[ANSYS, Inc. Logo] return to home search
next up previous contents index

11.3.10 Previewing the Dynamic Mesh

When you have specified the mesh update methods and their associated parameters, and you have defined the motion of dynamic zones, as described in Section  11.3.9, you can preview the motion of the mesh or the zone as it changes with time before you start your simulation. The same dynamic zone or mesh motion will be executed when you start your simulation.



Previewing Zone Motion


You can preview the motion of zones with rigid body motion using the Zone Motion dialog box (Figure  11.3.45) .

figure Dynamic Mesh figure Display Zone Motion...

Figure 11.3.45: The Zone Motion Dialog Box
figure

The zone motion preview only updates the graphical representation (in the graphics window) of the zones that you have selected using the Mesh Display dialog box. The zone motion preview will only update those zones that have solid body motion specified. To use the Zone Motion preview:

1.   Select the appropriate zones to display in the Display Mesh dialog box.

2.   In the Zone Motion dialog box, enter the Time Step and the Number of Steps under Motion History Integration.

3.   Click the Integrate button. This allows ANSYS FLUENT to create a table of surface positions in time.

4.   Under Preview Controls, specify the Time Step and the Number of Steps for preview. Note that the time step here can be larger than the integration time step.

5.   Click Preview to preview the zone motion. Click Apply to save your settings for zone motion. Click Reset to have the default inputs restored in the dialog box.

You can also use the slider bar on the Zone Motion dialog box to fast-forward or rewind the motion of the selected zones. Previewing the zone motion can also be used as a postprocessor for 6DOF simulations (see Section  11.3.7).



Previewing Mesh Motion


The mesh motion preview is different from the zone motion described above in that the mesh connectivity is changed in mesh motion.

To preview the dynamic mesh of a transient case, you can use the Mesh Motion dialog box (Figure  11.3.46)

figure Dynamic Mesh figure Preview Mesh Motion...

Figure 11.3.46: The Mesh Motion Dialog Box
figure

The procedure is as follows:

1.   Save the case file.

File $\rightarrow$ Write $\rightarrow$ Case...

figure   

Note that the mesh motion will actually update the node locations as well as the connectivity of the mesh, so you must be sure to save your case file before doing the dynamic mesh motion. Once you have advanced the mesh by a certain number of time steps, you will not be able to recover the previous status of the mesh, other than by reloading the appropriate ANSYS FLUENT case file.

2.   Specify the Number of Time Steps and the size of each time step ( Time Step Size). The current time will be displayed in the Current Mesh Time field after the dynamic mesh has been advanced the specified number of steps.

Note that if you turned on the in-cylinder option, the Time Step Size is automatically calculated from the Crank Angle Step Size and the Crank Shaft Speed that you have specified in the In-Cylinder Settings dialog box.

3.   To view the dynamic mesh in the graphics window, enable the Display Mesh option. In addition, you can control the frequency at which ANSYS FLUENT should display an updated mesh in the Display Frequency field. To save a picture file of the mesh each time ANSYS FLUENT updates it during the preview, turn on the Save Picture option. This opens the Save Picture dialog box (see Section  4.21).

4.   Turn on Enable Autosave to use the automatic saving feature to specify the file name and frequency with which case and data files should be saved during the solution process. This opens the Autosave Case During Mesh Motion Preview dialog box.

See Section  4.3.4 for details about the use of this feature. This provides a convenient way for you to save results at successive time steps for later postprocessing.

5.   Enable the Update Mesh Interfaces option to update the interface at every time step.

6.   Click Preview to start the preview. ANSYS FLUENT will update the dynamic mesh by moving and deforming the face and cell zones that you have specified as dynamic zones. Click Apply to save your settings for mesh motion.

During the preview, information about the dynamic mesh will be displayed in the console window for each time step. Note that for the in-cylinder option, the reported Maximum Cell Skew is calculated only from zones undergoing remeshing. This ensures that you can always ascertain whether the skewness is increasing in the deforming zones. To report the maximum skewness of a cell from any zone, you can click the Report Quality button in the General task page.

figure General figure Report Quality


next up previous contents index Previous: 11.3.9 Specifying the Motion
Up: 11.3 Using Dynamic Meshes
Next: 12. Modeling Turbulence
Release 12.0 © ANSYS, Inc. 2009-01-29