4.19.1 Performing Mesh-to-Mesh Solution Interpolation

The procedure for mesh-to-mesh solution interpolation is as follows:

1.   Set up the model and calculate a solution on the initial mesh.

2.   Write an interpolation file for the solution data to be interpolated onto the new mesh, using the Interpolate Data dialog box (Figure  4.19.1).

File $\rightarrow$ Interpolate...

Figure 4.19.1: The Interpolate Data Dialog Box

(a)   Under Options, select Write Data.

(b)   In the Cell Zones selection list, select the cell zones for which you want to save data to be interpolated.

Note:   If your case includes both fluid and solid zones, write the data for the fluid zones and the data for the solid zones to separate files.

(c)   Select the variable(s) for which you want to interpolate data in the Fields selection list. All ANSYS FLUENT solution variables are available for interpolation.

(d)   Click Write... and specify the interpolation file name in the resulting Select File dialog box. The file format is described in Section  4.19.2.

3.   Set up a new case.

(a)   Read in the new mesh, using the appropriate menu item in the File/Read/ or File/Import/ menu.

(b)   Define the appropriate models.

Enable all of the models that were enabled in the original case. For example, if the energy equation was enabled in the original case and you forget to enable it in the new case, the temperature data in the interpolation file will not be interpolated.

(c)   Define the boundary conditions, material properties, etc.

An alternative way to set up the new case is to save the boundary conditions from the original model using the write-bc text command, and then read in those boundary conditions with the new mesh using the read-settings text command. See Section  4.7 for further details.

4.   Read in the data to be interpolated.

File $\rightarrow$ Interpolate...

(a)   Under Options, select Read and Interpolate.

(b)   In the Cell Zones list, select the cell zones for which you want to read and interpolate data.

If the solution has not been initialized, computed, or read, all zones in the Cell Zones list are selected by default, to ensure that no zone remains without data after the interpolation. If all zones already have data (from initialization or a previously computed or read solution), select a subset of the Cell Zones to read and interpolate data onto a specific zone (or zones).

(c)   Click the Read... button and specify the interpolation file name in the resulting Select File dialog box.

If your case includes both fluid and solid zones, the two sets of data are saved to separate files. Hence perform these steps twice, once to interpolate the data for the fluid zones and once to interpolate the data for the solid zones.

5.   Reduce the under-relaxation factors and calculate on the new mesh for a few iterations to avoid sudden changes due to any imbalance of fluxes after interpolation. Then increase the under-relaxation factors and compute a solution on the new mesh.