Computational Study of Laminar Flowfield around a Square Cylinder using Ansys Fluent

Transcription

1 MEGR , Computational Fluid Dynamics :1 7 Spring 2015 Computational Study of Laminar Flowfield around a Square Cylinder using Ansys Fluent Rahul R Upadhyay Master of Science, Dept of Mechanical Engineering, UNC Charlotte SUMMARY In this work, we have computationally solved for the steady and unsteady laminar flowfield around a two-dimensional square cylinder using Ansys Fluent, a commerical CFD package. For a Reynolds number(re) of 1, steady state solution for the flowfield is obtained and streamlines of the flowfield are studied along with the calculation of C d, i.e co-effecient of drag. For a reynolds number of 300, a transient analysis was carried out. The strouhal number of time varying co-efficient of lift was calculated and time evolving vorticity field and streamlines of the flowfield were also analyzed. Some of the time evolving plots of vorticity and streamlines obtained during this work can be viewed as this link: KEY WORDS: Reynolds Number, Strouhal Number, Ansys, Vortex Shedding, Drag/Lift Coefficient PROBLEM STATEMENT: FLOW AROUND SQUARE CYLINDER Figure 1. Illustration of fluid flow around square cylinder. 1. Dimensions of cylinder: 1 cm x 1 cm. 2. Density of Fluid(ρ)= 1000 kg/m3. 3. Viscosity of Fluid(µ)= 1e-3 Pa-s. 4. Goal To calculate co-efficient of drag for steady state analysis with Re=1. To calculate Strouhal Number for oscillating time varying co-efficient of lift with Re= 300.To obtain vorticity field, streamlines of flowfield for flow around square cylinder at different timepoints.

2 2 PROBLEM 1: COMPUTATIONAL PARAMETERS Figure 2. Design of Domain: Fluid flow around square cylinder. 1. Design Methodology:In this work, fluid flow around a square cylinder with dimensions of 1 cm x 1 cm is modeled. At first, the fluid flow around the cylinder was modeled using two concentric squares. The inner square being the cylinder and the outer cylinder being the fluid. The domain was coarsely meshed and solved to get a general idea about the flow pattern. It was found that there was no physical phenomenon of interest, like vortex generation/shedding, occurring on the side of the cylinder facing the flow, i.e the left face. The generation of vortices followed by vortex shedding occured on the right face, i.e opposite to the side facing the flow. On the basis of the solutions of the preliminary design with the coarse mesh, the domain in Figure 2 was developed. The dimensions of fluid domain were chosen such that the vortex shedding phenomena is accurately captured in the longitudinal and lateral directions. 2. Boundary Setup: The boundary conditions for the fluid domain are illustrated in figure 2. The fluid boundary region towards the left face of the square cylinder was given the velocity inlet boundary condition. It is denoted by doted lines. For the density and viscosity value of water, the velocity was calculated for reynolds number of 1 and 300 and set as the velocity value at the inlet boundary condition. The fluid boundary region towards the right face of the square cylinder was given the pressure outlet

3 boundary condition. It is denoted by dashed lines. The sides of the cylinder were set as no-slip boundary condition. 3 Figure 3. Boundary setup of the fluid domain. 3. Solution Technique: In this work, steady state solutions are to be solved at a Reynolds number of 1 and unsteady-state solutions are to to solved for a Reynolds number of 300 with water being the fluid. For such a low velocity flow, Pressure-Based solvers are ideal as they require less memory storage and provide more procedural flexibility [4]. We have used Pressure-Based solver for solving the given low speed incompressible flow problem. 4. Spatial Discretization: The pressure-velocity coupling is performed using Ansys based SIMPLE scheme. Momentum Equations are discretized using Second Order Upwind Scheme which is a second order accurate method. Gradients are discretized using Least Square Cell Method. 5. Convergence Parameters for Steady State: The convergence threshold for x-velocity, v-velocity and continuity equation was set as 1e-6. The solution was initialized from the inlet. 6. Convergence Parameters for Unsteady State: The convergence threshold for x-velocity, v-velocity and continuity equation was set as 1e-5. The solution was initialized from the inlet.

4 4 PROBLEM2: MESH SPECIFICATIONS Figure 4. Regions in the mesh geometry. 1. Type: Mapped Face Meshing. 2. Mesh sizes in different regions: Region A: 40 divisions, biasing 10. Region B: 90 divisions, no biasing. Region C: 40 divisions, no biasing. Region D: 15 divisions, no biasing. Region E: 20 divisions, no biasing. Figure 5. Mesh Geometry of the domain.

5 3. In Figure 4 are illustrated the various regions on the mesh geometry. Figure 5 shows the actual mesh of the model. Vorticity generation and shedding phenomenon is most prominent in the region surrounding the cylinder. This region is meshed more finely compared to regions away from the cylinder to obtain accurate results in a computationally effecient manner. 5 PROBLEM 3: STEADY-STATE SOLUTION AT RE=1 Figure 6. Streamlines of flow at steady state 1. Figure 6 shows the streamlines for the flow at steady state. It can be seen that there is a seperation of flow field on the right face of the cylinder. This is a low pressure region. 2. The equation 1 gives the expression for C d. Here ρ is density, F D is drag force, u is the velocity of flow with respect to the cylinder and A is the projected area of the square towards the incident flow. For the 2D case, A is the same as the side dimension of the square cylinder, i.e D=1 cm. For the given values of density,viscosity,dimensions and Reynolds number(1), the value of u is 1e-4. The value of C d as computed by Ansys corresponding to this inlet velocity is C d = 2F D ρu 2 A (1)

6 6 PROBLEM 4: UNSTEADY-STATE SOLUTION AT RE=320 Figure 7. Instantaneous plot of vorticity field at different times within first 10 second of flow Figure 8. Instantaneous plot of streamlines at different times within first 10 second of flow 1. In the case of unsteady flow, for a time step of 0.25 and 0.15, the simulation was run for 320 iterations and 533 iterations respectively to obtain solution over a physical time of 80 seconds. 2. The time evolving solution of vorticity field and streamlines of fluid flow were obtained. These animated solutions can be viewed at gl/h9syx5.

7 3. Figure 7 shows the time evolution of vorticity field and Figure?? shows the time evolution of streamlines within the fluid domain at different time points.(the time stamp t1, t2, t3 and t4 are different for the two figures.) It was found for that the case of fluid flow over cylinder at Re=300, there is an alternate process of vortex formation followed by vortex shedding. 4. Strouhal Number for Vortex Shedding Process: Figure 9 shows the graph of variation of lift-coefficient with respect to time. The variation is found to be of oscillating nature. The Strouhal Number as calculated using equation 2 comes out to be In equation 2, f is the frequency of oscillation. 7 St = fd U inf (2) Figure 9. Instantaneous plot of streamlines at different times within first 10 second of flow 1. FUTURE EXTENSION OF WORK 1. Study of flow field around a square cylinder inclined to the flowfield. 2. Comparison of flow field around a square cylinder with flow field around an aero-foil. REFERENCES 1. Lecture notes of MEGR , Computational Fluid Dynamics,. 2. Handout given in MEGR : A Handout On Ansys Workbench:Laminar Pipe Flow Problem. 3. Mapped-Face-Meshing: 4. Ansys Solver Setting, Introductory FLUENT Notes: FLUENT v6.3 December Pressure Based Solver: