Include Page | ||||
---|---|---|---|---|
|
Include Page | ||||
---|---|---|---|---|
|
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.
HTML |
---|
<iframe width="640" height="360" src="//www.youtube.com/embed/WjOre55vkLA" frameborder="0" allowfullscreen></iframe> |
Summary of steps in the above video:
- Reports
- Fluxes
- Select mass flow rate
- Select inlet, outlet and top-inlet
- Look at the net results value and check if it makes sense, if mass is balanced
- Fluxes
- Plot
- Set-Up
- Click Add
- Find file with .out extension
- Click plot
- Click axis
- Select y
- Uncheck auto range
- Change min to -200,000 Pa
- Change max to 200,000 Pa
- Click apply
- Click Plot
- Try a range from -100,000 to 0 Pa in the y axis.
- Try a range from -7000 to -8000 Pa in the y axis
- Set-Up
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.
HTML |
---|
<iframe width="640" height="360" src="//www.youtube.com/embed/M4_YItFbhsk" frameborder="0" allowfullscreen></iframe> |
Summary of steps in the above video:
- Open CFD post
- Show three blades
- Double-click fluids to access the details of fluid toolbox
- Change the number of graphical instances to 3
- Make sure apply rotation is selected and that its defined to rotate about the z axis
- Change the instance definition to Custom
- Enable full circle
- Click apply
- Change blade color to white
- 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.
HTML |
---|
<iframe width="640" height="360" src="//www.youtube.com/embed/il58JvXEu-I" frameborder="0" allowfullscreen></iframe> |
Summary of steps in the above video:
- Insert vectors
- Name it blade velocity,
- Location: Blade
- Variable: velocity in stn frame
- Click Apply
- See that there’s too many lines, change sampling to equally space and click 500, apply
- Look at the max velocity
Velocity Streamlines
Let's now visualize the flow around the turbine using velocity streamlines.
HTML |
---|
<iframe width="640" height="360" src="//www.youtube.com/embed/_qjNCL288j4" frameborder="0" allowfullscreen></iframe> |
Summary of steps in the above video:
- Click on the streamline button and leave the name as velocity streamline
- Start from: click the 3 dots next to inlet and select inlet and outside inlet
- Change the number of points to 200
- Variable: Velocity in Stn frame
- In the color tab, change the range from global to user specified and put min=9m/s and max=13m/s.
- Click Apply
Pressure Contours
Next up, we'll look at the pressure distribution on the blade surface.
HTML |
---|
<iframe width="640" height="360" src="//www.youtube.com/embed/YoaZsYvynIw" frameborder="0" allowfullscreen></iframe> |
Summary of steps in the above video:
- Add contour, name it pressure contour
- Choose pressure
- Change # of contours to 110
- Go in render and uncheck lighting
Pressure Contours in the y-z Plane
To plot the pressure distribution at a cross section of the blade:
- Make sure to have only 1 graphical instance of the blade
- Create a plane
- Select 'Location' > 'Plane'
- Set method to YZ plane
- Set X to desired value (Note that blade is in -x direction)
- Click Apply
- Adjust view
- Click +X on the bottom right triad
- Create a pressure contour
- Select 'Insert' > 'Contour'
- Set location to the plane just created
- Make sure the variable is pressure
- Specify min and max values to show high/low pressure regions
- Go under the 'view' tab and check 'apply rotation'
- Set axis to X
- Set angle to 90 degrees
Pressure Contours along the z-axis
To plot the variation of pressure along the axis of rotation:
- Create a line to represent the z-axis (axis of rotation)
- Select 'Location' > 'Line'
- Name it 'AxisRotation'
- Set Point 1 to (0,0,90)
- Set Point 2 to (0,0,-180)
- Change # of samples to 200
- Create a chart
- Select 'Create chart'
- Under 'data series', create a new data series
- Set location to the line 'AxisRotation'
- Under 'x axis', set variable to Z
- Check 'invert axis' because wind is traveling in -Z direction
- Under 'y axis', set variable to Pressure
Torque
Let's now find the torque that the fluid is generating on the blade.
HTML |
---|
<iframe width="640" height="360" src="//www.youtube.com/embed/xoJp4HnIht8" frameborder="0" allowfullscreen></iframe> |
Summary of steps in the above video:
- Finding torque in CFD Post
- Click calculator tab
- Click Function calculator
- Select torque under function
- Select Blade surface under location
- Change axis to Z
- Calculate
- Finding torque in FLUENT (more detailed)
- Reports
- Forces
- Moment
- About z
- Apply
- Reports