Computational Fluid Dynamics modeling of a Water Flow Over an Ogee Profile

Transcription

1 FINITE ELEMENT METHOD TECHNICAL REPORT Computational Fluid Dynamics modeling of a Water Flow Over an Ogee Profile ANSYS CFX 12 ENME 547 Dr. Sudak Matias Sessarego Written Report Due Date: Friday December 10 th 2010 Date of Presentation: Friday November 26 th 2010

2 Abstract A consulting company named Canadian Projects Limited is sponsoring a team in the Mechanical Engineering Design Methodology and Application course (ENME 538) to investigate the flow pattern overtop of an Ogee profile, which will subsequently encounter the Very Low Head (VLH) Water Turbine. The team will be conducting experimental tests using the flume located at the Civil Engineering building with an Ogee profile fabricated from the Rapid Prototyping machine. A computational model of the flume and the rapid prototyped Ogee part has been made using ANSYS CFX to provide results that could be used to compare with or reinforce the results obtained from the experiment. Two approaches for meshing the model have been performed, and their results are compared. One approach involves using mesh refinement techniques, and the other does not, only a general volume mesh. The results obtained from using the mesh refinement techniques are much more rewarding. Flow circulation occurs on the back side of the Ogee, and the boundary layer on top of the Ogee surface is very well defined. The flow circulation is non-existent in the general volume mesh, and the boundary layer is thick and imprecise. For the moment, the most useful model for the VLH project is the one which the mesh refinement techniques were implemented, as it is more consistent with computational models of a very similar problem made from researchers [7] who have not used ANSYS CFX. Future improvements should be made to the CFX model, especially with the boundary conditions used. For example, the Free Slip Wall boundary condition set for the side walls of the CFX model should be changed such that they replicate the plexiglass walls on the flume, and the top of the CFX model should act as a free surface. Page 2

3 Introduction Canadian Projects Limited (CPL) is a consulting company who specialize in renewable energy development. Some examples of their projects include hydro, wind, bioenergy and solar. They are currently the sponsor for the Optimization of Very Low Head Water Turbine for Cold-Climate Conditions project in the Mechanical Engineering Design Methodology and Application course (ENME 538). Wes Dick, an employee of CPL, has asked the student team working on this project to answer a series of questions regarding a water turbine prototype that is currently being used in Millau, France. Companies such as Coastal Hydropower Corporation are currently interested in incorporating this new water turbine into potential sites in Canada. The designers of the water turbine, MJ2 Technologies, have named this turbine the VLH. VLH stands for Very Low Head. The VLH has a Kaplan runner, with a diameter between 3.55 m to 5.6 m and 8 adjustable blades. The magnet generator is located at the center of the turbine and runs directly from the shaft. The advantage of the VLH is its ability to be installed wherever civil infrastructures are already in place. For example, dams, weirs and canals. This reduces the cost considerably in comparison with other small hydro concepts, which require expensive civil work. Fig. 1 VLH Turbine installed in Millau, France. However, civil infrastructures such as weirs and dams have water flowing overtop of essential geometries integrated into them. Examples include the Carseland, Lock 25, and the Step profiles. The names of the Carseland and the Lock 25 profiles were derived from the locations where these geometries are situated. The Lock 25 profile is defined by the third order Bézier curve and is related to the gravitational constant. This particular profile is also known as the Ogee profile. One of the questions that the CPL sponsor has asked the student team to study was the effect of these different upstream geometries on approach flow leading up to the VLH. Page 3

4 Fig. 2 Side view schematic of the VLH and the different upstream geometries The focus of this report is to determine an approximation of the flow pattern across the Ogee profile using the computational fluid analysis capabilities of ANSYS CFX. Using this model, the team will have some insight as to how the flow pattern across the Ogee can affect the efficiency and performance of the VLH. The differences between two approaches of meshing the domain and their results will be analyzed. The geometric model made in ANSYS CFX will be based on the dimensions of the water flume located at the Civil Engineering building at the University of Calgary. The reason is because the team will be conducting experimental tests using this flume and an Ogee profile manufactured from a Rapid Prototyping machine. The team is interested in supporting the experimental results with results acquired from Computational Fluid Dynamics software. Fig. 3 Water flume located at the Civil Engineering Building Computational Method of ANSYS CFX ANSYS CFX is a computational tool commonly known as Computational Fluid Dynamics (CFD). CFD can be used to solve or model fluid flow and heat transfer problems. ANSYS CFX solves fluid flow problems by using the unsteady Navier-Stokes equations in their conservation form (or divergence form). These partial differential equations are shown Page 4

5 below in Cartesian coordinates for a compressible Newtonian fluid. Note that SM is the momentum source and ф is the dissipation function. Table 1 Governing Equations of Fluid Flow for a compressible Newtonian fluid [8] Although these equations are difficult to solve analytically, they can be discretized and solve numerically. This is the basis for the common solution methods that CFD codes use today, including ANSYS CFX. The solution method that ANSYS CFX uses is called the finite volume technique. This technique involves the process of dividing the entire domain into smaller control volumes, where for each control volume the governing equations are solved numerically. As a result, by combining the solutions for each and all of the control volumes, an approximation for variable values at numerous points throughout the entire domain is achieved. Domain and Boundary Physics The first step was to construct the Ogee profile using the Computer Aided Design software, SolidWorks. The model was then imported into ANSYS CFX, and the channel where the water would be flowing was included. Fig. 4 SolidWorks model of the Ogee (left) imported into ANSYS CFX with a channel (right) Page 5

6 After designing the domain and before solving the governing equations describing the water flow over the Ogee profile, many physics and boundary conditions must be inputted into ANSYS CFX. Tables 2 and 3 summarize the domain physics and boundary conditions that were entered in. Table 2 Domain Physics for Ogee Domain Type Location Water Fluid Definition Morphology Buoyancy Model Buoyancy Reference Temperature Gravity X Component Materials Settings Fluid B31 Material Library Continuous Fluid Buoyant 25 [C] 0 [m s^-2] Gravity Y Component -g Gravity Z Component Buoyancy Reference Location Domain Motion Reference Pressure Heat Transfer Model Fluid Temperature Turbulence Model Turbulent Wall Functions 0 [m s^-2] Automatic Stationary 1 [atm] Isothermal 25 [C] SST Automatic A fluid domain type was specified within the region of B31, which is the geometric model of the channel with the Ogee profile in place (as shown on the right figure of fig. 4). For the materials, water was selected from the material library already installed into ANSYS CFX, and for the morphology, a continuous fluid was selected. Water was selected due to the nature of the problem, and the fluid is treated as continuous rather than a dispersed or particle fluid. The effect of employing a buoyancy model is to exclude the hydrostatic pressure in the pressure field for the given problem. When it is activated, the hydrostatic gradient is excluded in the pressure term of the momentum equation. This would result in being able to observe the pressure field solely due to the dynamic component of pressure. The Reference pressure is the datum for all other pressures that will be calculated. Specified Relative pressures are relative to the Reference pressure. The k ω based Shear-Stress-Transport (SST) model was selected due to its accurate prediction of flow separation. It will later be shown what is meant by flow separation in the Results section of this report. ANSYS CFX has also recommended SST turbulence modelling for high accuracy boundary layer simulations, which will be needed to study the boundary layer that will form on top of the surface of the Ogee profile. Page 6

7 Table 3 Boundary Physics for Ogee Boundaries Type Location Flow Regime Mass And Momentum Normal Speed Turbulence Type Boundary Inflow (Fig. 5) Eddy Length Scale Settings INLET inlet Subsonic Normal Speed [m s^-1] Intensity & Length Scale 0.1 [m] Fractional Intensity 0.05 Location Flow Regime Boundary Outflow (Fig. 6) Mass And Momentum Type Relative Pressure Location Mass And Momentum Wall Roughness Type Location Settings OUTLET outlet Subsonic Static Pressure 0 [Pa] Boundary Body (Fig. 7) Settings WALL body, floor No Slip Wall Smooth Wall Boundary FreeWalls (Fig. 8) Mass And Momentum Settings WALL top, wall1, wall2 Free Slip Wall Fig. 5 Fig. 6 Fig. 7 Fig. 8 The flow through the channel is known to be subsonic, and have a normal speed of m/s. This value was calculated based on the width of the flume, and the flow rate and approach height of the water flow from an Excel file given to us from the project sponsor. The normal speed means that there is one velocity component of the flow, which is strictly normal to the surface from which the inlet boundary condition was selected. This simplifies Page 7

8 the complexity of the problem. The turbulence parameters such as the Eddy Length Scale and the Fractional Intensity were unknown, and thus the values recommended from ANSYS CFX for a similar problem were selected. For the outlet, the boundary condition was set to a subsonic flow, and a static Relative pressure of 0 Pa. Because of the necessity of specifying a static Relative pressure at the outlet, the geometric model in CFX had to be designed such that the downstream side of the Ogee must be very long. The reason is because of the coupled pressure and velocity terms in the governing equations of fluid flow. If the downstream side of the geometric model was made much shorter, and a static Relative pressure boundary condition was set at the end, then the flow behaviour past the Ogee would be restricted in too short of a distance in order to satisfy that boundary condition. By designing the downstream part of the geometric model to be very long, it will allow the water to flow until it stabilizes at the end, and thus the velocity field just after passing the Ogee will be much more accurate. For the Ogee surface and the floor, a No Slip Wall boundary condition and a Smooth surface were selected. What No Slip Wall means is that the velocity located right next to the wall is equal to the velocity of the wall, which in this case is zero because the Ogee surface and floor are not moving. A smooth surface was selected instead of a rough surface because if a rough surface were selected, then a surface roughness must be specified which was an unknown for the flume. For the top and the side walls, a Free Slip Wall boundary condition was chosen. What Free Slip Wall means is that the shear stress at the wall is zero. In other words, the fluid velocity located right next to the wall does not experience any kind of friction which slows it down. The reason why this was selected was to simplify the computation of the problem. Meshing the Domain This section outlines two different approaches of meshing the domain. One involves a high level of mesh refinement and requires some knowledge of where the boundary layers are likely to occur, and whether a turbulent flow exists. The other approach is by using a simpler mesh with no refinement. The purpose of using two different approaches of meshing is to demonstrate the importance of using mesh refinement to properly model fluid problems. The differences between the results from each approach will be shown in the Results section of this report. Meshing using Mesh Refinement Techniques To accurately model the water flow over the Ogee profile, it is important that the user knows the areas which require a higher level of mesh refinement. Before refining the mesh in these particular areas, the general mesh encompassing the geometric model should begin with a small amount of element spacing. The following figure displays the side view of the geometric model with a mesh grid of maximum element spacing equal to 0.05 m. It includes the mesh refinement made along the boundary of the floor and the Ogee surface. Page 8

9 Fig. 9 Side view of geometric model with mesh grid (refined volume mesh) The following figure illustrates in detail the mesh on top of the surface of the Ogee profile. Fig 10 Inflated Boundary mesh on top of the Ogee profile surface As shown in fig. 10, the mesh on top of the Ogee profile surface has been refined using a feature in ANSYS CFX called the Inflated Boundary. The Inflated Boundary refines the mesh on top of a surface to a specified number of element levels using wedge shaped elements. For the CFX model of the water flow over the Ogee profile, a number of 8 element levels were specified, with a maximum thickness of 0.05 m. By refining the mesh on top of the Ogee profile surface, the boundary layer that will occur in this region will be accurately captured. Fig. 11 displays the shape of the wedge finite volume element. Fig. 11 Wedge finite volume element The remainder of the mesh grid is composed of the default tetrahedral finite volume element, shown in fig. 12. Fig. 12 Tetrahedral finite volume element Page 9

10 The next step was to refine the mesh within the areas where turbulent flow would take place and where velocities would be rapidly changing. This was accomplished using a feature in ANSYS CFX called Mesh Adaption. Mesh Adaption works simultaneously with the CFX Solver. The CFX Solver is used once the entire preliminary meshing and the domain and boundary physics have been inputted, and is the last step before being able to analyze the results of the CFX model using CFX Post. While the CFX Solver is calculating the solutions for each finite volume, for a variable that user chooses, it automatically refines the areas of the mesh where the numerical solutions for this variable are rapidly changing, to a maximum specified amount of Adaption Levels. Fig. 13 illustrates an example of Mesh Adaption Level 1. Numerical Solutions are changing rapidly between elements in this area of the mesh (Adaption Level 1) Fig. 13 Example of Mesh Adaption Level 1 The wedge and the tetrahedral finite volumes would be refined as follows for Mesh Adaption Level 1. Fig. 14 Mesh refinement for wedge and tetrahedral finite volumes Adaption Level 2 would be one further mesh refinement within the refined mesh area made from Adaption Level 1. The CFX Solver knows whether it should proceed to mesh Adaption Level 1, or Adaption Level 1 and 2 by a Target Residual value inputted by the user. For the CFX model of the water flow over the Ogee profile, a maximum Mesh Adaption Level of 2 and a Target Residual value of were set. The variable selected which the CFX Solver used to determine the high variation in numerical solutions was velocity. The following figure illustrates the result of the Mesh Adaption feature. Page 10

11 Fig. 15 Resulting mesh after the implementation of the Mesh Adaption feature. From looking at fig. 15, it is known that velocity will rapidly change where the darkest regions of the mesh are located, because this is where the mesh is heavily refined. The following figures illustrate nicely the resultant finite volumes from the preliminary meshing and the Mesh Adaption feature at the mid-plane of the geometric model of the channel and the Ogee profile. Fig. 16 Finite volumes at mid-plane (top), tetrahedral (bottom-left), and wedge (bottom-right) The following table presents the total number of nodes and elements used to construct the final mesh. Table 4 Mesh nodes and elements (Refined Volume Mesh) Domain Nodes Elements Default Domain Page 11

12 Meshing using General Volume Mesh The second approach of meshing the domain involves starting CFX Mesh, and simply clicking on Generate Volume Mesh button and saving it. There are no mesh refinements, and it is strictly a tetrahedral mesh. The element spacing has been enlarged from the default spacing in CFX Mesh to observe its effect on the results, which will be discussed in the Results section of this report. Fig. 17 displays the side view of the geometric model with a mesh grid of maximum element spacing equal to 0.25 m. Fig. 17 Side view of geometric model with mesh grid (general volume mesh) The mesh shown on fig. 17 is much coarser than the mesh shown on fig. 9, and the Inflated Boundary feature on top of the Ogee profile surface has not been implemented (fig. 18). Fig. 18 Unrefined mesh on top of the Ogee profile surface The following table presents the total number of nodes and elements used to construct the general volume mesh. Note that the number of nodes and elements are much smaller in comparison with the refined volume mesh (Table 4). Table 5 Mesh nodes and elements (General Volume Mesh) Domain Nodes Elements Default Domain Page 12

13 Results This section outlines the results obtained from both approaches of meshing the domain. Results from using proper mesh refinement will be discussed first, and subsequently the results from using the general volume mesh. Results from using Mesh Refinement Techniques Fig. 19 is a side view vector plot placed at the mid-plane of the geometric model. The different magnitudes of velocity are shown as varied colors, yellow being the highest and dark blue being the lowest. Fig. 19 Side view of geometric model with velocity vector plot (refined volume mesh) From fig. 19, it can be seen that the flow from the inlet separates into two distinct regions when it encounters the Ogee profile. The velocity of the water flow on the upper region is horizontal and is high in magnitude, and on the lower region, the flow is circulating at a much lower speed. The phenomenon occurring at the lower region is known as flow circulation, and is shown more closely in fig. 20 below. Fig. 20 Flow circulation occurring on the back side of the Ogee profile The flow separation occurring on the above figure is the flow separation that was mentioned in the Domain and Boundary Physics section of this report, where the k - ω based Shear-Stress-Transport (SST) was selected for the turbulence modeling. Page 13

14 There is a paper published from the International Journal of Heat and Fluid Flow called Computational analysis of locally forced flow over a wall-mounted hump at high-re number by S. Saric, S. Jakirlic, A. Djugum, and C. Tropea, in which they have modeled a very similar problem using different computational methods. The time-averaged streamlines they obtained using the LES method (Large Eddy Simulation) over the hump is shown in the figure below, where c is the chord length and x is the position on the horizontal axis. Fig. 21 Time-averaged streamlines obtained by LES method It is reassuring that what has been modeled in ANSYS CFX with the Ogee profile is fairly consistent with the results obtained from researchers using other computational methods for a nearly identical problem. Fig. 22 is a contour velocity plot displaying in great detail the boundary layer that forms on top of the surface of the Ogee profile. The Inflated Boundary meshing technique has modeled the rapidly increasing velocity profile very well as shown from the numerous thin layers of varying colors. Fig. 22 Boundary layer formation on top of the Ogee surface due to the No Slip Wall boundary condition Page 14

15 Results from using General Volume Mesh The results gained from using the general volume mesh in comparison with those from using the mesh refinement techniques are poor. There is a significant loss of flow behavior. Fig. 23 Side view of geometric model with velocity vector plot (general volume mesh) The flow circulation happening on the back side of the Ogee profile shown on fig. 20 is nonexistent in fig. 24. The boundary layer in fig. 25 is also not as well defined as in fig. 22. The layers of varying colors on top of the Ogee surface are much thicker and imprecise. Fig. 24 Absent flow circulation on the back side of the Ogee profile Fig. 25 Boundary layer formation on top of the Ogee surface is not well defined Page 15

16 Further Useful Results and Future Improvements Some further useful results that can be gained from the CFX model with the refined mesh, or of an improved version of this model, that could be used for the VLH Water Turbine project are properties of the flow incident on the plane where the turbine would be installed. Some examples would include the pressure and the velocity distribution on the face of the plane as shown in figures 26, 27 and 28. However, it is very important to note that this CFX model does not include the turbine geometry, which would affect the flow conditions in the domain. In other words, all of the results from the CFX model of the Ogee alone will not be the same as the results from a CFX model with an Ogee and a turbine. Even though, the following figures do provide some idea as to what the turbine will experience in terms of the pressure and velocity of the water flow. Fig. 26 Example of a plane where the water turbine would be installed Fig. 27 Total pressure distribution (dynamic only) on the water turbine face Page 16

17 Fig. 28 Velocity distribution on the water turbine face Some improvements to this CFX model can be made in the future. The boundary conditions were over simplified. For example, for the top and the side walls, a Free Slip Wall boundary condition was set. This greatly simplifies the computing time, but does not accurately represent the walls in the actual experiment. The flume shown in fig. 3 has plexiglass walls, and the top of the water flow will act as a free surface. In the future, the boundary conditions will be improved such that they represent more closely with the walls in the actual experiment. Modeling the water flow over the Ogee profile with a free surface is currently underway. Fig. 29 Free surface water flow over a varying version of the Ogee profile Page 17

18 Conclusion In conclusion, a general approximation of the flow pattern overtop of the Ogee profile has been achieved. Before the simulation of this problem, it was unexpected to observe a circulating flow on the back side of the Ogee profile. A lot has been learned from meshing, setting the domain and boundary physics, and solving and analyzing the results of this problem. The results obtained from the approach using the mesh refinement techniques are much more useful for the VLH project, and more interesting that those obtained using the general volume mesh. They are also consistent with computational models made by researchers for a very similar problem. However, there are still some improvements that can be made with the CFX model. Especially with respect to the boundary conditions that were used. References [1] ANSYS CFX Release ANSYS Help [2] ANSYS CFX Release ANSYS Help (Source of fig. 13) [3] Aquaveo, GMS: Editing a 3D Mesh, (Source of fig. 11, 12 & 14) [4] Coastal Hydropower Corporation, Very Low Head Turbine Description. (n.d.) [5] DMCS, Fluids Mechanics and Fluids Properties. (n.d.) [6] Fraser, F., Deschênes, C., O Neil, C., and Leclerc, M., VLH: Development of a new turbine for Very Low Head sites. (n.d.) [7] Saric, S., Jakirlic, S., Djugum, A., and Tropea, C., Computational analysis of locally forced flow over a wall-mounted hump at high-re number. International Journal of Heat and Fluid Flow, [8] Versteeg, H.K., and Malalasekera, W., An Introduction to Computational Fluid Dynamics. Edinburgh Gate: Pearson Education, Page 18