Setting convection on structured mesh parameters

Iteration on a hybrid mesh

Flowchart of the solution procedure on the hybrid mesh. 

Figure 25. Flowchart of the solution procedure on the hybrid mesh.

The solution of the global thermal problem on a hybrid mesh consists of the alternating solution of all transport equations on the structured mesh and then of the enthalpy equation on the global level for both mesh types of the hybrid mesh.

In the first step the temperature values at the interface between the structured and unstructured domain is hold constant while solution iterations on the structured mesh only is running. After some iterations number on the structured mesh will be done or the interruption criterion will be achieved, the second step begins.

In the second step the solution of the transport equations everywhere on the structured mesh is hold. The global thermal problem is formulated on both mesh types. The discretization of the enthalpy equation is thereby repeated in the same way but the equations matrix is transferred not to the SIP solver responsible only for the structured domain but to the solver of the global thermal problem (typically GSSV, entered in the Forward tab of the Numerical Parameters dialog). The distribution of the convective fluxes and of the effective thermal conductivity on the structured mesh is accounted for turbulent flow. The global thermal problem with account of the radiative heat transfer is solved once in the second step. The next loop of the stacked iteration begins.

Creation of the structured mesh tabs

The numerical parameters for treatment of the transport equations on the structured mesh are accessible in the dialog tabs for structured mesh of the Convection Parameters window. The dialog tabs for structured mesh are reserved in the layout of the Convection Parameters window, but they will be activated only after the structured mesh is created.

The number of the tabs which will be activated depends on the number of created structured domains with different materials. A structured domain consists of a group of regions filled with the same material. An individual set of numerical parameters can be applied for each structured domain. For example in the Liquid Encapsulated Czochralski configuration three separated structured domains can be created for the melt, gas and liquid glass encapsulant.

Another possibility is, to separate the gas filled cavities into individual structured domains in order to switch on or off the turbulence modeling independently in each domain.

The materials in two structured domains are considered as "different" if the name identifier of one material is not contained in the name identifier of the other material. Otherwise both groups of regions are joined into the same structured domain.

The possibility of automatic merging together of materials with similar name identifiers into structured domains simplifies an application of materials with different properties in the same domain. The rheological properties should be the same for a consistent consideration of the fluid flow. The optical properties may be different. For example an introduction of the fictive opaque material "Material_Name_opaque" additionally to the transparent material "Material_Name" allows separation of the transparent radiative cavities for reduction of the size of the view factors matrix.

The named structured domains occurring as tabs in the Convection parameters dialog window get the name of the material which is available in the regions of the structured domain.


After the structured mesh is generated and the structured domains are created according to the materials distribution, the materials in regions of the structured domains cannot be exchanged. First the structured mesh should be deleted, then the materials distribution modified and the structured mesh generation repeated.

Parameters for equations on structured mesh

Structured mesh tab in the Convection parameters dialog 

Figure 26. Structured mesh tab in the Convection parameters dialog

The numerical parameters for the structured domain are accessible in the dialog tab of the corresponding structured domain. In the dialog tab they can be entered for each activated transport equation. The numerical parameters are arranged in columns and the transport equations in rows of the table. The meaning of individual numerical parameters for each structured domain is explained below.

  • stacked iterations number

    This parameter is important for organization of the solution procedure for the hybrid scheme consisting of the structured and unstructured meshes. It prescribes the number of iteration on structured mesh of the considered domain which should be done. The prescribed number of iterations is executed. The domain is then either in the waiting mode if there are other structured domains with larger stacked iterations number parameter or the "structured" part of the stacked iteration is left and the program is switched to the global thermal solution on both mesh types.

    The optimum number of the stacked iterations depends on the specific weight of the computational effort on the structured mesh with respect to the general computational cost. If a single iteration for the global thermal solution takes long time (because of e. g. a large view factors matrix), then the number of stacked iterations should be increased for an equilibrium distribution of the computational load between the structured and global levels. Typical number of stacked iterations is between 30 and 100 while the fluid flow is considered on structured mesh in a complex configuration.

  • underrelaxation

    The underrelaxation of the linearized transport equations on the structured mesh. The value should be positive between 0 and 1. Approaching unity means no underrelaxation for the transport equation, smaller value increases the underrelaxation and decelerates the numerical solution.

    Higher underrelaxation is required for strongly nonlinear problems as turbulent convection or laminar convection close to the stability boundary. The "secure" input for the turbulence model is to set all underrelaxation factors equal to 0.1 and about 0.5 for turbulent viscosity. For linear problems in contrary no underrelaxation is required. The best values of underrelaxation which enable a stable convergence and a minimum number of iterations are in general problem and mesh dependent. For any particular application they can be found from experience.

  • resid. reduction

    The factor of residual reduction for the SIP solver. The inner iterations for the considered structured mesh will be interrupted after the target residual reduction is achieved. The value 0.1 is typical, it means that the solver should reduce the total equation residual on the single structured domain by factor 10. The solution of the nonlinear coupled equations by the segregated method doesn't require the precise solution each time after the equations linearization. Therefore usually a small relative residual reduction is sufficient for the progress of the convergence procedure.

  • upwind

    The flux blending parameter between 0 and 1. It distributes the weight between the central differences and the pure upwind method for computation of the convective fluxes. The zero value corresponds to the pure upwind and unity stands for pure central differences.

    The upwinding increases the numerical stability but it introduces an artificial numerical diffusivity. The upwind method (value 0) is advised for all equations in case of the turbulent flow computation.

  • solver sweeps

    The maximum number of the internal SIP solver iterations before it breaks. Usually several iterations are enough in order to achieve the break criterion given in the dialog field resid. reduction . The solver interrupts either after the break criterion is achieved or the maximum number of inner iterations was executed.

Equations solved on the structured mesh

All equations are discretized according to the Finite Volume technique (FV) on the block-structured mesh. The equations are solved block-wise with exchange of the boundary values at the inner matched block boundaries.

  • temperature

    The enthalpy equation for temperature is solved on the structured mesh. The same discretization on the structured mesh is used also for matrix assembly of the global thermal problem including the unstructured mesh (hybrid method). The underrelaxation value may be a sensitive parameter for temperature equation. The underrelaxation value from this dialog is applied only for solution of the enthalpy equation on the structured mesh. Another underrelaxation parameter (in the dialog window Numerical Parameters-> Forward tab) is used for equations on the unstructured and structured mesh solved on the global level.

    The temperature row in the dialog is never switched off because the temperature field is always considered in the code. Other transport equations can be activated or deactivated in dependence of settings for the physical phenomena considered in the regions of the structured domain.

  • momentum

    The same parameters are applied to the radial and axial momentum equations on the structured mesh.

  • pressure

    SIMPLE method is used for the pressure correction in order to achieve the divergence free solution for the velocity field. The flow is considered as incompressible. The pressure correction equation should be usually stronger underrelaxated than the momentum equations. The value 0.1 for the pressure underrelaxation works mostly well.

  • rotation

    The transport equation for the azimuthal velocity. The requirements for these equations are analogous as for temperature because almost the same diffusive and convective terms in the differential equations are present.

  • species

    The species transport equation is discretized on the structured mesh of the domain using the same numerical method as for the other variables. The solution of the species equation is succeeded only on the global level. Instead of the SIP solver only the solver prescribed in the Forward tab of the Numerical Parameters dialog is used. The other numerical parameters which assist the work of the solver are entered and applied in the Species tab of the Numerical Parameters dialog. Therefore the numerical parameters of the species transport equation will be not used here. The enabled row of numerical parameters for the equation indicates only that the species transport is activated and the discretization will be assembled on the mesh of the domain.

    Usually no underrelaxation of the species transport equation is necessary. If the species transport computation fails without underrelaxation, this may show that the mesh density in the convective boundary layers is not sufficient. Then the Reynolds and Schmidt numbers should be estimated and the mesh refined according to the resulting thickness of the boundary layer.

    If more than one single species should be included into the consideration, then the chemistry model should be used instead of the single species transport equation, see the description of the Chemistry model setup procedure.

  • turb. energy

    The turbulent energy transport equation is the first of two transport equations solved additionally in the k-epsilon model. It describes the generation, transport and dissipation of the turbulent kinetic energy of small eddies in the turbulent flow. This equation is highly nonlinear, therefore a strong underrelaxation and sufficient size of the mesh, especially in the boundary layers, is necessary.

  • dissipation

    Eddy dissipation (epsilon in the k-epsilon turbulence model ) is the rate of the turbulent energy destruction. For the eddy dissipation a special transport equation is solved. The nonlinearity of the epsilon transport equation and resulting requirements to its numerical resolution are analogous to the turbulent energy transport equation.

  • turb. viscosity

    The turbulent viscosity is a field value in the turbulence model derived algebraically from the turbulent energy and its dissipation rate. The turbulent viscosity is the only variable which affects the solution of the momentum and enthalpy equations. No transport equations should solved directly for the turbulent viscosity. The row in the dialog tab is activated always together with the turbulent energy and eddy dissipation if the turbulence model is selected in the Physical phenomena tab for regions of the structured domain.