1. Right-click Mesh and select Import Mesh > CFX Mesh.

   The Import Mesh dialog box appears.

2. Configure the following setting(s):

   Setting	Value
   File name	Buoy.gtm

3. Click Open.

1. Select File > Import > CCL.

   The Import CCL dialog box appears.

2. Under Import Method, select Append. This will start with the existing CCL already generated by CFX-Pre and append the imported CCL.

   ---

   Note:  Replace is useful if you have defined physics and want to update or replace them with newly-imported physics.

   ---

3. Select Buoy.ccl.

4. Click Open.

5. Double-click the Expressions section in the Outline tree to see a list of the expressions that have been imported.

   All expressions required for this simulation are displayed. Take a moment to look over each expression. A brief description of each expression will be provided wherever it is implemented within this tutorial.

6. Close the Expressions section by clicking Close   located at the top of the left workspace.

   ---

   Note:  Note that you could have entered these expressions manually into CFX-Pre by inserting new expressions and defining each with an appropriate formula.

   ---

1. In the Outline tree view, right-click Analysis Type and select Edit.

2. Configure the following setting(s):

   Tab	Setting	Value
   Basic Settings	Analysis Type > Option	Transient
   	Analysis Type > Time Duration > Option	Total Time
   	Analysis Type > Time Duration > Total Time	7.0 [s]
   	Analysis Type > Time Steps > Option	Timesteps
   	Analysis Type > Time Steps > Timesteps	0.025 [s] [a]
   	Analysis Type > Initial Time > Option	Automatic with Value
   	Analysis Type > Initial Time > Time	0 [s]
   A total time of 7.0 [s] is implemented so that you get an adequate overview of the rigid body motion during postprocessing. The 0.025 [s] time step provides enough detail in the solution without requiring an excessive amount of computation time for CFX-Solver.

3. Click OK.

1. Edit Case Options > General in the Outline tree view, ensure that Automatic Default Domain and Automatic Default Interfaces are both selected, and click OK.

2. In the tree view, right-click Default Domain, select Rename, and set the new name to buoy.

3. In the tree view, right-click the newly renamed domain and select Edit.

4. Configure the following setting(s):

   Tab	Setting	Value
   Basic Settings	Location and Type > Location	Assembly [a]
   	Fluid and Particle Definitions	Delete Fluid 1 [b]
   	Fluid and Particle Definitions	Create a new fluid named Air at 25 C [c]
   	Fluid and Particle Definitions	Create a new fluid named Water at 25 C [c]
   	Fluid and Particle Definitions > Air at 25 C > Material	Air at 25 C
   	Fluid and Particle Definitions > Water at 25 C > Material	Water at 25 C [d]
   	Domain Models > Buoyancy Model > Option	Buoyant
   	Domain Models > Buoyancy Model > Gravity X Dirn.	0 [m s^-2]
   	Domain Models > Buoyancy Model > Gravity Y Dirn.	-g [e]
   	Domain Models > Buoyancy Model > Gravity Z Dirn.	0 [m s^-2]
   	Domain Models > Buoyancy Model > Buoy. Ref. Density	denAir [e][f]
   	Domain Models > Mesh Deformation > Option	Regions of Motion Specified [g]
   	Domain Models > Mesh Deformation > Mesh Motion Model > Option	Displacement Diffusion [h][i]
   	Domain Models > Mesh Deformation > Mesh Motion Model > Mesh Stiffness > Option	Value
   	Domain Models > Mesh Deformation > Mesh Motion Model > Mesh Stiffness > Mesh Stiffness	1.0 [m^5 s^-1] / volcvol [e][j]
   Fluid Models	Multiphase > Homogeneous Model	(Selected) [k]
   	Multiphase > Free Surface Model > Option	Standard
   	Multiphase > Free Surface Model > Interface Compression Level	(Selected)
   	Multiphase > Free Surface Model > Interface Compression Level > Interface Compression	2
   	Heat Transfer > Homogeneous Model	(Selected)
   	Turbulence > Option	Shear Stress Transport
   Fluid Pair Models	Fluid Pair > Air at 25 C | Water at 25 C > Interphase Transfer > Option[l]	Mixture Model
   	Fluid Pair > Air at 25 C | Water at 25 C > Interphase Transfer > Interface Len. Scale	1.0 [mm]
   Click Multi-select from extended list   to open the Selection Dialog box, then select Assembly from this list. Click OK. Ensure that you have Fluid 1 selected and click Remove Selected Item  . To create a new item, you must first click the Add new item   icon, then enter the name as required and click OK. Click Select from extended list   and then on Import Library Data   in the upper right corner of the resulting Material dialog box. When the Select Library Data to Import box appears, click Expand   located beside Water Data. Select Water at 25 C from the list. Click OK. In order to enter an expression, you must first click Enter Expression  . The buoyancy reference density is set to 1.185 kg/m3, which is representative of air. This mesh deformation option enables you to specify the motion of the boundary mesh nodes using user-defined expressions created in the CFX Expression Language (CEL). These expressions of mesh motion are included in the CCL file that was imported at the beginning of the tutorial. To see the additional mesh motion settings, you may need to click Roll Down   located beside Mesh Motion Model. The Displacement Diffusion model for mesh motion preserves the relative mesh distribution of the initial mesh. The variable volcvol (volume of finite volumes) is a predefined variable related to the local mesh element volume. It is used here in the calculation of the mesh stiffness value. In this example, the mesh stiffness is set to be inversely proportional to volcvol, which results in higher stiffness in regions of smaller element size; these are the regions that are most likely to experience mesh folding. This is similar to the default setting of Mesh Stiffness > Option set to Increase Near Small Volumes with Reference Volume > Option set to Mean Control Volume. In a homogeneous, multiphase model, all fluids share a flow field, turbulence field, and so on. This is valid for models where the fluids have completely stratified; this is the case in this simulation. The interphase transfer model controls the calculation of interfacial area density, which is required by certain interfacial transfer processes. In this case, the homogeneous model is used and no other interfacial transfer processes are active so the actual setting does not matter.

5. Click OK.

1. It is very important to give the rigid body a coordinate frame that is centered on its center of mass. Create a coordinate frame centered on the rigid body in its initial position, and oriented with its axes aligned with the rigid body axes/global coordinate axes as follows:

   1. Select Insert > Coordinate Frame.

   2. In the dialog box that appears, set Name to RigidBodyCoordFrame and click OK. The Basic Settings tab for the coordinate frame appears.

   3. Set Option to Axis Points.

   4. Set Origin to 0, —0.1438, 0.05.

   5. Set Z Axis Point to 0, —0.1438, 1.

   6. Set X-Z Plane Pt to 1, —0.1438, 0.05.

   7. Click OK.

2. In the Outline tree view, right-click Flow Analysis 1 and select Insert > Rigid Body.

3. Accept the default name, Rigid Body 1, by clicking OK.

4. Configure the following setting(s):

   Tab	Setting	Value
   Basic Settings	Mass	39.39 [kg] [a]
   	Location	BUOY
   	Coordinate Frame	RigidBodyCoordFrame
   	Mass Moment of Inertia > XX Component	4.5 [kg m^2]
   	Mass Moment of Inertia > YY Component	2.1 [kg m^2]
   	Mass Moment of Inertia > ZZ Component	6.36 [kg m^2]
   	Mass Moment of Inertia > XY Component	0 [kg m^2]
   	Mass Moment of Inertia > XZ Component	0 [kg m^2]
   	Mass Moment of Inertia > YZ Component	0 [kg m^2]
   Dynamics	Degrees of Freedom > Translational Degrees of Freedom > Option	X and Y axes
   	Degrees of Freedom > Rotational Degrees of Freedom > Option	Z axis
   	Gravity	(Selected)
   	Gravity > Option	Cartesian Components
   	Gravity > Gravity X Dirn.	0 [m s^-2]
   	Gravity > Gravity Y Dirn.	-g [b]
   	Gravity > Gravity Z Dirn.	0 [m s^-2]
   Initial Conditions	Center of Mass	(Selected)
   	Center of Mass > Option	Automatic[c]
   	Linear Velocity	(Selected)
   	Linear Velocity > Option	Automatic with Value
   	Linear Velocity > X Component	0 [m s^-1]
   	Linear Velocity > Y Component	0 [m s^-1]
   	Linear Velocity > Z Component	0 [m s^-1]
   	Angular Velocity	(Selected)
   	Angular Velocity > Option	Automatic with Value
   	Angular Velocity > X Component	0 [radians s^-1]
   	Angular Velocity > Y Component	0 [radians s^-1]
   	Angular Velocity > Z Component	0 [radians s^-1]
   The values in this table are taken directly from the problem description found in the Overview of the Problem to Solve section. In order to enter an expression, you must first click Enter Expression  . Setting this option to Automatic defaults the center of mass of the rigid body to the origin of the RigidBodyCoordFrame. In most cases, this will be the correct setting.

5. Click OK.

1. Click Global Initialization  .

2. Configure the following setting(s):

   Tab	Setting	Value
   Global Settings	Initial Conditions > Cartesian Velocity Components > U	0 [m s^-1]
   	Initial Conditions > Cartesian Velocity Components > V	0 [m s^-1]
   	Initial Conditions > Cartesian Velocity Components > W	0 [m s^-1]
   	Initial Conditions > Static Pressure > Option	Automatic with Value
   	Initial Conditions > Static Pressure > Relative Pressure	hypres [a][b]
   	Initial Conditions > Turbulence > Option	Intensity and Eddy Viscosity Ratio
   Fluid Settings	Fluid Specific Initialization > Air at 25 C > Initial Conditions > Volume Fraction > Volume Fraction	airvol [a]
   	Fluid Specific Initialization > Water at 25 C > Initial Conditions > Volume Fraction > Volume Fraction	watvol [a][c]
   In order to enter an expression, you must first click Enter Expression  . The expression hypres is defined in the CCL file and gives the relative pressure as a function of the volume of water in the fluid region and the vertical distance (Y direction value). The expression results in an initial pressure gradient that linearly decreases when the value of the Y-coordinate increases (or the water depth decreases). When the Y-coordinate reaches the interface between the air and water, the initial pressure plateaus at a value of zero (due to the reliance of the expression hypres on watvol). The initial pressure gradient produced by this expression can be observed in the image below. To create this plot in CFX-Pre: Double-click Expressions in the Outline tree view. Double-click the hypres expression. Select the Plot tab under Details of hypres. Select Expression Variables: Y. Set the Start of Range to -2.0 [m] and End of Range to 2.0 [m]. Click Plot Expression. The airvol and watvol expressions were provided in the CCL file. The expression watvol is a step function that returns a value of 1.0 for all Y-coordinate values less than the initial water height (0.05 [m]), 0.0 for all Y-coordinate values greater than the initial water height, and 0.5 when the Y-coordinate value is equal to the initial water height.

3. Click OK.

In this section, you will adjust the solver control settings to promote a quicker solution time and to enable the frequency of when the rigid body solver is run.

1. Click Solver Control  .

2. Configure the following setting(s):

   Tab	Setting	Value
   Equation Class Settings	Equation Class > Mesh Displacement	(Selected)
   	Equation Class > Mesh Displacement > Convergence Control	(Selected)
   	Equation Class > Mesh Displacement > Convergence Control > Max. Coeff. Loops	4 [a]
   	Equation Class > Mesh Displacement > Convergence Control > Min. Coeff. Loops	2
   Rigid Body Control	Rigid Body Control	(Selected)
   	Rigid Body Control > Rigid Body Solver Coupling Control > Update Frequency	Every Coefficient Loop [b]
   	Rigid Body Control > Angular Momentum Equation Control	(Selected) [c]
   Advanced Options	Multiphase Control	(Selected)
   	Multiphase Control > Initial Volume Fraction Smoothing	(Selected)
   	Multiphase Control > Initial Volume Fraction Smoothing > Option	Volume-Weighted [d]
   The maximum number of coefficient loops is set to 4 and the minimum number of coefficient loops to 2 to ensure that the solver completes at least 2 loops per time step, and no more than 4. In this simulation it will ensure a relatively resolved and accurate solution within a short period of time. By setting the update frequency to every coefficient loop you are specifying that CFX-Solver will call the rigid body solver during every coefficient loop within each time step. This may increase total solution time, however the motion of the rigid body will be better resolved. This sets the integration scheme for the angular momentum equations to the second-order Simo Wong scheme, which is robust and energy-conserving. If the initial conditions for volume fraction have a discontinuity, startup robustness problems may occur. Choosing volume-weighted smoothing of these volume fractions may improve startup robustness.

3. Click OK.

1. Click Output Control  .

2. Click the Trn Results tab.

3. In the Transient Results editor, click Add new item  , set Name to Transient Results 1, and click OK.

4. Configure the following setting(s) of Transient Results 1:

   Setting	Value
   Transient Results 1 > Option	Selected Variables
   Transient Results 1 > Output Variables List	Pressure, Total Mesh Displacement, Velocity, Water at 25 C.Volume Fraction [a]
   Transient Results 1 > Output Frequency > Option	Time Interval
   Transient Results 1 > Output Frequency > Time Interval	tOn[b]
   Click Multi-select from extended list  beside the entry box, and make multiple selections in the Output Variables List by holding down the Ctrl key and clicking on the required variables. In order to enter an expression, you must first click Enter Expression  .

5. Click the Monitor tab and configure the following setting(s):

   Monitor Objects	(Selected)
   Monitor Objects > Monitor Points and Expressions	Create a new Monitor Point and enter the name Buoy Force [a][b].
   Monitor Objects > Monitor Points and Expressions > Buoy Force > Option	Expression
   Monitor Objects > Monitor Points and Expressions > Buoy Force > Expression Value	force_y()@Buoy Surface
   Monitor Objects > Monitor Points and Expressions	Create a new Monitor Point and enter the name Buoy Torq [a][c].
   Monitor Objects > Monitor Points and Expressions > Buoy Torq > Option	Expression
   Monitor Objects > Monitor Points and Expressions > Buoy Torq > Expression Value	torque_z()@Buoy Surface
   To create a new item, you must first click the Add new item   icon, then enter the name as required and click OK. This monitor point will track the force acting on the rigid body in the Y direction. This monitor point will track the torque of the rigid body relative to the Z axis.

6. Click OK.

1. Click Define Run  .

2. Configure the following setting(s):

   Setting	Value
   File name	Buoy.def

3. Click Save.

   CFX-Solver Manager automatically starts and, on the Define Run dialog box, Solver Input File is set.

4. Quit CFX-Pre, saving the simulation (.cfx) file.

1. Right-click a blank area in the viewer and select Predefined Camera > View From +Z.

2. Create a new Plane and accept the default name.

3. Configure the following setting(s):

   Tab	Setting	Value
   Geometry	Definition > Method	XY Plane
   	Definition > Z	0.05 [m]

4. Click Apply.

5. Create new contour and accept the default name.

6. Configure the following setting(s):

   Tab	Setting	Value
   Geometry	Locations	Plane 1
   	Variable	Water at 25 C.Volume Fraction
   	Color Map	White to Blue
   	# of Contours	10

7. Click Apply.

8. Select File > Save State and choose the name Buoy.cst.

9. Click Save.

1. Ensure that Contour 1 is visible in the 3D Viewer (make sure there is a check mark beside Contour 1 in the Outline tree view).

2. Turn off the visibility of Plane 1 and Default Legend View 1 to better see the movement of the buoy.

3. Edit Wireframe and configure the following setting(s):

   Tab	Setting	Value
   Definition	Show surface mesh	(Selected)

4. Click Apply.

5. Click the Timestep Selector   in the toolbar. Select the 1^st time step and click Apply.

6. Click Animation   in the Timestep Selector dialog box.

   The Animation dialog box appears.

7. Set Type to Keyframe Animation.

8. Click New   to create KeyframeNo1.

9. Select KeyframeNo1, then set # of Frames to 93, then press Enter while the cursor is in the # of Frames box.

   ---

   Tip:  Be sure to press Enter and confirm that the new number appears in the list before continuing.

   ---

10. In the Timestep Selector, select time step 280 and click Apply.

11. In the Animation dialog box, click New   to create KeyframeNo2.

12. Ensure that More Animation Options   is pushed down to show more animation settings.

13. Select Loop.

14. Ensure that Repeat forever   (next to Repeat) is not selected (not pushed down).

15. Select Save Movie.

16. Set Format to MPEG1.

17. Prepare to save the movie file:

    1. If you want to save the file in your working directory, set File name to Buoy.mpg in the field beside Save Movie.

    2. If you want to save the file somewhere other than your working directory, click Browse   (next to Save Movie) set the new path and movie filename. Click Save.

       The movie filename (including the path) has been set, but the animation has not yet been produced.

18. Click To Beginning  .

    This ensures that the animation will begin at the first keyframe.

19. After the first keyframe has been loaded, click Play the animation  .

    • The MPEG will be created as the animation proceeds.

    • This will be slow, since results will be loaded and objects will be created for each time step.

    • To view the movie file, you need to use a viewer that supports the MPEG format.

    ---

    Note:  To explore additional animation options, click the Options button. On the Advanced tab of the Animation Options dialog box, there is a Save Frames As Image Files check box. By selecting this check box, the JPEG or PPM files used to encode each frame of the movie will persist after movie creation; otherwise, they will be deleted.

    ---

20. Close the Animation dialog box when the animation is complete.

1. Click the Timestep Selector  , select the 162^nd time step and click Apply.

2. Select Tools > Mesh Calculator or click the Calculators tab and select Mesh Calculator.

3. Configure the following setting(s):

   Tab	Setting	Value
   Mesh Calculator	Function	Minimum Face Angle

4. Click Calculate.

5. When you have finished, close the Timestep Selector dialog box and exit from CFD-Post.

1. Select Insert > Subdomain from the main menu or click Subdomain  .

2. Set the subdomain name to rot_trans and click OK.

3. Configure the following setting(s):

   Tab	Setting	Value
   Basic Settings	Location	B86
   Mesh Motion	Mesh Motion > Option	Rigid Body Solution
   	Mesh Motion > Rigid Body	Rigid Body 1
   	Mesh Motion > Motion Constraints	(Selected)
   	Mesh Motion > Motion Constraints > Motion Constraints	None

4. Click OK.

1. Edit Simulation > Flow Analysis 1 > buoy > Default Fluid Fluid Interface Side 1.

2. Configure the following setting(s):

   Tab	Setting	Value
   Basic Settings	Location	F74.27[a]
   Boundary Details	Mesh Motion > Option	Rigid Body Solution
   	Mesh Motion > Rigid Body	Rigid Body 1
   	Mesh Motion > Motion Constraints	(Selected)
   	Mesh Motion > Motion Constraints > Motion Constraints	Ignore Rotations[b]
   This is the outer cylindrical domain interface. Ignore Rotations constrains the outer domain interface to only translational motion.

3. Click OK.

4. Edit Simulation > Flow Analysis 1 > buoy > Default Fluid Fluid Interface Side 2.

5. Configure the following setting(s):

   Tab	Setting	Value
   Basic Settings	Location	F89.86[a]
   Boundary Details	Mesh Motion > Option	Rigid Body Solution
   	Mesh Motion > Rigid Body	Rigid Body 1
   	Mesh Motion > Motion Constraints	(Selected)
   	Mesh Motion > Motion Constraints > Motion Constraints	None
   This is the inner cylindrical domain interface.

6. Click OK.

1. Click Define Run  .

2. Configure the following setting(s):

   Setting	Value
   File name	Buoy_decoupled.def

3. Click Save.

   CFX-Solver Manager automatically starts and, on the Define Run dialog box, Solver Input File is set.

4. Quit CFX-Pre, saving the simulation (.cfx) file.

1. Select File > Load State and choose the name Buoy.cst.

2. Click Open.

1. Ensure that Contour 1 is visible in the 3D Viewer (make sure there is a check mark beside Contour 1 in the Outline tree view).

2. Turn off the visibility of Plane 1 and Default Legend View 1 to better see the movement of the buoy.

3. Edit Wireframe and configure the following setting(s):

   Tab	Setting	Value
   Definition	Show surface mesh	(Selected)

4. Click the Timestep Selector  . Select the 1^st time step and click Apply.

5. Click Animation   in the Timestep Selector dialog box.

   The Animation dialog box appears.

6. Set Type to Keyframe Animation.

7. Click New   to create KeyframeNo1.

8. Select KeyframeNo1, then set # of Frames to 93, then press Enter while the cursor is in the # of Frames box.

   ---

   Tip:  Be sure to press Enter and confirm that the new number appears in the list before continuing.

   ---

9. Use the Timestep Selector to load the 280^th time step.

10. In the Animation dialog box, click New   to create KeyframeNo2.

11. Ensure that More Animation Options   is pushed down to show more animation settings.

12. Select Loop.

13. Ensure that Repeat forever   (next to Repeat) is not selected (not pushed down).

14. Select Save Movie.

15. Set Format to MPEG1.

16. Set File name to Buoy_decoupled.mpg.

17. If you want to save the animation to a location other than your working directory, click Browse   (next to Save Movie) to set the path to a different directory and click Save.

    The movie filename (including the path) has been set, but the animation has not yet been produced.

18. Click To Beginning  .

    This ensures that the animation will begin at the first keyframe.

19. After the first keyframe has been loaded, click Play the animation  .

    • The MPEG will be created as the animation proceeds.

20. Close the Animation dialog box when the animation is complete.

1. Click the Timestep Selector   and load the 162^nd time step.

2. Select Tools > Mesh Calculator or click the Calculators tab and select Mesh Calculator.

3. Configure the following setting(s):

   Tab	Setting	Value
   Mesh Calculator	Function	Minimum Face Angle

4. Click Calculate.

   You can also check other time steps to calculate the mesh quality throughout the simulation.

5. When you have finished, close the Timestep Selector dialog box.