11.3.2 Dynamic Mesh Update Methods

Three groups of mesh motion methods are available in ANSYS FLUENT to update the volume mesh in the deforming regions subject to the motion defined at the boundaries:

• smoothing methods

• dynamic layering

• local remeshing methods

Note that you can use ANSYS FLUENT's dynamic mesh models in conjunction with hanging node adaption, with the exception of dynamic layering and face remeshing. For more information on hanging node adaption, see this section in the separate Theory Guide.

Under Mesh Methods, select Smoothing, Layering, and/or Remeshing and click the Settings... button. The Mesh Method Settings dialog box will open, where you will specify the various settings of the meshing methods. Details about these methods and their applicability to different cases are provided in this section.

Smoothing Methods

To enable spring-based smoothing (or Laplacian smoothing if the 2.5D remeshing method is enabled), enable the Smoothing option under Mesh Methods in the Dynamic Mesh task page (Figure  11.3.1). The relevant parameters are specified in the Smoothing tab which can be displayed by clicking Settings....

Figure 11.3.2: The Smoothing Tab in the Mesh Method Settings Dialog Box

Spring-Based Smoothing

You can control the spring stiffness by adjusting the value of the Spring Constant Factor between 0 and 1. A value of 0 indicates that there is no damping on the springs, and boundary node displacements have more influence on the motion of the interior nodes. A value of 1 imposes the default level of damping on the interior node displacements as determined by solving this equation (in the separate Theory Guide).

The effect of the Spring Constant Factor is illustrated in Figures  11.3.3 and 11.3.4, which show the trailing edge of a NACA-0012 airfoil after a counter-clockwise rotation of 2.3 $^\circ$ and the mesh is smoothed using the spring-based smoother but limited to 20 iterations. Degenerate cells (Figure  11.3.3) are created with the default value of 1 for the Spring Constant Factor. However, the original mesh distribution (Figure  11.3.4) is recovered if the Spring Constant Factor is set to 0 (i.e., no damping on the displacement of nodes on the airfoil surface).

Figure 11.3.3: Effect of a Spring Constant Factor of $1$ on Interior Node Motion

Figure 11.3.4: Effect of a Spring Constant Factor of $0$ on Interior Node Motion

If your model contains deforming boundary zones, you can use the Boundary Node Relaxation to control how the node positions on the deforming boundaries are updated. On deforming boundaries, the node positions are updated such that

where $\beta$ is the Boundary Node Relaxation. A value of 0 prevents deforming boundary nodes from moving (equivalent to turning off smoothing on deforming boundary zones) and a value of 1 indicates no under-relaxation.

You can control the solution of this equation (in the separate Theory Guide) using the values of Convergence Tolerance and Number of Iterations. ANSYS FLUENT solves this equation (in the separate Theory Guide) iteratively during each time step until one of the following criteria is met:

• The specified number of iterations has been performed.

• The solution is converged for that time step:

  
  

  
  

  where $\Delta\vec{x}^1_{\rm rms}$ is the interior and deforming nodes RMS displacement at the first iteration.

For additional information about spring-based smoothing, see this section in the separate Theory Guide.

Applicability of the Spring-Based Smoothing Methods

You can use the spring-based smoothing method to update any cell or face zone whose boundary is moving or deforming.

For non-tetrahedral cell zones (non-triangular in 2D), the spring-based method is recommended when the following conditions are met:

• The boundary of the cell zone moves predominantly in one direction (i.e., no excessive anisotropic stretching or compression of the cell zone).

• The motion is predominantly normal to the boundary zone.

If these conditions are not met, the resulting cells may have high skewness values, since not all possible combinations of node pairs in non-tetrahedral cells (or non-triangular in 2D) are idealized as springs.

By default, spring-based smoothing on non-triangular or non-tetrahedral cell zones are turned off. If you want to use spring-based smoothing on all cell shapes, you can turn on the model for these zones using the spring-on-all-shapes? text interface command:

define $\rightarrow$ models $\rightarrow$ dynamic-mesh-controls $\rightarrow$ smoothing-parameter $\rightarrow$ spring-on-all-shapes?

Laplacian Smoothing Method

Note that for 2.5D remeshing method modeling (3D flows only), you can only change the Boundary Node Relaxation and the Number of Iterations. Note that the Number of Iterations is used for both spring-based and Laplacian smoothing . The Boundary Node Relaxation is used differently by ANSYS FLUENT when the 2.5D remeshing method model is used. On deforming boundaries, the node positions are updated such that

For additional information about Laplacian smoothing, see this section in the separate Theory Guide.

Boundary Layer Smoothing Method

For additional information about boundary layer smoothing, see this section in the separate Theory Guide.

Dynamic Layering Method

To enable dynamic layering, enable the Layering option under Mesh Methods in the Dynamic Mesh task page (Figure  11.3.5). The layering control is specified in the Layering tab which can be displayed by clicking Settings....

Figure 11.3.5: The Layering Tab in the Mesh Method Settings Dialog Box

You can control how a cell layer is split by specifying either Height Based or Ratio Based under Options. Note that for Height Based, the height of the cells in a particular new layer will be constant, but you can choose to have this height vary from layer to layer as a function of time or crank angle when you specify the Cell Height in the Dynamic Mesh Zones dialog box (see Section  11.3.9 for further details).

The Split Factor and Collapse Factor ( $\alpha_s$ in this equation (in the separate Theory Guide) and $\alpha_c$ in this equation (in the separate Theory Guide) respectively) are the factors that determine when a layer of cells (hexahedra or wedges in 3D, or quadrilaterals in 2D) that is next to a moving boundary is split or merged with the adjacent cell layer, respectively.

For additional information about the dynamic layering method, see this section in the separate Theory Guide.

Applicability of the Dynamic Layering Method

You can use the dynamic layering method to split or merge cells adjacent to any moving boundary provided the following conditions are met:

• All cells adjacent to the moving face zone are either wedges or hexahedra (quadrilaterals in 2D) even though the cell zone may contain mixed cell shapes.

• The cell layers must be completely bounded by one-sided face zones, except when sliding interfaces are used (see Section  11.3.2).

• If the bounding face zones are two-sided walls, you must split the wall and wall-shadow pair and use the coupled sliding interface option to couple the two adjacent cell zones.

• Note that you cannot use the dynamic layering method in conjunction with hanging node adaption. For more information on hanging node adaption, see this section in the separate Theory Guide.

If the moving boundary is an internal zone, cells on both sides (possibly with different ideal cell layer heights) of the internal zone are considered for dynamic layering.

If you want to use dynamic layering on cells adjacent to a moving wall that do not span from boundary to boundary, you must separate those cells which are involved in the dynamic layering and use the sliding interfaces capability in ANSYS FLUENT to transition from the deforming cells to the adjacent non-deforming cells (see Figure  11.3.6). For a moving interior face, the zones must be separated such that they are either expanding or collapsing on the same side. No one zone can consist of both expanding and collapsing layers.

Figure 11.3.6: Use of Sliding Interfaces to Transition Between Adjacent Cell Zones and the Dynamic Layering Cell Zone

Remeshing Methods

On zones with a triangular or tetrahedral mesh, the spring-based smoothing method (described in Section  11.3.2) is normally used. When the boundary displacement is large compared to the local cell sizes, the cell quality can deteriorate or the cells can become degenerate. This will invalidate the mesh (e.g., result in negative cell volumes) and consequently, will lead to convergence problems when the solution is updated to the next time step.

To circumvent this problem, ANSYS FLUENT agglomerates cells that violate the skewness or size criteria and locally remeshes the agglomerated cells or faces. If the new cells or faces satisfy the skewness criterion, the mesh is locally updated with the new cells (with the solution interpolated from the old cells). Otherwise, the new cells are discarded.

ANSYS FLUENT includes several remeshing methods that include local remeshing, local face remeshing (for 3D flows only), face region remeshing, and 2.5D surface remeshing (for 3D flows only). The available remeshing methods in ANSYS FLUENT work for triangular-tetrahedral zones and mixed zones where the non-triangular/tetrahedral elements are skipped. The exception is the 2.5D model, where the available remeshing method only work on wedges extruded from triangular surfaces or hex meshes.

To enable remeshing methods, enable the Remeshing option under Mesh Methods in the Dynamic Mesh task page (Figure  11.3.7). The remeshing methods are specified in the Remeshing tab which can be displayed by clicking Settings....

You can view the vital statistics of your mesh by clicking the Mesh Scale Info... button at the bottom of the Mesh Method Settings dialog box. This dialog box displays the Mesh Scale Info dialog box where you can view the minimum and maximum length scale values as well as the maximum cell and face skewness values.

Figure 11.3.7: The Remeshing Tab in the Mesh Method Settings Dialog Box

In local remeshing, ANSYS FLUENT agglomerates cells based on skewness, size, and height (adjacent moving face zones) prior to the movement of the boundary. The size criteria are specified with Minimum Length Scale and Maximum Length Scale. Cells with length scales below the minimum length scale and above the maximum length scale are marked for remeshing. The value of Maximum Cell Skewness indicates the desired skewness of the mesh. By default, the Maximum Cell Skewness is set to 0.9 for 3D simulations and 0.6 for 2D simulations. Cells with skewness above the maximum skewness are marked for remeshing.

For 3D simulations, the Local Face remeshing method is available, allowing you the convenience of remeshing deforming boundary faces if you so desire. Once the option is enabled, you are able to set the Maximum Face Skewness to a specific value. In addition, you should enable the Remeshing option in the Meshing Options tab of the Dynamic Mesh Zones dialog box for a deforming zone type (see Section  11.3.9). You also have the option of choosing either the Local Cell remeshing method or the Region Face remeshing methods by selecting the appropriate option under Remeshing Methods for a deforming zone type. Note that depending on the case, either or both methods have to be enabled.

The marking of cells based on skewness is done at every time step when the local remeshing method is enabled. However, marking based on size and height is performed between the specified Size Remesh Interval since the change in cell size distribution is typically small over one time step.

By default, ANSYS FLUENT replaces the agglomerated cells only if the quality of the remeshed cells has improved.

When you use the Sizing Function remeshing option (see Figure  11.3.8), you can control three parameters that govern the size function. You can specify the Size Function Resolution, the Size Function Variation, and the Size Function Rate or you can return to ANSYS FLUENT's default values by using the Use Defaults button.

Figure 11.3.8: The Remeshing Tab in the Mesh Method Settings Dialog Box Using the Sizing Function Option

The size function Resolution controls the density of the background mesh (see Section  11.3.2). By default, it is equivalent to 3 in 2D simulations and 1 in 3D simulations.

The size function Variation corresponds to $\alpha$ in this equation (in the separate Theory Guide). It is the measure of the maximum permissible cell size and it ranges from $-1< \alpha < + \infty$.

The size function Rate corresponds to $\beta$ in this equation (in the separate Theory Guide). It is the measure of the rate of growth of the cell size, and it ranges from $-0.99< \beta < + + 0.99$. A value of 0 implies linear growth, whereas higher values imply a slower growth near the boundary with faster growth as one moves toward the interior.

Local Face Remeshing Method

The local face remeshing method only applies to 3D geometries. Using this method, ANSYS FLUENT marks the faces (and the adjacent cells) on the deforming boundaries based on the face skewness. Using this method, ANSYS FLUENT is able to remesh locally at deforming boundaries, however, you are not able to remesh across multiple face zones.

Applicability of the Local Face Remeshing Method

If you define deforming face zones in your model and you use local face remeshing in the adjacent cell zone, the faces on the deforming face zone can be remeshed only if the following conditions are met:

• The faces are triangular.

• The faces do not exists across zones or features.

• Note that you cannot use the local face remeshing method in conjunction with hanging node adaption. For more information on hanging node adaption, see this section in the separate Theory Guide.

Local Remeshing Based on Size Functions

Instead of marking cells based on minimum and maximum length scales, ANSYS FLUENT also marks cells based on the size distribution generated by the sizing function if the Sizing Function option is enabled.

Local remeshing using size functions can be used with the following remeshing methods:

• local remeshing

• 2.5D surface remeshing

For additional information about local remeshing using size functions, see this section in the separate Theory Guide.

For steady-state applications (see Section  11.3.5), you can instruct ANSYS FLUENT to perform a second round of cell marking and agglomeration after the boundary has moved, based on skewness criteria. The intent is to further improve the mesh quality through additional local remeshing. This optional feature works in conjunction with the Dynamic Mesh task page (Figure  11.3.7), and operates according to the skewness parameters you set in this dialog box. The size function parameters are not considered during this additional remeshing. Note that enabling this option will increase the time required to update the mesh during the solution.

Additional local remeshing after the boundary has moved is not available for transient dynamic mesh applications, as the resulting numerical method would no longer be conservative.

To employ additional local remeshing, first make sure that you have enabled the Remeshing option in the Dynamic Mesh task page, have entered the appropriate skewness parameters, and have clicked OK in the Mesh Method Settings dialog box. Then enter the following text command:

define $\rightarrow$ models $\rightarrow$ dynamic-mesh-controls $\rightarrow$ remeshing-parameter $\rightarrow$ remeshing-after-moving?

Finally, type yes to the question, optional remeshing after moving the mesh?

Face Region Remeshing Method

For additional information about local remeshing using size functions, see this section in the separate Theory Guide.

Applicability of the Face Region Remeshing Method

You can use the local remeshing method only in cell zones that contain tetrahedral or triangular cells.

If you define deforming face zones in your model and you use local remeshing in the adjacent cell zone, the faces on the deforming face zone can be remeshed only if the following conditions are met:

• The faces are triangular (or linear in 2D).

• Note that you cannot use the face region remeshing method in conjunction with hanging node adaption. For more information on hanging node adaption, see this section in the separate Theory Guide.

2.5D Surface Remeshing Method

The 2.5D surface remeshing method only applies to extruded 3D geometries and is similar to local remeshing in two dimensions on a triangular surface mesh (not a mixed zone). Faces on a deforming boundary are marked for remeshing based on face skewness, minimum and maximum length scale and an optional sizing function.

For additional information about 2.5D surface remeshing, see this section in the separate Theory Guide.

Applicability of the 2.5D Surface Remeshing Method

The following applies to the 2.5D surface remeshing method:

• Triangular faces get remeshed based on marking.

• Extruded prisms get remeshed based on the remeshing of the triangular face. Only extruded regions get remeshed, not mixed regions.

• Note that you cannot use the 2.5D surface remeshing method in conjunction with hanging node adaption. For more information on hanging node adaption, see this section in the separate Theory Guide.

• In the extruded/coopered mesh, area zone changes are not allowed. In such cases, make sure that the face zones at the extruded mesh area do not change from the top to the bottom. For more information about the 2.5D model, see Section  11.3.2.

• Periodics are not supported at the extruded zones.

Using the 2.5D Model

For 3D simulations only, you can select the 2.5D model under the Remeshing tab in the Mesh Method Settings dialog box. This model allows for a specific subset of remeshing techniques.

The 2.5D mesh essentially is a 2D triangular mesh which is expanded, or extruded, along the normal axis of the specific dynamic zone that you are interested in modeling. The triangular surface mesh is remeshed and smoothed on one side, and the changes are then extruded to the opposite side. Rigid body motion is applied to the moving face zones, while the triangular extrusion surface is assigned to a deforming zone with remeshing and smoothing enabled. The opposite side of the triangular mesh is assigned to be a deforming zone as well, with only smoothing enabled, as in Figure  11.3.10.

Figure 11.3.9: The Remeshing Tab for the 2.5D Model

For more information on setting smoothing and remeshing parameters, see Section  11.3.2.

The 2.5D model only applies to mapable (i.e., extrudable) mesh geometries such as pumps, as in Figure  11.3.10. Only the aspects of the geometry that represent the "moving parts" need to be extruded in the mesh.

Figure 11.3.10: 2.5D Extruded Gear Pump Geometry

You must only apply smoothing to the opposite side of the extruded mesh, since ANSYS FLUENT requires the geometry information for the dynamic zone. ANSYS FLUENT projects the nodes back to its geometry after the extrusion. Without this geometry information, the dynamic zones tends to lose its integrity.

In parallel, a partition method that partitions perpendicular to the extrusion surface should be used. For example, if the normal of the extrusion surface points in the x-direction then Cartesian-Y or Cartesian-Z would be the perfect partition methods.

The 2.5D model is used in combination with a DEFINE_GRID_MOTION UDF. (See this section in the separate UDF Manual for information about hooking this UDF.)

This UDF is associated with the extrusion surface that is adjacent to the cell zone, in turn applying the same deformation to the entire cell zone. This approach is particularly useful when modeling gear pumps that are predominantly extruded hexahedral meshes. For more information about this UDF, contact your support engineer.

Feature Detection

For 3D simulations, ANSYS FLUENT allows you to preserve features on deforming zones not only between the different face zones, but also within a face zone.

In the Geometry Definition tab of the Dynamic Mesh Zones dialog box, for any geometry definition, you can indicate whether you want to include features of a specific angle by selecting Include Features under Feature Detection and setting the Feature Angle (the zonal feature angle $\alpha$) in degrees. If the angle $\beta$ between adjacent faces is bigger than the specified angle, then the feature is recognized (i.e., $\cos (\beta) < \cos (\alpha)$).

Applicability of Feature Detection

The following items are applicable for use with feature detection:

• Feature remeshing is only possible with face region remeshing

• Features are preserved by local face remeshing, i.e. there is no local face remeshing across features

• Smoothing methods preserve features, i.e. nodes at feature edges are not allowed to be smoothed