1. Workshop 7 Tank Flushing
Introduction to CFX
Pardad Petrodanesh.Co
Lecturer: Ehsan Saadati

2. Introduction
This workshop models a water tank filling and then emptying through a siphon. The problem is transient in nature and solved as a two fluid multiphase case (air + water).
An initial water level is set in the tank. The water supply is turned on for the first second of the simulation and then shut off for the rest of the simulation. The water level rises until water flows out the U-tube generating a siphoning effect which effectively empties the tank.

3. Right-click on Mesh > Import Mesh >ICEM CFD
Start Workbench, add a CFX Component System, then edit the Setup to start CFX-Pre
Right-click on Mesh > Import Mesh >ICEM CFD
Set the Mesh Units to cm
For some mesh formats it is important to know the units used to generate the mesh
Import the mesh flush.cfx5

4. Define Simulation Type
The first step is to change the Analysis Type to Transient:
Edit the Analysis Type object in the Outline tree
Set the Analysis Type Option to Transient
Set the Total Time to 2.5 [s]
Set the Timesteps to 0.01 [s] and click OK
The simulation will have 250 timesteps

5. Edit Default Domain Edit Default Domain from the Outline tree
Delete Fluid 1 under Fluid and Particle Definition
Click on the New icon
Name the new fluid Air
Set the Material to Air at 25C and the Morphology to Continuous Fluid
Create another fluid named Water
Set the Material to Water and the Morphology to Continuous Fluid

6. Edit Default Domain
Turn on Buoyancy and set the (X, Y, Z) gravity components to (0, -g, 0)
Use the expression icon to enter -g ( g is a built-in constant )
Set the Buoy. Ref. Density to [kg m^-3]
This is the density of Air at 25 C. Search the help for “Buoyancy in Multiphase Flow” (including the quotes in the search) for more details

7. Edit Default Domain Switch to the Fluid Models tab
Under Multiphase Options, enable the Homogeneous Model
This makes the simplifying assumption that both phases share the same velocity field
Set the Free Surface Model Option to Standard
This changes some solver numerics to resolve the free surface interface better
Under Heat Transfer, enable the Homogeneous Model toggle and set the Option to None
Set the Turbulence Model Option to k-Epsilon

8. Edit Default Domain Switch to the Fluid Pair Model tab
Enable the Surface Tension Coefficient toggle and set the coefficient to [N m^-1]
Under Surface Tension Force, set the Option to Continuum Surface Force
Set the Primary Fluid to Water
Under Interphase Transfer, set the Option to Free Surface
Click OK to complete the changes to the domain

9. Create Boundary Conditions
Start by creating an Opening boundary at the top of the tank to allow air to escape as the tank is filled:
Insert a new boundary named Ambient
Set the Boundary Type to Opening and the Location to AMBIENT
On the Boundary Details tab, set the Mass and Momentum Option to Opening Pres. And Dirn with a Relative Pressure of 0 [Pa]
On the Fluid Values tab, set the Volume Fraction of Air to 1 and the Volume Fraction of Water to 0
Click Ok to create the boundary

10. Create Boundary Conditions
Now create the outlet and symmetry boundaries. Since recirculation may occur at the outlet this boundary will be specified as an Opening:
Insert a new boundary named Outlet with the Boundary Type as Opening and the Location as OUTLET
In the Boundary Details, use Opening Pres. And Dirn with a Relative Pressure of 0 [Pa]
In the Fluid Values, set the Volume Fraction of Air to 1 and the Volume Fraction of Water to 0
Click Ok to create the boundary
Insert a Symmetry boundary named Sym1 on the Location SYM1
Insert a Symmetry boundary named Sym2 on the Location SYM2

11. Inlet Water Flow Function
Water will flow into the tank at a rate of 0.2 [kg s^-1] for 1 [s]; it will then be shut off for the remainder of the simulation. Therefore the inlet flow rate must be a function of time. You will write an expression using the if() function to define this behavior, then create the Inlet boundary:
Right-click on Expressions in the Outline tree and select Insert > Expression
Enter the Name as flowProfile
Enter the Definition as: if(t<1 [s], 0.2 [kg/s], 0 [kg/s]) and click Apply
Insert a new boundary named Inlet
Set the Boundary Type to Inlet and the Location to INLET

12. Inlet Boundary Condition
In Boundary Details, set the Mass and Momentum Option to Bulk Mass Flow Rate
Set the Mass Flow Rate to the expression flowProfile
In the Fluid Values, set the Volume Fraction of Air to 0 and the Volume Fraction of Water to 1, then click OK

13. Insert the following expressions:
Define Expressions
Next you will create expressions to define the initial water height and the initial hydrostatic pressure field. These expressions must define the correct initial flow field because the transient simulation is started “cold” (it is not started from a converged steady-state simulation).
Insert the following expressions:
waterHt = 6 [cm]
waterVF = if(y<waterHt,1,0)*if(y>-0.01 [m],1,0)* if(x> [m],1,0)
waterDen = 998 [kg m^-3]
HydroP = waterDen * g * (waterHt - y) * waterVF
waterHt is the initial height of the water in the tank. waterVF provides the initial volume fraction distribution in the tank (see next slide). waterDen is the density of water. HydroP provides the initial pressure distribution due to the hydrostatic pressure of water.

14. Define Expressions
The expression for waterVF contains three step() function terms multiplied together. The first function, step((waterHt - y) / 1[m]), returns 1 when y < waterHt. In other words the volume fraction of water is 1 below the y = waterHt line shown to the right.
The second step() function returns 1 when y > -0.01[m]. The third step function returns 1 when x > [m].
The result is that the volume fraction of water is equal to 1 only in the shaded area shown to the right. This defines the initial water volume fraction.
Note that the arguments to the step() function must be dimensionless, hence each time we divide by 1[m].
x =
y = waterHt
y =

15. Define Initial Conditions
Now set the initial conditions using these expressions:
Right-click on Flow Analysis 1 in the Outline tree and select Insert > Global Initialisation
Set all Cartesian Velocities Components to 0 [m s^-1]
Set the Relative Pressure to the expression HydroP
On the Fluid Settings tab, set the Volume Fraction for Water to the expression waterVF. Set the Volume Fraction for Air to the expression 1 – waterVF
Click OK to set the initial conditions

16. Define Transient Results
By default results are only written at the end of the simulation. You must define transient results to view the intermediate solution:
Edit the Output Control object in the Outline tree
On the Trn Results tab, create a new Transient Results object, accepting the default Name
Set the Option to Selected Variables
This reduces the file size by only writing out selected variables
In the Output Variables List, use the … icon and the Ctrl key to pick Air.Volume Fraction, Velocity, and Water.Volume Fraction
Under Output Frequency, set the Timestep Interval to 2, then click OK
Transient results will be written every second timestep, thus creating a total of 125 Transient Results files

17. Edit the Output Control object in the Outline tree
Create Monitor Point
Next create a Monitor Point to track the volume of water in the domain during the solution:
Insert a new expression named waterVol with the Definition set to: volumeInt(Water.Volume Domain
This is the volume integral the water volume fraction in the domain
Edit the Output Control object in the Outline tree
On the Monitor tab, toggle Monitor Options, insert a new Monitor Point named Water Volume
Set the Option to Expression and enter the Expression Value as waterVol, then click OK

18. Close CFX-Pre and save the project as TankFlush.wbpj
Run Solver
Close CFX-Pre and save the project as TankFlush.wbpj
In the Project Schematic, Edit the Solution object to start the Solver Manager
Start the run from the Solver Manger
You can monitor the volume of water in the domain during the simulation on the User Points tab
The simulation will take about 2 hours to complete. Therefore results files have been provided with this workshop
After a few timesteps, Stop your run
Select File > Monitor Finished Run in the Solver Manager
Browse to the results file provided with the workshop
Note the shape of the Water Volume curve, and see that less water is in the domain after the run is complete than there was at the beginning

19. Post-Process Results
Using Windows Explorer, locate the supplied results file TankFlush_001.res, and drag it into an empty region of the Project Schematic
A new CFX Solution and Results cell will appear. Double-click on the Results object to open it in CFD-Post

20. Post-Process Results
Turn on Visibility for Sym1
On the Colour tab, set the Variable to Water.Volume Fraction and set the Colour Map to White to Blue

21. Post-Process Results
Use the Timestep Selector to load results from different points in the simulation
With the first Timestep loaded, open the Animation tool
Select the Quick Animation toggle and select Timesteps as the object to animate
Turn off the Repeat Forever button
Enable the Save Movie toggle and then click the Play icon to animate the results and generate an MPEG

22. Additional Notes
The results show that a significant amount of air becomes entrained in the water. For this situation running the Inhomogeneous model is recommended so that each phase has its own velocity field. This would allow entrained air bubble to rise out of the water. When both phases have the same velocity field there is no way for entrained air to separate from the water.
When running the Inhomogeneous model, the entrained phase should be set as a Dispersed Phase in CFX-Pre.