4.14.2 Mechanical APDL Files

Export to Mechanical APDL can only be invoked using the file/export/mechanical-apdl text command. You will be prompted to enter an Mechanical APDL file name and the Zone to Export.

The file written is a Mechanical APDL results file with a .rfl extension. This file preserves the cell zones defined in ANSYS FLUENT. The Mechanical APDL file is a single file containing coordinates, connectivity, and the scalars listed below:

"x-velocity'', "y-velocity'', "z-velocity'', "pressure'',
"temperature'', "turb-kinetic-energy'', "turb-diss-rate'',
"density'', "viscosity-turb'', "viscosity-lam'', "viscosity-eff'',
"thermal-conductivity-lam'', "thermal-conductivity-eff'',
"total-pressure'', "total-temperature'', "pressure-coefficient'',
"mach-number'', "stream-function'', "heat-flux'',
"heat-transfer-coef'', "wall-shear'', "specific-heat-cp''

Export to Mechanical APDL is available on a limited number of platforms (aix43, aix51, alpha hpux10p8, hpux11, irix65, irix65_mips4, and ultra).

To read this file into Mechanical APDL, do the following:

1.   In Mechanical APDL, expand the General Postproc item in the ANSYS Main Menu, and click Data & File Opts. Then perform the following steps in the Data and File Options dialog box that opens.

(a)   Make sure that Read single result file is enabled.

(b)   Click the browse button to open the Open dialog box, and select the .rfl file generated by ANSYS FLUENT.

(c)   Click Open in the Open dialog box.

(d)   Click OK in the Data and File Options dialog box.

2.   In the ANSYS Main Menu, click Results Summary in the expanded General Postproc list. A SET,LIST Command window will open, displaying a summary of the file contents.

3.   In the expanded General Postproc list, expand the Read Results item and click First Set to read the data from the file.

4.   Display the data from the file. You can display mesh information by selecting either the Plot/Nodes menu item or the Plot/Elements menu item from the Mechanical APDL menu bar. You can display results by selecting either the Plot/Results/Contour Plot/Nodal Solution... menu item or the Plot/Results/Contour Plot/Elem Solution... menu item, and then using the dialog box that opens.

You have the option of using the Execute Commands dialog box to export data to Mechanical APDL at specified intervals during the calculation. The text command for exporting can be entered directly into the Command text box (or the ANSYS FLUENT console, if you are defining a macro). It is of the following form:

file/export/mechanical-apdl file_name list_of_cell_zones ()

where

• file_name specifies the name (without the extension) of the file that you wish to write. You should include a special character string in the file name, so that the solver assigns a new name to each file it saves. See Section  4.1.7 for details. By using a special character string, you can have the files numbered by time step, flow time, etc.

• list_of_cell_zones specifies the list of cell zones (separated by commas) from which you want to export data. The () input terminates the list. For example, the input fluid-rotor, fluid-stator () will select the cell zones named fluid-rotor and fluid-stator.

See Section  26.14 for information about executing commands and creating and using command macros.