Tetramesh Panel

Location: 3D page

A region is considered enclosed if it is entirely bounded by a shell mesh (tria and/or quad elements). Other element configurations generated in this panel are hexahedral, wedge, and pyramids. These elements are typically generated when you need boundary layer type meshes on certain areas of the volume surface.

Tetra Mesh Subpanel

Use the Tetra Mesh subpanel to fill an arbitrary volume, defined by its surface using tria/quad elements, with tetrahedral elements.

Tetra Remesh Subpanel

Use the Tetra Remesh subpanel to regenerate the mesh for a single volume of tetrahedral elements.

The Free boundary faces option affects those faces of tetra elements which are on the outside of the volume, meaning the tetra faces which have only one tetra attached. Those faces are called free boundary faces.

fixed: Fix the free boundary faces.
swappable: Swapp the edges of the free boundary faces. The mesh nodes stay unchanged.
remeshable: Remesh the free boundary faces.

Figure 1. Fixed	Figure 2. Remeshable

Volume Tetra Subpanel

Use the Volume Tetra subpanel to generate a shell mesh and fill the enclosed volume with solid elements.

Given a solid entity or a set of surfaces representing a closed volume, this meshing option generates a shell mesh and fills the enclosed volume with solid elements. You can choose to create a shell mesh (2D) using quads, trias, or mixed elements and a solid mesh (3D) using tetrahedral elements only or mixed (tetras and penta) elements. In addition, you can use proximity meshing, which refines the mesh in areas where the features are small and closer together.

Figure 3. Without Proximity	Figure 4. With Proximity

You can also use surface curvature as a function of element density. This option creates a finer mesh in areas of high surface curvature.

Figure 5. With Proximity	Figure 6. With Proximity and Curvature

When you select quads or mixed as your 2D element type, HyperMesh creates quad elements and splits them diagonally into two trias during tetra face creation. This can create tetra elements whose triangular faces are right triangles (90-45-45 angles) instead of equilateral triangles (60-60-60 angles).

Figure 7. Triangular 2D Elements	Figure 8. Quad or Mixed 2D Elements

Note: Sometimes the meshing may fail to correctly interpolate from the surface mesh; when this occurs, the shell elements are cleaned up according to the same settings used in the Quick TetraMesh macro on the Utility menu, and a second attempt is made. This means that some of the features in a model may be smoothed over.

Element order can be defined as first or second. Existing elements will be used if the order of the elements are the same as the defined tetramesh element order. Meshing will fail if the shell elements of solids are present and are conflicting with the selection.

If you want to apply an extra stage of calculation to improve the overall mesh quality by removing some nodes and combining elements, select the Cleanup elements checkbox.

Tetramesh Parameters Subpanel

Use the Tetramesh Parameters subpanel to set general qualities of the tetrameshing engine, such as a maximum element size, growth rate, the balance between speed and element quality, or whether to perform smoothing operations after initial meshing.

Note: In all cases, the meshing engine uses a minimum Jacobian element quality check value of 0.05; this can result in some nodes being moved, especially when remeshing, in order to maintain a minimum level of element quality. When this occurs a message displays in the status bar informing you of how many mid-nodes were adjusted and saved.

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.
Standard / Aggressive / Gradual /Interpolate / User Controlled/ Octree based / Delaunay	Select a method for defining the growth rate of elements beyond the initial uniform layers (boundary layers). These growth options control the tradeoff between the number of elements generated and the element quality. 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 grown from the surface mesh and the Growth rate (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, Octree based, Delaunay Define your own values.
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.
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.

Refinement Box Subpanel

Use the Refinement Box subpanel to define a specific box-shaped volume within an existing tetramesh in which to generate finer mesh.

You can specify some elements to be fixed, and others to be floatable. A fixed tria-quad element is one that must be exactly represented as a face of a tetra/penta-pyramid/hexa element in the final mesh. A floatable element is one whose nodes locations are used, but the exact connectivity of those nodes can be modified if it produces a better mesh. Unless you need a special mesh type (for example surface layers of pentas/hexas), you should select as fixed only those elements that must match a pre-existing mesh, leaving the rest floatable. If the bounding surface contains quad elements, and if these quad elements are defined as fixed elements, then a first layer of elements is generated on the boundary, and pyramid elements are generated from the quad faces. However, when quad elements are defined as float elements, they are split into two trias, and the tetra meshing proceeds normally.

You can also specify various growth options in order to control the tradeoff between the number of tetras generated and their quality. Higher, more aggressive growth rates produce fewer elements, but they may be of poorer quality.

The Tetramesh panel allows you to choose from three different mesh generation priorities. The generate mesh normally option applies in most cases, but if your solver is particularly sensitive to element quality, use the optimize element quality option. This directs the tetramesher to spend more time trying to generate better quality elements. In particular, it employs the volumetric ratio (CFD "skew") measurement for rating potential tetras. For some applications, element quality considerations are less important than mesh generation time. In those cases, choose the optimize meshing speed option.

Option	Action
Define refinement	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 9. Boundary Region Selected as With BL (flat) and Remesh Figure 10. 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.

Tetramesh Panel Functions Subpanel

Use the Tetramesh Panel Functions subpanel to create a solid model of tetrahedral elements from an enclosed volume with a tria surface mesh.

Option	Action
float trias/quads	Match the node locations of the volume elements with those of the surface mesh, but the connectivity may be modified to produce a better mesh. Normally, this results in some tetra faces going across tria diagonals. Base quad surface elements are split into two trias
fixed trias/quads	Match the node locations of the volume elements with those of the surface mesh. It guarantees the connectivity of the tetras with the trias. Use this option whenever you need to match other components to the resulting volume mesh, or when you need to generate layers composed of pentas/hexas.
fix comp boundaries	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 11.
update input shells	Automatically update the shells on boundaries without boundary layers after the meshing step, and organize the updated shell elements in the initial boundary shell components.
Quad transition mode: split quads / smooth pyramid / simple pyramid	Select how the mesher creates a transition from quadrilateral surface elements to internal tetrahedral elements. Split quads Split the quads into trias, thus making them one face of a tetra element. Smooth pyramid Create a boundary layer of pyramidal prism elements, and then tetrameshe the interior normally. Simple pyramid Create pyramid elements from the quads, and then tetrameshe in accordance with each pyramid's triangular sides. Due to its simplicity, this option tends to produce a jagged tetramesh.
fixed with boundary layer	Select tria/quad elements that define the surface from which boundary layer elements are generated. Note: Available in the CFD mesh subpanel.
float w/o boundary layer	Select tria/quad elements on surfaces that do not require boundary layer elements (for example far-field, inlet, outlet, symmetry planes). Note: Available in the CFD mesh subpanel.
Total BL thickness / ratio of total thickness to element size / number of layers	Choose a method for dfining the thickness of the boundary layer(s). Total BL thickness Specify the BL thickness, but not the number of layers. Ratio of total thickness to element size Specify the ratio between the total boundary layer thickness and the average element size of the base surface elements. Number of layers Specify the total number of layers to be generated using the specified first layer thickness and growth rate. first layer thickness Thickness of first layer of elements generated from the base surface mesh. growth rate Boundary layer elements thickness growth rate. acceleration Growth acceleration for boundary layers (CFD mesh subpanel's native BL option only) Note: 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,... Note: Available in the CFD mesh subpanel.
structured isotropic prisms	Use the local element size for the initial thickness and a value of 1.0 for the growth rate and acceleration. You can use structured isotropic prism layers in any situation where ordered layers of tetras are required near the surface. The mesher uses as many layers of isotropic elements as possible until the elements in the next layer are of unacceptable quality, and then it switches to the normal meshing algorithm. Note: Available in the CFD mesh subpanel's native BL option.
exponential boundary layer	Use the first layer thickness, growth rate, and acceleration parameters to generate boundary layers up to a point where the thickness is of the same order as the base surface element, and then generate the remaining core with tetrahedral elements. Note: Available in the CFD mesh subpanel's native BL option.
tetra mesh normally / optimize meshing speed / optimize meshing quality	Choose a meshing optimization method. Tetra mesh normally Use the standard tetra-meshing algorithm. Optimize meshing speed Use an algorithm for faster meshing. Use this option if element quality considerations are less important than mesh generation time. Optimize meshing quality Direct the tetramesher to spend more time trying to generate high quality elements. It employs the volumetric ratio or CFD skew measurement as a quality measure. Use this option if your solver is sensitive to element quality.
Growth options	Select a growth option to control the tradeoff between the number of elements generated and the element quality. 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 grown from the surface mesh and the Growth rate (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 Note: Available when the growth method is set to user controlled.
initial layers	Specify a boundary region of d times the local surface element size where tetras should be of constant size. This value can be interpreted as the number of initial layers of tetrahedral elements generated without size correction by growth rate. Note: Available when the growth method is set to user controlled.

Command Buttons

Button	Action
mesh	Generate the 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.
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.