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

11.3 Using Dynamic Meshes

The steps for setting up a dynamic mesh problem are listed below. (Note that this procedure includes only those steps necessary for the dynamic mesh model itself; you will need to set up other models, cell zone conditions, boundary conditions, etc. as usual.)

1.   Enable the appropriate option for modeling transient or steady flow in the General task page. (See Section  26.12 for details about the transient modeling capabilities in ANSYS FLUENT.)

figure General

2.   Set cell zone conditions and boundary conditions as required in the Cell Zone Conditions and Boundary Conditions task page.

figure Cell Zone Conditions

figure Boundary Conditions

See Chapter  7 for details about input of conditions. The wall velocity is set up automatically when the motion attribute is set for wall zones, so you will not specify wall motion in the Wall dialog box.

3.   Enable the dynamic mesh model, and specify related parameters in the Dynamic Mesh task page.

figure Dynamic Mesh figure figure Dynamic Mesh

See Section  11.3.1 for details.

4.   Specify the motion of the dynamic zones in your model. You can display the motion of the moving zones with prescribed motion to verify the simulation setup.

figure Dynamic Mesh figure Display Zone Motion...

See Section  11.3.9 for details.

5.   Define the events that will occur during the calculation.

figure Dynamic Mesh figure Events...

See Section  11.3.8 for details.

6.   Save the case and data.

File $\rightarrow$ Write $\rightarrow$ Case & Data...

7.   Preview your dynamic mesh setup (when the motion is a prescribed motion). See Section  11.3.5 for previewing your steady-state dynamic mesh motion and refer to Section  11.3.10 for details.

figure Dynamic Mesh figure Preview Mesh Motion...

8.   Specify the pressure-velocity coupling scheme. For transient flow calculations, the PISO algorithm is recommended, as it is the most efficient for such cases (see Section  26.3.1 for details).

9.   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.

figure Calculation Activities figure Edit... (Autosave Every)

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.


You must save a case file each time you save a data file because the mesh position is stored in the case file. Since the mesh position changes with each time step, reading data for a given time step will require the case file at that time step so that the mesh will be in the proper position. You should also save your initial case file so that you can easily return to the mesh's original position to restart the solution if desired.

10.   (optional) If you want to create a graphical animation of the mesh over time during the solution procedure, you can use the Calculation Activities task page to set up the graphical displays that you want to use in the animation. See Section  26.16 for details.

next up previous contents index Previous: 11.2.4 Postprocessing for Sliding
Up: 11. Modeling Flows Using
Next: 11.3.1 Setting Dynamic Mesh
Release 12.0 © ANSYS, Inc. 2009-01-29