11.3.8 Defining Dynamic Mesh Events

If you are simulating a flow, you can use the events in ANSYS FLUENT to control the timing of specific events during the course of the simulation. With in-cylinder flows for example, you may want to open the exhaust valve (represented by a pair of deforming sliding interfaces) by creating an event to create the sliding interfaces at some crank angle. You can also use dynamic mesh events to control when to suspend the motion of a face or cell zone by creating the appropriate events based on the crank angle or time. Note that in-cylinder flows are crank angle-based, whereas all other flows are time-based.

Procedure for Defining Events

You can define the events using the Dynamic Mesh Events dialog box (Figure  11.3.33).

Dynamic Mesh Events...

Figure 11.3.33: The Dynamic Mesh Events Dialog Box

The procedure for defining events is as follows:

1.   Increase the Number of Events value to the number of events you wish to specify. As this value is increased, additional event entries in the dialog box will become editable.

2.   Enable the check box next to the first event and enter a name for the event under the Name heading.

3.   Specify either the time or the crank angle at which you want the event to occur.

For in-cylinder flows, specify the crank angle at which you want the event to occur under At Crank Angle.

For non-in-cylinder flows, specify the time (in seconds) at which you want the event to occur under At Time.

It is not necessary to specify the events in order of increasing time or crank angle, but it may be easier to keep track of events if you specify them in the order of increasing time or angle.

4.   Click the Define... button to open the Define Event dialog box (Figure  11.3.34).

Figure 11.3.34: The Define Event Dialog Box

5.   In the Define Event dialog box, choose the type of event by selecting Change Zone Type, Copy Zone BC, Activate Cell Zone, Deactivate Cell Zone, Create Sliding Interface, Delete Sliding Interface, Change Motion Attribute, Change Time Step Size, Change Under-Relaxation Factors, Insert Boundary Zone Layer, Remove Boundary Zone Layer, Insert Interior Zone Layer, Remove Interior Zone Layer, Insert Cell Layer, Remove Cell Layer, or Execute Command in the Type drop-down list. These event types and their definitions are described later in this section.

6.   Repeat steps 2-5 for the other events, if relevant.

7.   Click Apply in the Dynamic Mesh Events dialog box after you finish defining all events.

8.   To play the events to check that they are defined correctly, click the Preview... button in the Dynamic Mesh Events dialog box. This displays the Events Preview dialog box.

For in-cylinder flows, you use the Events Preview dialog box (Figure  11.3.35), to enter the crank angles at which you want to start and end the playback in the Start Crank Angle and End Crank Angle fields, respectively.

For non-in-cylinder flows, you use the Events Preview dialog box to enter the time at which you want to start and end the playback in the Start Time and End Time fields, respectively.

Specify the size of the step to take during the playback in the Increment field. Click Preview to play back the events. ANSYS FLUENT will play the events at the time (or crank angle in the case of in-cylinder flows) specified for each event and report when each event occurs in the text (console) window.

Figure 11.3.35: The Events Preview Dialog Box for In-Cylinder Flows

For in-cylinder simulations, you need to specify the events for one complete engine cycle. In the subsequent cycles, the events are executed whenever

where $\theta_{\rm event}$ is the event crank angle, $\theta_c$ is the current crank angle calculated from Equation  11.3-12, $\theta_{\rm period}$ is the crank angle period for one cycle, and $n$ is some integer.

As an example, for in-cylinder simulations, you are not required to specify the event crank angle to correspond exactly to the current crank angle calculated from Equation  11.3-12. ANSYS FLUENT will execute an event if the current crank angle is between $\pm0.5\Delta\theta$ where $\Delta\theta$ is the equivalent change in crank angle for the time step. For example, if the event preview is executed between crank angle of 340 $^\circ$ and 1060 $^\circ$ (crank period is 720 $^\circ$) using an increment of 1 $^\circ$, ANSYS FLUENT will report the following in the text window.

Execute Event: open-in-valve-left (defined at: 353.10, current angle: 353.00)
Execute Event: open-in-valve-right (defined at: 353.00, current angle: 353.00)
Execute Event: close-ex-valve-right (defined at: 355.60, current angle: 356.00)
Execute Event: close-ex-valve-left (defined at: 357.80, current angle: 358.00)
Execute Event: close-in-valve-left (defined at: 571.60, current angle: 572.00)
Execute Event: close-in-valve-right (defined at: 571.80, current angle: 572.00)
Execute Event: open-ex-valve-right (defined at: 137.10, current angle: 857.00)
Execute Event: open-ex-valve-left (defined at: 139.00, current angle: 859.00)

Notice that events defined at 137.10 $^\circ$ and 139 $^\circ$ are executed at 857 $^\circ$ and 859 $^\circ$, respectively, because they satisfy the condition of Equation  11.3-16.

Defining Events for In-Cylinder Applications

ANSYS FLUENT will automatically limit the valve lift values depending on the specified minimum valve lift value. However, the conversion of the sliding interface zones to walls (and vice versa) is accomplished via the in-cylinder events (see Section  11.3.8). For example, if the exhaust valve closes at $-5^\circ$ before TDC position, you must define a Delete Sliding Interface event at the crank angle of $-5^\circ\!$. You need to define similar events for the intake valve opening (using the Create Sliding Interface event), the intake valve closing ( Delete Sliding Interface event), and the exhaust valve opening ( Create Sliding Interface event) at the respective crank angles.

For the current example, the exhaust valve is assumed to be open between $131^\circ$ and $371^\circ$ and the intake valve is open between at $345^\circ$ and $584^\circ\!$.

Events

Each of the available events is described below.

Changing the Zone Type

You can change the type of a zone to be a wall, or an interface, interior, fluid, or solid zone during your simulation. To change the type of a zone, select Change Zone Type in the Type drop-down list in the Define Event dialog box (Figure  11.3.34). Select the zone(s) that you want to change in the Zone list, and then select the new zone type in the New Zone Type drop-down list.

Copying Zone Boundary Conditions

You can copy boundary conditions from one zone to other zones during your simulation. If, for example, you have changed an inlet zone to type wall with the Change Zone Type event, you can set the boundary conditions of the new zone type by simply copying the boundary conditions from a known zone with the corresponding zone type.

To copy boundary conditions from one zone to another, select Copy Zone BC in the Type drop-down list in the Define Event dialog box (Figure  11.3.34). In the From Zone drop-down list, select the zone that has the conditions you want to copy. In the To Zone(s) list, select the zone or zones to which you want to copy the conditions.

ANSYS FLUENT will set all of the boundary conditions for the zones selected in the To Zone(s) list to be the same as the conditions for the zone selected in the From Zone list. (You cannot copy a subset of the conditions, such as only the thermal conditions.)

Note that you cannot copy conditions from external walls to internal (i.e., two-sided) walls, or vice versa, if the energy equation is being solved, since the thermal conditions for external and internal walls are different.

Activating a Cell Zone

To activate a cell zone, select Activate Cell Zone in the Type drop-down list in the Define Event dialog box (Figure  11.3.34), then select the zone that you want to activate in the Zone(s) list. For more information, see Section  6.8.9.

Deactivating a Cell Zone

To deactivate a cell zone, select Deactivate Cell Zone in the Type drop-down list in the Define Event dialog box (Figure  11.3.34), then select the zone that you want to deactivate in the Zone(s) list.

Only deactivated zones can be activated. When a zone is deactivated, ANSYS FLUENT skips the zone during the calculations. For more information, see Section  6.8.9.

Creating a Sliding Interface

To create a sliding interface during your simulation, select Create Sliding Interface in the Type drop-down list in the Define Event dialog box (Figure  11.3.36). Enter a name for the sliding interface in the Interface Name field. Select the zones on either side of the interface in the Interface Zone 1 and Interface Zone 2 drop-down lists.

You have the option to select any number of zones listed under each of the interface zones. ANSYS FLUENT calculates intersections between all possible combinations of the left and right side of the interfaces, allowing you more flexibility in terms of creating zones and defining the interfaces.

Figure 11.3.36: The Define Event Dialog Box for the Creating Sliding Interface Option

If ANSYS FLUENT finds another interface with the same name as defined in the event, then the old interface will be deleted and a new one created as defined in the dynamic mesh event.

If the interface zones that you selected above do not overlap each other completely, the non-overlapped regions on each interface zones are put into separate wall zones by ANSYS FLUENT. If these wall zones (i.e., non-overlapped regions) have motion attributes associated with them, their motion can only be specified by copying the motion from another dynamic zone by selecting the appropriate dynamic zones in the Wall 1 Motion and Wall 2 Motion drop-down lists, respectively.

Note that you don't have to change the boundary type from wall to interface. When the Create Sliding Interface event is executed, ANSYS FLUENT will automatically change the boundary type of the face zones selected in Interface Zone 1 and Interface Zone 2 to type interface before the sliding interface is created.

Deleting a Sliding Interface

To delete a sliding interface that has been created earlier in your in-cylinder simulation, select Delete Sliding Interface in the Type drop-down list in the Define Event dialog box (Figure  11.3.34). Enter the name of the sliding interface to be deleted in the Interface Name field.

As with the Create Sliding Interface event, ANSYS FLUENT will automatically change the corresponding interface zones to wall. However, you may want to use the Copy Zone BC event to set any boundary conditions that are not the default conditions that ANSYS FLUENT assumes.

Changing the Motion Attribute of a Dynamic Zone

To change the motion attribute of a dynamic zone during your in-cylinder calculation, select Change Motion Attribute in the Type drop-down list in the Define Event dialog box (Figure  11.3.34). Select the Attribute ( slide, moving, or remesh) and set the appropriate Status ( enable or disable). Select the corresponding dynamic zones for which you want to change the motion attributes in the Dynamic Zones list.

The slide attribute is used to enable or disable smoothing of nodes on selected deforming face zones, the moving attribute is used to suspend the motion of selected moving zones, and the remesh attribute is used to enable and disable face remeshing on selected deforming face zones.

Changing the Time Step

To change the time step at some point during the simulation, select Change Time Step Size in the Type drop-down list in the Define Event dialog box. Specify the new physical time step size by entering the new Time Step Size in seconds.

For in-cylinder simulations, specify the new physical time step by entering the new Crank Angle Step Size value in degrees. The physical time step is calculated from

where the unit of $\Omega_{\rm shaft}$ is assumed to be in RPM.

Changing the Under-Relaxation Factor

To change one or more under-relaxation factors, select Change Under-Relaxation Factor in the Type drop-down list in the Define Event dialog box (Figure  11.3.34). Select the under-relaxation factor that you wish to change, and assign a new value to it in the Under-Relaxation Factors list. For more information on setting under-relaxation factors, see Section  26.3.2.

Inserting a Boundary Zone Layer

To insert a new cell zone layer as a separate cell zone adjacent to a boundary, select Insert Boundary Zone Layer in the Type drop-down list in the Define Event dialog box. Specify the Base Dynamic Zone, from which the layer of cells is to be created, and the Side Dynamic Zone, which represents the deforming face zone adjacent to the Base Dynamic Zone before the layer is inserted. The new cell zone will inherit the boundary conditions of the cell zone adjacent to the Base Dynamic Zone before the layer is inserted.

Note that a new cell layer can be inserted only from a one-sided Base Dynamic Zone. You cannot insert a new cell layer from an interior face zone.

Figure  11.3.37 and Figure  11.3.38 illustrate the insertion of a boundary zone layer. In both figures, the circular face at the top of the cylinder is the base dynamic zone.

Figure 11.3.37: Boundary Zone Before Insertion

Figure 11.3.38: Boundary Zone After Insertion

Removing a Boundary Zone Layer

To remove the cell zone layer inserted using the Insert Boundary Zone Layer event, select Remove Boundary Zone Layer in the Type drop-down list in the Define Event dialog box. Specify the same Base Dynamic Zone that you used when you defined the insert boundary layer event.

Note that a cell layer can be removed only from a one-sided Base Dynamic Zone.

Inserting an Interior Zone Layer

To insert a new zone layer as a separate cell zone adjacent to the internal side of a boundary, select Insert Interior Zone Layer in the Type drop-down list in the Define Event dialog box. Specify the Base Dynamic Zone and the Side Dynamic Zone as described in the Insert Boundary Zone Layer event. You also need to specify the names of the new interior face zones ( Internal Zone 1 Name and Internal Zone 2 Name) that will be created after the cell zone layer is created by ANSYS FLUENT.

ANSYS FLUENT inserts the interior cell layer by splitting the cell zone adjacent to the Base Dynamic Zone with a plane. The position of the plane and the normal direction of the plane are implicitly defined by the cylinder origin and cylinder axis of the Side Dynamic Zone.

Figure  11.3.39 and Figure  11.3.40 illustrate the insertion of an interior zone layer.

Figure 11.3.39: Interior Zone Before Insertion

Figure 11.3.40: Interior Zone After Insertion

Removing an Interior Zone Layer

To remove the zone layer inserted using the Insert Interior Zone Layer event, select Remove Interior Zone Layer in the Type drop-down list in the Define Event dialog box. Specify the same Internal Zone 1 Name and Internal Zone 2 Name that you used to define the Insert Interior Zone Layer event.

Inserting a Cell Layer

To manually insert a new cell layer to the existing cell zone, select Insert Cell Layer in the Type drop-down list in the Define Event dialog box. Specify the Adjacent Dynamic Face Zone and the Direction Parameter. This can only work on zones that are suited for layering (see Section  11.3.2).

Removing a Cell Layer

To manually remove a cell layer from an existing cell zone, select Remove Cell Layer in the Type drop-down list in the Define Event dialog box. Specify the Adjacent Dynamic Face Zone and the Direction Parameter. This can only work on zones that are suited for layering (see Section  11.3.2).

Executing a Command

To execute a command, select Execute Command in the Type drop-down list in the Define Event dialog box (Figure  11.3.34). A command can be a series of text or Scheme commands, or a macro you have defined (or will define) using the Define Macro dialog box (see Section  26.14.1). Enter the series of commands or the name of the macro in the Command text-entry box.

If the command to be executed involves saving a file, see Section  26.14.2 for important information.

Exporting and Importing Events

If you want to save the events you have defined to a file, click Write... in the Dynamic Mesh Events dialog box and specify the Event File in the Select File dialog box (see Section  2.1.6).

To read the events back into ANSYS FLUENT, click Read... in the Dynamic Mesh Events dialog box and specify the Event File in the Select File dialog box (see Section  2.1.6).