11.3.9 Specifying the Motion of Dynamic Zones

You need to 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 6DOF solver. If the zone is a deforming zone, you can define the geometry and the parameters that control face 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.

General Procedure

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

Dynamic Mesh Create/Edit...

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

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.

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.

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 Center of Gravity Orientation.

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.

Stationary Motion

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 11.3.41: 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, 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 ( $h_{\rm ideal}$ in this equation and this equation of the in the separate Theory Guide) 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 UDF Manual for information about UDFs.

4.   Click Create.

Rigid Body Motion

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

Figure 11.3.42: 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 Section  7.6 and Section  11.3.4 for information on profiles, and see the separate UDF Manual for information on user-defined functions.

4.   If you want to use the Six DOF Solver option, then select the appropriate UDF from the Six DOF UDF drop-down list in the Motion Attributes tab (see Figure  11.3.43). Note that you should make sure that On is enabled under Six DOF Solver Options to ensure that the Six DOF solver is being used. See the separate UDF Manual for information on user-defined functions. For more information about the 6DOF solver, see Section  11.3.7.

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

5.   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.

6.   Specify the orientation of the object with respect to the center of gravity (in the inertia coordinate system) by entering the orientations of the center of gravity in Center of Gravity Orientation.

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 center of gravity orientation is most useful when using the Six DOF solver, where it is used to compute the transformation matrices ( this section in the separate Theory Guide).

7.   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 center of gravity with respect to the inertia coordinate system by entering the angular velocity of the center of gravity in Center of Gravity Angular Velocity.

Figure 11.3.43: The Dynamic Mesh Zones Dialog Box for a Rigid Body Motion Using the Six DOF Solver

8.   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.

9.   If the rigid body zone is a face zone, specify

the Cell Height for each Adjacent Zone in the Meshing Options tab. The Cell Height is the ideal cell height ( $h_{\rm ideal}$ in this equation and this equation of the in the separate Theory Guide) 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 need to 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 separate UDF Manual for information about UDFs.

10.   Click Create.

Deforming Motion

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

Figure 11.3.44: The Dynamic Mesh Zones Dialog Box for a Deforming Motion

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. There are four options:

• 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 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 separate UDF Manual for information on user-defined functions.

For 3D simulations, ANSYS FLUENT allows you to preserve features not only between the different face zones, but also within a face zone. For any geometry definition ( faceted, plane, cylinder, or user-defined), you can indicate whether you want to include features of a specific angle by selecting Include Features under Feature Detection and setting the Feature Angle in degrees. For more information, see Section  11.3.2.

When available, the geometry information is used to project nodes on the deforming zone after remeshing the face zone, or if nodes are moved from the spring-based smoothing method.

4.   Specify the appropriate remeshing parameters in the Meshing Options tab.

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

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

If you selected a cell or face zone, you need to enter Minimum Length Scale, Maximum Length Scale and Maximum Skewness if you want impose a different set of remeshing criteria, other than those you specified globally in the Dynamic Mesh task page. This is not required for cell zones since the global settings for the dynamic mesh parameters are used if ANSYS FLUENT determines that the local settings are unreasonable. You should use the information found in the Zone Scale Info dialog box in order to set your values.

5.   Click Create.

User-Defined Motion

For a zone that is deforming and 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 and 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 separate UDF Manual for information on user-defined functions used to specify user-defined motion.

4.   For face zones, you can specify the Cell Height in the Meshing Options tab for any Adjacent Zone which is involved in local remeshing or dynamic layering. The Cell Height specifies the ideal height ( $h_{\rm ideal}$ in this equation and this equation of the in the separate Theory Guide) 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 UDF Manual for information about UDFs.

5.   Click Create.

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 defined using a user-defined function (UDF), as described in Section  11.3.9. To define a moving and deforming boundary layer, 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.

4.   Click Create.

5.   Create a deforming dynamic zone for the boundary layer fluid zone by selecting the zone in the Zone Names drop-down list. Note that the boundary layer has to be a separate fluid zone from the adjacent fluid zone. Select Deforming under Type and enable Smoothing on the boundary layer fluid zone.

6.   Click Create.

7.   Create a deforming dynamic zone for the fluid zone outside the boundary layer by selecting the appropriate zone from the Zone Names drop-down list. Select Deforming under Type and enable Smoothing and Remeshing in the Methods group box. Enabling both methods is necessary because the deforming boundary layer will deform the adjacent cells.

8.   Click Create.