10.6.2. 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:

Note that you can use ANSYS Fluent’s dynamic mesh models in conjunction with adaption, with the exception of dynamic layering (in almost all cases) and any remeshing method other than CutCell zone remeshing. For more information on the available adaption methods, see Hanging Node Adaption and Polyhedral Unstructured Mesh Adaption in the Theory Guide.

Details on how to set up the various dynamic mesh update methods are provided in the sections that follow.

10.6.2.1. Smoothing Methods

When smoothing is used to adjust the mesh of a zone with a moving and/or deforming boundary, the interior nodes of the mesh move, but the number of nodes and their connectivity does not change. In this way, the interior nodes “absorb” the movement of the boundary. To enable smoothing, perform the following steps:

  1. Enable the Smoothing option in the Mesh Methods group box of the Dynamic Mesh Task Page.

  2. Click the Settings... button to open the Mesh Method Settings dialog box.

    Figure 10.14:  The Smoothing Tab of the Mesh Method Settings Dialog Box (3D)

    The Smoothing Tab of the Mesh Method Settings Dialog Box (3D)

  3. If you want spring-based smoothing, select Spring/Laplace/Boundary Layer from the Method list and define the settings in the Parameters group box, which are described in Spring-Based Smoothing.

  4. If you want diffusion-based smoothing (described in Diffusion-Based Smoothing):

    1. Select Diffusion from the Method list.

    2. Make a selection from the Diffusion Function drop-down list, to indicate whether you want the diffusion coefficient to be a function of the boundary-distance or the cell-volume. These functions and suggested values for the Diffusion Parameter are described in Diffusivity Based on Boundary Distance and Diffusivity Based on Cell Volume.

  5. If you want smoothing using the linearly elastic solid method (described in Linearly Elastic Solid Based Smoothing Method):

    1. Select Linearly Elastic Solid from the Method list.

    2. Enter the Poisson’s Ratio in the Parameters group box.

  6. If you selected Diffusion or Linearly Elastic Solid smoothing and the simulation involves periodic or quasi-periodic motion, you can specify that the smoothing uses a reference position by using the following text command. This option may improve the mesh quality consistency from cycle to cycle—see Smoothing from a Reference Position for details.

    define → dynamic-mesh → controls → smoothing-parameters → smooth-from-reference-position?

  7. If you plan to apply the 2.5D remeshing method (as described in 2.5D Surface Remeshing Method), perform the following steps to set up Laplacian smoothing (as described in Laplacian Smoothing Method).

    1. Select Spring/Laplace/Boundary Layer from the Method list

    2. Define only the Laplace Node Relaxation and the Number of Iterations in the Parameters group box (the other settings are not relevant).

  8. If you plan to apply the boundary layer smoothing method (as described in Boundary Layer Smoothing Method), select Spring/Laplace/Boundary Layer from the Method list.

10.6.2.1.1. Spring-Based Smoothing

For spring-based smoothing, the edges between any two mesh nodes are idealized as a network of interconnected springs. The initial spacings of the edges before any boundary motion constitute the equilibrium state of the mesh. A displacement at a given boundary node will generate a force proportional to the displacement along all the springs connected to the node. Using Hook’s Law, the force on a mesh node can be written as

(10–2)

where and are the displacements of node and its neighbor , is the number of neighboring nodes connected to node , and is the spring constant (or stiffness) between node and its neighbor . The spring constant for the edge connecting nodes and is defined as

(10–3)

where is the value you enter for Spring Constant Factor.

At equilibrium, the net force on a node due to all the springs connected to the node must be zero. This condition results in an iterative equation such that

(10–4)

where is the iteration number.

Since displacements are known at the boundaries (after boundary node positions have been updated), Equation 10–4 is solved using a Jacobi sweep on all interior nodes. At convergence, the positions are updated such that

(10–5)

where and are used to denote the positions at the next time step and the current time step, respectively. The spring-based smoothing is shown in Figure 10.15: Spring-Based Smoothing on Interior Nodes: Start and Figure 10.16: Spring-Based Smoothing on Interior Nodes: End for a cylindrical cell zone where one end of the cylinder is moving.

Figure 10.15:  Spring-Based Smoothing on Interior Nodes: Start

Spring-Based Smoothing on Interior Nodes: Start

Figure 10.16:  Spring-Based Smoothing on Interior Nodes: End

Spring-Based Smoothing on Interior Nodes: End

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 Equation 10–4.

The effect of the Spring Constant Factor is illustrated in Figure 10.17: Interior Nodes Extend Beyond Boundary (Spring Constant Factor = 1) and Figure 10.18: Interior Nodes Remain Within Boundary (Spring Constant Factor = 0), which show the trailing edge of a NACA-0012 airfoil after a counter-clockwise rotation of 2.3° and the mesh is smoothed using the spring-based smoother but limited to 20 iterations. Degenerate cells (Figure 10.17: Interior Nodes Extend Beyond Boundary (Spring Constant Factor = 1)) are created with the default value of 1 for the Spring Constant Factor, as the interior nodes extend beyond the moving boundary. However, the original mesh distribution (Figure 10.18: Interior Nodes Remain Within Boundary (Spring Constant Factor = 0)) is recovered if the Spring Constant Factor is set to 0 (that is, no damping on the displacement of interior nodes near the airfoil surface).

Figure 10.17:  Interior Nodes Extend Beyond Boundary (Spring Constant Factor = 1)

Interior Nodes Extend Beyond Boundary (Spring Constant Factor = 1)

Figure 10.18:  Interior Nodes Remain Within Boundary (Spring Constant Factor = 0)

Interior Nodes Remain Within Boundary (Spring Constant Factor = 0)

You can control the solution of Equation 10–4 using the values of Convergence Tolerance and Number of Iterations. ANSYS Fluent solves Equation 10–4 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:

    (10–6)

    where is the interior and deforming nodes RMS displacement at the first iteration.

10.6.2.1.1.1. Applicability of the Spring-Based Smoothing Method

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 can be used when the following conditions are met:

  • The boundary of the cell zone moves predominantly in one direction (that is, 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. Polyhedral cells are particularly likely to become highly skewed with spring-based smoothing (regardless of whether the previous conditions are met), and so the diffusion-based smoothing method is generally recommended for polyhedra (see Diffusion-Based Smoothing).

By default, spring-based smoothing is disabled for cell zones that are not entirely composed of either tetrahedral or triangular cells. This is reflected in the Elements options under Parameters in the Mesh Method Settings dialog box (Figure 10.14: The Smoothing Tab of the Mesh Method Settings Dialog Box (3D)). By default, the Elements are set to Tet in Tet Zones in 3D (or Tri in Tri Zones in 2D). If you want to use spring-based smoothing on all element types, you can do that by selecting the All option.

If you have mixed element zones and you do not want spring-based smoothing on all element types, you can enable spring-based smoothing on only the tetrahedral or triangular cells by selecting Tet in Mixed Zones in 3D (or Tri in Mixed Zones in 2D). Selection of smoothing elements in the Mesh Method Settings dialog box applies by default to all cell zones that undergo spring-based smoothing. In order to have more precise control, it is possible to overwrite this global selection on individual dynamic cell zones (see Deforming Motion). This gives, for example, the flexibility to suppress smoothing in zones where dynamic layering (see Dynamic Layering) is used and allows at the same time smoothing of non-simplex (that is not tetrahedral or triangular) elements in other zones.

10.6.2.1.2. Diffusion-Based Smoothing

For diffusion-based smoothing, the mesh motion is governed by the diffusion equation

(10–7)

where is the mesh displacement velocity. The boundary conditions for Equation 10–7 are obtained from the user-prescribed or computed (six DOF) boundary motion. On deforming boundaries, the boundary conditions are such that the mesh motion is tangent to the boundary (that is, the normal velocity component vanishes). The Laplace equation Equation 10–7 then describes how the prescribed boundary motion diffuses into the interior of the deforming mesh.

The diffusion coefficient in Equation 10–7 can be used to control how the boundary motion affects the interior mesh motion. A constant coefficient means that the boundary motion diffuses uniformly throughout the mesh. With a nonuniform diffusion coefficient, mesh nodes in regions with high diffusivity tend to move together (that is, with less relative motion).

In Fluent, two different formulations are available for the diffusion coefficient . The first formulation allows you to have the diffusion coefficient be a function of the boundary distance, and is of the form

(10–8)

where is a normalized boundary distance. The second formulation allows you to have the diffusion coefficient be a function of the cell volume, and is of the form

(10–9)

where is the normalized cell volume. In both Equation 10–8 and Equation 10–9, is a user input parameter. See Diffusivity Based on Boundary Distance and Diffusivity Based on Cell Volume for information about defining the diffusion coefficient.

ANSYS Fluent uses different numerical methods to solve the vector Equation 10–7, depending on the element types present in the mesh. In the absence of polyhedral elements or elements with hanging nodes (that is, meshes that have undergone hanging node adaption and some hexcore or CutCell meshes) the equation is solved using a finite element discretization and the displacement velocity, , is obtained directly at each mesh node. If the mesh contains polyhedral elements or hanging nodes, the equation is discretized using ANSYS Fluent’s standard finite volume method and the cell-centered solution for the displacement velocity, , is interpolated onto the nodes using inverse-distance-weighted averaging. The node positions are then updated according to:

(10–10)

The finite element discretization is generally superior, as the solution is obtained directly at the nodes and no interpolation step is necessary. The finite volume method can be enforced for meshes of all element types by executing the TUI command:

/define/dynamic-mesh/controls/smoothing-parameters/diffusion-fvm? yes

Computationally, solving a PDE for mesh smoothing is generally more costly than spring-based smoothing. But it tends to produce better quality meshes than spring-based smoothing and often allows larger boundary deformations before breaking down. Figure 10.19: The Initial Mesh and Figure 10.20: Valid Mesh After 45 Degree Rotation Using Diffusion-Based Smoothing show a mesh before and after rotating the boundary by 45 degrees, using diffusion-based smoothing. With spring-based smoothing, the same mesh shows degenerated cells after a rotation of 40 degrees (Figure 10.21: Degenerated Mesh After 40 Degree Rotation Using Spring-Based Smoothing).

Figure 10.19:  The Initial Mesh

The Initial Mesh

Figure 10.20:  Valid Mesh After 45 Degree Rotation Using Diffusion-Based Smoothing

Valid Mesh After 45 Degree Rotation Using Diffusion-Based Smoothing

Figure 10.21:  Degenerated Mesh After 40 Degree Rotation Using Spring-Based Smoothing

Degenerated Mesh After 40 Degree Rotation Using Spring-Based Smoothing

It should be noted that with diffusion-based smoothing the interior mesh motion is governed by the solution to Equation 10–7 and the prescribed boundary motion, and not by mesh irregularities. Poor quality elements or mesh defects are not smoothed out by this method, but rather move together with the pre-computed (at the begin of each mesh update) displacement velocity .

It is also worth noting that the nature of the diffusion equation is such that the resulting solution (that is, the displacement velocity ) depends on the dimensionality of the problem and the type of boundary motion prescribed. To illustrate the impact of the type of boundary motion, consider the goal of boundary-distance-based diffusion (Equation 10–8): to control which parts of the mesh absorb the boundary motion, so that you can preserve the mesh in the vicinity of the moving boundary (at the expense of the interior of the mesh). For more translational (piston-type) boundary motions, you can preserve a reasonably “thick” region of the mesh adjacent to the boundary (that is, multiple layers of cells); for rotational boundary motions, the rate of decay for the solution as you move away from the boundary is such that it can be difficult to preserve even a “thin” region. For this reason, mesh smoothing can handle translational boundary motions generally much better than rotational motions.

Although it should in most cases not be necessary, the accuracy of the solution to the diffusion equation governing the mesh motion can be controlled by selecting the maximum number of iterations, max-iter, and the relative residual tolerance, relative-convergence-tolerance, in the text interface:

define → dynamic-mesh → controls → smoothing-parameters → max-iter

define → dynamic-mesh → controls → smoothing-parameters → relative-convergence-tolerance

You can enable printing of smoothing residuals in the text interface with the command:

/define/dynamic-mesh/controls/smoothing-parameters/verbosity 1

For simulations with periodic or quasi-periodic motion, you can improve the mesh quality consistency by specifying that the diffusion-based smoothing uses a reference position, as described in Smoothing from a Reference Position.

10.6.2.1.2.1. Diffusivity Based on Boundary Distance

Using boundary-distance-based diffusion (Equation 10–8) allows you to control how the boundary motion diffuses into the interior of the domain as a function of boundary distance. Decreasing the diffusivity away from the moving boundary causes those regions to absorb more of the mesh motion, and better preserves the mesh quality near the moving boundary. This is particularly helpful for a moving boundary that has pronounced geometrical features (such as sharp corners) along with a prescribed motion that is predominantly rotational.

You can manipulate the diffusion coefficient (in Equation 10–8) primarily by adjusting the Diffusion Parameter . A range of 0 to 2 has been shown to be of practical use. A value of 0 (the default value) specifies that and yields a uniform diffusion of the boundary motion throughout the mesh. Higher values of preserve larger regions of the mesh near the moving boundary, and cause the regions away from the moving boundary to absorb more of the motion.

The following two figures illustrate the effect of the Diffusion Parameter on the resulting mesh for a translational (piston-type) boundary motion, when the diffusivity is based on the boundary distance. In this example, an initially uniformly meshed square domain is deformed by moving the left boundary to the right.

Figure 10.22:  Effect of Diffusion Parameter of 0 on Interior Node Motion

Effect of Diffusion Parameter of 0 on Interior Node Motion

Figure 10.23:  Effect of Diffusion Parameter of 1 on Interior Node Motion

Effect of Diffusion Parameter of 1 on Interior Node Motion

For rotational boundary motions, a value of 1.5 for the Diffusion Parameter is recommended as a good starting point.

Two different methods are available for the evaluation of the boundary distance if boundary-distance-based diffusion is used. By default, Fluent uses the “standard” boundary distance in Equation 10–8, which is the normalized distance to the nearest wall boundary; note that none of the other boundary types (for example, inlets, outlets, symmetry, and periodic boundaries) are considered. This method is the same as that which is used to evaluate the boundary distance for turbulence models. An example of this method is shown in Figure 10.23: Effect of Diffusion Parameter of 1 on Interior Node Motion, where only the left and right boundaries are walls. You have the option of using a “generalized” boundary distance instead, which is the normalized distance to the nearest boundary that is not declared as deforming, regardless of type. Both methods use the largest distance found in all deforming cell zones to normalize the value.

You can specify that the generalized boundary distance is used via the following text command:

define → dynamic-mesh → controls → smoothing-parameters → boundary-distance-method

If the generalized boundary distance is used, an additional scalar equation for the boundary distance will be solved as part of the solution of Equation 10–7.

10.6.2.1.2.2. Diffusivity Based on Cell Volume

Using cell-volume-based diffusion (Equation 10–9) allows you to control how the boundary motion diffuses into the interior of the domain as a function of cell size. Decreasing the diffusivity in larger cells causes those cells to absorb more of mesh motion and therefore better preserves the cell quality of smaller cells.

You can manipulate the diffusion coefficient (in Equation 10–8) by adjusting the Diffusion Parameter . A value of 0 (the default value) specifies that and yields a uniform diffusion of the boundary motion throughout the mesh. Higher values of result in larger cells absorbing more of the motion than smaller cells.

Note that the cell volume used in Equation 10–9 is the local cell volume, normalized by the average cell volume of all deforming cell zones.

10.6.2.1.2.3. Applicability of the Diffusion-Based Smoothing Method

Diffusion-based mesh smoothing is an alternative method to spring-based smoothing. It is available for all element types, and you can use it to update any cell zone whose boundaries are moving or deforming.

Diffusion-based smoothing is computationally more expensive than spring-based smoothing, but likely results in better mesh quality (especially for non-tetrahedral / non-triangular cell zones, and for polyhedral cells in particular) and generally allows for larger boundary deformations before breaking down.

Similar to spring-based smoothing, diffusion-based mesh smoothing can handle translational boundary deformations much better than rotational motions.

Diffusion-based smoothing is not compatible with the boundary layer smoothing method or the face region remeshing method. For more information about these methods, see Boundary Layer Smoothing Method and Face Region Remeshing Method.

10.6.2.1.3. Linearly Elastic Solid Based Smoothing Method

With mesh smoothing based on the linearly elastic solid model, the mesh motion is governed by the following set of equations.

(10–11)

where is the stress tensor, is the strain tensor, and is the mesh displacement. For the solution of Equation 10–11 only the ratio between the shear modulus, , and Lamé’s first parameter, , matters. This ratio is parameterized through Poisson’s ratio:

(10–12)

which is made available as a user input.

The boundary conditions for Equation 10–11 are obtained from the user-prescribed or computed (in the case of six DOF motion) boundary deformations. These imposed deformations are transferred into the interior of the deforming mesh as if the mesh was a linearly elastic solid with the given material properties. On deforming boundaries you can either specify a geometry along which the mesh can slide, or leave the geometry unspecified. If a geometry is specified for the deforming boundary, then the boundary conditions are such that the deformation normal to the boundary vanishes and the stress tangential to the boundary is zero. If the geometry of the deforming boundary is unspecified, then the deforming boundary can also deform in the normal direction and the boundary conditions are such that the traction is zero in all directions. See Deforming Motion for details of how to specify geometry on deforming zones.

The linear system in Equation 10–11 is solved using a finite element discretization and the mesh displacements for the interior and deforming boundary nodes are obtained directly at the nodes. The accuracy to which the linear system is solved can be controlled by the maximum number of iterations max-iter, and the relative residual tolerance relative-convergence-tolerance in the text interface:

define → dynamic-mesh → controls → smoothing-parameters → max-iter

define → dynamic-mesh → controls → smoothing-parameters → relative-convergence-tolerance

The linearly elastic solid mesh smoothing model supports constant material properties only. The permissible range for Poisson’s ratio, , is between -1.0 and 0.5.

For simulations with periodic or quasi-periodic motion, you can improve the mesh quality consistency by specifying that the linearly elastic solid mesh smoothing uses a reference position, as described in Smoothing from a Reference Position.

10.6.2.1.3.1. Applicability of the Linearly Elastic Solid Based Smoothing Method

Mesh smoothing based on the linearly elastic solid model is an alternative method to diffusion-based and spring-based smoothing. Most of the properties and limitations discussed for diffusion-based smoothing (Applicability of the Diffusion-Based Smoothing Method) also apply to the linearly elastic solid model, particularly the mesh quality degradation for rotational motions. The linearly elastic solid model is computationally more expensive than diffusion-based smoothing, but for some meshes and mesh motions preserves the mesh quality better.

The current implementation with constant material properties can be a limitation compared with diffusion-based smoothing with non-uniform diffusivity. In cases with rotational boundary motion and sharp corners it may be advantageous to use diffusion-based smoothing with boundary-distance-dependent diffusivity.

The option to leave the geometry of deforming face zones unspecified is only available with the linearly elastic solid smoothing method.

The linearly elastic solid smoothing method supports triangular and quadrilateral elements in 2D and tetrahedral, hexahedral, wedge, and pyramid cells in 3D. It cannot be applied if the deforming cell zone contains polyhedral cells or hanging nodes. In such cases diffusion-based smoothing is recommended.

Linearly elastic solid smoothing is not compatible with the boundary layer smoothing method or the face region remeshing method. For more information about these methods, see Boundary Layer Smoothing Method and Face Region Remeshing Method.

10.6.2.1.4. Smoothing from a Reference Position

When the mesh smoothing is based on diffusion or the linearly elastic solid model, you have the option of specifying that the smoothing uses a reference position. This can be helpful when performing many cycles of periodic or quasi-periodic motion: when you ensure that the smoothing is always done from the same reference position, the mesh quality may remain more consistent from cycle to cycle. Note that no mesh manipulation should be done to the zone undergoing such smoothing.

To enable this option, use the following text command:

define → dynamic-mesh → controls → smoothing-parameters → smooth-from-reference-position?

The reference position is saved the first time you perform smoothing after enabling this option. The reference position is not saved to the case or data file, so restarting from a case file will imply that a different reference position is used after restart. This still provides the benefit of consistent quality, but the resulting meshes might be slightly different from a continuous run. The impact of such slight mesh changes on the solution results will be small, except for cases with a high degree of mesh dependence; for such exceptional cases, it is recommended that you evaluate the original mesh to ensure that it is suitable for the problem.

10.6.2.1.5. Laplacian Smoothing Method

Laplacian smoothing is the most commonly used and the simplest mesh smoothing method. This method adjusts the location of each mesh vertex to the geometric center of its neighboring vertices. This method is computationally inexpensive but it does not guarantee an improvement on mesh quality, since repositioning a vertex by Laplacian smoothing can result in poor quality elements. To overcome this problem, ANSYS Fluent only relocates the vertex to the geometric center of its neighboring vertices if and only if there is an improvement in the mesh quality (that is, the skewness has been improved).

This improved Laplacian smoothing can be enabled on deforming boundaries only (that is, the zone with triangular elements in 3D and zones with linear elements in 2D). The computation of the node positions works as follows:

(10–13)

where is the averaged node position of node at iteration , is the node position of neighbor node of at iteration , and is the number nodes neighboring node . The new node position is then computed as follows:

(10–14)

where is the Laplace node relaxation factor.

This update only happens if the maximum skewness of all faces adjacent to is improved in comparison to .

For details on applying Laplacian smoothing to either a cell zone (with 2.5D remeshing) or a face zone, see Smoothing Methods or Deforming Motion, respectively.

10.6.2.1.6. Boundary Layer Smoothing Method

The boundary layer smoothing method is used to deform the boundary layer mesh during a moving-deforming mesh simulation. For cases that apply mesh motion (either Rigid Body or User-Defined) to a face zone with adjacent boundary layers, the boundary layers can be made to deform accordingly by enabling Deform Adjacent Boundary Layer with Zone for the face zone in the Dynamic Mesh Zones Dialog Box. With boundary layer smoothing enabled, the nodal coordinates of each cell in the boundary layer zone are updated with the same displacement vector as the corresponding nodes on the underlying face zone. The boundary layer smoothing method can be applied to boundary layer zones of all mesh types (that is, wedges and hexahedra in 3D, quadrilaterals in 2D).

Consider the example below, where a UDF of the form DEFINE_GRID_MOTION provides the moving-deforming mesh model with the locations of the nodes located on the compliant strip on an idealized airfoil. The node motion varies sinusoidally in time and space (compare Figure 10.24: The Undeformed Mesh with Figure 10.25: The Deformed Mesh).

Figure 10.24:  The Undeformed Mesh

The Undeformed Mesh

Figure 10.25:  The Deformed Mesh

The Deformed Mesh

As a result of the boundary layer smoothing, the cells adjacent to the deforming wall are also deformed in order to preserve the quality of boundary layer zone. If you compare Figure 10.26: Zooming into the Undeformed Compliant Strip with Figure 10.27: Zooming into the Deformed Compliant Strip with Boundary Layer Smoothing Applied, you can see how the boundary layer cells have been deformed according to the motion of the nodes on the compliant strip.

Figure 10.26:  Zooming into the Undeformed Compliant Strip

Zooming into the Undeformed Compliant Strip

Figure 10.27:  Zooming into the Deformed Compliant Strip with Boundary Layer Smoothing Applied

Zooming into the Deformed Compliant Strip with Boundary Layer Smoothing Applied

Typically, the boundary layer smoothing method preserves the height of the boundary layer cells adjacent to the deformed face zone. However, note that this approach is primarily intended for translational motion. If the faces undergo substantial rotation, the boundary layer cells may become skewed. See Smoothing Methods and Specifying Boundary Layer Deformation Smoothing for details about enabling smoothing and defining a moving and deforming boundary layer, respectively. Note that boundary layer smoothing is compatible with spring-based smoothing only. It cannot be used with diffusion-based smoothing or linearly elastic solid smoothing. Also note that the boundary layer smoothing method will work whether or not you have segregated the boundary layer elements into a separate cell zone.

10.6.2.2. Dynamic Layering

In prismatic (hexahedral and/or wedge) mesh zones, you can use dynamic layering to add or remove layers of cells adjacent to a moving boundary, based on the height of the layer adjacent to the moving surface. The dynamic mesh model in ANSYS Fluent allows you to specify an ideal layer height on each moving boundary. The layer of cells adjacent to the moving boundary (layer in Figure 10.28: Dynamic Layering) is split or merged with the layer of cells next to it (layer in Figure 10.28: Dynamic Layering) based on the height () of the cells in layer .

Figure 10.28:  Dynamic Layering

Dynamic Layering

If the cells in layer are expanding, the cell heights are allowed to increase until

(10–15)

where is the minimum cell height of cell layer , is the ideal cell height, and is the layer split factor. Note that ANSYS Fluent allows you to define as either a constant value or a value that varies as a function of time or crank angle. When the condition in Equation 10–15 is met, the cells are split based on the specified layering option. This option can be height based or ratio based.

With the height-based option, the cells are split to create a layer of cells with constant height and a layer of cells of height . With the ratio-based option the cells are split such that, locally, the ratio of the new cell heights to old cell heights is exactly everywhere. Figure 10.29: Results of Splitting Layer with the Height-Based Option and Figure 10.30: Results of Splitting Layer with the Ratio-Based Option show the result of splitting a layer of cells above a valve geometry using the height-based and ratio-based option.

Figure 10.29:  Results of Splitting Layer with the Height-Based Option

Results of Splitting Layer with the Height-Based Option

Figure 10.30:  Results of Splitting Layer with the Ratio-Based Option

Results of Splitting Layer with the Ratio-Based Option

If the cells in layer are being compressed, they can be compressed until

(10–16)

where is the layer collapse factor. When this condition is met, the compressed layer of cells is merged into the layer of cells above the compressed layer in Figure 10.28: Dynamic Layering; that is, the cells in layer are merged with those in layer .

To enable dynamic layering, enable the Layering option under Mesh Methods in the Dynamic Mesh Task Page (Figure 10.31: The Layering Tab in the Mesh Method Settings Dialog Box). The layering control is specified in the Layering tab, which can be displayed by clicking Settings....

Figure 10.31:  The Layering Tab in the Mesh Method Settings Dialog Box

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 Specifying the Motion of Dynamic Zones for further details).

The Split Factor and Collapse Factor ( in Equation 10–15 and in Equation 10–16, 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.

10.6.2.2.1. 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:

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 that 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 10.32: Use of Sliding Interfaces to Transition Between Adjacent Cell Zones and the Dynamic Layering Cell Zone). 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 10.32:  Use of Sliding Interfaces to Transition Between Adjacent Cell Zones and the Dynamic Layering Cell Zone

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

10.6.2.3. Remeshing Methods

On zones with a triangular or tetrahedral mesh, the spring-based smoothing method (described in Spring-Based Smoothing) 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 (for example, 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 and the old cells are retained.

ANSYS Fluent includes several remeshing methods that include local cell remeshing, zone remeshing, local face remeshing (for 3D flows only), face region remeshing, CutCell zone remeshing (for 3D flows only), and 2.5D surface remeshing (for 3D flows only). The remeshing methods are suitable for particular kinds of cell types:

  • The local cell remeshing method only affects triangular and tetrahedral cell types in the mesh (that is, in mixed cell zones the non-triangular/tetrahedral cells are skipped).

  • The local face remeshing method is available in 3D only and can remesh tetrahedral cells and wedge cells in boundary layer meshes.

  • The zone remeshing method replaces all cell types with triangular tetrahedral cells (in 2D and 3D domains, respectively), and can remesh and produce wedge cells in 3D boundary layer meshes.

  • The face region remeshing method is applied to triangular cells in 2D, and tetrahedral cells in 3D. In 3D domains, the face region remeshing method can also remesh and produce wedge cells in 3D boundary layer meshes.

  • The CutCell zone remeshing method works for all cell types.

  • The 2.5D remeshing method only works on hexagonal meshes or wedge cells extruded from triangular surface elements.

To enable remeshing methods, enable the Remeshing option under Mesh Methods in the Dynamic Mesh Task Page (Figure 10.13: The Dynamic Mesh Task Page). Click the Settings... button to open the Mesh Method Settings dialog box, where you can specify the remeshing method and parameters in the Remeshing tab (Figure 10.33: The Remeshing Tab in the Mesh Method Settings Dialog Box).

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 button opens 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 10.33:  The Remeshing Tab in the Mesh Method Settings Dialog Box

The Remeshing Tab in the Mesh Method Settings Dialog Box

Figure 10.34:  The Remeshing Tab in the Mesh Method Settings Dialog Box Using the Sizing Function Option

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

10.6.2.3.1. Local Remeshing Method

Using the local remeshing method (that is, local cell remeshing, with or without local face remeshing), ANSYS Fluent marks cells based on cell skewness and minimum and maximum length scales as well as an optional sizing function.

ANSYS Fluent evaluates each cell and marks it for remeshing if it meets one or more of the following criteria:

  • It has a skewness that is greater than a specified maximum skewness.

  • It is smaller than a specified minimum length scale.

  • It is larger than a specified maximum length scale.

  • Its height does not meet the specified length scale (at moving face zones, for example, above a moving piston).

If local remeshing is not able to reduce the maximum cell skewness sufficiently, then the cell zone remeshing method is used to automatically remesh all of the cells in the cell zone, as well as the faces of all adjacent deforming dynamic face zones (see Cell Zone Remeshing Method for details). The maximum allowable cell skewness is set to be 0.98 by default. The cell zone remeshing method gives the mesher more flexibility to create a new mesh of better quality than the local cell remeshing method. The automatic remeshing of cell zones can be disabled using the following text command:

define → dynamic-mesh → controls → remeshing-parameter → zone-remeshing

10.6.2.3.1.1. Local Cell Remeshing Method

As previously mentioned, in local cell 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 0.7 for 2D simulations. Cells with skewness above the maximum skewness are marked for remeshing.

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 Remeshing 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.

Note that you cannot use the local cell remeshing method in conjunction with adaption. For more information on the available adaption methods, see Hanging Node Adaption and Polyhedral Unstructured Mesh Adaption in the Theory Guide.

10.6.2.3.1.2. Local Face Remeshing Method

The local face remeshing method only applies to 3D geometries. You can apply this method to the boundaries of deforming or user-defined zone types, so that ANSYS Fluent will mark faces (and adjacent cells) based on the face skewness, and then remesh them.

Local face remeshing also allows the remeshing of wedge cells in boundary layers at those boundaries. The detection of boundary layers (as well as the wedge element height distribution and number of layers) is automatic and does not require your input.

To apply local face remeshing, perform the following steps:

  1. Enable the Local Face option in the Remeshing tab of the Mesh Method Settings Dialog Box, and set the Maximum Face Skewness to an appropriate global value.

  2. For each deforming or user-defined boundary zone on which you want local face remeshing applied, enable the Local option (under Remeshing Methods) in the Meshing Options tab of the Dynamic Mesh Zones Dialog Box. (Note that for deforming zones, you must first enable the Remeshing option under Methods, and then Local will be enabled by default.) You can also revise the Maximum Skewness field in this tab if you want a value that is different from the global setting. For further details on the zone setup, see Deforming Motion and/or User-Defined Motion.

10.6.2.3.1.2.1. Applicability of the Local Face Remeshing Method

When you enable local face remeshing for a boundary, the faces can be remeshed only if the following conditions are met:

  • The faces are triangular.

  • The agglomerated faces do not span multiple zones or feature edges.

Note that you cannot use the local face remeshing method in conjunction with adaption. For more information on the available adaption methods, see Hanging Node Adaption and Polyhedral Unstructured Mesh Adaption in the Theory Guide.

10.6.2.3.1.3. 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.

Cells can be marked using size functions only with the following remeshing methods:

Figure 10.36: Mesh at the End of a Dynamic Mesh Simulation With Size Functions demonstrates the advantages of using size functions for local remeshing.

Figure 10.35:  Mesh at the End of a Dynamic Mesh Simulation Without Size Functions

Mesh at the End of a Dynamic Mesh Simulation Without Size Functions

Figure 10.36:  Mesh at the End of a Dynamic Mesh Simulation With Size Functions

Mesh at the End of a Dynamic Mesh Simulation With Size Functions

In determining the sizing function, ANSYS Fluent draws a bounding box around the zone that is approximately twice the size of the zone, and locates the shortest feature length within each fluid zone. ANSYS Fluent then subdivides the bounding box based on the shortest feature length and the Size Function Resolution that you specify. This allows ANSYS Fluent to create a background mesh.

You control the resolution of the background mesh and a background mesh is created for each fluid zone. The shortest feature length is determined by shrinking a second box around the object, and then selecting the shortest edge on that box. The size function is evaluated at the vertex of each individual background mesh.

Figure 10.37:  Size Function Determination at Background Mesh Vertex I

Size Function Determination at Background Mesh Vertex I

As seen in Figure 10.37: Size Function Determination at Background Mesh Vertex I, the local value of the size function is defined by

(10–17)

where is the distance from vertex on the background mesh to the centroid of boundary cell and is the mesh size (length) of boundary cell .

The size function is then smoothed using Laplacian smoothing. ANSYS Fluent then interpolates the value of the size function by calculating the distance from a given cell centroid to the background mesh vertices that surround the cell (see Figure 10.38: Interpolating the Value of the Size Function). The intermediate value of the size function at the centroid is computed from

(10–18)

Figure 10.38:  Interpolating the Value of the Size Function

Interpolating the Value of the Size Function

Next, a single point is located within the domain (see Figure 10.39: Determining the Normalized Distance) that has the largest distance to the nearest boundary to it. The normalized distance for the given centroid is given by

(10–19)

Figure 10.39:  Determining the Normalized Distance

Determining the Normalized Distance

Using the parameters and (the Size Function Variation and the Size Function Rate, respectively), you can write the final value of the size function at point as

(10–20)

where is the intermediate value of the size function at the cell centroid.

Note that is the size function variation. Positive values mean that the cell size increases as you move away from the boundary. Since the maximum value of is one, the maximum cell size becomes

(10–21)

therefore, is really a measure of the maximum cell size.

The factor is computed from

(10–22)

(10–23)

You can use Size Function Variation (or ) to control how large or small an interior cell can be with respect to its closest boundary cell. ranges from to , an value of 0.5 indicates that the interior cell size can be, at most, 1.5 the size of the closest boundary cell. Conversely, an value of indicates that the cell size interior of the boundary can be half of that at the closest boundary cell. A value of 0 indicates a constant size distribution away from the boundary.

You can use Size Function Rate (or ) to control how rapidly the cell size varies from the boundary. The value of should be specified such that . A positive value indicates a slower transition from the boundary to the specified Size Function Variation value. Conversely, a negative value indicates a faster transition from the boundary to the Size Function Variation value. A value of 0 indicates a linear variation of cell size away from the boundary.

You can also control the resolution of the sizing function with Size Function Resolution. The resolution determines the size of the background bins used to evaluate the size distribution with respect to the shortest feature length of the current mesh. By default, the Size Function Resolution is 3 in 2D problems, and 1 in 3D problems.

A set of default values (based on the current mesh) is automatically generated if you click Use Defaults.

In summary, the sizing function is a distance-weighted average of all mesh sizes on all boundary faces (both stationary and moving boundaries). The sizing function is based on the sizes of the boundary cells, with the size computed from the cell volume by assuming a perfect (equilateral) triangle in 2D and a perfect tetrahedron in 3D. You can control the size distribution by specifying the Size Function Variation and the Size Function Rate. If you have enabled the Sizing Function option, ANSYS Fluent will agglomerate a cell if

(10–24)

where is a factor defined by Equation 10–22 and Equation 10–23.

Note that the size function is only used for marking cells before remeshing. The size function is not used to govern the size of the cell during remeshing.

For steady-state applications (see Steady-State Dynamic Mesh Applications), 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 10.33: The Remeshing Tab in the Mesh Method Settings Dialog Box), 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.


Important:  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.


When you use the Sizing Function remeshing option (see Figure 10.34: The Remeshing Tab in the Mesh Method Settings Dialog Box Using the Sizing Function Option), 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.

The size function Resolution controls the density of the background mesh (see Local Remeshing Based on Size Functions). By default, it is equivalent to 3 in 2D simulations and 1 in 3D simulations.

The size function Variation corresponds to in Equation 10–20. It is the measure of the maximum permissible cell size and it ranges from .

The size function Rate corresponds to in Equation 10–20. It is the measure of the rate of growth of the cell size, and it ranges from . 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.


Note:  To employ additional local remeshing, first make sure that you have enabled the Remeshing option in the Dynamic Mesh Task Page.


You can also use the following text command:

define → dynamic-mesh → controls → remeshing-parameter → remeshing-after-moving?

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

10.6.2.3.2. Cell Zone Remeshing Method

The cell zone remeshing method allows for the remeshing of the complete cell zone, and provides the option to also remesh the faces of all adjacent deforming dynamic face zones. This remeshing method is enabled by default when local cell remeshing is enabled, and is performed automatically if the local cell remeshing does not produce an acceptable mesh (see Local Remeshing Method for the acceptability criteria). Cell zone remeshing can also be manually invoked, using the following text command:

define → dynamic-mesh → actions → remesh-cell-zone

The cell zone remeshing method is available for triangular cells in 2D meshes and tetrahedral cells in 3D meshes. For 3D meshes, the method also allows the remeshing of wedge cells in boundary layers. The detection of the boundary layers (as well as the wedge element height distribution and number of layers) is automatically performed by default, and allows for different layer parameters on each boundary zone. You can manually specify the parameters by entering nonzero values for first height, growth rate, and number of layers via the text commands available in the define/dynamic-mesh/controls/remeshing-parameters/prism-layer-parameters menu, although generally it is not necessary to do this. When you enter them manually, the boundary layer parameters are global: they apply to every prism layer detected in the remeshing zone.

Note that it is necessary to enable the dynamic mesh model and the remeshing method in order to attain access to the prism layer controls, even if the cell zone is remeshed manually and not as part of a dynamic mesh update.

10.6.2.3.2.1. Limitations of the Cell Zone Remeshing Method

Zone remeshing has the following limitations:

  • Only triangular, tetrahedral, and wedge cell types (when the wedge cells are part of a 3D boundary layer mesh) are remeshed.

  • Zones with hanging nodes cannot be remeshed.

10.6.2.3.3. Face Region Remeshing Method

The face region remeshing method allows for the remeshing of those triangular faces (in 3D meshes) and linear faces (in 2D meshes) that are on a deforming face zone and adjacent to a moving face zone (see layer j in Figure 10.40: Expanding Cylinder Before Region Face Remeshing). ANSYS Fluent marks the faces based on minimum and maximum length scales, and then remeshes the faces and the associated cells to produce a very regular mesh on the deforming boundary. Although primarily designed for in-cylinder type configurations, where the remeshing region is located where cylinder walls meet the moving piston, face region remeshing can be used for all applications where a moving dynamic zone abuts deforming dynamic face zones.

For 3D simulations, ANSYS Fluent allows face region remeshing with symmetric boundary conditions and across multiple face zones. The remeshing can preserve features not only between the different deforming face zones, but also within a face zone. For more information on feature preservation, see Feature Detection. ANSYS Fluent also allows face region remeshing of tetrahedral cell zones that contain wedge cells in boundary layers, as described in the section that follows.

To begin marking the faces for face region remeshing, ANSYS Fluent identifies the nodes at the intersection of a moving dynamic zone and the adjacent deforming zones. ANSYS Fluent then analyzes the height of the faces on the deforming zones that are in the range of the identified nodes, and then remeshes the faces depending on the specified maximum or minimum length scale.

Consider the simple tetrahedral mesh of a cylinder that has a moving end wall (see Figure 10.40: Expanding Cylinder Before Region Face Remeshing). The faces that are subject to remeshing are in layer j of the side wall. If the faces in layer j are expanding, the expansion continues until the height h reaches the maximum length scale, and then the layer is remeshed to form 2 layers of elements (see Figure 10.41: Expanding Cylinder After Region Face Remeshing). Conversely, if the faces of layer j are contracting, the contraction continues until h reaches the minimum length scale, and then layer j and the neighboring layer of faces (layer i) on the deforming zone are remeshed to form a single layer.

Figure 10.40:  Expanding Cylinder Before Region Face Remeshing

Expanding Cylinder Before Region Face Remeshing

Figure 10.41:  Expanding Cylinder After Region Face Remeshing

Expanding Cylinder After Region Face Remeshing

10.6.2.3.3.1. Face Region Remeshing with Wedge Cells in Prism Layers

In 3D simulations, the face region remeshing method can be applied on meshes that have wedge cells along the deforming face zones. When remeshing the faces on the deforming face zones, the associated wedge cells are remeshed as well. The layer parameters are based on the existing mesh by default; you have the option of manually setting these parameters, as described later in this section.

If the motion of the face zone is large compared to the height of the adjacent deforming face zones, it is recommended that you decompose the mesh volume in such a way as to create a dynamic cell zone that moves as a rigid body in between the moving face zone and the deforming dynamic cell zone on which face region remeshing is applied. Consider Figure 10.42: Volume Decomposition for Prism Layers, which displays only half of an in-cylinder mesh. The rigidly moving cell zone encapsulates the prism layers on the moving piston so that the layers are not remeshed, and therefore the risk of generating degenerate cells during the mesh motion update is reduced.

Figure 10.42:  Volume Decomposition for Prism Layers

Volume Decomposition for Prism Layers

It is preferable (and even mandatory, if the mesh is a half model with a symmetry plane) to decompose the volume such that the “corner” region of the prism layers (shown in the previous figure) exists entirely within the rigidly moving zone. This allows for the largest deformations without risking degenerate elements, because the prism normals of the remeshed cells are uniformly perpendicular to the faces undergoing remeshing.

If the range of motion does not allow you to encapsulate the entire corner region of the prism layers in a rigidly moving zone, it is recommended that you encapsulate the “base” of the prism layers (shown in Figure 10.43: Volume Decomposition for the Base of the Prism Layers) and move these cells with a rigid body motion. Although this is less ideal than encapsulating the corner region, it does reduce the risk of degenerate mesh elements.

Figure 10.43:  Volume Decomposition for the Base of the Prism Layers

Volume Decomposition for the Base of the Prism Layers

For piston-type applications that contain prism layers, a reasonable rule of thumb is that you should decompose the mesh volume if the piston motion is more than half the cylinder height. If you decide not to decompose the volume at all, you must at the very least enable the Deform Adjacent Boundary Layer with Zone option in the Meshing Options tab of the Dynamic Mesh Zone dialog box when setting up the moving face zone (see Rigid Body Motion for details). In any case, it is recommended that you always preview the mesh motion over the complete simulation time, to make sure that you will have a valid mesh at each time step.

The prism layer parameters (that is, element height, growth rate, and number of layers) are extracted automatically from the mesh and do not generally require your input. To prevent the prism parameters from drifting due to repeated remeshing, the prism parameters for first height, growth rate, and number of layers can be entered manually, using the text commands available in the define/dynamic-mesh/controls/remeshing-parameters/prism-layer-parameters menu.

10.6.2.3.3.2. Applicability of the Face Region Remeshing Method

Note the following limitations associated with face region remeshing:

  • You can use the face region remeshing method only in cell zones that contain triangular cells (in 2D) or tetrahedral cells, with or without prism layers (in 3D). For 3D meshes, the faces on the deforming boundaries that border the moving face must all be triangular.

  • The face region remeshing method is not compatible with diffusion-based smoothing or linearly elastic solid smoothing.

  • You cannot use the face region remeshing method in conjunction with adaption. For more information on the available adaption methods, see Hanging Node Adaption and Polyhedral Unstructured Mesh Adaption in the Theory Guide.

10.6.2.3.4. CutCell Zone Remeshing Method

The CutCell zone remeshing method is available to remesh a complete cell zone (including all boundary zones of the remeshed cell zone). This method is available for 3D simulations only. The existing volume mesh is replaced by a predominantly Cartesian mesh. Inflation layers can be added as an option. When used as part of a transient simulation, the remeshing occurs at predefined intervals and whenever the mesh quality in the cell zone is deemed poor. Examples of meshes before and after CutCell zone remeshing are shown in Figure 10.44: Unstructured Tetrahedral Mesh Before CutCell Zone Remeshing and Figure 10.45: Mesh After CutCell Zone Remeshing, respectively. Figure 10.46: CutCell Zone Remeshing With Inflation Layers shows a cut through a CutCell mesh with inflation layers.

Figure 10.44:  Unstructured Tetrahedral Mesh Before CutCell Zone Remeshing

Unstructured Tetrahedral Mesh Before CutCell Zone Remeshing

Figure 10.45:  Mesh After CutCell Zone Remeshing

Mesh After CutCell Zone Remeshing

Figure 10.46:  CutCell Zone Remeshing With Inflation Layers

CutCell Zone Remeshing With Inflation Layers

During CutCell zone remeshing, a uniform Cartesian grid is locally refined using size functions, in order to resolve the initial mesh with sufficient accuracy. The resulting mesh consists mostly of hexahedral elements, which reduces the cell count compared to unstructured tetrahedral meshing. Additional element types are used near the boundaries to closely resolve complex shapes. The remeshing takes place at regular intervals, or whenever the mesh quality deteriorates due to mesh motion.

The CutCell zone remeshing method not only replaces the volume mesh, it also replaces the complete surface mesh of the remeshed cell zone. Consequently, this method can only be used to remesh cell zones that are either stand-alone zones or are only connected to other cell zones through non-conformal interfaces. If inflation layers are added to a CutCell mesh, the inflation layers are grown from the remeshed surface mesh, and the CutCell mesh is morphed such that it smoothly matches the cap surfaces of the inflation layers.

The CutCell Zone remeshing method option is available in the Remeshing Methods group box. Note that the CutCell Zone remeshing method does not use any of the parameters specified in the Mesh Method Settings dialog box. The parameters used to control CutCell Zone remeshing are specified in the Dynamic Mesh Zones dialog box when setting up the zone and boundaries.

For more information about CutCell meshes, see the Fluent Meshing User’s Guide.

10.6.2.3.4.1. Applicability of the CutCell Zone Remeshing Method

The CutCell zone remeshing method can be applied to cell zones, with the following limitations:

  • The case must be 3D.

  • The cell zone cannot be conformally connected to other cell zones; that is, a CutCell zone must be a stand-alone cell zone, or can only be connected to another zone through a non-conformal interface. In the latter case, the non-conformal interface is cleared before the remeshing and automatically recreated after the remeshing.

Note that the CutCell zone remeshing method can be applied to cell zones that contain adapted cells.

In parallel, all cells of the remeshed zone will be automatically migrated to and remeshed on a single CPU. Consequently, the machine memory will limit the size of the zone that can be remeshed. The mesh is automatically repartitioned after the remeshing.

In addition to the limitations listed previously, you should also note the following with regard to CutCell zone remeshing:

  • Internal coupled walls, such as baffles, are discarded during the remeshing. The method is designed to primarily remesh cell zones with a single interior zone.

  • Interior jump boundary condition zones (for example, fans, porous jumps), are discarded during the remeshing.

  • Conformal periodic boundary conditions are not maintained after the remeshing. Any existing conformal periodic boundaries on the zone being remeshed should slit and replaced with non-conformal periodic boundaries.

  • If the zone being remeshed contains multiple interior zones prior to the remeshing, all interior zones will be collected into a single interior zone during the CutCell zone remeshing.

10.6.2.3.4.2. Using the CutCell Zone Remeshing Method

In order to apply CutCell zone remeshing to a cell zone, begin by enabling the CutCell Zone option in the Remeshing Methods group box in the Remeshing tab of the Mesh Method Settings dialog box (see Figure 10.33: The Remeshing Tab in the Mesh Method Settings Dialog Box). Next, use the Dynamic Mesh Zones dialog box to create a deforming dynamic zone for the cell zone (see Deforming Motion). Then enable CutCell in the Remeshing Options group box and enter the relevant remeshing parameters, including: the maximum mesh size for the Cartesian cells; the global size function growth rate; the minimum orthogonal quality and remeshing interval to control the remeshing frequency; and the optional global inflation layer settings.

ANSYS Fluent allows you to specify either a soft or a mesh-based size function to control how the Cartesian mesh increases in size from the boundary toward the interior of the cell zone. For the soft size function, you specify a maximum mesh size for each boundary zone of the CutCell cell zone. When you use the mesh-based size function, ANSYS Fluent analyzes the existing mesh to evaluate the necessary mesh refinement at the boundary. See step 4 of Stationary Zones for more information about these size functions. You have control over the size function types and parameters by defining the boundary zones as dynamic zones. If no boundary zone adjacent to the CutCell zone is defined as a dynamic zone, ANSYS Fluent will automatically apply mesh-based size functions to each CutCell boundary zone and use the global growth rate entered for the cell zone to control the remeshing.

Note that the size functions used by the CutCell zone remeshing method are unrelated to the size function used for local cell remeshing (as described in Local Remeshing Based on Size Functions).

ANSYS Fluent allows you to add inflation layers to a CutCell mesh in order to better resolve wall-bounded flow features. After enabling Inflation Layers under the CutCell Zone Parameters for the CutCell cell zone, you can specify the global inflation parameters in the Inflation Settings dialog box. There are two types of inflation layers available: a constant type, where you can specify the constant height of the first layer; and an aspect-ratio type, where the first layer height is locally evaluated based on the specified aspect ratio. The latter is recommended and used by default since it is more robust and generally produces higher quality CutCell meshes. By default, the inflation settings specified apply to every boundary of the cell zone. If you would like to specify different inflation settings for different boundaries, you can define these boundaries as dynamic zones and enable Zonal Inflation Layer Control. Note that the Number of Layers, other than 0, has to be the same on all boundary zones. If different numbers of layers are specified on different boundaries, ANSYS Fluent will only inflate up to the largest common number specified. By setting the number of layers on a boundary zone to 0, you can locally suppress the growth of inflation layers, however, note that the transition is handled by stair stepping and adding wedge elements, which tends to generate skewed elements for small layer element heights.

The cells that contain hanging nodes / edges as a result of the CutCell zone remeshing are automatically converted to polyhedral cells. See Limitations for details about limitations associated with polyhedral cells.

It is recommended that you first manually apply the CutCell zone remeshing method (as described in the section that follows) and inspect the mesh before using the method as part of a transient simulation, as this allows you to evaluate if your remeshing parameters are suitable before running a calculation that is computationally expensive.

10.6.2.3.4.3. Applying the CutCell Zone Remeshing Method Manually

Although the CutCell zone remeshing method is primarily intended as an automatic remeshing method during dynamic mesh updates, you can also manually create a CutCell mesh (that is, you can remesh without running a calculation) by using the following text command:

define → dynamic-mesh → actions → remesh-cell-zone-cutcell

You will be prompted to enter the global parameters for the CutCell zone remeshing. If no dynamic zones are set up in your case, ANSYS Fluent will use the global parameters you enter and apply mesh-based size functions to each boundary of the CutCell zone. If the case is set up as a dynamic mesh case, manual remeshing will use the information specified on each CutCell boundary zone, including the zonal inflation layer settings. During manual CutCell zone remeshing, the global parameters are taken from the text interface input, and the global parameters specified on the CutCell cell zone are ignored.

When executing manual remeshing through the remesh-cell-zone-cutcell text command, you will be prompted to specify whether topology warnings should be ignored. If you do not ignore the topology warnings, ANSYS Fluent will analyze the zone being remeshed and report any interior face zones that will get discarded during the remeshing. If the zone being remeshed has periodic boundary zones, you will also be prompted to either abort the remeshing process or slit the periodics in order to proceed.

You will also be prompted to specify whether the cells that contain hanging nodes / edges as a result of the CutCell zone remeshing should be converted to polyhedral cells. See Limitations for details about limitations associated with polyhedral cells. By default, all hanging node cells are converted to polyhedral cells.

10.6.2.3.5. 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; the 2.5D remeshing method also gives you the option of marking cells using size functions, as described in Local Remeshing Based on Size Functions.

Figure 10.47:  Close-Up of 2.5D Extruded Flow Meter Pump Geometry Before Remeshing and Laplacian Smoothing

Close-Up of 2.5D Extruded Flow Meter Pump Geometry Before Remeshing and Laplacian Smoothing

Figure 10.48:  Close-Up of 2.5D Extruded Flow Meter Pump Geometry After Remeshing and Laplacian Smoothing

Close-Up of 2.5D Extruded Flow Meter Pump Geometry After Remeshing and Laplacian Smoothing

10.6.2.3.5.1. 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 wedges get remeshed based on the remeshing of the triangular face. Only extruded regions get remeshed, not mixed regions.

  • The 2.5D remeshing method does not support remeshing or moving nodes on the perimeter of the extruded zone(s).

  • Note that you cannot use the 2.5D surface remeshing method in conjunction with adaption. For more information on the available adaption methods, see Hanging Node Adaption and Polyhedral Unstructured Mesh Adaption in the Theory Guide.

  • The extrusion must be along a straight line normal to the deforming zone and the cross-section of the extruded/coopered mesh must be constant along the extrusion direction. For more information about the 2.5D model, see Using the 2.5D Model.

  • Periodics are not supported at the extruded zones.

10.6.2.3.5.2. 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 10.50: 2.5D Extruded Gear Pump Geometry.

Figure 10.49:  The Remeshing Tab for the 2.5D Model

The Remeshing Tab for the 2.5D Model

For more information on setting smoothing and remeshing parameters, see Dynamic Mesh Update Methods.

The 2.5D model only applies to mappable (that is, extrudable) mesh geometries such as pumps, as in Figure 10.50: 2.5D Extruded Gear Pump Geometry. Only the aspects of the geometry that represent the “moving parts” must be extruded in the mesh.

Figure 10.50:  2.5D Extruded Gear Pump Geometry

2.5D Extruded Gear Pump Geometry


Important:  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.



Important:  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 Hooking DEFINE_GRID_MOTION UDFs in the Fluent Customization 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.

10.6.2.4. Volume Mesh Update Procedure

The volume mesh is updated automatically based on the methods described in Dynamic Mesh Update Methods. ANSYS Fluent decides which method to use for a particular zone based on which model is enabled and the shape of the cells in the zone. For example, if the boundaries of a tetrahedral cell zone are moving, and unless the zone has been set up for CutCell zone remeshing, the mesh smoothing and local remeshing methods will be used to update the volume mesh in this zone. If the zone consists of prismatic (hexahedral and/or wedge) cells, then the dynamic layer method will be used to determine where and when to insert and remove cell layers. On extruded prism zones, the 2.5D surface meshing method will be used.

Depending on which model is enabled, ANSYS Fluent automatically determines which method to use by visiting the adjacent cell zones and setting appropriate flags for the volume mesh update methods to be used. If you specify the motion for a cell zone, ANSYS Fluent will visit all of the neighboring cell zones and set the flags appropriately. If you specify the motion of a boundary zone, ANSYS Fluent will analyze only the adjacent cell zones. If a cell zone does not have any moving boundaries, then no volume mesh update method will be applied to the zone.


Important:  Note that as a result of the remeshing procedures, updated meshes may be slightly different when dynamic meshes are used in parallel ANSYS Fluent, and therefore very small differences may arise in the solutions.



Important:  Note that if your dynamic mesh model consists of numerous shell conduction zones, the mesh update may be very time consuming because all shells are deleted and recreated during the mesh update.


10.6.2.5. Transient Considerations for Remeshing and Layering

The second order in time transient formulation can be used with remeshing, layering, and smoothing cases. In such cases, second order in time accuracy is preserved during layering events and/or mesh smoothing. However, during remeshing events, the time advancement accuracy reverts to first order. Therefore, it is recommended that you only use second order in time for cases with very low remeshing frequency, that is, for cases where remeshing occurs every several timesteps or more. If remeshing occurs every timestep, the method reduces to a first order formulation. For cases that need very frequent remeshing, it is recommended that you retain the first order in time formulation. For details, see Dynamic Mesh Theory in the Fluent Theory Guide.

The switch to first order happens automatically when the solver detects a topology change as a result of remeshing within a timestep. You will not see a change in the user interface, however you can monitor the switch between first and second order in time by using the following text command to enable the verbosity with dynamic meshes:

define → dynamic-mesh → transient-settings → verbosity

A message showing the active time formulation will print to the console when verbosity is set to 1.


Note:  For cases with second order in time with dynamic mesh enabled, any mesh swapping and manual mesh manipulation will trigger a switch to first order in time.



Release 18.2 - © ANSYS, Inc. All rights reserved.