25.2 Procedures for Modeling Continuous Casting

As described in this section and this section in the separate Theory Guide , you can include the pull velocities in your solidification/melting calculation to model continuous casting. There are three approaches to modeling continuous casting in ANSYS FLUENT:

• Specify constant or variable pull velocities.

  To use this approach (the default), do not enable the Compute Pull Velocities option.

  If you use this approach, you will need to patch constant values or custom field functions for the pull velocities, after you initialize the solution.

  Solution Initialization Patch...

  See Section  26.9.2 for details about patching values. Note that it is acceptable to patch values for the pull velocities in the entire domain, because the patched values will be used only if the liquid fraction, $\beta$, is less than 1.

• Have ANSYS FLUENT compute the pull velocities (using this equation in the separate Theory Guide) during the calculation, based on the specified velocity boundary conditions.

  To use this approach, enable the Compute Pull Velocities option. This method is computationally expensive, and is recommended only if the pull velocities are strongly dependent on the location of the liquid-solid interface.

  If you have ANSYS FLUENT compute the pull velocities, then there are no additional inputs or setup procedures beyond those presented in Section  25.1.

• Have ANSYS FLUENT compute the pull velocities just once, and then use those values for the remainder of the calculation.

  To use this approach, perform one iteration with ANSYS FLUENT computing the pull velocities, and then turn off the Compute Pull Velocities option and continue the calculation. For the remainder of the calculation, ANSYS FLUENT will use the values computed for the pull velocities at the first iteration.