4.12.9 IC3M Files

ANSYS FLUENT has the ability to import in-cylinder simulation files that have been created using the IC3M preprocessor of ICEM CFD. For information about creating and setting up such files, see the IC3M User Guide & Tutorial Manual (available to licensed ICEM CFD IC3M users).

When importing IC3M files, first make sure that all of the relevant files exported from ICEM CFD IC3M are in the same folder and uncompressed. Then import the files, using the File/Import/IC3M... menu item.

File $\rightarrow$ Import $\rightarrow$ IC3M...

IC3M files can only be imported into the 3D version of ANSYS FLUENT(single or double precision). Note that IC3M files should not be used with ANSYS FLUENT in Workbench.

In the Select File dialog box, specify the name of the mesh file, which should have a .msh extension. After the file is selected, ANSYS FLUENT will read in the mesh and automatically set up the case file to run a dynamic mesh simulation, using the parameters defined in the IC3M preprocessor. You can make certain changes to the dynamic mesh setup, but this is not necessary. See Section  11.3 for further details about setting up the dynamic mesh. Note that you cannot change the engine parameters for an engine set up using IC3M, except for the time step size

The information read in from the IC3M files includes the starting and ending crank angle for the simulation. After reading the .msh file, ANSYS FLUENT will position the mesh such that it corresponds to the starting crank angle. This process may take a few minutes. You will be informed of the status of this process through messages in the console.

Save the case file at this point, to retain a copy of the settings from the IC3M files. You may start the simulation from this case file, as long as it is in a folder that contains all of the uncompressed files exported by ICEM CFD IC3M. It is recommended that you preview the mesh motion prior to running the simulation, using the same time step size that will be used in the simulation. See Section  11.3.10 for further details.

Note that you will not be able to run the mesh preview or simulation beyond the ending crank angle specified in the IC3M preprocessor, even if the motion is periodic. ANSYS FLUENT sets the end crank angle based on the information imported from the IC3M files, and will automatically stop when this angle is reached.

You cannot reuse the same ANSYS FLUENT session for engines set up using IC3M, i.e., for each new calculation, you must exit ANSYS FLUENT and begin a new session.