CFD Tetramesh Panel

Use the CFD Tetramesh panel to generate hybrid grids, containing hexa/penta/tetra elements in the boundary layer and tetra elements in the core or fare field.

Location: 3D page

Buttons to mesh, reject a mesh, mesh to file, or check 2D mesh exist on all subpanels except for the Refinement box, meaning you have access to the meshing functionality from almost each subpanel. You can mesh from one of the parameter panels, and if the mesh results are not satisfactory, you can reject the mesh, change some parameters and regenerate the mesh without leaving the subpanel.

Boundary Selection Subpanel

Use the Boundary selection subpanel to select the elements/components that define the surface area on which you need to generate boundary layers.


Option	Action
Advanced select / Simple select	Choose a method for selecting boundary regions. Advanced select All options for boundary selection are exposed yielding a maximum on control/flexibility. Example: Use the With BL (fixed/float) and W/o BL (fixed/float) options to select your elements, components or solids. Selecting the fixed option for either choice means the base 2D mesh will not be modified in any way. The float option, which can be swap only or remesh, dictates that the edges of the base 2D mesh may be swapped or may be remeshed in order to produce better quality 3D tetra elements. With BL (fixed/float) Selects tria/quad elements that define the surface area on which you need to generate boundary layers. If a refinement box includes boundary shells selected via the With BL (float) selector and the remesh option is used, the surface elements are remeshed using the element size assigned to the refinement box. W/o BL (fixed/float) Selects tria/quad elements that define the boundary regions where a boundary layer is not desired. The Remesh toggle means that the defined elements will be remeshed after being deformed by the boundary layer growth from adjacent surface areas. The Morph toggle means the shell elements of this region will be morphed to make room for the newly generated boundary layer elements. Quad elements will be split into trias. The option W/o BL (fixed) can be used, for example, if two adjacent volumes are meshed sequentially and a matching interface has to be ensured. In that case the common interface elements have to be selected as W/o BL (fixed). fix comp borders If the float option is chosen for some boundary regions HyperMesh is allowed to swap surface shell edges during mesh generation. If this option is checked, the edges between two components are not swapped. update input shells The shells on all boundaries will be updated automatically after the meshing step. The updated shell elements will be placed in the initial boundary shell components. Simple select Only With BL (fixed) and W/o BL (float) are exposed, therefore your input is reduced to a minimum. If the fluid domain consists of multiple volumes and interface shells between two adjacent volumes, the interface shells do not have to be selected separately. They are automatically treated as W/o BL (float). Example: Select all the components (outer wall, inflow/outflow and interface) as With BL (fixed) and inflow/outflow as W/o BL (float). Figure 1. Figure 2.
Smooth BL / Smooth/Truncate BL / Native BL	Smooth BL Produce a smooth orthogonal boundary layer and better element quality. Smooth/Truncate BL Compress (squeeze) and/or truncate (chop off/remove) BL based on the given parameters. With this method you have more control to generate BL to deal with complex CFD problems. Tip: It is recommended that you use this method. Native BL Provided primarily for legacy purposes.
With BL (fixed/float)	Select tria/quad elements that define the surface area on which you need to generate boundary layers. If a refinement box includes boundary shells selected via the With BL (float) selector and the remesh option is used, the surface elements are remeshed using the element size assigned to the refinement box.
W/o BL (fixed / float)	Select tria/quad elements that define the boundary regions where a boundary layer is not desired. The option W/o BL (fixed) can be used, for example, if two adjacent volumes are meshed sequentially and a matching interface has to be ensured. In that case the common interface elements have to be selected as W/o BL (fixed).
Remesh/Morph	Remesh Remesh defined elements after being deformed by the boundary layer growth from adjacent surface areas. Morph Morph the shell elements of this region to make room for the newly generated boundary layer elements. Quad elements will be split into trias. Morph keeps the topology of the base surface mesh intact. These regions are morphed if they are in contact with boundary layer regions. Figure 3 shows the starting surface mesh for an inlet and symmetry plane. Figure 3. Starting Surface Mesh. The symmetry plane is blue, and the inlet area is dark yellow. The Figure 4 shows the result when Morph is selected. The quad elements are morphed and split to connect them to the tetra elements in the core. The boundary layer elements are in violet, and the inner core tetrahedral elements are in brown. Figure 4. Resulting Mesh, Morph Selected The Figure 5 shows the resulting mesh when Remesh is selected. The boundary layer elements are in violet, and the inner core tetrahedral elements are in brown. Figure 5. Resulting Mesh, Remesh Selected Note: Available when Smooth BL is selected.
swap only / remesh	Choose a method for managing the edges of the base 2D mesh in order to produce better quality 3D tetra elements. swap only Edges of the base 2D mesh may be swapped. remesh Edges of the base 2D mesh may be remeshed.
fix comp borders	Maintain anchor nodes during CFD tetrameshing, so that the new mesh must adhere to them. You can also select 1D elements instead of nodes if you need a tetra element edge at a certain location. Tip: Use this option when certain mesh nodes or edges are required on a certain location, such as for post-processing purposes. If the float option is chosen for some boundary regions, HyperMesh is allowed to swap surface shell edges during mesh generation. However, this prevents the swapping of edges between two components. Figure 6. Example: Fix Comp Borders
update input shells	Automatically update the shells on all boundaries after the meshing step. The updated shell elements will be placed in the initial boundary shell components.
fluid volumes selection	Specify fluid and solid volumes if multiple volumes exist. The boundary layer will be grown only in the fluid volumes, whereas the solid volumes are filled with a pure tetra mesh without boundary layers. The use case is electronic cooling, where you have several electronic components (solids) and usually one large fluid domain. All volumes are fluid Consider all volumes as fluid volume. Touched volumes are fluid Select an element. All volumes touching this particular element are considered as fluid domain. Boundary layers will be grown on all fluid domains defined as With BL. No boundary layer will be grown on the solid side of the boundaries, even if they are defined as With BL. Normals point into fluid Select an element. The normal vector of the selected element points into the fluid domain. Figure 7. Solid (no BL) Figure 8. Fluid (with BL) Figure 9. BL Only in Fluid Domain
anchor nodes	Maintain anchor nodes during CFD tetrameshing, so that the new mesh must adhere to them. You can also select 1D elements instead of nodes if you need a tetra element edge at a certain location. Use this option when certain mesh nodes or edges are required on a certain location, such as for post-processing purposes.
comp per volume	Meshing multiple volumes with CFD Tetramesh will create two components for each volume, one for the boundary layer elements and one for the core (tetra) elements. For pure tetra meshing only one component per volume will be generated. Enable this checkbox to generate several components. Figure 10. Example: Comp Per Volume

BL Parameters Subpanel

Use the BL parameters subpanel to specify the general boundary layer behavior. These settings affect how other CFD subpanels generate mesh when meshing with boundary layers.

Table 1. Panel Options
Option	Action
BL thickness: Number of Layers	Specify the total number of layers to be generated using the specified first layer thickness and growth rate. Note: Available when Smooth BL is selected.
BL thickness: Total Thickness	Specify the BL thickness, but not the number of layers. Note: Available when Smooth BL is selected.
BL thickness: Ratio of Total Thickness/Elem Size	Specify the ratio between the total boundary layer thickness and the average element size of the base surface elements. Note: Available when Smooth BL is selected.
Exponential Boundary Layer / Structured Isotropic Layers	Choose between Exponential Boundary Layer and Structured Isotropic Layers. Note: Available when Native BL is selected.
Simple settings	Grow BL until it matches final layer height/base surface size ratio. The number of layers to grow are decided based on the inputs. Note: Available when Smooth/Truncate BL is selected.
User controlled	Define settings for two BL groups. The purpose of the first BL group is to define BL with a smaller growth rate to better physics capturing. The second group enables a smooth transition between BL layers and the tet core. User controlled enables BL to grow with a higher growth rate until the final layer height is X * the base size/tetra layer size. (X is the Final layer h/base ratio that you define.) Note: Available when Smooth/Truncate BL is selected. Figure 11. Example: User Controlled. The first arrow indicates the second BL group, where the number of layers = 4 and the growth rate = 1.5. The second arrow indicates the first BL group, where the number of layers = 8 and the growth rate is 1.1.
First layer thickness	Specify the thickness of the first layer. This utility helps you estimate the proper first cell height (first layer thickness) for the boundary layer generation, based on the flow characteristics and fluid properties. You can open this dialog by clicking on the 1st cell height calc icon on the BL Parameters subpanel. The entry fields on this dialog are actually settings for the Calculate first layer thickness button. Once you supply the required data, clicking this button causes the dialog to automatically calculate and suggest an appropriate thickness. Bulk velocity (meters/sec): an average flow velocity. Length scale (meters): A characteristic length of your model, for example in case of a tube, it can be the diameter of the tube. Kinematic viscosity (meters^2/sec): the viscosity of the fluid. y+ value: the y+ value required by the turbulence model. Calculation Schemes: Choose the scheme most appropriate to your problem. Once all of these qualities are specified, clicking Calculate first layer thickness produces a suggested thickness. You can either Accept this value, in which case the window closes and the value is automatically placed into the First layer thickness field of the CFD Tetramesh panel, or you can click Close to close the window without accepting the suggested value.
BL growth rate	Specify the non-dimensional factor that controls the change in layer thickness from one layer to the next.
Acceleration	A growth acceleration for boundary layers beyond the first few layers; in effect, this acts as a growth rate on the growth rate, but only after the first few initial boundary layers. By default, the first two boundary layers grow by the growth rate as described above. However, subsequent layers grow by the growth rate multiplied by the acceleration factor. Thus, if d is the initial thickness, r is the initial growth rate, and a is the acceleration rate, then the thicknesses of the successive layers are d, dr, dr(ra), dr(r*a)^2, and so on. Note: Available when Native BL is selected and Exponential Boundary Layer is chosen.
BL hexa transition mode: Simple Pyramid	Use one pyramid element to transition from a BL hexahedral’s quad face to the tetrahedral core mesh. The height of these pyramids is controlled by simple transition ratio parameter, which represents the ratio between the transition pyramid height and the characteristic size of the base quad. Note: Available when Smooth BL is selected.
BL hexa transition mode: Smooth Pyramid	Generate a transition layer composed of pyramid and tetrahedral elements. The thickness of this layer is controlled by the parameter smooth transition ratio, which represents the ratio between the transition layer thickness and the characteristic size of the base quads. Note: Available when Smooth BL is selected.
BL hexa transition mode: All Prism	If there are quad elements in the surface mesh, those will be split into two trias each so that there is no need to transition from quad faces to tria faces when transitioning from the last boundary layer to the tetrahedral core. This option is very important when there are quad elements on areas with (low) distributed BL thickness ratio, because in such areas the thickness of the transition elements (for example simple pyramid) was not taken into account when doing the interference study to assign distributed BL thickness ratio to those elements. Note: Available when Smooth BL is selected.
BL hexa transition mode: All Tetra	Generate tetra elements only in the boundary layer, and split the quad elements of the surface mesh into tria elements. Note: Available when Smooth BL is selected.
Export settings	Save the settings to a file.
Create prism elements	Clear this checkbox to create tetra elements rather than triangular prisms during meshing. Note: Available when Native BL is selected.
BL only	Generate only the boundary layer, stopping before generating the tetrahedral core. It also modifies adjacent surface meshes to reflect changes introduced by the boundary layer thickness, and creates a collector named ^CFD_trias_for_tetramesh that is typically used to generate the inner core tetrahedral mesh using the Tetramesh parameters subpanel. Boundary layer elements are placed in a collector named CFD_boundary_layer and the core tetrahedral elements in another collector named CFD_Tetramesh_core. Both collectors are automatically created if they do not exist. However, if these collectors do exist, it might make sense to empty them before meshing; otherwise there will be more than one set of elements occupying the same physical volume. If you mesh the volume in several steps (multi-volume meshing), then you might not want to empty the collector before generating the mesh for the next adjacent volume.
BL reduction	Define the parameters for scaling the boundary layer thicknesses to avoid narrow or closed channels. Several BL reduction mechanisms are available, and can be combined with each other. Dynamic Perform the proximity check for the BL, while the layers are generated and the BL thickness is adjusted accordingly. The advantage of this method is that no estimated BL is used, and therefore a more accurate BL thickness reduction can be performed. Pre calc In the first step, define the BL scaling factors before the BL is actually grown. These factors describe how much the total BL thickness is reduced at a particular location. For example, a value of 0.5 will reduce the BL thickness to one half of its initial thickness. The scaling factors are stored in a load collector called CFD_BL_Thickness. Using the Auto option, the BL scaling factors are computed automatically based on an estimated boundary layer. Using the Manual option, you can define the scaling factors on components or individual nodes. In the second step, the BL is generated considering the BL scaling factors from the first step. Parameters Open the Dynamic BL thickness reduction dialog via the green parameters button on the BL Parameters subpanel when you select Smooth BL from the toggle in the bottom-left corner of the panel. The Minimum (Tetrahedral-Core/Boundary Layer) thickness ratio value is the minimum ratio between the thickness of the tetrahedral core and the boundary layer. This value must be more than zero, but decimal values are accepted. The higher this value, the more the boundary layer elements will be compressed to keep the core open. The Bound Layer thickness at corners adjusts the total thickness of boundary layers in corners to avoid elements getting distorted or interfering with other boundary layer elements because of the default hyperbolic growth of the boundary layer. The smaller this value is, the smaller the thickness of the boundary layer at corners will be relative to the nominal total boundary layer thickness. The image below shows the effects on the same model using values of 1 and 5. Manual Open the Distributed BL thickness ratio dialog by clicking Manual in the CFD Tetramesh panel, BL parameters subpanel when Smooth BL is selected from the toggle in the bottom-left corner of the panel. This dialog enables you to manually specify distributed thickness ratios for groups of nodes or whole components. This approach is useful when you need to reduce or increase the BL thickness throughout a component, or at a clearly identified group of nodes. Use the Select Nodes or Select Components button to select nodes or components on which you would like to alter the BL thickness, and then select the desired entities. Thickness Ratio value - the ratio between the local boundary layer thickness for the selected nodes/components, and the global value specified in the CFD Tetramesh panel, for example a ratio of 0.5 will reduce the BL thickness to one half of its initial thickness. At any time you can review the assigned thickness ratio values by clicking Contours of BL Thickness Ratio. This opens the Contour panel with a contour plot of the ratio values. Auto Open the Generate boundary layer distributed thickness values dialog via the green Auto button on the BL parameters subpanel when you select Smooth BL from the toggle in the bottom-left corner of the panel. This utility identifies narrow regions in the model and scales the total boundary layer thickness according to your input. If you already selected components on the Boundary selection subpanel, those components display automatically in this utility with the appropriate Bound Type. Otherwise, you can click the Add collectors with surface elements button and then pick the desired parts of the model. When selecting components this way, you will need to also specify the Bound Type for each component. Each component also has a Remove button to remove it from the list (the component itself is not deleted from the model, only removed from this dialog). Finally, you can clear all components by clicking the Remove all the above added collectors button. The Number of Layers, First layer thickness, and Layers’ thickness growth rate are automatically populated with the values from the CFD Tetramesh panel. The Minimum (Tetrahedral-Core/Boundary Layer) thickness ratio value is the minimum ratio between the thickness of the tetrahedral core and the boundary layer. This value must be more than zero, but decimal values are accepted. The higher this value, the more the boundary layer elements will be compressed to keep the core open. Figure 12. The Bound Layer thickness at corners adjusts the total thickness of boundary layers in corners to avoid elements getting distorted or interfering with other boundary layer elements because of the default hyperbolic growth of the boundary layer. The smaller this value is, the smaller the thickness of the boundary layer at corners will be relative to the nominal total boundary layer thickness. The image below shows the effects on the same model using values of 1 and 5. Figure 13. The Check for closed volume checkbox causes the utility to run a check to make sure that the selected elements form enclosed volumes without any holes. Enclosed volumes simplify meshing because the direction of boundary layer growth is always inward. However, in some cases where a volume is not enclosed, the mesher creates boundary layers based on the elements' normal direction. If the normal faces the wrong way, the boundary layers might accidentally extend in the wrong direction; when this occurs, you can uncheck this option, and then click the Adjust Element Normals button to switch the normals of the elements that generated boundary layers in the wrong direction. Finally the Generate Distributed BL Thickness Ratio button creates the distributed boundary layers, placing their thickness values in the load collector ^CFD_BL_Thickness. If you wish to display contours of the Boundary Layers' Thickness Ratio, click the Display Contours of BL Thickness Ratio button. Figure 14. When finished generating the distributed boundary layers, click Close to close the dialog and return to the BL parameters subpanel.
1st cell height	Calculate the first cell height via the First cell height dialog. This utility helps you estimate the proper first cell height (first layer thickness) for the boundary layer generation, based on the flow characteristics and fluid properties. You can open this dialog by clicking on the 1st cell height calc icon on the BL Parameters subpanel. The entry fields on this dialog are actually settings for the Calculate first layer thickness button. Once you supply the required data, clicking this button causes the dialog to automatically calculate and suggest an appropriate thickness. Bulk velocity (meters/sec): an average flow velocity. Length scale (meters): A characteristic length of your model, for example in case of a tube, it can be the diameter of the tube. Kinematic viscosity (meters^2/sec): the viscosity of the fluid. y+ value: the y+ value required by the turbulence model. Calculation Schemes: Choose the scheme most appropriate to your problem. Once all of these qualities are specified, clicking Calculate first layer thickness produces a suggested thickness. You can either Accept this value, in which case the window closes and the value is automatically placed into the First layer thickness field of the CFD Tetramesh panel, or you can click Close to close the window without accepting the suggested value.
Advanced settings	Open the Advanced BL parameters dialog, and define advanced parameters to control the BL. Note: Available when Smooth BL or Smooth/Truncate BL is selected.

Clicking Advanced settings opens the Advanced BL parameters dialog. Use these parameters to control the BL, such as sharp corners and close proximity elements.

Note: Available when Smooth BL or Smooth/Truncate BL is selected.

Table 2. Advanced BL Parameters
Option	Action
BL gen speed vs quality	Select a method for controlling the growth of the boundary layer. Quality focused Use a set of meshing parameters to ensure a good quality boundary layer in most cases. Meshing speed focused The meshing parameters are chosen in a way that the meshing time is minimized and an acceptable boundary layer quality is achieved in most situations. User defined Define the relevant parameters individually.
Interpolated layers (available when User Defined is selected)	Define the number of layers that are generated by interpolation. For example, for a value of three, one "thick" layer will be generated and the smoothing step to improve the element quality will be performed. Then, the "thick" layer will be split into three layers, and the spacing is defined by the BL growth rate. In general a large number of interpolated layers will decrease the meshing time but might also decrease the element quality. Figure 17. One "Thick" Layer + Smoothing Figure 18. "Thick" Layer is Divided Note: Available when BL gen speed vs quality is set to User defined.
Residual threshold (available when User Defined is selected)	Define the stopping criteria (upper bound) for the smoothing step during BL generation. For each new layer, smoothing steps are applied to improve the element quality and the overall BL quality. The smoothing step is an iterative process and the smoothing residual is a measurement for the quality of boundary layer, meaning the smaller the residual the better the BL quality. In general, a small residual threshold ensures good quality of the boundary layer but might require more CPU time (under the assumption that the value for maximum smoothing iterations is set large enough). A relatively large residual threshold will usually decrease the CPU time and also decrease the element quality. Note: Available when BL gen speed vs quality is set to User defined.
Maximum smoothing iterations (available when User Defined is selected)	Define the maximum number of smoothing steps allowed to improve the element quality in the boundary layer. Note: Available when BL gen speed vs quality is set to User defined.
Sharp edges handling	Node collapse For some surface mesh nodes it is mathematically impossible to compute a normal offset direction for growing the boundary layers. Those nodes are called unoffsetable nodes and require the BL to collapse. Figure 19. Unoffsetable Node For complex geometry, some surface mesh nodes are often close to being an unoffsetable node, causing problems during BL generation since the computation of the normal offset direction is not straight forward. Specify a threshold for boundary layer collapse. For each node, a node angle can be computed, which is a function of the normals of the attached elements. If the node angle is below the threshold, the boundary layer will collapse. For an unoffsetable node, the node angle is zero or negative. Figure 20. Threshold for Boundary Layer Collapse This enhancement enables the growth of boundary layers, even on very complex geometry. Figure 21. Baffles. This example shows a baffle (yellow) with the Node collapse option enabled. The BL is collapsed along the free edge of the baffle. Figure 22. Sharp Edges. This example shows a sharp edge (yellow) with the Node collapse option enabled. Only one normal is generated at the sharp edge to generate the BL. Multiple normals Specify a threshold angle to control the normal computation on a sharp edge pointing into the volume, or on the free edge of a baffle. If two adjacent elements enclose an angle smaller than the threshold (meaning a sharp edge pointing into the volume), two normals are computed on that edge and the boundary layer will consider the two normals. Otherwise, only one normal is considered. For baffles (zero thickness walls), the option will use two normals at the free edge to generate the boundary layer. Note: Available when Smooth BL is selected.
Min imprint angle from BL to non-BL	Control which cases you want to imprint BL on without BL components. If the angle between the BL component and the non BL component is really high imprinting will create high aspect ratio elements. If the angle between BL and No-BL entities (component elements) is less than the imprint angle or greater than (180-imprint angle) it will collapse the BL, rather than imprint on non-BL entities. Important: Recommended range is 6-10. Note: Available when Smooth/Truncate BL is selected.
Max layer diff between neighbor elems	Control the maximum layer difference between neighboring elements. This helps to avoid a situation where all BLs collapse at once. This parameter also provides smooth BL transition in case of BL truncation. One fourth of the total BL layers is a good number for this parameter. It also depends on layer height. Important: Recommended range depends on how many layers you are growing. Figure 23. Max Layer Diff Between Neighbor Elems = 2. Two layers are collapsed at a time when required. Note: Available when Smooth/Truncate BL is selected.
Max BL compression	When there is not enough space available for BL to grow, this parameter enables BL compression, or squeezing. Entering a value of zero enforces no BL compression, which is useful if you want to maintain BL height. Entering a value of one enables the maximum possible compression. First, the BL will try to compress by the max BL compression factor. For example, if the original total BL height is defined as 1, with 0.4 max BL compression, it will try to squeeze the BL layers until 0.6 of the total height. After compressing BL until this value, if there is not enough space the mesher will start chopping off layers. Important: Recommended range is 0-0.6. Note: Available when Smooth/Truncate BL is selected.
Min BL thickness/base size ratio	By default this value is zero, which disables the effects of this parameter. Sometimes due to close proximity the BL will only be able to generate one to two layers (very small total BL height at that location). It might be possible that at that location the transition between BL layers and tet core is very bad. With this factor, if the total BL height is less than the defined factor base size, it will chop off all of the BL layers. Note: Available when Smooth/Truncate BL is selected.
Min tetcore/final layer height ratio	After creating BL in close proximity, there will be a small space available for tetramesh. This results in high aspect ratio tet elements. This parameter controls the minimum height of tet core as a factor of the final layer height. Important: The default value is 1.3, which is the recommended value. Note: Available when Smooth/Truncate BL is selected.
Max cell skewness	Avoid creating highly skewed elements. The tetra mesher sometimes creates better quality elements compared to the BL mesher. It is best to define a higher value if your input 2D mesh has bad element quality and topology. Any BL cells exceeding the max cell skewness will be chopped off. Important: Recommended range is 0.8-0.95. Note: Available when Smooth/Truncate BL is selected.
Min normalized Jacobian	Any BL cells exceeding the min normalized Jacobian will be chopped off. This parameter avoids generating negative elements. Important: Recommended range is 0.05-0.2. Note: Available when Smooth/Truncate BL is selected.

Tetramesh Parameters Subpanel

Use the Tetramesh Parameters subpanel to set default tetrameshing behavior, such as target element size or meshing algorithm, which will then influence how the mesh is generated on the other subpanels.


Option	Action
Max tetra size	Specify a size that tetra elements will not exceed in any dimension.
Optimize Mesh Quality / TetraMesh Normally / Optimize Mesh Speed	Optimize Mesh Quality Direct the tetramesher to spend more time optimizing element quality. It employs the volumetric ratio, or CFD skew measurement for tetras as a quality measure. Use this option if your solver is sensitive to element quality. TetraMesh Normally Use the standard tetra-meshing algorithm if possible. Optimize Mesh Speed Use an algorithm for faster meshing. Use this option if element quality considerations are less important than mesh generation time.
Growth options	Standard Recommended for most cases. Aggressive Generates fewer tetrahedral elements than Standard because it uses a larger growth rate. Gradual Generates more elements because the growth rate is lower than with the Standard option. Interpolate Useful when the core mesh size should be interpolated from the surface mesh size. User Controlled Control the number of Uniform layers (see below in this table) grown from the surface mesh and the Growth rate (see below in this table), which acts as an accumulative size multiplier on each layer of elements beyond the uniform layers. Octree based A very fast tetra mesher, that provides a nice BL transition. Delaunay Implemented based on the delaunay approach. This method is recommended for improved performance.
Uniform layers	Select how far the constant tetra size should be maintained from the surface mesh during tetrameshing. The distance is internally calculated by multiplying the user defined factor by the local surface mesh size.HyperMesh specifies different default value of this parameter. Standard 2.0 Aggressive 0.5 Gradual 2.5 Interpolate -1.0 User Controlled Define your own values. Octree based -1.0 Delaunay -1.0
Growth rate	If d is the initial thickness and r is the initial growth rate, then the thicknesses of the successive layers are d, dr, dr^2, dr^3, dr^4, and so on. If element quality is very important and you are not concerned with the total number of elements created, then Interpolate will produce the best results because the element size changes smoothly and therefore the element quality is better. HyperMesh specifies different default value of this parameter. Standard 1.2 Aggressive 1.35 Gradual 1.08 Interpolate 1.08 User Controlled Define your own values. Octree based -1.0 Delaunay 1.3
Pyramid transition ratio	Specify the relative height of pyramid elements used for the transition from hexa elements in the boundary layer to the tetra elements in the core.
Export settings	Save the settings to a file.
Refinement box	Specify the refinement boxes which should be considered during volume meshing. Refinement boxes not selected will be ignored.
smoothing	Apply an extra stage of calculation to improve overall mesh quality. Additional smoothing and swapping steps will be performed and tetra elements will be split to achieve a smoother mesh transition. If tetra elements are used in the boundary layer those elements will be excluded from smoothing to maintain the original distribution.
Number of layers	Specify the number of tetrahedral layers to generate. The Tetramesher ensures the tetracore contains, at minimum, the specified number of tetra layers in the model. This functionality ensures a certain mesh resolution in case of close proximity or thin channels. When generating multiple tetrahedral layers, keep the following restrictions in mind: Do not generate more than three or four layers, unless you refine the surfaces to have a fine mesh at close proximity areas. HyperMesh will not create layer meshes near the narrow strip surfaces, as the current algorithm does not alter the surface mesh given.
fill voids	Mesh all volumes, if your geometry includes volumes inside of another volume. For example if you had a sphere inside of a larger sphere, checking this option would cause the volume of the inner sphere as well as the volume between the two spheres to be meshed.
Fix Midnodes	In case of 2nd order tetras, this option fixes the mid edge node of surface mesh while volume meshing
Elem quality target	Select an element criteria and a threshold. After the tetrameshing step, HyperMesh performs a mesh optimization step to fulfill the defined threshold for the selected element criteria.
Min Tetra Height	Generate tetramesh with a minimum height above the value defined. The tetramesh algorithm will try to enforce the user-defined minimum height.

2D Parameters Subpanel

If solids are used as input for CFD tetrameshing, use the 2D Parameters subpanel to set the default traits of the 2D meshes that are generated on the surfaces of the components that you wish to tetramesh. This 2D mesh is then used as the basis from which the internal tetras are generated.


Option	Action
Select 2D element type	Select a type of 2D elements.
Use curvature	Create finer mesh in areas of high surface curvature.
Use proximity	Refine the mesh in areas where the features are small and closer together.
Element size	Specify the target size for 2D elements.
Cleanup elements	Apply an extra stage of calculation to improve overall mesh quality by removing some nodes and combining elements.
Export settings	Save the settings to a file.

Refinement Box Subpanel

Use the Refinement Box subpanel to create localized mesh refinement within a user-specified box-shaped volume.


Option	Action
Define refinem	By Center & Sizes Select the center node, then use the sx, sy, and sz fields to specify the size/width of each side of the box in the x, y, and z dimensions. For instance, a size of 5 creates a 5x5x5 box centered around the center node. By Four Nodes Select a base node and three additional nodes. These four total nodes cannot be coplanar. The base node, N1, and N2 form a triangle, which is then flipped 180 degrees to form a rectangular base for the refinement box. The vector from the base node to N3 defines the box's height and direction from this base. By Two Nodes Select nodes which represent opposite corners of a cubic volume. By Elems Box Select elements that define the volume. Update Refinement Select an existing refinement box, change its refinement size, and remesh the refinement volume.
Scaling factor	Specify the box size relative to the selected elements. A scale factor of 1 creates the smallest box that can still enclose the selected elements, while a factor of 2 creates a box twice as large in every dimension. Note: Available when Define refinement box is set to By Elems Box.
Refinement size	Specify the target element size for mesh inside of the refinement box. Note: The actual mesh size will vary in order to maintain mesh connectivity at the edges of the box. Figure 24. Boundary Region Selected as With BL (flat) and Remesh Figure 25. Remeshed Surface. The region included in the refinement box has been remeshed with the elements size assigned to the refinement box.
freehand edit	Open the morphing Freehand panel, from which you can alter the shape and dimensions of the refinement box to better suit your mesh.

Command Buttons


Button	Action
mesh	Generate the CFD mesh.
reject	Undo the creation of the mesh, discarding all related elements.
mesh to file	Store the generated mesh in a .nas or .hmx file after meshing is finished. When enabled, specify a location to export the mesh.
check 2D mesh	Validate the input surface mesh before performing volume mesh generation using the Boundary Shell Checker tool.
manual	Manual Open the Distributed BL thickness ratio dialog by clicking Manual in the CFD Tetramesh panel, BL parameters subpanel when Smooth BL is selected from the toggle in the bottom-left corner of the panel. This dialog enables you to manually specify distributed thickness ratios for groups of nodes or whole components. This approach is useful when you need to reduce or increase the BL thickness throughout a component, or at a clearly identified group of nodes. Use the Select Nodes or Select Components button to select nodes or components on which you would like to alter the BL thickness, and then select the desired entities. Thickness Ratio value - the ratio between the local boundary layer thickness for the selected nodes/components, and the global value specified in the CFD Tetramesh panel, for example a ratio of 0.5 will reduce the BL thickness to one half of its initial thickness. At any time you can review the assigned thickness ratio values by clicking Contours of BL Thickness Ratio. This opens the Contour panel with a contour plot of the ratio values.
auto	Auto Open the Generate boundary layer distributed thickness values dialog via the green Auto button on the BL parameters subpanel when you select Smooth BL from the toggle in the bottom-left corner of the panel. This utility identifies narrow regions in the model and scales the total boundary layer thickness according to your input. If you already selected components on the Boundary selection subpanel, those components display automatically in this utility with the appropriate Bound Type. Otherwise, you can click the Add collectors with surface elements button and then pick the desired parts of the model. When selecting components this way, you will need to also specify the Bound Type for each component. Each component also has a Remove button to remove it from the list (the component itself is not deleted from the model, only removed from this dialog). Finally, you can clear all components by clicking the Remove all the above added collectors button. The Number of Layers, First layer thickness, and Layers’ thickness growth rate are automatically populated with the values from the CFD Tetramesh panel. The Minimum (Tetrahedral-Core/Boundary Layer) thickness ratio value is the minimum ratio between the thickness of the tetrahedral core and the boundary layer. This value must be more than zero, but decimal values are accepted. The higher this value, the more the boundary layer elements will be compressed to keep the core open. Figure 26. The Bound Layer thickness at corners adjusts the total thickness of boundary layers in corners to avoid elements getting distorted or interfering with other boundary layer elements because of the default hyperbolic growth of the boundary layer. The smaller this value is, the smaller the thickness of the boundary layer at corners will be relative to the nominal total boundary layer thickness. The image below shows the effects on the same model using values of 1 and 5. Figure 27. The Check for closed volume checkbox causes the utility to run a check to make sure that the selected elements form enclosed volumes without any holes. Enclosed volumes simplify meshing because the direction of boundary layer growth is always inward. However, in some cases where a volume is not enclosed, the mesher creates boundary layers based on the elements' normal direction. If the normal faces the wrong way, the boundary layers might accidentally extend in the wrong direction; when this occurs, you can uncheck this option, and then click the Adjust Element Normals button to switch the normals of the elements that generated boundary layers in the wrong direction. Finally the Generate Distributed BL Thickness Ratio button creates the distributed boundary layers, placing their thickness values in the load collector ^CFD_BL_Thickness. If you wish to display contours of the Boundary Layers' Thickness Ratio, click the Display Contours of BL Thickness Ratio button. Figure 28. When finished generating the distributed boundary layers, click Close to close the dialog and return to the BL parameters subpanel.
fix 3D elements	Fix 3D elements in the following ways using the Solid Mesh Optimization tool. Fix hexa and tetra element quality with respect to several element criteria. Fix second order element's maximum angle, and minimum and maximum length ratio and Jacobian.
return	Apply all changes and close the panel.