CFX-Intro 14.5 WS09 Tank-Flush [PDF]

Zitiervorschau

Workshop 09 Tank Flush 14.5 Release

Introduction to ANSYS CFX © 2012 ANSYS, Inc.

December 17, 2012

1

Release 14.5

Introduction Workshop Description:

This workshop models a water tank filling and then emptying through a siphon. The problem is transient 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. Learning Aims: This workshop introduces several new skills: • Setting up and post-processing a transient simulation • Setting up a multiphase simulation • Using if statements to initialize physics

Introduction © 2012 ANSYS, Inc.

Setup December 17, 2012

Solution 2

Results

Summary Release 14.5

Mesh Import 1. Start Workbench, add a CFX Component System and edit Setup to start CFX-Pre 2. Right-click on Mesh > Import Mesh > ICEM CFD 3. Set the Mesh Units to cm • For some mesh formats it is important to know the units used to generate the mesh

4. Import the mesh called flush.cfx5

Introduction © 2012 ANSYS, Inc.

Setup December 17, 2012

Solution 3

Results

Summary Release 14.5

Define Simulation Type The first step is to change the Analysis Type to Transient: 1. Edit the Analysis Type object in the Outline tree 2. Set the Option for Analysis Type to Transient

3. Set the Total Time to 2.5 [s] 4. Set the Timesteps to 0.01 [s] and click OK • The simulation will have 250 timesteps

Introduction © 2012 ANSYS, Inc.

Setup December 17, 2012

Solution 4

Results

Summary Release 14.5

Edit Default Domain 1. Edit Default Domain from the Outline tree

2. Delete Fluid 1 under Fluid and Particle Definition 3. Click on the New icon

4. Name the new fluid Air 5. Set the Material to Air at 25C and the Morphology to Continuous Fluid

6. Create another fluid named Water 7. Set the Material to Water and the Morphology to Continuous Fluid Introduction © 2012 ANSYS, Inc.

Setup December 17, 2012

Solution 5

Results

Summary Release 14.5

Edit Default Domain 8. 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 )

9. Set the Buoy. Ref. Density to 1.185 [kg m^-3] •

•

This is the density of Air at 25 C. In this simulation there is a distinct interface between the two fluids, rather than one being dispersed in the other. For a “free-surface” model such as this, the buoyancy reference density is set to that of the less dense fluid. The hydrostatic head then appears in the pressure field of the more dense fluid, which is more natural. Also the momentum source is added to the fluid with the greater inertia, making the solution more stable. Search the help for “Buoyancy in Multiphase Flow” (including the quotes in the search) for more details. Introduction © 2012 ANSYS, Inc.

Setup December 17, 2012

Solution 6

Results

Summary Release 14.5

Edit Default Domain 10. Switch to the Fluid Models tab 11. Under Multiphase enable the Homogeneous Model • This makes the simplifying assumption that both phases share the same velocity field

12. Set the Free Surface Model Option to Standard • This changes some solver numerics to resolve the free surface interface better

13. Under Heat Transfer enable the Homogeneous Model toggle and set the Option to None 14. Set the Turbulence Model Option to k-Epsilon Introduction © 2012 ANSYS, Inc.

Setup December 17, 2012

Solution 7

Results

Summary Release 14.5

Edit Default Domain 15. Switch to the Fluid Pair Models tab 16. Enable the Surface Tension Coefficient toggle and set the coefficient to 0.072 [N m^1] 17. Under Surface Tension Force set the Option to Continuum Surface Force 18. Set the Primary Fluid to Water –

For liquid-gas, free-surface flows the primary fluid should be the liquid

19. Under Interphase Transfer set the Option to Free Surface 20. Click OK to complete the changes to the domain Introduction © 2012 ANSYS, Inc.

Setup December 17, 2012

Solution 8

Results

Summary Release 14.5

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: 1. Insert a new boundary named Ambient 2. Set the Boundary Type to Opening and the Location to AMBIENT 3. On the Boundary Details tab set the Mass and Momentum Option to Opening Pres. And Dirn with a Relative Pressure of 0 [Pa] 4. On the Fluid Values tab set the Volume Fraction of Air to 1 and the Volume Fraction of Water to 0 5. Click OK to create the boundary

Introduction © 2012 ANSYS, Inc.

Setup December 17, 2012

Solution 9

Results

Summary Release 14.5

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 to allow flow both into and out of the domain: 1. Insert a new boundary named Outlet of the Boundary Type, Opening, and the Location set to OUTLET

2. In the Boundary Details use Opening Pres. And Dirn with a Relative Pressure of 0 [Pa] 3. In the Fluid Values set the Volume Fraction of Air to 1 and the Volume Fraction of Water to 0

4. Click OK to create the boundary 5. Insert a Symmetry boundary named Sym1 on the Location SYM1 6. Insert a Symmetry boundary named Sym2 on the Location SYM2 Introduction © 2012 ANSYS, Inc.

Setup December 17, 2012

Solution 10

Results

Summary Release 14.5

Inlet Water Flow Function Water flows into the tank at a rate of 0.2 [kg s^-1] for 1 [s], after which time it is shut off. Therefore the inlet flow rate is a function of time. You will write an expression using the if() function to define this behavior on the inlet boundary: 1. Right-click on Expressions in the Outline tree and select Insert > Expression 2. Enter the Name as flowProfile 3. Enter the Definition as: if(t-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. Introduction © 2012 ANSYS, Inc.

Setup December 17, 2012

Solution 12

Results

Summary Release 14.5

Define Expressions x = - 0.028

The expression for waterVF contains three if() function terms multiplied together. The first function, if(y 0.01[m]. The third function returns 1 when x > 0.028 [m].

y = waterHt y = - 0.01

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.

Introduction © 2012 ANSYS, Inc.

Setup December 17, 2012

Solution 13

Results

Summary Release 14.5

Define Initial Conditions Now set the initial conditions using these expressions: 1.

Right-click on Flow Analysis 1 in the Outline tree and select Insert > Global Initialisation

2.

Set all Cartesian Velocities Components to 0 [m s^-1]

3.

Set the Relative Pressure to the expression HydroP

4.

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

5.

Click OK to set the initial conditions

Introduction © 2012 ANSYS, Inc.

Setup December 17, 2012

Solution 14

Results

Summary Release 14.5

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: 1. Edit the Output Control object in the Outline tree 2. On the Trn Results tab create a new Transient Results object, accepting the default Name 3. Set the Option to Selected Variables • This reduces the file size by only writing out selected variables

4. In the Output Variables List, use the … icon and the Ctrl key to pick Air.Volume Fraction, Velocity, and Water.Volume Fraction 5. Under Output Frequency, set the Timestep Interval to 2 and click OK • Transient results will be written every second timestep, thus creating a total of 125 Transient Results files

Introduction © 2012 ANSYS, Inc.

Setup December 17, 2012

Solution 15

Results

Summary Release 14.5

Create Monitor Point Next create a monitor point to track the volume of water in the domain during the solution: 1. 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

2. Edit the Output Control object in the Outline tree 3. On the Monitor tab, toggle Monitor Options, insert a new Monitor Point named Water Volume 4. Set the Option to Expression and enter the Expression Value as waterVol, then click OK

Introduction © 2012 ANSYS, Inc.

Setup December 17, 2012

Solution 16

Results

Summary Release 14.5

Run Solver 1. Close CFX-Pre and save the project as TankFlush.wbpj 2. In the Project Schematic, Edit the Solution object to start the CFX-Solver Manager 3. Start the run from the CFX-Solver Manager • You can monitor the volume of water in the domain during the simulation on the User Points tab • The simulation will take about 30 minutes to complete. Therefore results files have been provided with this workshop

4. After a few timesteps stop your run from the Project Schematic by rightclicking on the Solution cell and selecting Interrupt Update 5. Select File > Monitor Finished Run in the CFX-Solver Manager 6. Browse to the results file provided with the workshop •

Note the shape of the Water Volume curve (User Points) and see that less water is in the domain at the end of the run than at the beginning Introduction © 2012 ANSYS, Inc.

Setup December 17, 2012

Solution 17

Results

Summary Release 14.5

Post-Process Results

1. Using Windows Explorer, locate the results file supplied, TankFlush_001.res, and drag it into an empty region of the Project Schematic 2. A new CFX Solution and Results cell will appear. Double-click on the Results object to open the file in CFD-Post

Introduction © 2012 ANSYS, Inc.

Setup December 17, 2012

Solution 18

Results

Summary Release 14.5

Post-Process Results 1. Click on Z-axis to align view and turn on Visibility for Sym1

2. On the Color tab set the Variable to Water.Volume Fraction and the Color Map to White to Blue 3. Use the Timestep Selector to load results from different points in the simulation 4. With the first Timestep loaded open the Animation tool 5. Select the Quick Animation toggle and select Timesteps as the object to animate 6. Turn off the Repeat Forever button

7. Enable the Save Movie toggle and then click the Play icon to animate the results and generate an MPEG

Introduction © 2012 ANSYS, Inc.

Setup December 17, 2012

Solution 19

Note that Air (white) becomes entrained in Water (blue) Results

Summary Release 14.5

Summary A tank flush has been simulated using a transient simulation with multiphase flow. Due to the nature of transient simulations, they tend to take longer to solve and post-process.

The results show that a significant amount of air became entrained in the water. As the Homogeneous multiphase model was used and the fluids shared the same velocity field, it was not possible for the air to separate out from the water as a result of buoyancy. In order for this to have happened, the Inhomogeneous multiphase model would have been required. Each phase would then have had its own velocity field and the entrained air bubble could have risen relative to the water. When running the Inhomogeneous model the entrained phase should be set as a Dispersed Phase in CFX-Pre.

Introduction © 2012 ANSYS, Inc.

Setup December 17, 2012

Solution 20

Results

Summary Release 14.5