4.20.2 Using the FSI Mapping Dialog Boxes

To begin the process of mapping ANSYS FLUENT data, you must first create a mesh file that can be used as the input file in the steps that follow. The resolution of the mesh should be appropriate for your eventual finite element analysis. You are free to use the method and preprocessor of your choice in the creation of this file, but the end result must correspond to one of the entries in the Input File column of Table  4.20.1.

When creating the input file, note the following:

• While the input file may be scaled when it is read into ANSYS FLUENT, the volumes or surfaces on which the data is to be mapped must otherwise be spatially coincident with their counterparts in the ANSYS FLUENT simulation.

• The input file can be only a portion of the overall FEA model (i.e., you can exclude the parts of the model on which you are not mapping ANSYS FLUENT data). When this is the case, note that the numbering of the nodes and elements in the input file must match the numbering of the nodes and elements in the complete file you will use for your finite element analysis.

Next, read a case file in ANSYS FLUENT and make sure data is available for mapping, either by running the calculation or by reading a data file. The data should be from a steady-state solution.

Finally, perform the following steps to generate an output file in which the ANSYS FLUENT data has been mapped to the mesh of the input file:

1.   Open the ANSYS FLUENT dialog box that is appropriate for the zones from which the data is to be taken. If the data you are mapping is from a volume (e.g., the cell zone of a solid region), open the Volume FSI Mapping dialog box using the File/FSI Mapping/Volume... menu item (Figure  4.20.1). If instead the data is from a surface (e.g., a face boundary zone), open the Surface FSI Mapping dialog box using the File/FSI Mapping/Surface... menu item (Figure  4.20.2).

File $\rightarrow$ FSI Mapping $\rightarrow$ Volume...

or

File $\rightarrow$ FSI Mapping $\rightarrow$ Surface...

Figure 4.20.1: The Volume FSI Mapping Dialog Box for Cell Zone Data

Figure 4.20.2: The Surface FSI Mapping Dialog Box for Face Zone Data

2.   Specify the parameters of the input file and read it into ANSYS FLUENT.

(a)   Select the format of the input file from the Type list in the Input File group box, based on the FEA software with which it is associated. The choices include:

• ABAQUS

• I-deas

• Mechanical APDL

• NASTRAN

• PATRAN

For a list of the file extensions associated with these types, see the Input File column of Table  4.20.1.

(b)   Enter the name and extension (along with the folder path, if it is not in the current folder) of the input file in the FEA File text-entry box. Alternatively, you can specify it through the Select File dialog box, which is opened by clicking the Browse... button.

(c)   Specify the length units that were used in the creation of the input file by making a selection from the Length Units drop-down menu. This ensures that the input file is scaled appropriately relative to the ANSYS FLUENT file.

(d)   Click the Read button to read the input file into memory.

Note that the input file will only be held in memory until the output file is written, or until the FSI mapping dialog box is closed.

3.   Display the meshes so that you can visually verify that the input file is properly scaled and aligned with the ANSYS FLUENT mesh file.

(a)   Make sure that the FEA Mesh and FLUENT Mesh options are enabled in the Display Options group box. Note that you can disable either of these options if you want to examine one of the meshes independently.

(b)   Click the Display button to display the meshes in the graphics window.

For the ANSYS FLUENT mesh, only the zones selected in the FLUENT Zones group box will be displayed--in this case, the default selections. If the default zones are not appropriate, you should redisplay the meshes after you make your zone selections in a later step.

4.   Specify the type of data variables to be mapped.

(a)   Select either Structural or Thermal in the Analysis group box. Your selection should reflect the kind of further analysis you intend to pursue, and will determine what variables are available for mapping.

(b)   Enable the variables you want to map in the Structural Loads or Thermal Loads group box. When mapping volume data, you can enable only Temperature. When mapping surface data, you can enable Force, Pressure, and Temperature for structural analysis, or Temperature, Heat Flux, and Heat Trans Coeff for thermal analysis.

Note that the Energy Equation must be enabled in the Energy dialog box if you want to map temperature for a structural analysis or any variable for a thermal analysis.

5.   Select the zones that contain the data to be mapped in the FLUENT Zones group box. You can select individual zones in the Cell Zones or Face Zones selection lists, or select all zones of a particular type in the Zone Type selection list. If you modify the default selections, you should display the meshes again, as described previously.

Note that all wall zones in the Face Zones selection list are selected by default in the Surface FSI Mapping dialog box, and this includes the shadow walls created for two-sided walls. If your ANSYS FLUENT file contains a wall/shadow pair (e.g., separating a solid zone from a fluid zone), you should make sure that only the correct wall or shadow of the pair is selected.

Inlet zones do not have heat transfer coefficient data, and so any attempts to map this combination will be ignored.

6.   Specify the parameters of the output file and write it.

(a)   Select the format of the output file from the Type list in the Output File group box, based on the software with which you plan to perform your finite element analysis. The choices in this list are the same as those for the input file type. Note that you can select an output file type that is different from the input file type.

For details about the file extensions associated with the various types of output files, see the Output File column of Table  4.20.1.

(b)   Enter the name (with the folder path, if appropriate) of the output file in the File Name text-entry box. Alternatively, you can specify it through the Select File dialog box, which is opened by clicking the Browse... button.

(c)   If you would like to include additional FEA information like node/element information in the exported output file, enable Include FEA Mesh. By default, this option is disabled and therefore, only the selected boundary condition values are exported.

(d)   When mapping temperature for a structural analysis or any variable for a thermal analysis, make a selection in the Temperature Units drop-down menu. Table  4.20.2 shows the units for the mapped variables, depending on the Temperature Units selection.

Table 4.20.2: Units Associated with the Temperature Units Drop-Down List Selections

Temperature	Temperature	Heat	Heat
Units		Flux	Transfer
Selection			Coefficient
K	K	W/m $^2$	W/m $^2$-K
C	$^\circ$C	W/m $^2$	W/m $^2$- $^\circ$C
F	$^\circ$F	BTU/ft $^2$-hr	BTU/ft $^2$-hr- $^\circ$F

(e)   When mapping the heat transfer coefficient for a thermal analysis, make a selection in the HTC Type drop-down menu to determine how the heat transfer coefficient $h_{\rm eff}$ is calculated.

ref-temp   calculates $h_{\rm eff}$ using Equation  31.4-40, where $T_{\rm ref}$ is the reference temperature defined in the Reference Values task page. Note that this option has the same definition as the field variable Surface Heat Transfer Coef., as described in Section  31.4.

cell-temp   calculates $h_{\rm eff}$ using the general form of Equation  31.4-40, but defines $T_{\rm ref}$ as the temperature of the cell adjacent to the face.

wall-func-htc   calculates $h_{\rm eff}$ using Equation  31.4-51. Note that this option has the same definition as the field variable Wall Func. Heat Tran. Coef., as described in Section  31.4.

(f)   Click Write to write an output file in which the ANSYS FLUENT data has been mapped to the mesh of the input file.

The input file will be released from memory when the output file is written.