Engineering Solutions

CFD Tetramesh panel

CFD Tetramesh panel

 Previous topic Next topic Expand/collapse all hidden text  

CFD Tetramesh panel

 Previous topic Next topic JavaScript is required for expanding text JavaScript is required for the print function  

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.  

 

Panel Usage

Separate subpanels exist for Boundary selection, Boundary Layer (BL) parameters, Tetramesh parameters, 2D parameters, and Refinement boxes.

new_cfd_tetramesh_panel

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.    

 

Subpanels and Inputs

The CFD Tetramesh panel contains the following subpanels and command buttons:

expand-green-10Boundary selection

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

The panel layout changes depending on your choice of boundary layer options, which are determined by a toggle in the bottom-left corner of the panel labeled Smooth BL, Smooth/Truncate BL or Native BL. Altair Engineering strongly recommends using the Smooth/Truncate BL method, which is robust and produces a better quality of elements. Smooth/Truncate BL has the capability to both compress (squeeze) and/or truncate (chop off/remove) BL based on the given parameters. It allows for more control to BL to deal with complex CFD problems. However, the Native BL method is provided primarily for legacy purposes. The Smooth BL method produces a smooth orthogonal boundary layer.            

Panel inputs

Input

Action

Advanced/Simple Selection

The Advanced selection and Simple selection options are available to ease the selection of boundary regions.  

•Advanced selection: All options for boundary selection are exposed yielding a maximum on control/flexibility.
•Simple selection: Only With BL (fixed) and W/o BL (float) are exposed, so 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).

Smooth BL / Smooth/Truncate BL/ Native BL
•Smooth BL produces a smooth orthogonal boundary layer and better element quality.
•Smooth/Truncate BL has the capacity to both compress (squeeze) and/or truncate (chop off/remove) BL based on the given parameters.
•Native BL method is provided primarily for legacy purposes.

With BL (fixed/float):

This 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)

This selects 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

The Remesh/Morph options are available when Smooth BL is selected.

 

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 Morph toggle keeps the topology of the base surface mesh intact. These regions are morphed if they are in contact with boundary layer regions, as illustrated in the figure below for an inlet and symmetry plane. The upper figure shows the starting surface mesh - the symmetry plane is blue, and the inlet area is dark yellow. The middle figure 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 lower figure shows the resulting mesh when the Remesh option being used. In both lower images the boundary layer elements are in violet, and the inner core tetrahedral elements are in brown.

remesh_1

Starting Surface Mesh

remesh_4

standard_arrow_beforeafter

remesh_2

remesh_5

standard_arrow_beforeafter

remesh_3

swap only/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.

fix comp borders

Anchor nodes are maintained 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.

If the float option is chosen for some boundary regions, Engineering Solutions is allowed to swap surface shell edges during mesh generation. However, this prevents the swapping of edges between two components.

tetramesh_fix_comp_boundaries

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.

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: All volumes are considered as fluid volume.
•Touched volumes are fluid: An element can be selected. 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: An element can be selected. The normal vector of the selected element points into the fluid domain.

Anchor nodes

Anchor nodes are maintained 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.

comps 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.

If the comp per volume check box is activated then several components will be generated.

 

Simple Selection Example

Below is an example for simple selection. Select all the components (outer wall, inflow/outflow and interface) as With BL (fixed) and inflow/outflow as W/o BL (float).

simple_boundary_selection_example

simple_boundary_selection_example2

 

Advanced Selection 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): This 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): This 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.

 

 

Check 2D Mesh

The check 2D mesh utility can be used to validate the input surface mesh before performing volume mesh generation. The input shell mesh, forming the closed volume, needs to be selected via the four boundary selectors.

Clicking check 2D mesh opens the Boundary Mesh Checker dialog.

boundary_mesh_checker_dialog

Two checks are available:

•Intersection tol.  An intersection check for the selected shell elements forming one volume is performed. The check will detect a penetration (for example two elements cutting each other) as well as an "almost" penetration (for example one node is very close to an element). To detect the latter situation, an intersection tolerance can be specified. The actual search tolerance is relative to the local minimum edge length and is defined by search tol. = (intersection tol) * (local min. edge length). The failed elements are duplicated and are placed in the component ^error_elems.

intersection_check

 

almost_intersection_check

This image shows penetration, where two or more elements are cutting each other.

 

This image shows an "almost" intersection, where one mesh node is coming very close to the shell elements. The node and shell elements belong to the same volume.

•Dihedral angle.  The selected input mesh will be checked for adjacent elements which form a sharp angle, for example a needle pocket. The threshold angle is user defined. The failed elements are duplicated and are placed in the component ^error_elems.

needle_pocket

This image shows a needle pocket. The involved elements form a sharp pocket pointing outwards of the volume.

•Per vol check.  Finds the intersections that are only within the shell volumes. Intersections across volumes and open shells will not be found. If this check box is disabled, intersections will be checked for all of the input elements/components even if the input shells do not form closed volume.

Along with intersecting and diehedral elements, all duplicate elements and close proximity elements within the user defined tolerance will also be found. All of the failed elements will be placed into a separate component for review.

o^err_x_elems.  Contains intersecting elements.
o^err_agl_elems.  Contains failed dihedral angle check elements.
o^err_prx_elems.  Contains close proximity elements within the user defined tolerance.
o^minus_prx_elems.  Contains close proximity elements for a per volume check which has opposite orientation. These elements are safe for volume meshing.
o^minus_agl_elems.  Contains dihedral angle check elements for a per volume check which has opposite orientation. These elements are safe for volume meshing.
o^err_dup_elems.  Contains duplicate elements.

 

Solid and Fluid Domains

There is also an option to 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.

cfd_solid_fluid_example

There are three ways to select the fluid volume:

•All are fluid: All volumes are considered as fluid volume.
•Touched volumes are fluid: An element can be selected. 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: An element can be selected. The normal vector of the selected element points into the fluid domain.

 

Meshing Multiple Volumes

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.

If the comp per volume check box (shown below) is activated then several components will be generated.

comp_per_volume_option

seperate_components_example
expand-green-10BL parameters

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.

Panel inputs

Input

Action

BL thickness: Number of Layers

Specifies the total number of layers to be generated using the specified first layer thickness and growth rate.

This option is only available when Smooth BL is selected.

BL thickness: Total Thickness

Specify the BL thickness, but not the number of layers.

This option is only available when Smooth BL is selected.

BL thickness: Ratio of Total Thickness/Elem Size

Ratio between the total boundary layer thickness and the average element size of the base surface elements.

This option is only available when Smooth BL is selected.

Exponential Boundary Layer / Structured Isotropic Layers

Choose between Exponential Boundary Layer and Structured Isotropic Layers.

This option only appears if Native BL is selected.

Simple settings

Will grow BL until it matches final layer height/base surface size ratio. The number of layers to grow are decided based on the inputs.  

This option only appears if 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. 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.)

user_controlled_example

This option only appears if Smooth/Truncate BL is selected.

First layer thickness

Indicate the thickness of the first layer. If you are unsure what thickness to use, access the First cell height calculator to calculate it.

BL growth rate

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, d*r, d*r*(r*a), d*r*(r*a)^2, and so on.

This option only appears if Native BL is selected and Exponential Boundary Layer is chosen.

BL hexa transition mode: Simple Pyramid

Uses 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.

This option is only available when Smooth BL is selected.

BL hexa transition mode: Smooth Pyramid

Generates 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.

This option is only available when Smooth BL is selected.

BL hexa transition mode: All Prism

If there are any 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.

This option is only available when Smooth BL is selected.

BL hexa transition mode: All Tetra

Generates tetra elements only in the boundary layer and will split the quad elements of the surface mesh into tria elements.

This option is only available when Smooth BL is selected.

Export settings

Saves the settings to a file.

Create prism elements

If left unchecked, the mesher will create tetra elements rather than triangular prisms.

Displays only when Native BL is selected.

BL only

This option generates 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, that if these collectors do, 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

Displays when Smooth BL is selected.

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 checkbox: This is a one step approach. The proximity check for the BL is performed 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 checkbox: This is a two step approach. In the first step, the BL scaling factors are defined 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 step one.
•Parameters button opens the Dynamic BL thickness reduction dialog.
•Manual button opens the Distributed BL thickness ratio dialog to define the BL thickness scaling factors manually.
•Auto button opens the Generate boundary layer distributed thickness values dialog to define the BL thickness scaling factors automatically.

1st cell height calc

Calculates the first cell height via the First cell height dialog.

Advanced settings

This button is available when Smooth BL and Smooth/Truncate BL are selected, however the options in the Advanced BL parameters dialog differ depending on your choice of boundary layer options. See below for more information.                      

Clicking Advanced settings opens the Advanced BL parameters dialog, enabling access to BL gen speed vs quality, Sharp edges handling, BL propagation controls, Proximity controls and Quality controls. Parameters in advanced settings provide more power to you to control BL in special cases, such as sharp corners and close proximity elements.

sharp_corner

sharp corner

 

close_proximity

close proximity

advanced_bl_parameters_dialog_smooth_truncate

The functionality BL gen speed vs quality contains three options, controlling the growth of the boundary layers.

•Quality focused: A set of meshing parameters is used, which ensures 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: You can define the relevant parameters individually. When User defined is selected, three additional options are exposed in the dialog: Interpolated layers, Residual threshold and Maximum smoothing iterations.

For the generation of boundary layers (BL), three parameters are used to control the quality and the required meshing time.

•Interpolated layers:
-This option defines 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.

interpolated_layers_example

•Residual threshold:
-This option defines 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.
•Maximum smoothing iterations:

-   This option defines the maximum number of smoothing steps allowed to improve the element quality in the boundary layer.

advanced_bl_parameters_dialog_2

The functionality Sharp edges handling contains the Node collapse angle option for the BL generation at a baffle's free edge and sharp corners pointing into the volume.      

•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.

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.

Use Node collapse to 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.

node_example

This enhancement enables the growth of boundary layers, even on very complex geometry.

Baffles

baffles_with_node_collapse_option

This image shows a baffle (in yellow) with the Node collapse option selected.

The BL is collapsed along the free edge of the baffle.

 

Sharp edge

cfd_sharp_edge_node_collapse

The image above shows a sharp edge (in yellow) with

the Node collapse option selected. Only one normal

is generated at the sharp edge to generate the BL.

propogation_controls

BL propagation controls: Controls how to propogate BL in special cases.    

•Min imprint angle from BL to non-BL: (recommended range is 6-10). This parameter controls 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.
•Max layer diff between neighbor elems: (recommended range depends on how many layers you are growing). This parameter controls 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.  

max_layer_diff

Proximity controls: Special treatment for close proximity area.

•Max BL compression: (recommended range is 0-0.6). 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.
•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.
•Min tetcore/base size ratio: The default value is 1.3, which is the recommended value. 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.

Quality controls: Controls the quality of boundary layers. If the quality of the BL will not meet any of the two criterion, the layer will be trimmed.

•Max cell skeweness: (recommended range is 0.8-0.95). With this parameter you can 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.    
•Min normalized Jacobian: (recommended range is 0.05-0.2). Any BL cells exceeding the min normalized Jacobian will be chopped off. This parameter avoids generating negative elements.

Clicking Advanced settings opens the Advanced BL parameters dialog, enabling access to BL gen speed vs quality and Sharp edges handling. Parameters in advanced settings provide more power to you to control BL in special cases, such as sharp corners and close proximity elements.

sharp_corner

sharp corner

 

close_proximity

close proximity

advanced_bl_parameters_dialog

The functionality BL gen speed vs quality contains three options, controlling the growth of the boundary layers.

•Quality focused: A set of meshing parameters is used, which ensures 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: You can define the relevant parameters individually. When User defined is selected, three additional options are exposed in the dialog: Interpolated layers, Residual threshold and Maximum smoothing iterations.

For the generation of boundary layers (BL), three parameters are used to control the quality and the required meshing time.

•Interpolated layers:
-This option defines 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.

interpolated_layers_example

•Residual threshold:
-This option defines 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.
•Maximum smoothing iterations:

-   This option defines the maximum number of smoothing steps allowed to improve the element quality in the boundary layer.

The functionality Sharp edges handling contains the Node collapse and Multiple normals options.

advanced_bl_parameters_dialog_sharp_edges

•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.

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.

Use Node collapse to 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.

node_example

This enhancement enables the growth of boundary layers, even on very complex geometry.

Baffles

baffles_with_node_collapse_option

This image shows a baffle (in yellow) with the Node collapse option selected.

The BL is collapsed along the free edge of the baffle.

 

Sharp edge

cfd_sharp_edge_node_collapse

The image above shows a sharp edge (in yellow) with

the Node collapse option selected. Only one normal

is generated at the sharp edge to generate the BL.

•Multiple normals allows you to 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.
expand-green-10Tetramesh parameters

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.

Panel inputs

Input

Action

Max tetra size

Tetra elements will not exceed this measurement in any dimension.

Optimize Mesh Quality

Directs 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

Applies in most cases, and uses the standard tetra-meshing algorithm as in previous versions of Engineering Solutions. This option is available in each tetramesh subpanel.

Optimize Mesh Speed

Uses an algorithm for faster meshing. Use this option if element quality considerations are less important than mesh generation time. This option is available in each tetramesh subpanel.

Standard / Aggressive / Gradual /Interpolate / User Controlled/ Octree based

Affects 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 is 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 is 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 is a very fast tetra mesher, and due to the logic behind this scheme, it provides a very nice BL transition.

Uniform Layers

This factor specifies 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 for the following growth options:

•Standard:  2.0
•Aggressive:  0.5
•Gradual:  2.5
•Interpolate:  -1.0
•User Controlled: You can define your own value when you select this option.
•Octree based:  2

Growth rate

The Growth rate parameter works thusly: if d is the initial thickness and r is the initial growth rate, then the thicknesses of the successive layers are d, d*r, d*r^2, d*r^3, d*r^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 for the following growth options:

•Standard:  1.2
•Aggressive:  1.35        
•Gradual:  1.08        
•Interpolate:  1.08
•User Controlled: You can define your own value when you select this option.
•Octree based:  1.2

Pyramid transition ratio

Defines 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

To apply an extra stage of calculation to improve overall mesh quality, select the smoothing check box. 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

Select this check box to specify the number of tetrahedral layers to generate.

When this check box is selected, 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.
•Engineering Solutions will not create layer meshes near the narrow strip surfaces, as the current algorithm does not alter the surface mesh given.

fill voids

If your geometry includes volumes inside of another volume, select the fill voids check box. All volumes will be meshed.

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

You can select an element criteria and a threshold. After the tetrameshing step, Engineering Solutions will perform a mesh optimization step to fulfill the defined threshold for the selected element criteria.

expand-green-102D parameters

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.

Panel inputs

Input

Action

Select 2D element type

You can pick between quads, trias, mixed (quads and trias), and R-trias (right-angle trias).

Use curvature

This option creates finer mesh in areas of high surface curvature.

Use proximity

Refines the mesh in areas where the features are small and closer together.

Element size

The target size for 2D elements.

Cleanup elements

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

Export settings

Save the settings to a file.
expand-green-10Refinement box

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

Panel inputs

Input

Action

Define refinement box: By Center and Sizes

Use the selector to pick the center node, and then use the sx, sy, and sz numeric boxes 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.

Define refinement box: By Four Nodes

Use the selectors to pick 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.

Define refinement box: By Two Nodes

Use the selectors to pick nodes which represent opposite corners of a cubic volume.

Define refinement box: By Elems Box:

Use the elems selector to pick elements that define the volume, such as by means of a <shift+L-click> dragged frame.

Define refinement box: Update Refinement

Use this option to select an existing refinement box, change its Refinement size, and remesh the refinement volume.

Scaling factor

Display when the Define refinement box option is set to By Elems Box. determines 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.

Refinement size

This is 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.

In the example below, the boundary region has been selected as With BL (float) and remesh, therefore the region included in the refinement box has been remeshed with the elements size assigned to the refinement box.

remeshed_surface_example

remeshed_surface_example2

freehand edit

Opens the morphing Freehand panel, from which you can alter the shape and dimensions of the refinement box to better suit your mesh.
expand-green-10Command Buttons

The following action buttons appear throughout the subpanels:

Button

Action

mesh

Generate the CFD mesh.

reject

Undo the creation of the mesh, discarding all related elements.

mesh to file

Reverts any changes and returns to the main Card Editor panel.  All changes made while editing are discarded.

check2Dmesh

Validate the input surface mesh before performing volume mesh generation.      

Manual

Open the Distributed BL Thickness Ratio dialog.

Auto

Open the Generate Boundary Layer Distributed Thickness Values dialog.

return

Applies all changes and closes the panel.