76.82 Right after Fan [Pa] 39.08 50 This phenomenon is also related to the donut shape of the velocity contour at the outlet; the air movement generated by the fan surface is what causes this contour. This approach generates a very smooth velocity profile. Nevertheless, this is not an accurate approach as the lack of rotational motion results in a loss of information. In addition, the air in a fan does not behave like this as the velocity is higher on the walls because of the shape of the blades, the air is too laminar, hence this approach is not faithful to reality. 51 3.2 Results of Rotational Reference Frame Approach Figure 42. Velocity contour on the YX and ZX planes – Rotating Reference Plane approach Figure 43. Pressure contours on the YX and ZX planes – Rotating Reference Plane approach 52 Figure 44. Velocity streamlines on the XY plane – Rotational Reference Frame approach Figure 45. Velocity contour at the outlet (465 rpm) – Rotational Reference Frame approach 53 Table 12. Results of Rotational Reference Frame approach at 850 rpms. For the two moving mesh approaches, two simulations have been performed: one at 465 rpm and another at 850 rpm. The figures of the velocity and pressure contours of the heat exchanger will be displayed when the fan moves at 850 revolutions per minute. Regarding the experimental data, it has only been provided the velocity map, therefore the contours of velocity at the outlet will be displayed for the simulations at 465 rpms. This will be used to validate the numerical model. In this approach, the mass flow rate is the same as the experimental result. The fan generates the pressure jump progressively as the air gets closer to the fan blades as can be seen in Figures 41, where the dark blue zone just before the fan indicates the most negative pressure and right before in red, there is the pressure rises at its most. Although this is a steady state approach and therefore a time averaged solution, there is high resolution on the air motion as the velocity is not uniform, it raises at the walls and so does the pressure. The pressure jumps is of 95 Pa which is very close to the 98 Pa working point. In the plenum it can be seen how the pressure when colliding with the coils, being the stronger parts at the wall and lesser at the centre. Geometry Pressure values (Pa) Mass Flow Rate (kg/s) 8,7493 Entrata mezzo 63,78 Entrata Plenum 51,3545 Before Fan -53,3986 Right after Fan 42,21 Pa 54 3.4 Moving mesh Figure 46. Velocity contour on the YX and ZX planes – Moving mesh approach Figure 47. Pressure contours on the YX and ZX planes – Moving Mesh approach 55 Figure 48. Velocity streamlines on the XY plane – Moving Mesh approach Figure 49. Velocity contour at the outlet (465 rpm) – Moving Mesh approach 56 Table 13. Results of Moving Mesh approach at 850 rpms The outlet velocity profile is very similar and validates the numerical model. The obtained contour has a circular red shape in the points where the air is travelling at its highest velocity. The mass flow rate error is less than a 0,25%. In the velocity contour it can be seen how the velocity is at its highest on the outer part of the blades and this is a sign of the accurateness of this model as the rotational information of the forces and drags generated is preserved. Geometry Pressure values (Pa) Mass Flow rate (kg/s) 8,65 Entrata mezzo [Pa] 61,58 Entrata Plenum [Pa] 49,375 Before Fan [Pa] -55,46 Right after Fan [Pa] 42,21 Pa 57 4. Conclusions Table 14. Results at 850 rpm 850 rpms Manufacturer data Fan model Rotational reference frame Sliding planes Mass Flow rate (kg/s) 8,59 8,54 8,72 8,75 Pressure Jump [Pa] 98 110 102 96 ε mass flow rate [%] - 0,58 1,51 1,65 ε Pressure Jump [%] - 12,24 4,08 2,04 Table 15. Results at 465 rpm 465 rpms Manufacturer data Rotational reference frame Sliding planes Mass Flow rate (kg/s) 4,70 4,72 4,72 Pressure Jump [Pa] 32 34,8 34 ε mass flow rate [%] - 0,43 0,43 ε Pressure Jump [%] - 8,75 6,25 Given the results, the model has been validated and the best approach is the Sliding Plane. This approach matches the outlet velocity map, gives the less error in mass flow rate and is the only approach that calculates all the forces within the rotation. Three different vortexes are observed on the velocity streamlines on the moving meshes approach: two on the corners of the plenum and one in the middle. The explanation of the two vortexes of turbulence generated at the corners is that on steady state and because of the square shaped geometry, the air direction is not able to pass right forward through the plenum and coil, but it is dragged to the corner because of the air expansion due to the geometry. Therefore, as the fan continues to spin, the air particles that are collision on the corners generates this turbulence that is at some point positive, because the air is not more dragged to the wall and it allows the air that keeps entering the exchanger to pass right through the middle. This is an important thing to keep in mind when trying to optimise the geometry of the machine as increasing or decreasing this effect might lead to improving the overall performance.