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...".

FIGURE 1

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.

FIGURE 2

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.

FIGURE 3

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.

In Workbench, under Project Schematic, double click Results. This will launch CFD-Post

FIGURE 4Image Added

CFD-Post usually opens with an isometric view of the part. Since we're in a 2D analysis, this is not very useful for us. So, the first thing to do is click on the Z axis arrow (bottom-right corner of graphics window) to change the view.

Now insert a Contour. Click on the Contour icon (or Insert > Contour)

FIGURE 5Image Added

Name it "Velocity contour". A new box will appear on the left side of the screen. Summary of what to do:

...

Locations: click on the three dots "..." on the side. select all names with "symmetry 1" in it. Hold the Ctrl key for that. You will select 5 zones in total, see figure.

FIGURE 6Image Added

Variable: change is to "Velocity".

...

Click Apply.

You can zoom into the bughub, drawing a box with the right mouse button.

FIGURE 7Image Added

Note that it's very clear the effect of when the blade is perpendicular to the flow: a huge recirculation bubble is made. This will negatively affect other turbines placed downstream of this one. This is a very important thing to consider when designing an array of VAWTs.

...

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

FIGURE 8Image Added

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 

Check mass flow

Velocity contours

(save image)

Blade velocity (TSR)?

Pressure contours

Torque

Vorticity?

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).

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