To simplify the solution process, you may want to merge zones. Merging zones involves combining multiple zones of similar type into a single zone. Setting boundary conditions and postprocessing may be easier after you have merged similar zones.

Zone merging is performed in the Merge Zones Dialog Box (Figure 6.90: The Merge Zones Dialog Box).

 Domain → Zones → Combine → Merge...

Figure 6.90: The Merge Zones Dialog Box

Upon reading a mesh file, Ansys Fluent automatically performs zone separations in two conditions. If a face zone is attached to multiple cells zones in the preprocessor, the face zone will be separated so that each one is attached to only one cell zone. Furthermore, if you have defined an internal face as a wall type, an additional shadow wall zone will be generated (for example, for a wall named baffle, a shadow wall zone named baffle-shadow will be generated).

There are several methods available in Ansys Fluent that allow you to manually separate a single face or cell zone into multiple zones of the same type. If your mesh contains a zone that you want to break up into smaller portions, you can make use of these features. For example, if you created a single wall zone when generating the mesh for a duct, but you want to specify different temperatures on specific portions of the wall, you will need to break that wall zone into two or more wall zones. If you plan to solve a problem using the sliding mesh model or multiple reference frames, but you forgot to create different fluid zones for the regions moving at different speeds, you will need to separate the fluid zone into two or more fluid zones.

There are four ways to separate face zones and two ways to separate cell zones. The face separation methods will be described first, followed by the cell separation tools. Decoupling of periodic zones is discussed in Decoupling Periodic Zones.

Note that all of the separation methods allow you to report the result of the separation before you commit to performing it.

 

6.12.2.1. Separating Face Zones

For more information, see the following sections:

• 6.12.2.1.1. Methods for Separating Face Zones
• 6.12.2.1.2. Inputs for Separating Face Zones

 

6.12.2.1.1. Methods for Separating Face Zones

For geometries with sharp corners, it is often easy to separate face zones based on significant angle. Faces with normal vectors that differ by an angle greater than or equal to the specified significant angle will be placed in different zones. For example, if your mesh consists of a cube, and all 6 sides of the cube are in a single wall zone, you would specify a significant angle of 89°. Since the normal vector for each cube side differs by 90° from the normals of its adjacent sides, each of the 6 sides will be placed in a different wall zone.

If you have a small face zone and would like to put each face in the zone into its own zone, you can do so by separating the faces based on face. Each individual face (triangle, quad, or polygon) will be separated into different zones.

You can also separate face zones based on cell registers. For example, you can mark cells based on their location in the domain (region register), their boundary closeness (boundary register), field values of some variable, or any of the cell marking methods discussed in Using Cell Registers. When you specify which register is to be used for the separation of the face zone, all faces of cells that are marked will be placed into a new face zone.

Finally, you can separate face zones based on contiguous regions. For example, when you use coupled wall boundary conditions you need the faces on the zone to have a consistent orientation. Consistent orientation can only be guaranteed on contiguous regions, so you may need to separate face zones to allow proper boundary condition specification.

 

6.12.2.1.2. Inputs for Separating Face Zones

To break up a face zone based on angle, face, cell register mark, or region, use the Separate Face Zones Dialog Box (Figure 6.91: The Separate Face Zones Dialog Box).

 Domain → Zones → Separate → Faces...

Figure 6.91: The Separate Face Zones Dialog Box

---

Important:  If you are planning to separate face zones, you should do so before performing any adaptions using the hanging node adaption method. Face zones that contain hanging nodes cannot be separated.

---

The steps for separating faces are as follows:

1. Select the separation method (Angle, Face, Mark, or Region) under Options.

2. Specify the face zone to be separated in the Zones list.

3. If you are separating by face or region, skip to the next step. Otherwise, do one of the following:

   • If you are separating faces by angle, specify the significant angle in the Angle field.

   • If you are separating faces by mark, select the cell register to be used in the Registers list.

4. (optional) To check what the result of the separation will be before you actually separate the face zone, click the Report button. The report will look like the following example:

    45 faces in contiguous region 0
    30 faces in contiguous region 1
    11 faces in contiguous region 2
    14 faces in contiguous region 3
    Separates zone 4 into 4 zone(s).
   

5. To separate the face zone, click the Separate button. A report will be printed in the console like the following example:

    45 faces in contiguous region 0
    30 faces in contiguous region 1
    11 faces in contiguous region 2
    14 faces in contiguous region 3
    Separates zone 4 into 4 zone(s).
    Updating new zone information ...
       created new zone wall-4:001 from wall-4
       created new zone wall-4:002 from wall-4
       created new zone wall-4:010 from wall-4
    done.
   

---

Important:  When you separate the face zone by cell register mark, you may sometimes find that a face of a corner cell will be placed in the wrong face zone. You can usually correct this problem by performing an additional separation, based on angle, to move the offending face to a new zone. You can then merge this new zone with the zone in which you want the face to be placed, as described in Merging Zones.

---

 

6.12.2.2. Separating Cell Zones

For more information, see the following sections:

• 6.12.2.2.1. Methods for Separating Cell Zones
• 6.12.2.2.2. Inputs for Separating Cell Zones

 

6.12.2.2.1. Methods for Separating Cell Zones

If you have two or more enclosed cell regions sharing internal boundaries (as shown in Figure 6.92: Cell Zone Separation Based on Region), but all of the cells are contained in a single cell zone, you can separate the cells into distinct zones using the separation-by-region method. Note that if the shared internal boundary is of type interior, you must change it to another double-sided face zone type (fan, radiator, and so on) prior to performing the separation.

Figure 6.92: Cell Zone Separation Based on Region

You can also separate cell zones based on the marks stored in cell registers. You can mark cells using any of the methods discussed in Using Cell Registers (for example, you can mark cells with a certain field value range or cells inside or outside a specified region). When you specify which register is to be used for the separation of the cell zone, cells that are marked will be placed into a new cell zone.

 

6.12.2.2.2. Inputs for Separating Cell Zones

To break up a cell zone based on region or cell register mark, use the Separate Cell Zones Dialog Box (Figure 6.93: The Separate Cell Zones Dialog Box).

 Domain → Zones → Separate → Cells...

Figure 6.93: The Separate Cell Zones Dialog Box

---

Important:  If you are planning to separate cell zones, you should do so before performing any adaptions using the hanging node adaption method. Cell zones that contain hanging nodes cannot be separated.

---

The steps for separating cells are as follows:

1. Select the separation method (Mark or Region) under Options.

2. Specify the cell zone to be separated in the Zones list.

3. If you are separating cells by mark, select the cell register to be used in the Registers list.

4. (optional) To check what the result of the separation will be before you actually separate the cell zone, click the Report button. The report will look like this:

    Separates zone 14 into two zones, with 1275 and 32 cells.
   

5. To separate the cell zone, click the Separate button. Ansys Fluent will print the following information:

    Separates zone 14 into two zones, with 1275 and 32 cells.
    No faces marked on thread, 2
    No faces marked on thread, 3
    No faces marked on thread, 1
    No faces marked on thread, 5
    No faces marked on thread, 7
    No faces marked on thread, 8
    No faces marked on thread, 9
    No faces marked on thread, 61
    Separates zone 62 into two zones, with 1763 and 58 faces.
    All faces marked on thread, 4
    No faces marked on thread, 66
    Moved 32 cells from cell zone 14 to zone 10
    Updating new zone information ...
       created new zone interior-4:010 from interior-4
       created new zone interior-6:009 from interior-6
       created new zone fluid-14:008 from fluid-14
    done.
   

As shown in the example above, separation of a cell zone will often result in the separation of face zones as well. When you separate by mark, faces of cells that are moved to a new zone will be placed in a new face zone. When you separate by region, faces of cells that are moved to a new zone will not necessarily be placed in a new face zone.

If you find that any faces are placed incorrectly, see the comment above, at the end of the inputs for face zone separation.

The face-fusing utility is a convenient feature that can be used to fuse boundaries (and merge duplicate nodes and faces) created by assembling multiple mesh regions. When the domain is divided into subdomains and the mesh is generated separately for each subdomain, you will combine the subdomains into a single file before reading the mesh into Fluent. For details, see Reading Multiple Mesh/Case/Data Files. This situation could arise if you generate each block of a multiblock mesh separately and save it to a separate mesh file. Another possible scenario is that you decided, during mesh generation, to save the mesh for each part of a complicated geometry as a separate part file. (Note that the mesh node locations need not be identical at the boundaries where two subdomains meet; see Non-Conformal Meshes for details.)

The Fuse Face Zones dialog box (Figure 6.94: The Fuse Face Zones Dialog Box) allows you to merge the duplicate nodes and delete these artificial internal boundaries.

 Domain → Zones → Combine → Fuse...

Figure 6.94: The Fuse Face Zones Dialog Box

The boundaries on which the duplicate nodes lie are assigned zone ID numbers (just like any other boundary) when the mesh files are combined, as described in Reading Multiple Mesh/Case/Data Files. You need to keep track of the zone ID numbers when tmerge or the meshing mode of Fluent reports its progress or, after the complete mesh is read in, display all boundary mesh zones and use the mouse-probe button to determine the zone names (see Controlling the Mouse Button Functions for information about the mouse button functions). Alternatively, you can specify a name for the fused zone.

 /mesh/modify-zones > fuse-face-zones

 ()
 Zone to fuse(1) [()]  w1.top

 Zone to fuse(2) [()]  w3

 Zone to fuse(3) [()]  [Enter]

 Choose from list (automatic w3 w1.top) or pick your own
 Enter the fused zone name: [automatic]  w3

   Name of zone 14 is changed into w3.

 Fused list of zones successfully.

Ansys Fluent allows you to assign periodicity to your mesh by coupling a pair of face zones. If the two zones are conformal (that is, have identical node and face distributions), then you can change them to be a pair of coupled zones that are both of type periodic. If the two zones are not identical at the boundaries within a specified tolerance, then you can change them both to be of type interface and include them in a non-conformal mesh interface that is periodic.

To create a periodic boundary zone pair or interface, perform the following steps:

Note that the functionality of the Create Periodic dialog box can also be accessed through the define/boundary-conditions/modify-zones/create-periodic-interface text command.

For more information about non-conformal periodic boundaries and an alternate way to create them, see Non-Conformal Meshes and Using a Non-Conformal Mesh in Ansys Fluent, respectively.

If you want to decouple the zones in a periodic pair (also referred to as "deleting" or "slitting" a periodic pair), right-click the periodic zone in the Outline View (under Setup/Boundary Conditions/Periodic), and select Delete in the menu that opens. For conformal pairings, both of the zones in the periodic pair are changed to be of type symmetry; for non-conformal pairings, the original face zones remain as type interface and the associated mesh interface and periodic zone are deleted.

The face-zone slitting feature has two uses:

When you slit a face zone, Fluent will duplicate all faces and nodes, except those nodes that are located at the ends (2D) or edges (3D) of the zone. One set of nodes and faces will belong to one of the resulting boundary zones and the other set will belong to the other zone. The only ill effect of the shared nodes at each end is that you may see some inaccuracies at those points when you graphically display solution data with a slit boundary. (Note that if you adapt the boundary after slitting, you will not be able to fuse the boundaries back together again.)

Before you can slit, you first need to select the zone in the Boundary Condition task page and change the Type to wall. Upon changing the Type to wall, another shadow zone will be created (that is, if the original zone is called rad-outlet, another zone called rad-outlet-shadow will be created). Then you can apply the mesh/modify-zones/slit-face-zone text command on either of the walls (that is, rad-outlet or rad-outlet-shadow) to separate them into two distinct walls.

For example, the outlet of the radiator in an underhood application is typically of interior type (that is, has cells on both sides). If you know the mass flow rate through this zone (either from other CFD models or from test data) and want to apply it as a boundary condition at the radiator outlet, you first need to slit the radiator outlet. To be able to slit it, select wall from the Type drop-down list in the Boundary Conditions task page for this outlet. It will create a wall and a shadow. Then you can use the TUI command (mesh/modify-zones/slit-face-zone) to slit them. After it is slit, two additional walls will be created, one facing one side of the outlet and another facing the other. Then you can select the appropriate wall and change the Type to mass-flow-inlet and specify the mass flow rate using the Mass-Flow Inlet Dialog Box. There is no option of mass-flow-inlet without first slitting it.

 /mesh/modify-zones > slit-face-zone

  Face zone id/name [] wall-4

    zone 4 deleted
    face zone 4 created
    face zone 10 created 

The faces of a boundary face zone (which have cells only on one side) are oriented such that the normals are all pointing in one direction. However, for internal face zones (which have cells on both sides), the normals are allowed to point in either direction. To orient them so that they all point in one direction, you can use the following TUI command:

mesh → modify-zones → orient-face-zone

Having all of the normals oriented in one direction is needed for some boundary condition types. For example, the fan boundary condition type determines the flow direction based on its normals. If some of the normals are pointing in one direction and some in the other, the correct flow orientation cannot be determined, which leads to incorrect results.

The ability to extrude a boundary face zone allows you to extend the solution domain without having to exit Fluent. A typical application of the extrusion capability is to extend the solution domain when recirculating flow is impinging on a flow outlet. The current extrusion capability creates prismatic or hexahedral layers based on the shape of the face and normal vectors computed by averaging the face normals to the face zone’s nodes. You can define the extrusion process by specifying a list of displacements (in SI units) or by specifying a total distance (in SI units) and parametric coordinates.

Ansys Fluent allows you to append or replace an existing cell zone in the mesh. You can also permanently delete a cell zone and all associated face zones, or temporarily deactivate and activate zones from your Ansys Fluent case.

 

6.12.9.1. Replacing Zones

This feature allows you to replace a small region of a computational domain with a new region of different mesh quality. This functionality will be required where you may want to make changes to the geometry or mesh quality for any part of the domain. This ability of Ansys Fluent will save you time, since you can modify only the required part of the domain without remeshing the whole domain every time.

The replacement mesh must be prepared in advance, with the following considerations:

• The replacement mesh must contain a single cell zone.

• The cell zone in the replacement mesh must be of the same zone type as the zone that is being replaced.

• If the boundaries of the replacement mesh will form a non-conformal interface with existing zones (that is, zones that are not replaced in the existing mesh), these boundaries should be based on the same geometry as the existing zones. If there are sharp features (for example, 90-degree angles) or curvature in the mesh, it is especially important that both sides of the interface closely follow that feature.

• The replacement cell zone does not need to have the same name as the existing zone being replaced.

• When naming the boundary zones of the replacement cell zone, note that boundary conditions will be automatically transferred from the existing cell zone based on name. All boundaries of the replacement cell zone that have unique names will be assigned the default boundary condition for that zone type.

• When selecting the file with the replacement cell zone, note that legacy mesh files (.msh) and legacy case files (.cas) may be selected, but default CFF mesh files (.msh.h5) and CFF case files (.cas.h5) may not.

Replacing a zone is performed using the Replace Cell Zone Dialog Box (Figure 6.96: The Replace Cell Zone Dialog Box).

 Domain → Zones → Replace Zone...

Figure 6.96: The Replace Cell Zone Dialog Box

To replace a zone, do the following:

1. Click Browse... and select the new or modified mesh containing the cell zone that will replace one of the cell zones in the current mesh.

   The name of the cell zone in the replacement mesh will be displayed in the Replace with list.

2. Under Existing Zones, select the zone you want to replace.

3. Under Replace with, select the zone from the replacement mesh.

4. Enable/Disable Interpolate Data, if data already exists. If the replacement cell zone is geometrically different, then Interpolate Data can be turned off to prevent data interpolation over the non-matching geometries.

   ---

   Important:  Disable Interpolate Data if the zone being replaced is part of an overset interface.

   ---

5. Click Replace to replace the selected zone.

6. Set up the boundary conditions for any of the boundaries of the replacement mesh that do not share a name with one of the existing boundaries.

 

6.12.9.2. Deleting Zones

To permanently delete zones, select them in the Delete Cell Zones Dialog Box (Figure 6.97: The Delete Cell Zones Dialog Box), and click Delete.

 Domain → Zones → Delete...

Figure 6.97: The Delete Cell Zones Dialog Box

All of the cells, faces, and nodes associated with the cell zone will be deleted. If one of the faces is of type interior and borders another cell zone, the face will automatically be changed to a wall and will stay attached to the remaining cell zone.

 

6.12.9.3. Deactivating Zones

To deactivate zones, select them in the Deactivate Cell Zones Dialog Box (Figure 6.98: The Deactivate Cell Zones Dialog Box), and click Deactivate.

 Domain → Zones → Deactivate...

Figure 6.98: The Deactivate Cell Zones Dialog Box

Deactivation will separate all relevant interior face zones (that is, fan, interior, porous-jump, or radiator) into wall and wall-shadow pairs.

---

Note:  When you deactivate a zone using the Deactivate Cell Zones dialog box, Ansys Fluent will remove the zone from the mesh and from all relevant solver loops.

---

---

Important:  If a cell zone contains mesh interfaces it cannot be deactivated until the solution has been initialized.

---

 

6.12.9.4. Activating Zones

You can reactivate the zones and recover the last data available for them using the Activate Cell Zones Dialog Box (Figure 6.99: The Activate Cell Zones Dialog Box).

 Domain → Zones → Activate...

Figure 6.99: The Activate Cell Zones Dialog Box

---

Note:  The Activate Cell Zones dialog box will only be populated with zones that were previously deactivated.

---

After reactivation, you need to make sure that the boundary conditions for the wall and wall-shadow pairs are restored correctly to what you assigned before deactivating the zones. If you plan to reactivate them at a later time, make sure that the face zones that are separated during deactivation are not modified. Adaption, however, is supported.

You can create a copy of a cell zone that is offset from the original either by a translational distance or a rotational angle. Note that in the copied zone, the bounding face zones are all converted to walls, any existing cell data is initialized to a constant value, and non-conformal interfaces and dynamic zones are not copied; otherwise, the model settings are the same as in the original zone.

To copy a zone, use the following text command:

mesh → modify-zones → copy-move-cell-zone

You will then be prompted to enter the ID of the zone you want to copy, and either the distance for translation in each of the axes or the rotational angle, origin, and axis.

Note that if you want the copied zone to be connected to existing zones, you must either fuse the boundaries (as described in Fusing Face Zones) or set up a non-conformal interface (as described in Using a Non-Conformal Mesh in Ansys Fluent).

Ansys Fluent allows you to replace your mesh, so that you can continue to run your simulation on a new mesh without having to manually copy the case file settings or interpolate the existing data. Replacing the mesh globally may be helpful, for example, if you would like to perform a mesh refinement study with a prepared series of meshes, or if your results indicate that your current mesh is not of sufficient quality. Note that the data interpolation is done automatically during the replacement if data exists (that is, you have initialized the flow field or run a calculation).

Global mesh replacement is performed by clicking Replace Mesh... in the Domain ribbon tab Zones group box), which opens the Select File dialog box (Figure 6.100: The Select File Dialog Box).

Figure 6.100: The Select File Dialog Box

In some cases you may want to identify and display the face zones which are adjacent to a cell zone. You can do this using the Adjacency dialog box.

 Domain → Zones → Adjacency...

Figure 6.101: The Adjacency Dialog Box

Using the Adjacency dialog box (Figure 6.101: The Adjacency Dialog Box) you can also optionally rename zones based on their adjacency or with default names based on zone type. The steps to use the Adjacency dialog box are:

In a Fluent session that uses multiple processes, the mesh domain is automatically reordered when it is read, in order to increase memory access efficiency. The reordering uses the Reverse Cuthill-McKee algorithm  [35], and is applied to cells and faces.

A typical output produced during the domain reordering at read is shown below:

Building...
     mesh
	auto partitioning mesh by Metis (fast),
	distributing mesh
		parts...,
		faces...,
		nodes...,
		cells...,
        bandwidth reduction using Reverse Cuthill-McKee: 3875/150 = 25.8333

The bandwidth is the maximum difference between neighboring cells in the zone—that is, if you numbered each cell in the zone list sequentially and compared the differences between these indices.

Internally, Ansys Fluent stores the computational mesh in meters, the SI unit of length. When mesh information is read, it is assumed that the mesh was generated in units of meters. If your mesh was created using a different unit of length (inches, feet, centimeters, and so on), you must scale the mesh to meters. To do this, you can select from a list of common units to convert the mesh or you can supply your own custom scale factors. Each node coordinate will be multiplied by the corresponding scale factor.

Scaling can also be used to change the physical size of the mesh. For instance, you could stretch the mesh in the direction by assigning a scale factor of 2 in the direction and 1 in the and directions. This would double the extent of the mesh in the direction. However, you should use anisotropic scaling with caution, since it will change the aspect ratios of the cells in your mesh.

 

6.12.14.1. Scaling the Entire Mesh

You will use the Scale Mesh Dialog Box (Figure 6.102: The Scale Mesh Dialog Box) to scale the entire mesh, either to change the unit of measurement or to apply custom scaling factors.

 Setup →   General → Mesh → Scale...

Figure 6.102: The Scale Mesh Dialog Box

The procedure for scaling the mesh is as follows:

1. Use the conversion factors provided by Ansys Fluent by selecting Convert Units in the Scaling group box. Then indicate the units used when creating the mesh by selecting the appropriate abbreviation for meters, centimeters, millimeters, inches, or feet from the Mesh Was Created In drop-down list. The Scaling Factors will automatically be set to the correct values (for example, 0.0254 meters/inch).

   If you created your mesh using units other than those in the Mesh Was Created In drop-down list, you can select Specify Scaling Factors and enter values for X, Y, and Z manually in the Scaling Factors group box (for example, the number of meters per yard).

2. Click the Scale button. The Domain Extents will be updated to show the correct range in meters. If you prefer to use your original unit of length during the Ansys Fluent session, you can follow the procedure described below to change the unit.

 

6.12.14.1.1. Changing the Unit of Length

As mentioned in Step 2. of the previous section, when you scale the mesh you do not change the units; you just convert the original dimensions of your mesh points from your original units to meters by multiplying each node coordinate by the specified Scaling Factors. If you want to work in your original units, instead of in meters, you can make a selection from the View Length Unit In drop-down list. This updates the Domain Extents to show the range in your original units and automatically changes the length unit in the Set Units Dialog Box (see Customizing Units). Note that this unit will be used for all future inputs of length quantities.

 

6.12.14.1.2. Unscaling the Mesh

If you use the wrong scale factor, accidentally click the Scale button twice, or want to undo the scaling for any other reason, you can click the Unscale button. “Unscaling” simply divides each of the node coordinates by the specified Scale Factors. (Selecting m in the Mesh Was Created In list and clicking on Scale will not unscale the mesh.)

 

6.12.14.1.3. Changing the Physical Size of the Mesh

You can also use the Scale Mesh Dialog Box to change the physical size of the mesh. For example, if your 2D mesh is 5 feet by 8 feet, and you want to model the same geometry with dimensions twice as big (10 feet by 16 feet), you can enter 2 for X and Y in the Scaling Factors group box and click Scale. The Domain Extents will be updated to show the new range.

You can “move” the mesh by applying prescribed offsets to the Cartesian coordinates of all the nodes in the mesh. This would be necessary for a rotating problem if the mesh were set up with the axis of rotation not passing through the origin, or for an axisymmetric problem if the mesh were set up with the axis of rotation not coinciding with the axis. It is also useful if, for example, you want to move the origin to a particular point on an object (such as the leading edge of a flat plate) to make an XY plot have the desired distances on the axis.

 

6.12.15.1. Translating the Entire Mesh

You can translate the entire mesh using the Translate Mesh Dialog Box (Figure 6.103: The Translate Mesh Dialog Box).

 Domain → Mesh → Transform → Translate...

Figure 6.103: The Translate Mesh Dialog Box

The procedure for translating the mesh is as follows:

1. Enter the desired translations in the , , and (for 3D) directions (that is, the desired delta in the axes) in the X, Y, and Z text-entry boxes in the Translation Offsets group box. You can specify positive or negative real numbers in the current unit of length.

2. Click the Translate button and redisplay the mesh. The Domain Extents will be updated to display the new extents of the translated mesh. (Note that the Domain Extents are purely informational; you cannot edit them manually.)

The ability to rotate the mesh is analogous to the ability to translate the mesh in Ansys Fluent. You can rotate the mesh about the , , or (for 3D) axis and also specify the rotation origin. This option is useful in the cases where the structural mesh and the CFD mesh are offset by a small angle.

 

6.12.16.1. Rotating the Entire Mesh

You can rotate the entire mesh using the Rotate Mesh Dialog Box (Figure 6.104: The Rotate Mesh Dialog Box).

 Domain → Mesh → Transform → Rotate...

Figure 6.104: The Rotate Mesh Dialog Box

The procedure for rotating the mesh is as follows:

1. Specify the required Rotation Angle for the mesh. You can specify any positive or negative real number in the correct unit of angle.

2. In the Rotation Origin group box, enter X, Y, and (for 3D) Z coordinates to specify a new origin for the axis of rotation.

3. In the Rotation Axis group box, enter values for the X, Y, and (for 3D) Z axes to specify the vector for the axis of rotation.

4. Click the Rotate button and redisplay the mesh.

   The Domain Extents will be updated to display the new extents of the rotated mesh. (Note that the Domain Extents are purely informational; you cannot edit them manually.)

Smoothing and face swapping are tools that complement mesh adaption by increasing the quality of the final numerical mesh. Smoothing repositions the nodes, and face swapping modifies the cell connectivity to achieve these improvements in quality.

 

6.12.17.1. Smoothing

The three smoothing methods that are available in Ansys Fluent are:

• quality-based smoothing

  This method is the only recommended method, and is available for all types of meshes in serial and parallel.

• Laplacian smoothing

  This method is not recommended, though it is available for all types of meshes in serial (and is best suited for quadrilateral and hexahedral meshes).

• skewness-based smoothing

  This method is not recommended, though it is available for triangular and tetrahedral meshes in serial; it can be used alternatively with face swapping (see Combining Skewness-Based Smoothing and Face Swapping).

 

6.12.17.1.1. Quality-Based Smoothing

Smoothing that is based on quality is performed using the Improve Mesh Dialog Box (Figure 6.105: The Improve Mesh Dialog Box).

 Domain → Mesh → Quality → Improve Mesh Quality...

Figure 6.105: The Improve Mesh Dialog Box

Ansys Fluent divides the mesh into a number of “bins”, each of which contain a certain number of cells. Improvements are attempted on the cells in those bins that exhibit the lowest orthogonal quality (as defined in Mesh Quality). As part of this method, you specify the percentage of the total number of cells, in order to determine how many bins are modified.

Note that this smoothing is similar to when you use the mesh/repair-improve/improve text command. The advantage of using the Improve Mesh dialog box rather than the text command is that you can control the percentage of the cells that Ansys Fluent attempts to improve.

To perform quality-based smoothing, do the following steps:

1. In the Improve Mesh Dialog Box (Figure 6.105: The Improve Mesh Dialog Box), enter the Percentage of Cells to be Improved.

   ---

   Important:  Quality-based smoothing will be CPU intensive if you specify a large value for the Percentage of Cells to be Improved. It is recommended that you enter a small value initially, and then perform the smoothing process multiple times, if necessary. Note that the maximum percentage allowed is 10%.

   ---

2. Specify the number of successive smoothing sweeps to be performed on the mesh in the Number of Iterations number-entry box. The default value is 4.

3. Click the Improve button.

 

6.12.17.1.2. Laplacian Smoothing

When you use this method, a Laplacian smoothing operator is applied to the unstructured mesh to reposition nodes. The new node position is the average of the positions of its node neighbors. The computed node position increment is multiplied by the relaxation factor (which is set to a value between 0.0 and 1.0). A value of zero for the relaxation factor results in no movement of the node, and a value of unity results in movement equivalent to the entire computed increment. Figure 6.106: Result of Smoothing Operator on Node Position illustrates the new node position for a typical configuration of quadrilateral cells. The dashed line is the original mesh and the solid line is the final mesh.

Figure 6.106: Result of Smoothing Operator on Node Position

This repositioning strategy improves the skewness of the mesh, but relaxes the clustering of node points. In extreme circumstances, the present operator may create mesh lines that cross over the boundary, creating negative cell volumes. This is most likely to occur near sharp or coarsely resolved convex corners, especially if you perform multiple smoothing operations with a large relaxation factor. Figure 6.107: Initial Mesh Before Smoothing Operation illustrates an initial tetrahedral mesh before one unrelaxed smoothing iteration creates mesh lines that cross over each other (Figure 6.108: Mesh Smoothing Causing Mesh-Line Crossing).

Figure 6.107: Initial Mesh Before Smoothing Operation

Figure 6.108: Mesh Smoothing Causing Mesh-Line Crossing

The default smoothing parameters are designed to improve mesh quality with minimal adverse effects, but it is recommended that you save a case file before smoothing the mesh. If you apply a conservative relaxation factor and start with a good quality initial mesh, the frequency of failure due to smoothing is extremely low in two dimensions. However, corruption of the mesh topology occurs much more frequently in three dimensions, particularly with tetrahedral meshes.

The smoothing operator can also be applied repeatedly, but as the number of smoothing sweeps increase, the node points have a tendency to pull away from boundaries and the mesh tends to lose any clustering characteristics.

To perform Laplacian smoothing, enter the mesh/smooth-mesh text command in the console and respond to the prompts as follows:

1. Enter "laplace" for the type of smoothing.

2. Specify the number of successive smoothing sweeps to be performed on the mesh in response to the number of iterations prompt. The default value is 4.

3. Specify the factor by which to multiply the computed position increment for the node in response to the relaxation factor prompt. The lower the factor, the more reduction in node movement.

 

6.12.17.1.3. Skewness-Based Smoothing

When you use skewness-based smoothing, Ansys Fluent applies a smoothing operator to the mesh, repositioning interior nodes to lower the maximum skewness of the mesh. Ansys Fluent will try to move interior nodes to improve the skewness of cells with skewness greater than the specified “skewness threshold”. This process can be very time consuming, so perform smoothing only on cells with high skewness.

Improved results can be obtained by smoothing the nodes several times. There are internal checks that will prevent a node from being moved if moving it causes the maximum skewness to increase, but it is common for the skewness of some cells to increase when a cell with a higher skewness is being improved. Thus, you may see the average skewness increase while the maximum skewness is decreasing.

---

Important:  Carefully consider whether the improvements to the mesh due to a decrease in the maximum skewness are worth the potential increase in the average skewness. Performing smoothing only on cells with very high skewness (for example, 0.8 or 0.9) may reduce the adverse effects on the average skewness.

---

To perform skewness-based smoothing, enter the mesh/smooth-mesh text command in the console and respond to the prompts as follows:

1. Enter "skewness" for the type of smoothing.

2. Specify the number of successive smoothing sweeps to be performed on the mesh in response to the number of iterations prompt. The default value is 4.

3. Specify the minimum cell skewness value for which node smoothing will be attempted in response to the skewness threshold prompt. Ansys Fluent will try to move interior nodes to improve the skewness of cells with skewness greater than this value. By default, skewness threshold is set to 0.4 for 2D cases and 0.8 for 3D cases.

 

6.12.17.2. Face Swapping

While it is not recommended over smoothing (and support for it may be removed in future releases), face swapping can be used to improve the quality of a triangular or tetrahedral mesh in the serial version of Ansys Fluent.

To perform face swapping, enter the mesh/swap-mesh-faces text command repeatedly until the console report declares that 0 faces were swapped out. The console report will display the total number of faces that were visited and tested for possible face swapping.

 

6.12.17.2.1. Triangular Meshes

The approach for triangular meshes is to use the Delaunay circle test to decide if a face shared by two triangular cells should be swapped. A pair of cells sharing a face satisfies the circle test if the circumcircle of one cell does not contain the unshared node of the second cell. Figure 6.109: Examples of Cell Configurations in the Circle Test illustrates cell neighbors in the circle test. In cases where the circle test is not satisfied, the diagonal or face is swapped, as illustrated in Figure 6.110: Swapped Faces to Satisfy the Delaunay Circle Test.

Figure 6.109: Examples of Cell Configurations in the Circle Test

Figure 6.110: Swapped Faces to Satisfy the Delaunay Circle Test

Repeated application of the face-swapping technique will produce a constrained Delaunay mesh. If you have a Delaunay mesh, it is a unique triangulation that maximizes the minimum angles in the mesh. Thus, the triangulation tends toward equilateral cells, providing the most equilateral mesh for the given node distribution. For more information on Delaunay mesh generation, see Generating Tetrahedral Meshes in the Fluent Meshing section of the User’s Guide.

 

6.12.17.2.2. Tetrahedral Meshes

For tetrahedral meshes, face swapping consists of searching for configurations of three cells sharing an edge and converting them into two cells sharing a face to decrease skewness and the cell count (see Figure 6.111: 3D Face Swapping).

Figure 6.111: 3D Face Swapping

After performing mesh operations, the boundary layer zone may not satisfy the original growth rate. When the boundary layer is composed of hex and/or wedge cells, you can restore the desired growth rate by using the mesh/redistribute-boundary-layer text command. You will be prompted to enter a face zone and the desired growth rate. The face zone you specify must be adjacent to the boundary layer zone that you want to redistribute.

>  mesh redistribute-boundary-layer
face zone id/name [] wall-fluid
growth rate [1.1] 1.2

Fluent will redistribute the nodes in a boundary region that extends into the mesh from the face zone you specify until one of the following criteria is encountered:

You can delete cells that are marked by a specified cell register. After the cells are deleted, one boundary zone of type symmetry is created for each cell zone at the faces that the deleted cells shared with their neighboring cells.

To delete cells marked by a cell register, perform the following steps: