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...".

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.

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.

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

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.

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. 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

FIGURE 11

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 our simulation might be good.

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.

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).

Go to Step 7: Verification & Validation

Go to all (ANSYS or FLUENT) Learning Modules