25.1 Setup Procedure

The procedure for setting up a solidification/melting problem is described below. (Note that this procedure includes only those steps necessary for the solidification/melting model itself; you will need to set up other models, boundary conditions, etc. as usual.)

1.   To activate the solidification/melting model, enable the Solidification/Melting option in the Solidification and Melting dialog box (Figure  25.1.1).

This is available only when Species Transport is enabled in the Species Model dialog box.

Models Solidification & Melting Edit...

Figure 25.1.1: The Solidification and Melting Dialog Box

ANSYS FLUENT will automatically enable the energy equation, so you do not have to visit the Energy dialog box before turning on the solidification/melting model.

2.   Under Parameters, specify the value of the Mushy Zone Constant ( $A_{\rm mush}$ in this equation in the separate Theory Guide).

Values between $10^4$ and $10^7$ are recommended for most computations. The higher the value of the Mushy Zone Constant, the steeper the damping curve becomes, and the faster the velocity drops to zero as the material solidifies. Very large values may cause the solution to oscillate as control volumes alternately solidify and melt with minor perturbations in liquid volume fraction.

3.   If you want to include the pull velocity in your simulation (as described in this section and this section in the separate Theory Guide), enable the Include Pull Velocities option under Parameters.

4.   If you are including pull velocities and you want ANSYS FLUENT to compute them (using this equation in the separate Theory Guide) based on the specified velocity boundary conditions, as described in this section in the separate Theory Guide , enable the Compute Pull Velocities option and specify the number of Flow Iterations Per Pull Velocity Iteration.

It is not necessary to have ANSYS FLUENT compute the pull velocities. See Section  25.2 for information about other approaches.

The default value of 1 for the Flow Iterations Per Pull Velocity Iteration indicates that the pull velocity equations will be solved after each iteration of the solver. If you increase this value, the pull velocity equations will be solved less frequently. You may want to increase the number of Flow Iterations Per Pull Velocity Iteration if the liquid fraction equation is almost converged (i.e., the position of the liquid-solid interface is not changing very much). This will speed up the calculation, although the residuals may jump when the pull velocities are updated.

5.   Under Options, select either Lever Rule or Scheil Rule. See this section in the separate Theory Guide for details.

6.   In the Create/Edit Materials dialog box (Figure  25.1.2), specify the Melting Heat ( $L$ in this equation in the separate Theory Guide), Solidus Temperature ( $T_{\rm solidus}$ in this equation in the separate Theory Guide), and Liquidus Temperature ( $T_{\rm liquidus}$ in this equation in the separate Theory Guide) for the material being used in your model.

Materials

Figure 25.1.2: The Create/Edit Materials Dialog Box for Melting and Solidification

If you are solving for species transport, you will also have to specify the Melting Temperature of the pure solvent ( $T_{\rm melt}$ in this equation and this section in the separate Theory Guide). The solvent is the last species material of the mixture material. For each solute, you will have to specify the slope of the liquidus surface ( Slope of Liquidus Line) with respect to the concentration of the solute ( $m_i$ in this equation and this equation in the separate Theory Guide), the Partition Coefficient ( $K_i$), and the rate of Diffusion in Solid (if Lever Rule is selected in the Solidification and Melting dialog box). It is not necessary to specify $m_i$ and $K_i$ for the solvent.

For the mixture material, specify the Liquidus Temperature and the Solidus Temperature method. The default method is the phase diagram, in which the liquidus temperatures and the solidus temperatures are calculated from the phase diagram parameters (such as the slope or partition coefficient) provided for each solute. However, a user-defined function of type DEFINE_PROPERTY can be used to specify both these temperatures. See the separate UDF Manual. for examples of DEFINE_PROPERTY.

It is highly recommended that you use the same method for specifying the Liquidus Temperature and the Solidus Temperature.

7.   Set the boundary conditions.

Boundary Conditions...

In addition to the usual boundary conditions, consider the following:

• If you want to account for the presence of an air gap between a wall and an adjacent solidified region (as described in this section in the separate Theory Guide), specify a nonzero value, a profile, or a user-defined function for Contact Resistance ( $R_c$ in this equation in the separate Theory Guide) under Thermal Conditions in the Wall dialog box.

• If you want to specify the gradient of the surface tension with respect to the temperature at a wall boundary, you can use the Marangoni Stress option for the wall Shear Condition. See Section  7.3.14 for details.

• If you want ANSYS FLUENT to compute the pull velocities during the calculation, note how your specified velocity conditions are used in this calculation (see this section in the separate Theory Guide).

Section  25.2 contains additional information about modeling continuous casting. See Sections  25.3 and 25.4 for information about solving a solidification/melting model and postprocessing the results.