Numerical Results

Results in FLUENT

We can view various results using both FLUENT and CFD-Post. We will start by looking at a few results in FLUENT like mass flow rate and the integral static pressure surface monitor.

Summary of steps in the above video:

1. Reports
   1. Fluxes
      1. Select mass flow rate
      2. Select inlet, outlet and top-inlet
   2. Look at the net results value and check if it makes sense, if mass is balanced
2. Plot
   1. Set-Up
      1. Click Add
      2. Find file with .out extension
      3. Click plot
      4. Click axis
         1. Select y
         2. Uncheck auto range
         3. Change min to -200,000 Pa
         4. Change max to 200,000 Pa
         5. Click apply
      5.  Click Plot
      6. Try a range from -100,000 to 0 Pa in the y axis. 
      7. Try a range from -7000 to -8000 Pa in the y axis

Graphical Instances

Let's now go in CFD-Post for the remaining numerical results. We'll start by enabling the visualization of a full 3 blade rotor. 

Summary of steps in the above video:

1. Open CFD post
2. Show three blades
   1. Double-click fluids to access the details of fluid toolbox
   2. Change the number of graphical instances to 3
   3. Make sure apply rotation is selected and that its defined to rotate about the z axis
   4. Change the instance definition to Custom
   5. Enable full circle
   6. Click apply
3. Change blade color to white
   1. Click on blade surface and change color to white

Blade Velocity

The following video will show you how to find blade velocity at different radii. 

Summary of steps in the above video:

1. Insert vectors 
   1. Name it blade velocity, 
   2. Location: Blade
   3. Variable: velocity in stn frame
   4. Click Apply
2. See that there’s too many lines, change sampling to equally space and click 500, apply
3. Look at the max velocity 

Velocity Streamlines

Let's now visualize the flow around the turbine using velocity streamlines. 

Summary of steps in the above video:

1. Click on the streamline button and leave the name as velocity streamline
   1. Start from: click the 3 dots next to inlet and select inlet and outside inlet
   2. Change the number of points to 200
   3. Variable: Velocity in Stn frame
   4. In the color tab, change the range from global to user specified and put min=9m/s and max=13m/s. 
   5. Click Apply

Pressure Contours

Next up, we'll look at the pressure distribution on the blade surface. 

Summary of steps in the above video:

1. Add contour, name it pressure contour
   1. Choose pressure
   2. Change # of contours to 110
   3. Go in render and uncheck lighting

Pressure Contours in the y-z Plane

Summary of steps in the above video:

1. Make sure to have only 1 graphical instance of the blade
2. Create a plane
   1. Select 'Location' > 'Plane'
   2. Set method to YZ plane
   3. Set X to desired value (Note that blade is in -x direction) 
   4. Click Apply
3. Create a pressure contour
   1. Select 'Insert' > 'Contour'
   2. Set location to the plane just created
   3. Make sure the variable is pressure
   4. Specify "local" for range
      
      

Velocity Vectors in the y-z Plane

Tip: The results shown in the video below can be updated for another plane by just changing the x location of the plane already defined.

Pressure Variation along the z-axis

To plot the variation of pressure along the axis of rotation, follow the steps below. You may also want to review this video from our laminar pipe flow tutorial which shows how to use the chart feature.

1. Create a line to represent the z-axis (axis of rotation)
   1. Select 'Location' > 'Line'
   2. Name it 'AxisRotation'
   3. Set Point 1 to (0,0,90)
   4. Set Point 2 to (0,0,-180)
   5. Change # of samples to 200
2. Create a chart
   1. Select 'Create chart'
   2. Under 'data series', create a new data series
   3. Set location to the line 'AxisRotation'
   4. Under 'x axis', set variable to Z 
   5. Check 'invert axis' because wind is traveling in -Z direction
   6. Under 'y axis', set variable to Pressure

Torque

Let's now find the torque that the fluid is generating on the blade. 

Summary of steps in the above video:

1. Finding torque in CFD Post
   1. Click calculator tab
   2. Click Function calculator
   3. Select torque under function
   4. Select Blade surface under location
   5. Change axis to Z
   6. Calculate
2. Finding torque in FLUENT (more detailed)
   1. Reports
      1. Forces
      2. Moment
      3. About z
      4. Apply

Go to Step 7: Verification & Validation

Go to all FLUENT Learning Modules