Numerical Results

We can use either FLUENT or CFD-Post as post-processing tool. CFD-Post is preferable as it is more user friendly and gives you more freedom. The first check, however, will be made in FLUENT

Check mass flow

It's always good to check the mass flow rate after CFD simulation. The solver tries to keep it satisfied, but sometimes a representative imbalance is obtain, showing that something has to be done in order to get more accurate results.

To do this, we will use FLUENT.

Highlight "Reports" in the left box. Then select "Fluxes" and click "Set Up...".

Image Removed

Note that "Mass flow rate" is already selected.

Here you can play around to see the mass balance through each boundaries. Since most of our boundaries are single circular element, it is expected that the imbalance at each boundary alone be zero. We will check the mass flow rate though two boundaries.

First, the external boundaries. In the "Flux Reports" window, locate and highlight "farfield1" and "farfield2" and hit "Compute". The mass flow rate though that boundary is now printed in the command window.

Image Removed

Note that 73.5kg/s get into out domain and virtually everything leaves. The imbalance is 7.4e-9kg/s which is negligible considering the total amount of flux in the system. Nice!

Now, let's check the imbalance inside the hub. For that we only have one boundary completely circling the zone, hub_inner (note that hub_outer is essentially the same boundary).

Proceed similarly as before and check the mass flow through the hub_inner boundary. You could also select hub_outer and the result would be almost identical.

Image Removed

Remember to deselect farfield1 and farfield2 before hitting compute!

You should get an imbalance of 3.42e-10kg/s which is essentially zero. Cool!

Velocity Contours

To plot the velocity contours we will use CFD-Post. You can now close FLUENT.

...

To probe: Click on "Probe" icon. Then change the variable to "Velocity" and click on the screen where you wanna probe.

Tip speed ratio (TSR)

To calculate the TSR we first need to extract the velocity from CFD-Post. Since our reference is the value of velocity at r=0.04m, we need to find some way to extract the velocity of the blade at that particular location.

One can plot the velocity vectors and read off the legend. However this is quite imprecise.

One of the ways to do this trick is to plot the velocity distribution along the X coordinate for the whole surface of the right blade, and then extract the value at x=0.04m. Since the "wall" entity is a closed line, the plot should also be circular. As the blade is rectangular, we should expect abrupt change in velocity very close to the maximum and minimum X. Let's do it!

First thing to do is to create a Polyline over the wall of the right blade. Select Location > Polyline. 

FIGURE 9

Name it "wall right" and for "Method" select "Boundary Intersection". For "Boundary List" select "blade_right symmetry 1" and for "Intersection With", select "wall_blade_right". Click Apply.

FIGURE 10

Next, insert a chart (Insert > Chart). Name it "Veloc at blade". Under "Data Series" tab, change the Location to the created "wall right".

Under "X Axis" tab, change the Variable to "X".

Under "Y Axis" tab, change the Variable to "Velocity in Stn Frame v". This is the velocity in the Stationary frame of reference (our interest). We are taking only the y component because we know that the velocity of the blade should be only in the y direction at that location. Click Apply.

The chart should look like this. The point of interested is marked by the dashed lines. Also notice that at the edges of the plot there is an abrupt change in velocity, as expected. The "closed loop" plot expect is in fact happening, but the curve collapsed into a single line. You can she the curves separated if you choose "Velocity in Stn Frame" as Y Variable instead

FIGURE 11

note it's circular so there should be two plots superimposed.

Recall from pre-analysis that we calculated the expected value 

Check mass flow

Velocity contours

(save image)

Blade velocity (TSR)?

Pressure contours

Torque

Vorticity?

Cp=Cm (from fluent) * TSR

When extracting the Torque, explain that the Moving Frame of Reference is used to calculate (FOR FEA) omega squared times the radius times the mas of each element to compute the force exerted by the fluid on the blades. (check Wind Blade 2 tutorial, under Physics Setup, second video, around 3:30. It is for FEA, we should get the analogy to fluid before).

Vorticity Contours

Another interesting thing to analyze is the Vorticity distribution downstream of the turbine. This strongly affects how you would distribute more turbines in case you are designing an array of them.

But to do that we have to tell Fluent to export Vorticity Magnitude to CFD-Post. To do that, go back to Workbench, and double click "Solution".

Under "Run Calculation", click on "Data File Quantities". Select "Vorticity Magnitude" from the list and click Ok.

Image Added

Run the simulation again so Fluent can retrieve the desired value. It will converge in 2 iterations. Close Fluent and Refresh the project.

Open CFD-Post and create a new contour. Name it "Vorticity Contour".

For "Locations", do the same procedure as for the velocity contours (click on "..." and select all "[...] symmetry 1" zones).

For "Variable", select "Vorticity".

For "Range", change it to "User Specified", and change the value for Min to 0, and for Max to 2000 [s^-1].

Change the number of contours to 101.

Image Added

You should get something as the following figure.

Image Added

You can see the vorticity emanting from the tips of the blades. If you ever seen a video from a flow over a plate perpendicular to the direction of the flow, you might remember the vorticies being generated at the tips of the plate.

Also note that for the blade that is almost aligned with the flow, the vorticity does not propagate much (is less intense).

One could also plot some cool pictures for pressure (you will notice some relationship with the velocity contours) and for Turbulent Kinetic Energy (you will notice some relationship with the vorticity contours). For the latter one, change the scale from Min=0 to Min=7 J/kg and enjoy a very beautiful turbulent kinetic energy distribution! Note how close the contour will be to the Vorticity one.

Go to Step 7: Verification & Validation

Go to all (ANSYS or FLUENT ) Learning Modules