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

7.6.3 Using Profiles

The procedure for using a profile to define a particular cell zone or boundary condition is outlined below.

1.   Create a file that contains the desired profile, following the format described in Section  7.6.2.

2.   Read the profile using the Read... button in the Profiles dialog box (Figure  7.6.1) or the File/Read/Profile... menu item.

figure Cell Zone Conditions figure Profiles...

figure Boundary Conditions figure Profiles...

File $\rightarrow$ Read $\rightarrow$ Profile...

Note that if you use the Profiles dialog box to read a file, and a profile in the file has the same name as an existing profile, the old profile will be overwritten.

3.   If it is a point profile, you can choose the method of interpolation using the Profiles dialog box (Figure  7.6.1):

figure Cell Zone Conditions figure Profiles...

figure Boundary Conditions figure Profiles...

Select the point profile in the Profile selection list. Then select one of the three choices in the Interpolation Method list and click the Apply button. The three choices include:

  • Constant

    This method is zeroth-order interpolation. For each cell face at the boundary, the solver uses the value from the profile file located closest to the cell. Therefore, the accuracy of the interpolated profile will be affected by the density of the data points in your profile file. This is the default interpolation method for point profiles.

  • Inverse Distance

    This method assigns a value to each cell face at the boundary based on weighted contributions from the values in the profile file. The weighting factor is inversely proportional to the distance between the profile point and the cell face center.

  • Least Squares

    This method assigns values to the cell faces at the boundary through a first-order interpolation method that tries to minimizes the sum of the squares of the offsets (residuals) between the profile data points and the cell face centers. The least squares solution is found using Singular Value Decomposition (SVD).

For information about the interpolation methods employed for other profile types (i.e., line, mesh, radial, or axial profiles), see Section  7.6.1.

4.   In the boundary conditions dialog boxes (e.g., the Velocity Inlet and Pressure Inlet dialog boxes), the fields defined in the profile file (and those defined in any other profile file that you have read in) will appear in the drop-down list to the right of or below each parameter for which profile specification is allowed. To use a particular profile, select it in the appropriate list.

5.   Initialize the solution to interpolate the profile.


Profiles cannot be used to define volumetric source terms. If you want to define a non-constant source term, you will need to use a user-defined function.

For more information on UDFs, refer to the separate UDF Manual.

Checking and Deleting Profiles

Each profile file contains one or more profiles, and each profile has one or more fields defined in it. Once you have read in a profile file, you can check which fields are defined in each profile, and you can also delete a particular profile. These tasks are accomplished in the Profiles dialog box (Figure  7.6.1).

figure Cell Zone Conditions figure Profiles...

figure Boundary Conditions figure Profiles...

Figure 7.6.1: The Profiles Dialog Box

To check which fields are defined in a particular profile, select the profile name in the Profile list. The available fields in that file will be displayed in the Fields list. In Figure  7.6.1, the profile fields from the profile file of Section  7.6.2 are shown.

To delete a profile, select it in the Profile list and click the Delete button. When a profile is deleted, all fields defined in it will be removed from the Fields list.

Viewing Profile Data

The Plots task page options allow you to generate XY plots of data related to profiles. You can plot the original data points from the profile file you have read into ANSYS FLUENT, or you can plot the values assigned to the cell faces on the boundary after the profile file has been interpolated. See Section  29.9.4 for the steps to generate these plots.

You have the additional option of viewing the parameters of the boundary condition to which the profile has been "hooked" (i.e. has a field from the profile set as one or more of the parameters) using the Plot or the Contours options. Note that these display options do not allow you to plot the actual values of the cell faces (as is done with the Interpolated Data option), because they interpolate the values stored in the adjacent cells. To view the boundary condition parameters you must first read in the profile, save a boundary condition with a profile field selected as a parameter, and initialize the flow solution. Then you can you can view the surface data as follows:


For the example given in Section  7.6.2, the profiles are used for inlet values of $x$ velocity, turbulent kinetic energy, and turbulent kinetic energy dissipation rate, as illustrated in Figure  7.6.2. (The $y$ velocity is set to a constant value of zero, since it is assumed negligible. However, a profile of $y$ velocity could also be used.)

Figure 7.6.2: Example of Using Profiles as Boundary Conditions

next up previous contents index Previous: 7.6.2 Profile File Format
Up: 7.6 Profiles
Next: 7.6.4 Reorienting Profiles
Release 12.0 © ANSYS, Inc. 2009-01-29