The block-structured mesh shown in the previous figure should be used for computation of the turbulent gas convection in the gas filled cavities of the VCz facility. A high mesh quality is required for application of the turbulence model. Special care should be taken on the numerical resolution in the turbulent boundary layers and on the minimum orthogonality of the mesh.

The default mesh created in the previous example with automatical mesh refinement in the boundary layers of thickness 10 mm, distance of the last node 1 mm and the default mesh density of 5 mm is not everywhere satisfactory. Therefore an additional effort should be invested into the mesh quality.

The preprocessor tools ** Grid properties at the line**
and ** Shift edges between two selected
lines** can be used for local modification of the
structured mesh, see
Structured mesh generation and adjustment
for details.

A minimum mesh density should be assured everywhere. Therefore first increase the edge number on the lines at the external domain boundary, if where is apparently to few edges. For example there are only 2 edges at the line of the auxiliary drawing at the inner surface of the vertical crucible wall in the figure above.

The selected line of the auxiliary drawing (middle mouse button)
is marked by a red segment. The number of selected lines,
current number of edges at the single selected
line and the refinement factor for it are indicated in the
**Structured Grid** dialog. For change of the
number of edges at the line enter a new number of edges into the dialog window
and press the button **accept and regenerate
grid**.

The number of edges will be changed at the selected line. The same change will be done at the block side opposite to the selected line. An increase of the mesh density will be distributed homogeneously over the segments at the opposite block side. Therefore first the mesh density at segments with the smallest mesh density will be increased. By the reduction of the edges number in opposite first the edges number is reduced for segments with the highest edges number at the opposite block side.

After the change in the mesh size according to the change of the edges number at the selected line is done for the block, the preprocessor will search for the other blocks in contact with the changed block. If for example the selected line is shared by two neighboring blocks, the mesh changes will be done for the neighbor too. Then the preprocessor propagates in the same manner changes of the mesh density to other blocks if they are connected with the changed blocks. The changes are done recursively until they will be aborted at the external block boundary of the structured domain in all directions of the propagation. This procedure assures that the condition of the matched boundaries at the shared inner block interfaces will be preserved after any local change of the mesh density was done

The sequence of the edge lengths in the marked boundary layer is
created automatically by the mesh generated for given parameters of
the boundary layer. These parameters are unique for all blocks and
for all structured domains. A higher mesh density can be required at
some specified location in the boundary layer. In this case the
parameter ** refinement factor ** in the
** grid properties at the line ** dialog box other
than unity can be entered. Accordingly the change is confirmed
by the **accept and regenerate
grid** button press, exactly as by the change of the
edge number at the line.

The refinement factor different from 1 causes the geometrical progression of the edge lengths at the selected line. This procedure has a higher priority than the automatical mesh distribution rules in the boundary layer which are applied otherwise. The refinement factor affects change of the distance between the last node in the fluid and the liquid-solid interface. One should avoid the refinement factor values outside of the [0.8...1.2] interval, because too quick change in the mesh density can lead to problems by computation of the fluid flow.

Next you can redistribute the number of edges between two selected lines of the auxiliary drawing. Both selected lines should be at the same block side and belong only to the single block, i. e. they should be at the external boundary of the structured domain. The aim of the redistribution is an improvement of the mesh orthogonality, because the redistribution changes angles between two systems of the mesh lines xi and eta.

The result of such mesh adjustment is shown in the figure below.

**Figure 102. Block-structured mesh around crystal after manual
improvement addressing mesh density and orthogonality**

Almost everywhere the deviation of the mesh from orthogonality is within the specified visualization threshold of 30 degrees. This mesh can be already successfully used for computation of the turbulent buoyancy driven convection at a high gas pressure.

The mesh orthogonality is important not only inside of the numerical block but also at the internal block boundary. The knick of the mesh lines at the shared block boundary has the same influence on the numerical solution as the knick in the inner part of the block-structured mesh. The mesh deviation from orthogonality is indicated in color only for the mesh lines inside of the blocks. The orthogonality at the shared block boundaries is not included into the graphical precaution.

The error introduced by angle between two mesh line systems at the block boundary depends on the angle between the lines and the size of the last control volume.

The general rule for an acceptable meshing is, the line connecting central nodes of the adjacent control volumes at both sides from the shared block boundary, should be fully contained inside of both control volumes. Otherwise the interpolation error may became critical.

This rule is illustrated in the following figure where an acceptable and a bad transition between the blocks are shown. The shared block boundary is indicated with a green line, red lines connect the central nodes in the last 2D control volumes at the block boundary.

**Figure 103. The correct (A )and wrong (B) mesh transition at the
shared block boundary. The line connecting central nodes of
the adjacent control volumes leaves their area in the case B.**

The thickness of boundary layer is defined by the numerical solution for the transported value in vicinity of the solid-liquid interface. The diffusive momentum transport (shear forces) is concentrated inside of the momentum boundary layer. Therefore the numerical resolution of the velocity profile there is important for the numerical prediction of the flow properties.

The minimum required number of nodes to be placed into the boundary layer across to the solid-liquid interface varies typically from 5 till 8. Other than advised no satisfactory numerical resolution can be achieved.

A minimum mesh size needed in order to obtain the converged and physically meaningful solution can be obtained in each particular modeling case from experience. Usually for the given process parameters (Grashof number etc.) the estimation of the boundary layer thickness is sufficient for determination of the mesh density. A useful rule for estimation of the boundary layer thickness d is

with Re Reynolds number, L characteristical length of the
considered geometry. For the buoyancy driven flow the
corresponding Reynolds number is calculated as a square root from
the Reynolds number. For the tools for computation of the
Reynolds, Grashof and Prandtl characteristic numbers by means of
the *CrysMAS* user interface, see the corresponding section
Computing Characteristic Numbers.

The diffusive heat and species transport have their maximum value also in the boundary layer. The thickness of the temperature boundary layer is related to the thickness of the momentum boundary layer divided by Prandtl number. Analogously the diffusive boundary layer for the species transport is estimated as the momentum boundary layer divided by the Schmidt number.

The field values of the turbulence model have usually very sharp profiles in the boundary layer and require an accurate resolution there in order to reduce the grid dependence. An accurate resolution in the boundary layer is especially important for the turbulent buoyancy driven thermally coupled fluid flow, obvious wall functions are applied for the heat flux, diffusive species flux and the shear force there. The reason for it is in case of the turbulent gas flow (moderate Prandtl number) the velocity profile in the boundary layer along the vertical wall, which has usually its local maximum close to the solid-liquid interface. Sufficient number of numerical nodes should be placed inside of the boundary layer.

If the generated mesh works not properly by the computation of convection and variation of the numerical parameters (underrelaxation) doesn't help, the user should return to the preprocessing and try to increase the mesh density or repeat the mesh generation from scratch with another settings which are closer to the demands of the numerical formulation.