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. 

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

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)

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

Domains: leave default ("All Domains")

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.

Variable: change is to "Velocity".

Range: leave as "Global".

# of Contours: change to around 51.

Click Apply.

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

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.

This is a single snapshot of the spinning of the turbine, or a particular position. A transient analysis with a complete animation will be created in the future.

You can also zoom out and see that far downstream of the turbine, the flow has not yet recover its freestream condition. If you probe the velocity inside that slightly brighter area you will see that the velocity is around 9m/s (instead of 10m/s of the freestream).

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

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.

FIGURE N

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

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

Tip speed ratio (TSR)

In practice, this is extracted directly from the Boundary Conditions, since we will essentially check that the velocity at the wall is zero. Therefore the purpose of this check is more to verify if we had correctly inputted the mathematical model into Fluent.

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 fluid particles in touch with 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. 

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.

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. CFD Post uses the variable Velocity as relative to the rotating frames). 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

The point is slightly above the halfway between 0.165 and 0.170. Recall from pre-analysis that we calculated the expected value as 0.1676m/s. The value is virtually the same, indicating that we might have inputted the right mathematical model into the tool.

But we're not done! To calculate the TSR we still have to perform one short step. Recall that TSR=veloc blade/veloc wind, so all we have to do is divide the calculated velocity by 10m/s, the wind speed.

So, our TSR is 0.01676. We will use this value to estimate the value of Cp.

Go to Step 7: Verification & Validation

Go to all (ANSYS or FLUENT) Learning Modules