10.6.7. Contact Detection Settings

Contact detection is used to detect if the computed mesh motion will result in contact of a moving surface with other surrounding surfaces. If there is contact within specified tolerances, then the mesh motion of the moving zone can be constrained using nodal contact information within user-defined functions (See Example 2 under DEFINE_CONTACT in the Fluent ).

To enable contact detection in your dynamic mesh simulation, select the Contact Detection check box in the Options group of the Dynamic Mesh task page. Click the Settings... button to open the Options dialog box and select the Contact Detection tab (see Figure 10.73: The Contact Detection Tab of the Options Dialog Box).

Figure 10.73:  The Contact Detection Tab of the Options Dialog Box

The Contact Detection Tab of the Options Dialog Box

You can select the face zones that will be involved in the contact detection process from the Face Zones list. While all eligible face zones in the Face Zones list are selected by default, you can choose to exclude certain zones for efficiency. Only walls and dynamic zones of type Rigid Body or User-Defined can be selected for contact detection.

From the UDF drop-down list, you can specify a user-defined function that will be invoked when contact has been detected. For more information about contact UDFs, see DEFINE_CONTACT in the Fluent Customization Manual.

You must specify a Proximity Threshold value in order to enable the contact detection process. When the distance between face zones falls below this threshold value, the UDF specified in the UDF drop-down list is invoked.

Cells adjacent to face zones that fall below the Proximity Threshold distance can also be tagged and separated into new cell zones during the contact detection process. This is useful for specifying different flow conditions in contact regions during the simulation.

To enable flow control options, select the Flow Control check box in the Contact Detection tab. Additional settings for flow control can then be specified by clicking the Controls... button to display the Flow Controls dialog box (see Figure 10.74: The Flow Controls Dialog Box).

Figure 10.74:  The Flow Controls Dialog Box

The Flow Controls Dialog Box

In the Flow Controls dialog box, you can specify a flow control zone (for example, restrictions, and so on) for any cell zone in the mesh. To create a flow control zone, select a zone from the Cell Zones list, specify a new name in the Flow Control Zone text box, and click the Create Zone button. Once the flow control zone has been created, it becomes available in the Cell Zone Conditions task page, where additional physical properties (for example, inertial and/or viscous porous resistance) can be specified. During the simulation, once cells in the contact region have been separated into new zones, the physical properties specified in the respective flow control zone are copied to the newly separated cell zone.


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