1. Workshop 5 Cavitating Centrifugal Pump
Introduction to CFX
Pardad Petrodanesh.Co
Lecturer: Ehsan Saadati

2. Introduction
The Purpose of the tutorial is to model cavitation in a centrifugal pump, which involves the use of a rotation domain and the cavitation model.
The problem consists of a five blade centrifugal pump operating at 2160 rpm. The working fluid is water and flow is assumed to be steady and incompressible.
Due to rotational periodicity a single blade passage will be modeled.
The initial flow-field will be solved without cavitation. It will be turned on later.

3. Workbench
Start Workbench and save the project as centrifugalpump.wbpj
Drag CFX into the Project Schematic from the Component Systems toolbox
Start CFX-Pre by double clicking Setup
When CFX-Pre opens, import the mesh by right-clicking on Mesh and selecting Import Mesh > ICEM CFD
Browse to pump.cfx5
Keep Mesh units in m
Click Open

4. Creating Working Fluids
Modifying the material properties:
Expand Materials in the Outline tree
Double-click Water
On the Material Properties tab change Density to 1000 [kg/m3]
Change Dynamic Viscosity to [kg m^-1 s^-1] under Transport Properties
Click OK

5. Setting up the Fluid Domain
Double-click on Default Domain
Under Fluid and Particle Definitions, delete Fluid 1 and then create a new Fluid named Water Liquid
Set Material to Water
Create another new Fluid named Water Vapour
Next to the Material drop-down list, click the “…” icon, then the Import Library Data icon (on the right of the form), and select Water Vapour at 25 C under the Water Data object
Click OK
Back in the Material panel, select Water Vapour at 25 C

6. Setting up the Fluid Domain
Set the Reference Pressure to 0 [Pa]
Set Domain Motion to Rotating
Set Angular Velocity to 2160 [rev min^-1]
Switch on Alternate Rotation Model
Make sure Rotation Axis under Axis Definition is set to Global Z
Switch to the Fluid Models tab, and set the following:
Turn on Homogeneous Model in the Multiphase section
Under Heat Transfer set the Option to Isothermal, with a Temperature of 25 C
Set Turbulence Option to Shear Stress Transport
Click OK

7. Inlet Boundary Condition
Insert a boundary condition named Inlet
On the Basic Settings tab, set Boundary Type to Inlet
Set Location to INLET
Set Frame Type to Stationary
Switch to the Boundary Details tab
Specify Mass and Momentum with a Normal Speed of [m/s]
Switch to the Fluid Values tab
For Water Liquid, set the Volume Fraction to a Value of 1
For Water Vapour, set the Volume Fraction to a Value of 0
Click OK

8. Outlet Boundary Condition
Inset a boundary condition named Outlet
On the Basic Settings tab, set Boundary Type to Opening
Set Location to OUT
Set Frame Type to Stationary
Switch to the Boundary Details tab
Specify Mass and Momentum using Entrainment, and enter a Relative Pressure of 600,000 [Pa]
Enable the Pressure Option and set it to Opening Pressure
Set Turbulence Option to Zero Gradient
Switch to the Fluid Values tab
For Water Liquid, set the Volume Fraction to a Value of 1
For Water Vapour, set the Volume Fraction to a Value of 0
Click OK

9. Periodic Interface Click to create an Interface, and name it Periodic
Set the Interface Type to Fluid Fluid
For Interface Side 1, set the Region List to DOMAIN INTERFACE 1 SIDE 1 and DOMAIN INTERFACE 2 SIDE 1 (use the “…” icon and the Ctrl key)
For Interface Side 2, set the Region List to DOMAIN INTERFACE 1 SIDE 2 and DOMAIN INTERFACE 2 SIDE 2
Set the Interface Models option to Rotational Periodicity
Under Axis Definition, select Global Z
Set Mesh Connection Option to 1:1
Click OK

10. Wall Boundary Conditions
Insert a boundary condition named Stationary
Set it to be a Wall, using the STATIONARY location
On the Boundary Details tab, enable a Wall Velocity and set it to Counter Rotating Wall
Click OK
In the Outline Tree, right-click on the Default Domain Default boundary and rename it to Moving
The default behavior for the Moving boundary condition is to move with the rotating domain, so there is nothing that needs to be set

11. Initialization Click to initialize the solution
On the Fluid Settings form, set Water Liquid Volume Fraction to Automatic with Value, and set the Volume Fraction to 1
Set Water Vapour Volume Fraction to Automatic with Value, and set the Volume Fraction to 0
Click OK

12. Solver Control Double click Solver Control in the Outline tree
Set Timescale Control to Physical timescale
A commonly used timescale in turbomachinery is 1/omega, where omega is the rotation rate in radians per second. You can use an expression to determine a timestep from this. In this case, 2/omega will be used to achieve faster convergence.
Enter the following expression in the Physical Timescale box: 1/(pi*2160 [min^-1])
Set Residual Target to 1e-5
On the Advanced Options tab, turn on Multiphase Control, then turn on Volume Fraction Coupling and set the Option to Coupled
Click OK

13. Output Control Double Click on Output Control in the Outline tree
On the Monitor tab, turn on Monitor Options
Under Monitor Points and Expressions, create a new object and call it InletPTotalAbs
Set Option to Expression
Specify the following expression: massFlowAve(Total Pressure in Stn Frame
Create a new object called InletPStatic, and set Option to Expression
Specify the following expression: areaAve(Pressure
Click OK

14. Solver Close CFX-Pre and switch to the Workbench Project window
Save the project
Now double click on Solution in the Project Schematic to start the Solver Manager
When the Solver Manager opens, click Start Run
When the solution has completed, close the Solver Manager and return to the Project window

15. Post-processing
View the results in CFD-Post by double clicking Results in the Project Schematic
Insert a Contour by clicking
For the Location, click , expand Regions and then select BLADE
Set Variable to Absolute Pressure from the extended list
Set Range to Global
On the Render tab switch off Lighting and Show contour Lines
Click Apply

16. Post-processing
Insert another Contour on the HUB location, using the variable Absolute Pressure coloured by Local Range. Turn off Lighting and Show Contour Lines.
Insert another Contour on the SHROUD location, using the variable Absolute Pressure coloured by Local Range. Turn off Lighting and Show Contour Lines.
The minimum pressure is above the Saturation Pressure of 2650 Pa for Water here. In the next step, the outlet pressure will be reduced enough to initiate Cavitation.

17. Adding another Analysis
Close CFD-Post and return to the Project Schematic
Click the arrow next to the A cell and select Duplicate
A new CFX project is created as a copy of the first
Change the name of the new Simulation to Cavitation
Use the arrow next to the A cell to Rename it to No Cavitation
Save the Project
Double-click Setup for the Cavitation simulation to open CFX-Pre

18. Physics Modifications
Edit the Default Domain
On the Fluid Pair Models tab set Mass Transfer to Cavitation
Set Option to Rayleigh Plesset
Turn on Saturation Pressure
Set a Saturation Pressure of 2650 [Pa]
Click OK
Edit the Outlet Boundary Condition
On the Boundary Details tab, set the Relative Pressure to 300,000 [Pa]
Most cavitation solutions should be performed by turning cavitation on and then successively lowering the system pressure over several runs to more gradually induce cavitation. To speed up this workshop, a sudden change in pressure is introduced. Note that this approach may not be suitable for modelling some industrial cases.

19. Physics Modifications
Edit Solver Control
Set the Max. Iterations to 150
Set the Residual Target to 1e-4
Click OK
Close CFX-Pre and save the project
In the Project Schematic, drag cell A3 onto cell B3
The non-cavitating solution will be used as the initial guess for the cavitating solution
Double-click Solution for the Cavitation system
In the Solver Manager note that the initial conditions have been provided from the project schematic
Click Start Run

20. Cavitation Solution
There is a significant spike in residuals, in part due to the outlet pressure difference, but also due to the fact that the absolute pressure is low enough to induce cavitation.
When the run completes, close the Solver Manager and return to the Project Schematic
Save the project
Double-click Results for the Cavitation project to open CFD-Post

21. Post-processing
If it is not enabled, turn on visibility for the Wireframe and turn off visibility for any User Locations and Plots
Create an XY Plane at Z = 0.01 [m]
Colour it by Absolute Pressure (the variable is available in the Extended List by clicking ). Use a Global Range
The minimum absolute pressure is equivalent to the Saturation Pressure specified earlier, which is a strong hint that some cavitation has occurred
Change the Colour Variable to Water Vapour.Volume Fraction
Change the Colour Map to Blue to White

22. Post-processing Turn off visibility for Plane 1
Create a Volume using the Isovolume method
Set the Variable to Water Vapour.Volume Fraction
Set Mode to Above Value, and enter a value of 0.5
To view 360 degrees of the model, double-click Default Transform
Uncheck Instancing Info from Domain
Set # of copies to 5
Set # of Passages to 5
Click OK

23. Post-processing
The main area of cavitation exists between the suction side of the blade and the shroud in this geometry. A secondary area of cavitation is just behind the leading edge of the blade on the pressure side
Further steps to try:
Calculate torque on the BLADE using the function calculator (hint, use the extended region list to find the BLADE, and use Global Z axis)
Plot velocity Vectors on Plane 1, using the variable Water Liquid.Velocity in Stn. Frame
Calculate the mass flow through the pump (hint: use the function calculator to evaluate massFlow at the Outlet region)
Using a similar method to step 2, calculate the drop in Total Pressure from Inlet to Outlet
Plot Streamlines, starting from the Inlet location