3D Tetrahedral Mesh dialog box

Mesh Name
Mesh Name	Lets you specify a name for the mesh.
Objects to Mesh
Select Objects	Lets you select the bodies (volumes) to mesh or existing meshes to remesh. You can also select a selection recipe that contains the geometry or meshes that you want to mesh.
Element Properties
Type	Specifies the type of 3D element to create, such as linear or parabolic tetrahedral elements. The types of elements available depend upon the solver you selected when you created the FEM file.To specify an alternative formulation of an Abaqus element, such as a hybrid, click Edit Mesh Associated Data and select the appropriate Element Formulation.
Mesh Associated Data	Available when you select an element type that requires the definition of additional properties.Opens the Mesh Associated Data dialog box where you can define solver-specific properties for the elements. The software applies these properties uniformly to all the elements in the mesh.
Mesh Parameters
Element Size	Regulates the edge length of a tetrahedral element over the whole solid. Use Element Size to specify the size of the elements if no local element sizes have been defined for any of the edges or faces on the solid. See Setting element size for more information.To specify the element size as a function of frequency, click the DesignLogic list and select Function to use the SizeForAcoustics function. For more information, see Element size for acoustic analysis.
Automatic Element Size	Examines the selected geometry and calculates an estimated element size. The Overall Element Size field updates to show this element size.Note: The element size calculated by Automatic Element Size is an estimate based upon certain characteristics of the currently selected geometry. You should always carefully evaluate your model and use good engineering judgment when determining the element size, regardless of whether you accept the software’s estimate or specify a different size. This evaluation should consider both the unique features of your model's geometry and the requirements of your analysis.See Understanding the Automatic Element Size calculation.
Surface Maximum Growth Rate	For the triangular 2D mesh on the surface of the volume, limits the growth of element size in the interior of a surface. This option controls the maximum amount of element edge length growth from one edge to the next. For example, if you specify a Maximum Growth Rate of 1.3, the edge length growth between adjacent element edges cannot increase more than 30%.
Surface Meshing Method	Controls the method that the software uses to generate the mesh on the surface of the volume. Select Standard when you want more control over how the software generates the mesh. This option is best when the underlying CAD geometry was defined in Modeling, for example.Select Mesh from Facets to give the software more control over the mesh generation process. This option is best when you are working with a model that contains faceted or convergent geometry that may be too complex to mesh with other commands.For more information on these methods, see 3D tetrahedral meshing.
Mesh Quality OptionsAvailable if Surface Meshing Method is set to Standard.
Midnode Method	For parabolic elements, specifies how their midnodes are projected onto geometry.MixedThe midnodes on an element are projected to the geometry unless this causes the element's Jacobian value to exceed specified the Jacobian threshold.CurvedAll midnodes are projected to the geometry regardless of the resulting element quality.LinearAll midnodes are positioned in a straight line between the two corner nodes.For more information, see Midnode placement for parabolic elements.
Geometry Tolerance	Available when Midnode Method is set to Mixed.Lets you specify the maximum linear distance that the software is allowed to move a node off the polygon geometry.
Jacobian	Sets the maximum acceptable Jacobian value for an element. When the threshold value for Jacobian is exceeded for any given element and Midnodes is set to Mixed, the element's midnodes are not projected to geometry.
Surface Mesh SettingsOptions available if Surface Meshing Method is set to Standard.
Attempt Free Mapped Meshing	Controls whether the software attempts to create a mapped-like mesh within the context of a free mesh. These types of meshes are known as “free mapped” meshes. See Understanding free mapped meshes for more information.
Attempt Multi-Block Cylinders	For cylindrical faces, uses the multi-block meshing approach to produce a more regular mesh around the circumference of cylinders.Note: This option only applies to cylinders with a linear axis.See Multi-block decomposition in meshing.
Transition with Pyramid Elements	Appears only if your model meets the criteria necessary for creating pyramid elements.If you are working in the Nastran, ANSYS, Thermal/Flow, Electronic Systems Cooling, Space Systems Thermal, or Samcef solver environment, creates pyramid elements to transition between a tetrahedral mesh and an adjacent hexahedral mesh. See Pyramid element transitions for more information.Note: When you have a Boundary Layer mesh control assigned to the selected body, the software can generate transitional pyramid elements between the boundary layer region and the tetrahedral mesh even if the Transition with Pyramid Elements check box is cleared.
Surface Mesh SettingsOptions available if Surface Meshing Method is set to Meshing from Facets.
Minimum Element Size (% Target Element Size)	Controls the length of the smallest element in the model.
Minimum Element Size	Displays the length of the shortest element edge in the model based on the Target Element Size and the setting of the Minimum Element Size (% Target Element Size) slider.
Level of Discretization Based on Curvature	Specifies the amount that the software can vary the length of elements in regions of high curvature.
Distance Based Size Variation	Controls the availability of additional options that you can use to vary the density of the elements in the mesh based on the curvature of the facet geometry.
Maximum Distance to Geometry	Available if the Distance Based Size Variation check box is selected.Specifies the maximum deviation allowed from the facet geometry and the resulting mesh. This option primarily affects the appearance of the resulting mesh in regions of curvature.Note: The software create elements in the new 2D mesh that are than the facets in the input geometry.
Maximum Level of Discretization Based on Curvature	Available if the Enable Distance Based Size Variation check box is selected.Specifies the upper limit on the amount that the software can vary the length of elements in regions of high curvature.
Surface Proximity Based Size Variation	Controls whether the software refines the mesh based on the proximity between surfaces. If you select this check box, the software varies the refinement of the 2D mesh as follows to facilitate the creation of 3D tetrahedral elements in the gaps between the surfaces:The software refines the mesh (decreases the element size) more in areas where the distance between the surfaces is smaller.The software refines the mesh less in areas where the distance between the surfaces is greater.For more information, see Surface and edge proximity settings with 2D Mesh from Facets.
Search Direction	Controls the direction that the software searches relative to the surface normal direction for proximate surfaces.Select Forward to search forward from the surface normal.Select Backward to search backwards from the surface normal.Note: In general, you should select the Backward option when you are meshing a manifold solid body.
Number of 3D Elements Between Surfaces	Specifies the target number of 3D elements to create in gaps between two surfaces. In general, the software creates 3D element that have the same element edge length as the elements in the 2D surface mesh. In some cases, as you increase this value, the software may decrease the size of the elements in the 2D surface mesh. In other cases, the software may create fewer elements than you request. For example, if you specify a value of 3, and the software can fill the gap with 2 elements, then the software creates 2 elements only.
Edge Proximity Based Size Variation	Controls whether the software refines the mesh based on the proximity between edges within a surface. If you select this check box, the software varies the refinement of the 2D mesh as follows to facilitate the creation of 2D elements in the gaps between the edges:The software increases the mesh refinement (decreases the element size) in areas where the distance between the edges is smaller.The software decreases the mesh refinement in areas where the distance between the surfaces is greater.
Number of 2D Elements Between Edges	Specifies the target number of 2D elements to create in gaps between two edges. In general, as you increase this value, the software may decrease the size of the elements in the 2D surface mesh that are closest to the gap. In some cases, the software may create fewer elements than you request. For example, if you specify a value of 3, and the software can fill the gap with 2 elements, then the software creates 2 elements only.
Volume Mesh Settings
Internal Mesh Gradation	Specifies the value that the software uses as a multiplier for increasing the length of one internal element edge to the next internal edge. Use this option to control the how the length of tetrahedral elements increases in the interior of the mesh.Moving the slider towards the minimum setting specifies that tetrahedral elements should remain approximately constant in size throughout the body.Moving the slider towards the maximum setting specifies that the size of tetrahedral elements should increase towards the center of the body.Note: If you do not want the size of the elements to change, specify a value of 0 in the Internal Mesh Gradation box.
Target Internal Edge Length Limit	Use the Target Internal Edge Length Limit option to specify a desired upper or lower limit for the length of element edges in the interior of the volume. If you specify a value that is larger than the overall Element Size, then this option sets the maximum size of elements inside the volume.If you specify a value that is smaller than the overall Element Size, then this option sets the minimum size of elements inside the volume.
Minimum Two Elements Through Thickness	Controls whether the software produces a minimum of two elements through the thickness of very thin regions.See Creating at least two elements through the thickness of tetrahedral meshes for more information.
Auto Fix Failed Elements	Select Auto Fix Failed Elements to have the software automatically reduce the element size by 10% if it detects element quality issues during meshing.See Understanding the Auto Fix Failed Elements process and Understanding 3D tetrahedral mesh quality evaluation for more information.
Model Cleanup Options
Small Feature Tolerance	Specifies the percentage of the element size to use to characterize small features. The software uses the small feature tolerance to determine which features to eliminate during the abstraction process that precedes meshing.Use this option to define a small feature as a percentage of the total element size between zero and 20%. If you specify zero, the software attempts to mesh all features and does not perform any abstraction.The default value is 10.0%. For example, if the element size is 10 mm, the software ignores features such as holes or faces that are 1 mm or less in size.For more information, see Understanding the geometry abstraction process.
Boundary Layer Options
Appears only when you have at least one Boundary Layer mesh control assigned to the selected body. For more information on options in this group, see Boundary Layer Options group.
Destination Collector
Automatic Creation	Select Automatic Creation to have the software automatically create a new destination collector for the current mesh. If you select this option, the software creates a collector using the default physical properties and inherits the material properties of the idealized part.Note: If you did not use a midsurface to generate the 2D mesh, you must edit the automatically created mesh collector to specify a physical property table that includes thickness properties.Clear the Automatic Creation check box to choose an existing mesh collector from the Mesh Collector list.
Mesh Collector	Lets you select an existing collector. Click New Collector to use the Mesh Collector dialog box to create additional mesh collectors. See Mesh collectors for more information.
Preview
Boundary Nodes	Click Boundary Nodes to view the approximate nodal density along the boundaries of the selected geometry. Boundary Nodes can help you determine whether the element size you specified is appropriate.

How do I

Create a 3D tetrahedral mesh

Learn more

3D tetrahedral meshing

Understanding 3D tetrahedral mesh quality evaluation

Understanding the Auto Fix Failed Elements process

Pyramid element transitions

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

3D Tetrahedral Mesh dialog box, Simcenter 3D 2021.1 Series

© 2020 Siemens

window.mainLanguage="en_US"

window.delivId=""

window.projectId=""

MathJax.Hub.Config({ TeX: { extensions: ["autoload-all.js"] }, tex2jax: { displayMath: [ ] }, "SVG": { scale: 125 } });