10.6.9. Specifying the Motion of Dynamic Zones

You must define the motion of the dynamic zones in your model. If the zone is a rigid body, you can use a profile or user-defined function (UDF) to define the motion of the rigid body or use the six DOF solver. If the zone is a deforming zone, you can define the geometry and the parameters that control the face or zone remeshing, if applicable. For a zone that is deforming and moving at the same time, you can use a user-defined function to define the geometry and motion of the zone as they change with time.

10.6.9.1. General Procedure

You will specify the motion of the dynamic zones in your model using the Dynamic Mesh Zones dialog box

 Setup →   Dynamic Mesh → Create/Edit...

Details about specifying different types of motion are provided in this section.

10.6.9.1.1. Creating a Dynamic Zone

When you have completed the specification of a dynamic zone, click Create in the Dynamic Mesh Zones Dialog Box to complete the specification and add the zone to the Dynamic Mesh Zones list.

10.6.9.1.2. Modifying a Dynamic Zone

If you want to make a change to the specification of a dynamic zone, select the zone in the Dynamic Mesh Zones list, change the specification, and then click Create in the Dynamic Mesh Zones Dialog Box to update the specification.

10.6.9.1.3. Checking the Center of Gravity

If a dynamic zone has solid body motion, you can view its current position and orientation of the center of gravity (with respect to initial data) by selecting the zone in the Dynamic Mesh Zones list and viewing the values under Center of Gravity Location and Rigid Body Orientation.

10.6.9.1.4. Deleting a Dynamic Zone

To delete a dynamic zone that you have specified, select the zone in the Dynamic Mesh Zones list, and click Delete or Delete All. The zone or zones will be removed from the Dynamic Mesh Zones list.

10.6.9.2. Stationary Zones

By default, if no motion (moving or deforming) attributes are assigned to a face or cell zone, then the zone is not considered when updating the mesh to the next time step. However, there are cases where an explicit declaration of a stationary zone is required. For example, if a cell zone is assigned some solid body motion, the positions of all nodes belonging to the cell zone will be updated even though some of the nodes may also be part of a non-moving boundary zone. An explicit declaration of a stationary zone excludes the nodes on these zones when updating the node positions.

Figure 10.83:  The Dynamic Mesh Zones Dialog Box for a Stationary Zone

The Dynamic Mesh Zones Dialog Box for a Stationary Zone

To define a stationary zone in your model, follow the steps below.

  1. Select the stationary zone in the Zone Names drop-down list.

  2. Select Stationary under Type.

  3. If the stationary zone is a face zone that is not a boundary of a CutCell dynamic cell zone, then define the Cell Height in the Meshing Options tab for any Adjacent Zone that is involved in local remeshing or dynamic layering. The Cell Height specifies the ideal height ( in Equation 10–15 and Equation 10–16 of the adjacent cells. Make a selection in the Cell Height drop-down menu to specify this value as either a constant or a compiled user-defined function.

    If you select the constant option, enter a value in the Cell Height text-entry box.

    If you choose to use a compiled user-defined function to define an ideal cell height that varies as a function of time or crank angle, you must first define a DEFINE_DYNAMIC_ZONE_PROPERTY UDF. After you have compiled the UDF source file, built a shared library, and loaded it into ANSYS Fluent, the name of the UDF library will be available for selection in the Cell Height drop-down list.

    Refer to the Fluent Customization Manual for information about UDFs.

  4. If the stationary zone is a boundary of a CutCell dynamic cell zone (this is automatically detected if the CutCell dynamic cell zone is created first), then enter values for the Maximum Mesh Size and Growth Rate in the Meshing Options tab. If you have enabled Inflation Layers for the cell zone, then you will also have the option to enable Zonal Inflation Layer Control on the boundary zone and specify local inflation settings in the Inflation Settings dialog box (using the Settings... button). See Figure 10.84: The Dynamic Mesh Zones Dialog Box for a CutCell Boundary Zone for an example of the Dynamic Mesh Zones dialog box with the Meshing Options tab as it appears for CutCell boundary zones. (The same meshing input is required at all CutCell boundary zones, whether the motion type is Stationary, Rigid Body, Deforming, or User-Defined.)

    Two different size functions are available to control the local mesh refinement:

    • soft size function

      For this size function, the Cartesian mesh is locally refined such that the resulting mesh size is smaller or equal to the Maximum Mesh Size specified.

    • mesh-based size function

      For this size function, the Cartesian mesh is locally refined such that the resulting mesh size is locally of the same size as the input mesh provided.

    The switch between using the soft or the mesh-based size function depends on the value entered for the Maximum Mesh Size. A value of 0 specifies that the mesh-based size function is used. If a positive value is entered, then the soft size-function is used and the value entered locally limits the mesh size. The Growth Rate controls the rate at which the Cartesian mesh grows away from the boundary. The maximum Cartesian mesh size obtained in the cell zone is always controlled by the specified Maximum Mesh Size for the CutCell cell zone.

    Figure 10.84:  The Dynamic Mesh Zones Dialog Box for a CutCell Boundary Zone

    The Dynamic Mesh Zones Dialog Box for a CutCell Boundary Zone

    You can view the vital statistics of your zone by clicking on the Zone Scale Info… button. This opens the Zone Scale Info Dialog Box, where you can view the minimum, maximum, and average length scale values, as well as the maximum skewness value.

  5. For cases with strong fluid-structure interaction, solution stabilization may help convergence for boundary zones. Solution stabilization can be set in the Solver Options tab. See Solution Stabilization for Dynamic Mesh Boundary Zones for details.

  6. Click Create.

    Note that if you specify inflation layer parameters in the Inflation Settings dialog box, these settings are not saved until you create or update the dynamic zone.

10.6.9.3. Rigid Body Motion

To define a rigid-body zone in your model, follow the steps below.

Figure 10.85:  The Dynamic Mesh Zones Dialog Box for a Rigid Body Motion

The Dynamic Mesh Zones Dialog Box for a Rigid Body Motion

  1. Select the rigid body zone in the Zone Names drop-down list.

  2. Select the Rigid Body option under Type.

  3. If you want to specify the motion of the rigid body zone using a profile or user-defined function, then select a profile or user-defined function from the Motion UDF/Profile drop-down list in the Motion Attributes tab. See Profiles and Solid-Body Kinematics for information on profiles, and see the Fluent Customization Manual for information on user-defined functions.

  4. If you enabled the In-Cylinder option in the Dynamic Mesh Task Page, ANSYS Fluent provides built-in functions in the Motion UDF/Profile drop-down list that can be useful for defining the rigid body motion of a piston. If you would like the motion of the piston to be a function of crank angle (that is, governed by Equation 10–25), then you should select **piston-full**. For further information, see In-Cylinder Settings.

  5. If you enabled the Six DOF option in the Dynamic Mesh Task Page, make sure that On is enabled in the Six DOF group box in the Motion Attributes tab (see Figure 10.87: The Dynamic Mesh Zones Dialog Box for a Rigid Body Motion Using the Six DOF Solver), to ensure that the six DOF solver is being used. Then make a selection from the Six DOF UDF/Properties drop-down list; for details on creating the selections available in this list, Setting Rigid Body Motion Attributes for the Six DOF Solver.

    Note that the Passive option in the Six DOF group box is used when you do not want the forces and moments on the zone to be taken into consideration.

  6. Specify the initial location of the center of gravity for the rigid body by entering the coordinates of the center of gravity in Center of Gravity Location. Note that for one DOF dynamic zones, this field will be overwritten when you click Create by the Center of Rotation values you specified in the Six DOF Properties Dialog Box.

  7. If you want a rigid body to move relative to another rigid body, then you must enable Relative Motion and specify the Relative Zone.


    Note:  You must create the relative rigid body zone before creating a rigid body that is dependent on that zone, if you are setting up the motion using the graphical user interface (GUI). The order in which you specify the zones does not matter if you set up the motion using the text user interface (TUI).


  8. Specify the orientation of the rigid body (in the inertial coordinate system) by entering the orientations of the rigid body in Rigid Body Orientation.

    Together, the Rigid Body Orientation and the Center of Gravity Location are the local reference frame that you can choose to use for your user-defined function (UDF) or set of six DOF properties that describes the motion of the rigid body. For additional information about creating UDFs for solid-body kinematics, see DEFINE_CG_MOTION in the Fluent Customization Manual; for details on creating UDFs / properties for the six DOF solver, see Setting Rigid Body Motion Attributes for the Six DOF Solver.

    For most cases, this is an initial reference orientation that ANSYS Fluent later updates, letting you keep track of the object’s current orientation. The rigid body orientation is most useful when using the six DOF solver, where it is used to compute the transformation matrices (Six DOF Solver Theory in the Theory Guide).

    If needed, you can use the Orientation Calculator to convert a rotation matrix or Euler angles into the required axis and angle inputs. You can also use this calculator if you know the rotations the rigid body will experience, but do not know its final orientation.

    Figure 10.86:  Orientation Calculator Dialog Box

    Orientation Calculator Dialog Box

    To use the Orientation Calculator:

    1. Enter a value, either in Axis and Angle, Rotation Matrix, or Euler Angle format, and click Evaluate to see the value in the output format.

      The calculator also converts the entered values into the other two “grayed-out” input formats.


      Note:  There are several possible Euler angle representations. Fluent uses a vector defined by , , and where: is the rotation about the original Z axis, is the rotation about the rotated Y axis, and is the rotation about the rotated X axis.


    2. Enable Concatenate Next Input if you want the next input to be concatenated to the previous output.

    3. Click Fill to use the current Output as your Rigid Body Orientation in the Dynamic Mesh Zones dialog box.

  9. When using the six DOF solver, specify the velocity of the center of gravity with respect to the inertia coordinate system by entering the velocity of the center of gravity in Center of Gravity Velocity. Also, specify the angular velocity of the rigid body with respect to the inertia coordinate system by entering the angular velocity of the rigid body in Rigid Body Angular Velocity. Note that these fields are ignored for one DOF rotation and translation, respectively.

    Figure 10.87:  The Dynamic Mesh Zones Dialog Box for a Rigid Body Motion Using the Six DOF Solver

    The Dynamic Mesh Zones Dialog Box for a Rigid Body Motion Using the Six DOF Solver

  10. If you are solving an in-cylinder problem, specify the direction of the reference axis of the valves or piston in Valve/Piston Axis.

    The current valve lift or piston stroke is automatically updated in Lift/Stroke when you click Create based on the parameters you have specified earlier when you first invoke the in-cylinder option.

  11. By default, the boundary mesh motion is taken into consideration when imposing the physical boundary conditions, even if the boundary moves because of a moving adjacent cell zone and no dynamic zone has been created for the boundary. If this is not the desired behavior, and if you would like to exclude the mesh motion from contributing to the boundary conditions, then you need to enable the Exclude Mesh Motion in Boundary Conditions option for that zone.

  12. If the rigid body zone is a face zone that is not a boundary of a CutCell dynamic cell zone, specify the Cell Height for each Adjacent Zone in the Meshing Options tab. The Cell Height is the ideal cell height ( in Equation 10–15 and Equation 10–16 that is used by ANSYS Fluent to determine when the prismatic layer next to the rigid body should be split or merged with the layer next to it. If the adjacent zone is tetrahedral or triangular, the ideal height is used by ANSYS Fluent to determine if adjacent cells must be agglomerated for local remeshing. Make a selection in the Cell Height drop-down menu to specify this value as either a constant or a compiled user-defined function.

    If you select the constant option, enter a value in the Cell Height text-entry box.

    If you choose to use a compiled user-defined function to define an ideal cell height that varies as a function of time or crank angle, you must first define a DEFINE_DYNAMIC_ZONE_PROPERTY UDF. After you have compiled the UDF source file, built a shared library, and loaded it into ANSYS Fluent, the name of the UDF library will be available for selection in the Cell Height drop-down list.

    Refer to the Fluent Customization Manual for information about UDFs.

  13. If the rigid body zone is a boundary of a CutCell dynamic cell zone (this is automatically detected if the CutCell dynamic cell zone is created first), then enter values for the Maximum Mesh Size and Growth Rate in the Meshing Options tab, as described in step 4 of Stationary Zones. If you have enabled Inflation Layers for the cell zone, then you will also have the option to enable Zonal Inflation Layer Control on the boundary zone and specify local inflation settings in the Inflation Settings dialog box (using the Settings... button).

  14. If the dynamic zone is a face zone with an adjacent boundary layer mesh, you must apply boundary layer smoothing using the Deform Adjacent Boundary Layer with Zone option in the Meshing Options tab if you want the boundary layer to move with the moving face zone. For example, this option is necessary if you are applying face region remeshing with prism layers and you have not decomposed the mesh volume (see Face Region Remeshing with Wedge Cells in Prism Layers). In such circumstances, the Deform Adjacent Boundary Layer with Zone option ensures that the base prism elements shown in Figure 10.43: Volume Decomposition for the Base of the Prism Layers will move rigidly with the piston.

    Note that the boundary layer smoothing method is primarily intended for translational motion of the face zone. If significant rotation is applied to the face zone, the boundary layer cells may become skewed. For more information refer to Boundary Layer Smoothing Method.

  15. For cases with strong fluid-structure interaction, solution stabilization may be necessary for boundary zones if the use of implicit mesh updating (described in Implicit Update Settings) is insufficient to stabilize the solver due to the fluid motion. Solution stabilization options can be set in the Solver Options tab. See Solution Stabilization for Dynamic Mesh Boundary Zones for details.

  16. Click Create.

10.6.9.4. Deforming Motion

To define a deforming zone in your model, follow the steps below.

Figure 10.88:  The Dynamic Mesh Zones Dialog Box for a Deforming Motion with Cell Zone Options

The Dynamic Mesh Zones Dialog Box for a Deforming Motion with Cell Zone Options

  1. Select the deforming zone in the Zone Names drop-down list.

  2. Select the Deforming option under Type.

  3. Specify the geometry of the deforming zone in the Geometry Definition tab.

    • If no geometry is available, select faceted in the Definition drop-down list.

    • If the geometry is a plane, select plane in the Definition drop-down list. To define the plane, enter the position of a point on the plane in Point on Plane and the plane normal in Plane Normal.

    • If the geometry is a cylinder, select cylinder in the Definition drop-down list. To define the cylinder, enter the Cylinder Radius, the Cylinder Origin and the Cylinder Axis.

    • If the geometry is unspecified and mesh motion normal to the boundary is permissible, select unspecified in the Definition drop-down list. This option is only available if the linearly elastic solid mesh smoothing method is enabled (Linearly Elastic Solid Based Smoothing Method).

    • If the geometry is described by a user-defined function, select user-defined in the Definition drop-down list and the appropriate user-defined functions in the Geometry UDF drop-down list. See the Fluent Customization Manual for information on user-defined functions.

    For 3D simulations, ANSYS Fluent allows you to preserve features on the boundary zones that are important for the flow. Such features may be at the juncture of different boundary zones, or they may be on a single non-planar boundary zone. For any geometry definition (faceted, plane, cylinder, or user-defined), you can indicate whether you want to preserve features of a specific angular range by selecting Include Features under Feature Detection and setting a threshold value for the Feature Angle in degrees. For more information (including how the Feature Angle is defined), see Feature Detection.

    When available, the geometry information is used to project nodes on the deforming zone after remeshing the face zone, or if nodes are moved through smoothing.

  4. For deforming face and cell zones that are not CutCell zones, specify the appropriate remeshing parameters in the Meshing Options tab.

    You can locally disable or enable Smoothing and/or Remeshing and use any Smoothing Methods and/or Remeshing Methods.

    You can view the vital statistics of your zone by clicking the Zone Scale Info... button. This opens the Zone Scale Info Dialog Box, where you can view the minimum and maximum length scale values, as well as the maximum skewness values.

    You can revise the Minimum Length Scale, Maximum Length Scale and/or Maximum Skewness if you want to specify local values for this dynamic zone that differ from those you specified globally in the Mesh Method Settings Dialog Box. Note that the global settings may still be used if ANSYS Fluent determines that your local settings are unreasonable. You should use the information found in the Zone Scale Info Dialog Box in order to set your values.

    If spring-based smoothing is used and you selected a cell zone, then you have the option to overwrite the element type selection made in the Mesh Method Settings dialog box (see Figure 10.14: The Smoothing Tab of the Mesh Method Settings Dialog Box (3D)). Select Global Settings if no zone specific smoothing element type is desired.

  5. To specify that a deforming cell zone is remeshed using the CutCell zone method, enable the CutCell option in the Remeshing Options group box of the Meshing Options tab (see Figure 10.89: The Dynamic Mesh Zones Dialog Box for a Deforming CutCell Cell Zone). Note that this option is only available if you have previously enabled the CutCell Zone option in the Remeshing tab of the Mesh Method Settings dialog box (see Figure 10.33: The Remeshing Tab in the Mesh Method Settings Dialog Box).

    Figure 10.89:  The Dynamic Mesh Zones Dialog Box for a Deforming CutCell Cell Zone

    The Dynamic Mesh Zones Dialog Box for a Deforming CutCell Cell Zone

    After the CutCell option has been enabled, you must enter values for the global CutCell parameters Maximum Mesh Size and Growth Rate, as well as the controls for the remeshing frequency, Minimum Orthogonal Quality and Remeshing Interval. You also have the option to enable Inflation Layers for the cell zone and specify the global inflation parameters in the Inflation Settings dialog box. See Using the CutCell Zone Remeshing Method for more information about adding inflation layers to a CutCell mesh.

    The Maximum Mesh Size specified for the CutCell cell zone controls the global maximum size of the Cartesian cells. The global Growth Rate is used for all mesh-based size functions applied to CutCell boundary zones that are not defined as dynamic zones. When selecting values for these controls, it may be helpful to view the statistics of your cell zone by clicking on the Zone Scale Info… button. This opens the Zone Scale Info Dialog Box, where you can view the minimum and maximum length scale values, as well as the maximum skewness values.

    The CutCell remeshing is performed automatically whenever cells exhibit an orthogonal quality (as defined in Mesh Quality) that is less than the specified Minimum Orthogonal Quality. The remeshing is also performed periodically after the calculation has undergone the number of time steps you specified for the Remeshing Interval.

    Click the Boundary Zones Info… button to open the CutCell Boundary Zones Info dialog box (Figure 10.90: The CutCell Boundary Zones Info Dialog Box). This dialog box lists all the boundary zones associated with the CutCell cell zone, along with the associated size functions and zonal meshing parameters. The inflation layer settings used on all boundaries are also shown. It is recommended that you revisit this dialog box after you have created all of the dynamic zones, in order to review all of the parameters you have set.

    Figure 10.90:  The CutCell Boundary Zones Info Dialog Box

    The CutCell Boundary Zones Info Dialog Box

  6. If the deforming zone is a boundary of a CutCell dynamic cell zone (this is automatically detected if the CutCell dynamic cell zone is created first), then enter values for the Maximum Mesh Size and Growth Rate in the Meshing Options tab, as described in step 4 of Stationary Zones. If you have enabled Inflation Layers for the cell zone, then you will also have the option to enable Zonal Inflation Layer Control on the boundary zone and specify local inflation settings in the Inflation Settings dialog box (using the Settings... button).

  7. For cases with strong fluid-structure interaction, solution stabilization may help convergence for boundary zones. Solution stabilization can be set in the Solver Options tab. See Solution Stabilization for Dynamic Mesh Boundary Zones for details.

  8. Click Create.

10.6.9.5. User-Defined Motion

For a zone that is deforming and/or moving, you can define the position of each node on the general deforming / moving zone using a user-defined function (UDF). To define a moving / deforming zone, follow the steps below.

  1. Select the moving and deforming zone in the Zone Names drop-down list.

  2. Select the User-Defined option under Type.

  3. In the Motion Attributes tab, select the user-defined function that defines the geometry and motion of the zone from the Mesh Motion UDF drop-down list. See the Fluent Customization Manual for information on user-defined functions used to specify user-defined motion.

  4. By default, the boundary mesh motion is taken into consideration when imposing the physical boundary conditions, even if the boundary moves because of a moving adjacent cell zone and no dynamic zone has been created for the boundary. If this is not the desired behavior, and if you would like to exclude the mesh motion from contributing to the boundary conditions, then you need to enable the Exclude Mesh Motion in Boundary Conditions option for that zone.

  5. If you want the movement / deformation to be relative to the rigid body motion of a cell zone, then you can enable Relative Motion and select the cell zone from the Relative Zone list.


    Note:  You must specify the movement / deformation in your UDF using NODE_COORD_NEST, rather than specify the final coordinates (as you would if you were NOT specifying it relative to a cell zone). For additional information, see DEFINE_GRID_MOTION in the Fluent Customization Manual.

    You must create the relative rigid body zone before creating the user-defined zone if you are setting up the zones using the graphical user interface (GUI). The order in which you create the zones does not matter if you set up the zones using the text user interface (TUI).


  6. For a face zone that is not a boundary of a CutCell dynamic cell zone, you can specify the Cell Height in the Meshing Options tab for any Adjacent Zone that is involved in local remeshing or dynamic layering. The Cell Height specifies the ideal height ( in Equation 10–15 and Equation 10–16 of the adjacent cells. Make a selection in the Cell Height drop-down menu to specify this value as either a constant or a compiled user-defined function.

    If you select the constant option, enter a value in the Cell Height text-entry box.

    If you choose to use a compiled user-defined function to define an ideal cell height that varies as a function of time or crank angle, you must first define a DEFINE_DYNAMIC_ZONE_PROPERTY UDF. After you have compiled the UDF source file, built a shared library, and loaded it into ANSYS Fluent, the name of the UDF library will be available for selection in the Cell Height drop-down list.

    Refer to the separate Fluent Customization Manual for information about UDFs.

  7. If the face zone is a boundary of a CutCell dynamic cell zone (this is automatically detected if the CutCell dynamic cell zone is created first), then enter values for the Maximum Mesh Size and Growth Rate in the Meshing Options tab, as described in step 4 of Stationary Zones. If you have enabled Inflation Layers for the cell zone, then you will also have the option to enable Zonal Inflation Layer Control on the boundary zone and specify local inflation settings in the Inflation Settings dialog box (using the Settings... button).

  8. If the dynamic zone is a face zone with an adjacent boundary layer mesh, and you want to use the boundary layer smoothing method (as described in Boundary Layer Smoothing Method), enable the Deform Adjacent Boundary Layer with Zone option in the Meshing Options tab.

  9. For a 3D boundary zone, you can allow local face remeshing by enabling the Local option (under Remeshing Methods) in the Meshing Options tab. For details, see Local Face Remeshing Method. Enabling this option allows you to do the following:

    • You can revise the Maximum Skewness allowed for faces if you want to specify a local value for this dynamic zone that differs from the one you specified globally in the Mesh Method Settings Dialog Box. Note that the global setting may still be used if ANSYS Fluent determines that your local setting is unreasonable.

    • You can preserve features, not only at the juncture of different boundary zones, but also on a single non-planar boundary zone. In the Geometry Definition tab, you can indicate whether you want to include features of a specific angular range by selecting Include Features under Feature Detection and setting a threshold value for the Feature Angle in degrees. For more information (including how the Feature Angle is defined), see Feature Detection.

  10. For cases with strong fluid-structure interaction, solution stabilization may help convergence for boundary zones. Solution stabilization can be set in the Solver Options tab. See Solution Stabilization for Dynamic Mesh Boundary Zones for details.

  11. Click Create.

10.6.9.5.1. Specifying Boundary Layer Deformation Smoothing

For a boundary layer that deforms according to the adjacent face zone, the zone that is deforming and moving is usually defined using a user-defined function (UDF), as described in User-Defined Motion. To define a moving and deforming boundary layer, perform the steps that follow.

If the boundary layer borders a face zone that is only moving and is not deforming, you should consider applying rigid body motion to the face zone (see Rigid Body Motion) rather than user-defined motion, as rigid body motion usually involves a simpler UDF.

  1. Set up the moving and deforming zone.

    1. Select the moving and deforming zone in the Zone Names drop-down list.

    2. Select the User-Defined option under Type.

    3. In the Motion Attributes tab, select the user-defined function that defines the geometry and motion of the zone from the Mesh Motion UDF drop-down list.

    4. In the Meshing Options tab, enable the Deform Adjacent Boundary Layer with Zone option.

    5. Click Create.

  2. Set up a deforming dynamic zone for the fluid zone that contains the boundary layer.

    1. Select the fluid zone that contains the boundary layer from the Zone Names drop-down list.

    2. Select Deforming from Type list.

    3. In the Meshing Options tab, enable Smoothing and Remeshing in the Methods group box.

    4. Click Create.

  3. If the fluid zone set up in the step 2 consists entirely of the boundary layer elements, set up a deforming dynamic zone for the neighboring fluid zone. This step is necessary because the deforming boundary layer will deform the adjacent cells.

    1. Select the fluid zone that neighbors the boundary layer zone from the Zone Names drop-down list.

    2. Select Deforming from Type list.

    3. In the Meshing Options tab, enable Smoothing and Remeshing in the Methods group box.

    4. Click Create.

10.6.9.6. System Coupling Motion

For a zone that is involved in a system coupling, the motion is defined by the application that ANSYS Fluent is coupled with on this zone. For more details about setting up a simulation with system coupling see the Fluent in Workbench User's Guide and the System Coupling Guide. To define a system coupling region, follow the steps below.

  1. Select the moving and deforming zone in the Zone Names drop-down list.

  2. Select the System Coupling option under Type.

  3. The system coupling region cannot be a boundary of a CutCell dynamic cell zone, so you can specify the Cell Height in the Meshing Options tab for any Adjacent Zone that is involved in local remeshing or dynamic layering. The Cell Height specifies the ideal height ( in Equation 10–15 and Equation 10–16 of the adjacent cells. Make a selection in the Cell Height drop-down menu to specify this value as either a constant or a compiled user-defined function.

    If you select the constant option, enter a value in the Cell Height text-entry box.

    If you choose to use a compiled user-defined function to define an ideal cell height that varies as a function of time or crank angle, you must first define a DEFINE_DYNAMIC_ZONE_PROPERTY UDF. After you have compiled the UDF source file, built a shared library, and loaded it into ANSYS Fluent, the name of the UDF library will be available for selection in the Cell Height drop-down list.

    Refer to the separate Fluent Customization Manual for information about UDFs.

  4. For cases with strong fluid-structure interaction, solution stabilization may be necessary to achieve convergence for boundary zones undergoing system coupling motion. Solution stabilization options can be set in the Solver Options tab. See Solution Stabilization for Dynamic Mesh Boundary Zones for details.

  5. Click Create.


Note:   If the System Coupling option is enabled, and ANSYS Fluent is not involved with a system coupling simulation, then this zone type behaves in the same way as a stationary zone.


10.6.9.7. Solution Stabilization for Dynamic Mesh Boundary Zones

For cases with strong fluid-structure interaction, stabilization is achieved through a boundary source coefficient introduced in the continuity equation, designed to improve the diagonal dominance of the matrix system in the cells adjacent to dynamic mesh boundary zones. Two methods for this boundary source coefficient are available:

  • volume-based

    This method uses the cell volume to re-scale the diagonal entry of the linear matrix system corresponding to the discretized continuity equation () as :

    (10–32)

  • coefficient-based

    This method directly re-scales the diagonal entry of the linear matrix system corresponding to the discretized continuity equation () as :

    (10–33)

where is the scale factor and is the number of cells. Note that the value you choose for will only affect the rate of convergence, and will not affect the converged solution.


Note:  While solution stabilization is available for all types of dynamic mesh boundary zones, it is more commonly needed for rigid body motion with the six degree of freedom (six DOF) solver or for system coupling motion. It is not recommended for boundary zones of type interior, as it can adversely affect convergence.


Solution stabilization can be enabled for a boundary zone by opening the Solver Options tab in the Dynamic Mesh Zones Dialog Box, enabling the Solution Stabilization option, and then defining the settings under Stabilization Parameters. Available settings include the Scale Factor () and the Method, which can be either volume-based (default) or coefficient-based. The Scale Factor must be set to a nonzero value for the stabilization to have an effect.

The solver option settings can also be defined using the define/dynamic-mesh/zones/create text command, and a summary of these settings can be printed in the console for each dynamic zone by using the define/dynamic-mesh/zones/list text command.

10.6.9.8. Solid-Body Kinematics

ANSYS Fluent uses solid-body kinematics if the motion is prescribed based on the position and orientation of the center of gravity of a moving object. This is applicable to both cell and face zones.

The motion of the solid-body can be specified either as a profile or as a user-defined function (UDF). A profile may be defined by the following profile fields:

  • time (time)

  • crank angle (angle) (in-cylinder flows only)

  • position (, , )

  • linear velocity (, , )

  • angular velocity (, , )

  • orientation (, , )

For in-cylinder simulations, the velocity profiles for valves can be expressed as a function of crank angle instead of time. In addition, transient boundary condition profiles can also be expressed as a function of crank angle instead of time. For more information about transient profiles, see Defining Transient Cell Zone and Boundary Conditions.

Below are two examples of a profile format:

 ((movement_linear 3 point)
 (time
 0  1  2 )
 (x
 2  3  4 )
 (v_y
 0  -5  0 )
 )
 ((movement_angular 3 point)
 (time
 0  1  2 )
 (omega_x
 2  3  4 )
 )

For in-cylinder flows, crank angles can be included in transient tables as well as transient profiles, in a similar fashion to time. An example of a transient table using (crank) angle is as follows:

 example 2 3 1
 angle temperature 
 0  300 
 180 500 
 360 300 

An example of a transient profile using (crank) angle is as follows:

 ((example transient 3 1)
 (angle 
 0.000000e+00 1.800000e+02 3.600000e+02)
 (temperature 
 3.000000e+02 5.000000e+02 3.000000e+02)
 )

In addition to the motion description, you must also specify the starting location of the center of gravity and orientation of the solid body. In 2D cases (and 3D cases that do not use the six DOF solver), ANSYS Fluent automatically updates the center of gravity position and orientation at every time step such that

(10–34)

where and are the position and orientation of the center of gravity, and are the linear and angular velocities of the center of gravity. 3D, six DOF cases use a more complex form of Equation 10–34 when updating .

Typically, is chosen to be an appropriate set of Euler angles. In this case, the solid-body motion must be specified using a user-defined function (DEFINE_CG_MOTION).

Figure 10.91:  Solid Body Rotation Coordinates

Solid Body Rotation Coordinates

The position vectors on the solid body are updated based on rotation about the instantaneous angular velocity vector . For a finite rotation angle = , the final position of a vector on the solid body with respect to can be expressed as (See Figure 10.91: Solid Body Rotation Coordinates)

(10–35)

where can be shown to be

(10–36)

The unit vectors and are defined as

(10–37)

(10–38)

If the solid body is also translating with , the position vector on the solid body can be expressed as

(10–39)

where is given by Equation 10–35.


Release 18.2 - © ANSYS, Inc. All rights reserved.