Workshop 7 Tank Flushing Introduction to CFX

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.

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

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

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

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 1.185 [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

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

Edit Default Domain Switch to the Fluid Pair Model tab Enable the Surface Tension Coefficient toggle and set the coefficient to 0.072 [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

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

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

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

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

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>-0.028 [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.

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 > -0.028 [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 = - 0.028 y = waterHt y = - 0.01

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

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

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 Fraction)@Default 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

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

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

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

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

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.