Workshop 1: Bubbly Flow in a Rectangular Bubble Column. Multiphase Flow Modeling In ANSYS CFX Release ANSYS, Inc. WS1-1 Release 14.

Size: px

Start display at page:

Download "Workshop 1: Bubbly Flow in a Rectangular Bubble Column. Multiphase Flow Modeling In ANSYS CFX Release ANSYS, Inc. WS1-1 Release 14."

Rudolph Goodwin
5 years ago
Views:

Workshop 1: Bubbly Flow in a Rectangular Bubble Column 14.

1 Workshop 1: Bubbly Flow in a Rectangular Bubble Column Release Multiphase Flow Modeling In ANSYS CFX 2013 ANSYS, Inc. WS1-1 Release 14.5

2 Introduction This workshop models the dispersion of air bubbles in water in a rectangular bubble column. Gas is supplied through a sparger at the bottom of the bubble column and the rising action of bubbles provides agitation of the liquid. Although the boundary conditions are steady and the geometry is simple, there is a transient character to the solution In this workshop, you will set up and run a basic bubbly flow simulation. In the second workshop, you will add non-drag forces to the model ANSYS, Inc. WS1-2 Release 14.5

Rectangular Bubble Column Geometry Vessel Details Height of column Width of column Depth of column Height of sparger Length of sparger Width of sparger 1.00 m 0.10 m 0.

3 Rectangular Bubble Column Geometry Vessel Details Height of column Width of column Depth of column Height of sparger Length of sparger Width of sparger 1.00 m 0.10 m 0.02 m 0.01 m 0.01 m 0.02 m Air inlet at the bottom via a sparger (porous aquarium stone) Air superficial velocity: m/s 2013 ANSYS, Inc. WS1-3 Release 14.5

4 Expected Behavior Measurements: High speed video camera: Gas velocity Bubble size Wire mesh sensor Gas volume fraction Bubble sizes Bubbles dispersed across the column Narrow plume of bubbles near the inlet 2013 ANSYS, Inc. WS1-4 Release 14.5

5 Computational Mesh outlet = opening Hexahedral mesh (ICEM-CFD Hexa) Mesh element size: x= y= z=0.005m cells 16,000 elements 21,105 nodes inlet (sparger) 2013 ANSYS, Inc. WS1-5 Release 14.5

6 Importing the Mesh Copy the file ICEM CFD mesh file rectangularcolumn.msh from the input files folder into a working directory. Start CFX-Pre from the ANSYS CFX Launcher after changing to this working directory and open a new case (File/New Case/General) Right-click on Mesh in the Outline and select Import Mesh/ICEM CFD and import rectangularcolumn.msh into the simulation, setting the Mesh Units to m ANSYS, Inc. WS1-6 Release 14.5

mesh in the pop-up window, Note that the height of the vertical column ranges

7 Imported Mesh Hightlight the imported mesh in the Outline view. Right-click on it and select Mesh Statistics Note the dimensions of the imported mesh in the pop-up window, Note that the height of the vertical column ranges from a y-value of 0.0 [m] at the bottom and 1.0 [m] at the top 2013 ANSYS, Inc. WS1-7 Release 14.5

On the Basic Settings tab of the Details form for the domain: Set the Domain Type to Fluid Domain Highlight Fluid 1 in the Fluid and Particle Definition

8 Defining Domain Fluids (Continuous Phase) Double-click the Default Domain created for your imported mesh to edit it (if a default domain was not created, create one). On the Basic Settings tab of the Details form for the domain: Set the Domain Type to Fluid Domain Highlight Fluid 1 in the Fluid and Particle Definition window and click on the Delete icon to remove it Click on the New icon in the Fluid and Particle definition window and insert a new fluid named water Select the predefined constant property material Water and set the Morphology Option to Continuous Fluid 2013 ANSYS, Inc. WS1-8 Release 14.5

Defining Domain Fluids (Dispersed Phase) Still on the Basic Settings tab of the Details form for the domain: Click on the New icon next to the Fluid and Particle Definition window and insert a new

9 Defining Domain Fluids (Dispersed Phase) Still on the Basic Settings tab of the Details form for the domain: Click on the New icon next to the Fluid and Particle Definition window and insert a new fluid definition named air For the new fluid air, select the predefined constant property material Air at 25 C and set the Morphology Option to Dispersed Fluid with a size of [m] 2013 ANSYS, Inc. WS1-9 Release 14.5

10 Viewing the Fluid Densities Expand the Materials entry in the outline and double-click on the Material definitions for the Air at 25 C and Water materials used to define the fluid properties for this simulation and note the values of the constant densities set for these fluids (1.185 kg/m 3 for Air at 25 C and 997 kg/m 3 for Water) These values will be important in defining the reference density for the buoyancy settings for the domain as well as the hydrostatic head for the initial guess for the pressure 2013 ANSYS, Inc. WS1-10 Release 14.5

Setting the Buoyancy Properties Buoyancy effects are very important for gasliquid settings and therefore buoyancy properties must be defined for the domain On the Basic Settings form for the Domain

11 Setting the Buoyancy Properties Buoyancy effects are very important for gasliquid settings and therefore buoyancy properties must be defined for the domain On the Basic Settings form for the Domain under the Domain Models section, set the Buoyancy Option to Buoyant and enter the X,Y, and Z components of the gravity vector as [0, -9.81, 0] m/s 2. Set the buoyancy reference density to the density of water [997.0 kg/m 3 ] which is the continuous phase for this problem Set the Reference Location option for Buoyancy to Cartesian Coordinates and enter values consistent with the top surface of the domain [0 1 0 ] m 2013 ANSYS, Inc. WS1-11 Release 14.5

12 Fluid Domain: Fluid Models Left-Click the Fluid Models tab for the Domain. Leave the Homogeneous Model toggle unchecked Set the Free Surface Model to None since this is a dispersed/continuous type of flow Set Heat Transfer option to Isothermal with a Fluid temperature of 25 [C]. Set the Turbulence option to Fluid Dependent 2013 ANSYS, Inc. WS1-12 Release 14.5

Dispersed Phase Zero Equation Click on water and set: Fluid Buoyancy Model Option to Density Difference

13 Fluid Domain: Fluid Specific Models Click on the Fluid Specific Models tab on the Domain form and select air Set the Fluid Buoyancy Model Option to Density Difference Set the Turbulence Model to Dispersed Phase Zero Equation Click on water and set: Fluid Buoyancy Model Option to Density Difference Turbulence Model to Shear Stress Transport Buoyancy Turbulence Option to None 2013 ANSYS, Inc. WS1-13 Release 14.5

Fluid Pair Models Click on the Fluid Pair Models tab and: Click on the Surface Tension Coefficient toggle and enter a value of 0.

14 Fluid Pair Models Click on the Fluid Pair Models tab and: Click on the Surface Tension Coefficient toggle and enter a value of N/m (the surface tension force will not be modeled in this tutorial but the surface tension coefficient will be used in the Grace correlation for the drag) Set the Interphase Transfer Option to Particle Model Under Momentum Transfer, set the Drag Force Option to Grace Enable the Volume Fraction Correction Exponent and enter a value of 3. This value will help keep the drag law well behaved in the gas headspace region above the liquid Leave Non-drag forces unset and set the Turbulence Transfer Option to Sato Enhanced Eddy Viscosity Click OK to complete the domain definition 2013 ANSYS, Inc. WS1-14 Release 14.5

$has only air flowing through it (air volume fraction =1) The outlet at the top of the geometry will be a pressure specified opening through which either air or water could flow.$

15 Flow Boundary Condition Strategy The bubble column modeled in this simulation is semi-batch where air flows continuously through a batch layer of liquid The sparger inlet at the bottom of the vessel has only air flowing through it (air volume fraction =1) The outlet at the top of the geometry will be a pressure specified opening through which either air or water could flow. To preserve the initial liquid loading set in the initial guess, an air headspace above the liquid will be specified in the initial guess for the volume fraction field. As long as convergence is reasonable, only air will leave this boundary and the initial amount of liquid will be preserved even for a steady simulation Air Inlet Outlet Air Head Space Batch Liquid 2013 ANSYS, Inc. WS1-15 Release 14.5

Inlet Boundary Condition: inlet Insert an Inlet boundary named inlet and assign it to the location INLET On the Boundary details tab: Set the Mass and Momentum Option to Bulk Mass

cross-sectional area, and the gas density The superficial velocity, J SG, is defined as the volumetric gas flow rate divided by the cross-sectional area of the column: J SG =0.

16 Inlet Boundary Condition: inlet Insert an Inlet boundary named inlet and assign it to the location INLET On the Boundary details tab: Set the Mass and Momentum Option to Bulk Mass Flow Rate Click on the expression toggle next to the Mass Flow Rate entry box The mass flow rate of gas will be calculated based on its superficial velocity, the column cross-sectional area, and the gas density The superficial velocity, J SG, is defined as the volumetric gas flow rate divided by the cross-sectional area of the column: J SG =0.01 m/s CSA = 0.01 m x 0.2 m = m 2 Air Density = kg/m 3 Mass Flow Rate = 0.01 [m/s]*0.002 [m^2]*1.185 [kg/m^3] Enter this expression for the Bulk Mass Flow Rate 2013 ANSYS, Inc. WS1-16 Release 14.5

1.0 Highlight water and set the Volume Fraction to 0.

17 Inlet Boundary Condition: Fluid Values On the Fluid Values tab: Highlight air and set the Volume Fraction to 1.0 Highlight water and set the Volume Fraction to 0.0 Click OK to create the boundary 2013 ANSYS, Inc. WS1-17 Release 14.5

Opening Boundary Condition: outlet Insert a boundary named

For Boundary Details: Set the Mass and Momentum Option to

0 Pa Click the Fluid Values tab (these are only applied if

18 Opening Boundary Condition: outlet Insert a boundary named outlet. Set the type to Opening and Location to OUTLET. For Boundary Details: Set the Mass and Momentum Option to Opening Pres. and Dirn. Enter a Relative Pressure of 0.0 Pa Click the Fluid Values tab (these are only applied if fluid is entrained at the outlet) Highlight air and set the Volume Fraction to 1.0 Highlight water and set the Volume Fraction to 0.0 Click OK to create the boundary 2013 ANSYS, Inc. WS1-18 Release 14.5

Default Wall Boundary Condition Double click the default boundary created for the

Edit Boundary form On the Boundary details tab, set the Mass and Momentum Option to

Option to Free Slip Wall Highlight water and set the Mass and Momentum Option to No

19 Default Wall Boundary Condition Double click the default boundary created for the domain (Default Domain Default for a domain named Default Domain) to bring up the Edit Boundary form On the Boundary details tab, set the Mass and Momentum Option to Fluid Dependent On the Fluid Values tab: Highlight air and set the Mass and Momentum Option to Free Slip Wall Highlight water and set the Mass and Momentum Option to No Slip Wall Click OK to update the wall boundary settings 2013 ANSYS, Inc. WS1-19 Release 14.5

20 Boundary Condition Summary Top Opening Side and Bottom Walls Sparger Inlet 2013 ANSYS, Inc. WS1-20 Release 14.5

$9 m) This will be implemented by using a step function for gas volume fraction that is zero for y < 0.9 m and 1 for y > 0.90 m. The air volume fraction expression will be: step((y - 0.90 [m])/1.$

21 Initial Condition The initial condition for this simulation will set up a gas headspace in the upper 10% of the domain (i.e. for y > 0.9 m) This will be implemented by using a step function for gas volume fraction that is zero for y < 0.9 m and 1 for y > 0.90 m. The air volume fraction expression will be: step((y [m])/1.0 [m]) Headspace We must also enter the correct hydrostatic pressure for this initial condition relative to the buoyancy reference density of 997 kg/m^3 and the buoyancy reference position (y = 1.0 m): P = ( )[kg/m^3]*g*(1.0[m] - y)* step((y [m])/1.0 [m]) This will be zero in the liquid region and hydrostatic in the gas * Note: g is a CFX system variable which is predefined as 9.81 [m/s^2] 2013 ANSYS, Inc. WS1-21 Release 14.5

Global Initialization Click the Global Initialization icon from the menu bar On the Global Settings tab, set the Static Pressure Option to Automatic with Value Enter the following expression for

22 Global Initialization Click the Global Initialization icon from the menu bar On the Global Settings tab, set the Static Pressure Option to Automatic with Value Enter the following expression for Relative Pressure which was given on the previous slide (be sure to click on the Equation toggle next to the Relative Pressure entry box): ( ) [kg/m^3] *g* (1.0 [m] - y)* step((y-0.9 [m])/1.0 [m]) 2013 ANSYS, Inc. WS1-22 Release 14.5

Global Initialization: Fluid Settings On the Fluid Settings tab, highlight air and set: U, V, and W Cartesian Velocity Components to Automatic with Value

0 [m]) Highlight water and set: U, V, and W Cartesian Velocity Components to Automatic with Value with all at 0.

23 Global Initialization: Fluid Settings On the Fluid Settings tab, highlight air and set: U, V, and W Cartesian Velocity Components to Automatic with Value with all at 0.0 [m/s] the Volume Fraction Option to Automatic with Value with the expression set to: step((y [m])/1.0 [m]) Highlight water and set: U, V, and W Cartesian Velocity Components to Automatic with Value with all at 0.0 [m/s] Turbulence Option to Medium (Intensity = 5%) the Volume Fraction Option to Automatic with Value with the expression set to: step((y [m])/1.0 [m]) Click OK to complete the Initialization 2013 ANSYS, Inc. WS1-23 Release 14.5

Solver Parameters Click on the Solver Control icon from the menu bar On the Basic Settings tab: Set the Advection Scheme Option to High Resolution Set the Timescale Control to Physical Timescale and

24 Solver Parameters Click on the Solver Control icon from the menu bar On the Basic Settings tab: Set the Advection Scheme Option to High Resolution Set the Timescale Control to Physical Timescale and enter a Physical Timescale of 0.01 s Set the Max. Iterations to 100 Enter 1e-4 for the Residual Target Leave the other settings at their default values and click OK to apply the solver settings 2013 ANSYS, Inc. WS1-24 Release 14.5

Output Control: Monitor Point Click on the Output Control icon from the menu bar Click on the Monitor tab and: Enable the Monitor Options toggle Under Monitor Points and Expressions, click on the New

25 Output Control: Monitor Point Click on the Output Control icon from the menu bar Click on the Monitor tab and: Enable the Monitor Options toggle Under Monitor Points and Expressions, click on the New icon Enter holdup as the name of the new monitor point Set the Option for Holdup to Expression and enter the Expression Value as:: Domain This gives the average volume fraction of air in the domain, commonly known as the gas hold-up. (If your domain name is not Default Domain, use that name in its place). Click OK to create the monitor 2013 ANSYS, Inc. WS1-25 Release 14.5

26 Write Solver File and Define Run Click the Define Run icon from the menu bar Enable the Quit CFX-Pre toggle and click Save to write the input file Click Save and Quit when prompted to save the simulation file 2013 ANSYS, Inc. WS1-26 Release 14.5

27 Running the Solver When the Solver Manager Define Run form appears, click Start Run It should take about five minutes to solve 100 iterations 2013 ANSYS, Inc. WS1-27 Release 14.5

28 Monitoring the Residuals 2013 ANSYS, Inc. WS1-28 Release 14.5

29 Assessing Convergence After 100 iterations, the run has not converged very well in terms of the magnitudes of the residuals Browse the output file and check the imbalances for mass and the volume fraction of Air at 25 C. They are also still quite high. Click on the User Points tab of the Solver Manager to display the change in the computed gas phase holdup over time. The initial value near 0.10 corresponds to the initial headspace set in the initial guess Start CFX-Post and load the results file from your run 2013 ANSYS, Inc. WS1-29 Release 14.5

$Clearly, the air volume fraction field is still evolving (The ANSYS CFX solver is time marching, even for a steady-state run).$

30 Post-Processing Select the -z view. Create a xy-plane for a z-value of 0.01 m and color it according to air.volume Fraction. Clearly, the air volume fraction field is still evolving (The ANSYS CFX solver is time marching, even for a steady-state run). This is reflected in the high mass imbalances ANSYS, Inc. WS1-30 Release 14.5

Find the Solver Control section in the Definition File Editor and expand Convergence Control Double-click Physical

31 Continuing the Run From the Solver Manager, click on Tools/Edit CFX Solver File and select the results file for your current run. Find the Solver Control section in the Definition File Editor and expand Convergence Control Double-click Physical Timescale and change it to 0.02 s. Double-click Maximum Number of Iterations and change it to 400 Click File/Save then File/Exit. Click the Restart icon to resume the run with the new settings 2013 ANSYS, Inc. WS1-31 Release 14.5

32 Solver Monitor The second run will require about 20 minutes to reach 400 iterations 2013 ANSYS, Inc. WS1-32 Release 14.5

33 Imbalance and Holdup Continuation from First Run Convergence and imbalances are still not great but we can examine the Results File in CFD-Post to look for causes 2013 ANSYS, Inc. WS1-33 Release 14.5

34 Post-Processing Start Post and load the current results file. Select the -z view. Create a XY-Plane for a z-value of 0.01 m and color it according to air.volume Fraction. Next, clip the range by setting a user-specified range from 0 to The bubble plume is unsteady which causes the wiggles in the convergence behavior ANSYS, Inc. WS1-34 Release 14.5

35 Comparison to Experiment The current steady-state simulation results predict an oscillating relatively narrow plume of bubbles rising up the center of the column. The experimental pictures show that the length of the initial narrow plume of bubbles is much shorter than what the simulation predicts Bubbles dispersed across the column Narrow plume of bubbles near the inlet 2013 ANSYS, Inc. WS1-35 Release 14.5

Adding Non-Drag Forces One reason for the difference between the experimental bubble plume and the simulation prediction is the neglecting of several important

36 Adding Non-Drag Forces One reason for the difference between the experimental bubble plume and the simulation prediction is the neglecting of several important non-drag forces including lift, turbulent dispersion, and wall lubrication. These will be included in the second workshop ANSYS, Inc. WS1-36 Release 14.5

37 2013 ANSYS, Inc. WS1-37 Release 14.5

Numerical Simulations of a Train of Air Bubbles Rising Through Stagnant Water

Numerical Simulations of a Train of Air Bubbles Rising Through Stagnant Water Hong Xu, Chokri Guetari ANSYS INC. Abstract Transient numerical simulations of the rise of a train of gas bubbles in a liquid