Pre-Analysis & Start-Up

Pre-Analysis

In the Pre-Analysis step, we'll review the following:

• Mathematical model: (e.g.: We'll look at the governing equations + boundary conditions and the assumptions contained within the mathematical model.)
• Numerical solution procedure in ANSYS: (e.g.: We'll briefly overview the solution strategy used by ANSYS and contrast it to the hand calculation approach.)
• Hand-calculations of expected results: (e.g.: We'll use an analytical solution of the mathematical model to predict the expected stress field from ANSYS. We'll pay close attention to additional assumptions that have to be made in order to obtain an analytical solution.)

Mathematical Model 

Governing Equations

The governing equations solved here are the conservation of mass and the conservation of momentum (Navier-Stokes equations), taken in a frame of reference moving with the turbine:

• Conservation of Mass:
  
• Navier-Stokes equations, simplified for constant angular velocity, in a moving frame of reference:
  
  where:
   and 

FLUENT will solve this in a moving frame of reference. This is a good simplification, because with it we don't have to deal with moving mesh. (yet! Keep checking for future tutorials on that!)

Note that we're solving a turbulent problem, and we will assume k-epsilon model with default FLUENT values

Boundary Conditions

To solve in FLUENT we'll need to create a region a few times larger than the main geometry of the turbine. This region is where the presence of the turbine disturbs the flow. This can be seen as the outer circle from the following figure. Note that we could have made any geometry for this "far-field" zone, but to simplify the boundaries a circle was chosen. 

The boundary conditions are:

• Inlet (far-field): constant velocity in the x-direction of 10m/s, with turbulent intensity of 5% and turbulent viscosity ratio of 1.
• Outlet (far-field): absolute pressure of 101325 Pa, or 1 atm, with same turbulent parameters as above. 
• Blades: wall, so no velocity. (No-slip condition).

Numerical Solution Procedure in ANSYS

FLUENT will follow the Finite-Volume Method and will divide the domain into multiple control volumes or "cells".
From the integral form of the governing equations, it will perform a control volume balance for each cell and write algebric nonlinear equations for them, and then linearize these equations..
Next, it will solve iteratively these equations and stop the iteration when the Residuals are below a certain specified tolerance.

Velocity, pressure, angular velocity and turbulence parameter k are calculated in the cell centers, after inverting the matrix of the system of algebric equations of cell-center values.
With these values, the post-process tool will derive everything else that we might want, like wall shear, etc.

Hand-Calculations of Expected Results

Calculate Cp? need first to see if its possible to calculate that. Maybe from the torque.... from the Ct

We expect large vortices downstream the turbine?

We may want to use the following simplifications:

• Assume the airfoils are flat plates of 0.1x2cm, positioned on a pitch angle of 20deg, i.e. the plates are placed such that when they are at the upper-most part its trajectory, they form an angle of 20deg with the horizontal.
• Incoming flow with a constant profile of 10m/s in the horizontal direction
• The downstream pressure is constant 101325 Pa.
• Air with density of 1.225kg/m3 and viscosity of 1.7894e-5 Pa.s. 
• 2D analysis

Start-Up

Now we'll start with the Ansys part. It is recommended that you leave this tutorial side by side with the Ansys screen, with Ansys taking 2/3 of the screen and the tutorial, 1/3.

Start by opening ANSYS Workbench. 

If your screen doesn't look like this, you can click View > Reset Window Layout. 

Locate Fluid Flow (Fluent) under Analysis Systems on the left portion of the window. 

Click, hold the button down, and drag it into the Project Schematics, the central region of the screen. Note that a red rectangle will show up before you drag, indicating where you should "drop" the dragged item

After releasing the click your window will look similar to this:

Rename the project to VAWT - Moving Frame of Reference

Now, Save your project by clicking File > Save and selecting the desired location and name.

Note: Ansys creates two entities when saving: and .wbpj file and a folder. You will need to have both on the same directory in order to resume the project. It is possible to save it into a single file by going to File > Archive. This will generate a single .wbpz file, which is easier to move in case you're on a temporary directory.

Go to Step 2: Geometry

Go to all (ANSYS or FLUENT) Learning Modules