Steady Vs Unsteady flow over a cylinder

Aim & Theory

In this exercise, we will be analyzing the flow of a fluid over a cylinder of diameter 2.0m. The flow will be entirely dependent on the Reynolds number of the flow which will be controlled by varying the velocity of the fluid. The flow over a cylinder is done to observe the phenomenon of Von Karmen Vortex street.

The phenomenon of vortex shedding was first described by Theodore Von Karmen, a Hungarian-American physicist, form which it got the name of Von Karmen vortex street. In layman's terms, vortex shedding is caused when fluid flow is disturbed by an object. When a fluid comes in contact with an object it produces large eddies at the rear of the object as it flows around it. Vortex shedding can be seen in any fluid flow such as air flowing around an island or mountain peak, or air blowing around tall buildings. This phenomenon is caused when the Reynolds No. of the fluid flow is above the value of about 90. This phenomenon causes unwanted vibrations on the object. This is a problem faced in airplanes while landing too. Thus the drag and lift experienced by the object must be observed when it experiences vortex shedding.

Solving and Modeling Approach

The model is designed in SPACE CLAIM. A section of the flow volume is used to analyze the effect of fluid flow. After the geometry is constructed, we move on to create the mesh. The mesh must be fine and inflation lines are used around the cylinder section of the geometry. Then we move to name the lines in the geometry. After this is done we move on to the pre-processing in the setup.

In pre-processing, we use a pressure-based model, with laminar viscosity. For the steady-state velocities, we use steady-state and for the time-dependent flow, we use transient. New material must be created with a defined density and viscosity, this material will be used for all the different Reynolds numbers that have to be analyzed. To change in the Reynolds number is regulated by changing the velocity through the inlet section. The method used for pressure-velocity coupling is of the SIMPLE scheme.

We must create a monitor point behind the cylinder to extract the velocity at every time step/iteration. After this is done we must also be obtaining the plot for the coeff. of lift and coeff. of drag on the cylinder due to the fluid flow. The values of these coefficients must be extracted to obtain the STROUHAL's number. Now we initialize the setup using hybrid initialization. We then run the calculation for around 2000 iterations or more depending on the obtained residuals, this must be run till be reach a conserved solution .i.e. no change in the residuals. For the transient flow, after the Cd and Cl values are plotted we plot the Strouhal number using the FFT plot.

This must be Re= 10, 100, 1000, 10000, 100000 and 100(transient).

Pre-Processing and Solver Settings:

Open the ANSYS then from the Analysis Systems drag ANSYS (Fluent) to the project schematic section to load the fluent system.

Geometry:

• Right-click on geometry > select Space CLAIM.
• Under design select circle > click on the origin on XY-plane> drag away from the center> in diameter set 2m.
• Create a construction line from the center of the circle towards negative x-direction > and set it to 20m.
• From the end of that line drag two construction lines of 10m towards positive and negative y-axis direction.
• Then from any one end of the above-created construction line draw an 80m long construction line towards the positive X-axis.
• Select the rectangle option in the design tab and create a rectangle using the construction lines of dimension 20mX80m.
• Now go to pull and pull the cylindrical sketch and then delete that structure.
• The geometry is ready for meshing.

Mesh

• Double click on the mesh in the project schematic and the geometry is loaded in the mesh modeler.
• The idea here is to create a fine mesh with an inflation layer at the cylinder.
• Create four named selections wall, inlet, outlet, and symmetry. This can be done by clicking the edge selection option > then select the edge to be named > then name it. The inlet is the left edge, the outlet is the left edge, the top and bottom edges are symmetry and the cylinder edge is the wall.

• Right click on the mesh > insert > select inflation > scoping method should be geometry selection select the face > the boundary is the wall > first layer height 5mm > maximum layers : 8 > then growth rate is set as 1.2.
• Again, right-click on mesh > insert > method >scoping method: geometry selection > in geometry select the flow field > in method: set it as triangles.
• Again, right-click on mesh > insert > sizing > scoping method: named selection > named selection: wall > type: number of divisions > no. of divisions: 60.
• Now we click on mesh > element size : 9e-002m > then we click generate.

Setup

• The general settings were the solver should be pressure-based, the velocity formulation is Absolute and time for steady-state must be steady and for the time-dependent state, it must be transient.
• The model for viscosity must be laminar and the energy should be off.

• Go to the Physics panel > click on materials > name it as user_material and type must be fluid > here I am using a material with a density of 1.225 kg/m3 and viscosity of 0.245 kg/ms.
• Specify the cell zone condition material as the created user material.
• Now go to the boundary conditions > set inlet as velocity inlet with an assigned velocity > outlet as pressure outlet. According to the user density and viscosity conditions, the velocity is set in accordance with the Reynolds number under observation.

• Go to Reference values > set the Area as 2 and length as 2. Also, check if the viscosity and velocity are correctly applied.
• Finally, in methods set the scheme as SIMPLE.

Plots and Animations

• In the outline view go to results > right-click surfaces > select New > then click on point > name it as Monitor-point > set Y=0 and X = 7m.
• For velocity, go to the solution browser, and in reports click Definition > new > surface report > vertex average > field variable must be velocity > the surface must be monitor-point > create report file & report plot.
• For Cl and Cd, go to the solution browser, and in reports click Definition > new > force report > drag/lift > report output type must be Lift/drag coefficients > the zone must be the wall > create report file & report plot.
• Under the solution, initialize using hybrid initialization.
• After the initialization is complete, go to results > create a new contour for velocity and animation for it too.
• Set the no. of iteration and click on run.
• For the transient state, we need to set the number of time steps and size of the time step. The size of the time step is 0.1 and the number of time steps is 1000. This can be extended if the residuals re not converged.
• After the solution is extracted we need to obtain the strouhals number. This can be done by going to plots > select the FFT > set the Y-Axis function as magnitude and X-axis function as Strouhal Number. Now load the input file which is the report file of cl plot and plot FFT.

Results

Case 1: Re 10

No vortex shedding is observed at this velocity as it has Re < 90. This can be seen in the contour plot as well as the velocity plot at the monitor point. The velocity, coefficient of lift, and drag are constant after 3000 iterations approx. The velocity, cd, and cl are all at its peak at the beginning of the simulation. The residuals keep falling at a constant rate but there is no change in the obtained report plots so we can conclude that the solution has conserved.

Case 2: Re 100

In the velocity contour, we can observe a wavy pattern in the fluid flow at the trailing end of the cylinder, this is the vortex shedding. The velocity at the monitor point is seen to increase and decrease constantly after 500 iterations. This fluctuation of velocity at the monitor point reaches a consistent fluctuation after 600 iterations approx. The same is observed with the coefficient of lift, but the peak of every fluctuation increases with time until it reaches a constant value whereas the drag is similar to that of fluid flow with Re 10. The solution is converged as the residuals reach a constant value around 1600 iterations.

Case 3: Re 100 (Transient state)

This setup was run for a duration of 750s, which is a time step of 7500 with every time step equal to 0.1s. A distinct vortex shedding is noticed in the velocity contour and is evident by the vertex average of the velocity plot. In the lift plot, the coefficient of lift reaches a maximum value of around 0.17 at 150s into the flow time. After that the coeff. of lift consistently increases and decreases whereas in the coeff. of drag, the difference between the maximum and minimum of one wavelength (in the plot) is very small, so small that it is almost constant to a value of about 1.35.

Case 4: Re 1000

Vortex shedding is observed for this Reynolds number. In the contour, we can also see that the velocity of the fluid at the trailing edge is smaller than the initial velocity whereas it is greater in the vortex region. In comparison to Re 10 in steady-state, the coefficient of lift does not have increasing peaks and decreasing minimum, however, it stays constant. The pattern in the velocity at the monitor point increases drastically in the beginning but then the rise and fall follow the same pattern.

For cases 5 and 6 since the velocity is very high the velocity, coefficient of lift, and drag vary abruptly with different peaks and minima. The fluctuation is less abrupt for case 5 while comparing it to case 6, which is due to the difference in velocity for both the cases.

Case 5: Re 10000

Case 6: Re 100000

Conclusion:

For Re 100 - 100000, the Cl and Cd values were obtained by averaging the maximum and minimum values of it. We can also infer that vortex shedding is not observed for fluid with Re < 100. The coeff of lift is seen to increase as the Reynolds number increases.