2D Mesh dialog box

Mesh Name
Mesh Name	Lets you specify a name for the mesh.
Objects to Mesh
Select Objects	Lets you select the faces, polygon bodies, existing meshes, or selection recipes that you want to mesh.
Stacked Smart Selector Methods	Opens the Smart Selector Methods dialog box where you can specify a progression of smart selection filters to help you select the appropriate faces, polygon bodies, or existing meshes..For more information, see Smart Selector Methods dialog box.
Element Properties
Type	Specifies the type of 2D element to create, such as linear triangular or linear quadrilateral 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 .
Edit Mesh Associated Data	Appears 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.
Retain Type	Available when you select multiple meshes with different 2D element types in the Simulation Navigator, then right-click and choose Edit Mesh.Preserves the existing element type for each selected mesh.When you select this option, the Destination Collector options in the Edit Mesh dialog box are not available. The software uses the existing collector for each selected mesh.
Mesh Parameters
Meshing Method	Controls the algorithm the software uses to create the 2D mesh on the selected geometry.Choose Subdivision to have the software use a recursive subdivision approach to generate a free, unstructured mesh.Choose Paver to have the software use a hybrid meshing method to generate a more structured mesh around the outer boundary and any interior holes and a free mesh on the rest of the geometry.For more information, see Understanding the 2D meshing methods .
Element Size	Specifies the target element size for the selected faces.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.For more information, see Understanding the Automatic Element Size calculation.
Maximum Growth Rate	For triangular meshes, 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%.
Export Mesh to Solver	Controls whether the software includes the 2D mesh data in your solver input file when you export or solve the model. If you plan to only use this 2D mesh as a seed mesh for a 3D mesh, you should clear this option.Note: This option does not appear in the Simcenter 3D Multiphysics environment because a 2D mesh is used only as seed mesh and is not exported to the solver.
Advanced Parameters
Attempt Multi-Block Decomposition	Internally subdivides faces with a number of near 90° corners into a cluster of convex regions. The software then generates meshes on each convex region. In general, the resulting meshes are more orthogonal in nature. If you select both the Attempt Multi-Block Decomposition and the Attempt Free Mapped Meshing options, the software creates a structured mesh on more regions of your model.For more information, see Multi-block decomposition in meshing.
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. For more information, see Understanding free mapped meshes.
Attempt Quad Only	If you clear the Attempt Free Mapped Meshing check box, lets you control whether the software tries to generate a mesh that contains only quadrilateral elements:Off - Allow Triangles: The software creates a quadrilateral mesh that also contains some triangular elements. This type of mesh is called a “quadrilateral dominant” mesh.On - Zero Triangles: The software creates a mesh that does not contain any triangular elements at all. With this option, if the software cannot create a mesh with only quadrilateral elements, it does not generate a mesh at all.Note: This option is available only when both the Attempt Multi-Block Decomposition and Attempt Free Mapped Meshing check boxes are cleared.On - Minimize Triangles: The software creates a mesh that contains a minimum number of triangular elements. With this option, the software inserts a triangular element only if it cannot establish nodal parity (an even number of nodes) along the boundary of a face.For more information, see Quadrilateral only meshing.
Curvature Based Size Variation	Lets you vary the size of your elements in regions of higher curvature. This allows you to create more, smaller elements in areas of higher curvature. For example:If you specify 0, the software uses the overall element length throughout the model regardless of the curvature.If you specify 50%, the software varies the element length between 60% and 100% of the overall element size based on the surface curvature.If you specify 100%, the software varies the element length between 10% and 100% of the overall element size.The software implicitly transitions the element size from a local length to the global length in appropriate situations when you set the Curvature Based Size Variation slider to a value greater than 10%. The curvature of the surfaces you select determines whether the software transitions the element size:For more information, see Understanding curvature-based size variation.
Curvature Threshold (Read Only)	Displays the smallest element size based on the overall Element Size and the setting of the Curvature Based Size Variation slider. This value decreases, for example, as the amount of surface curvature based variation increases.
Create Separate Meshes	Controls whether the software creates a single mesh or multiple meshes for the selected faces or polygon bodies. Creating separate meshes allows you to apply the same mesh parameters, such as element size and meshing method, across all selected geometry, while allowing you to assign different properties, such as different materials, to the individual faces or polygon bodies.Select Off - Single Mesh to create a single mesh for all selected faces or polygon bodies.Select On - For Each Face to create a separate mesh for each selected face. The software creates a parent mesh recipe that contains separate element collectors for the mesh on each individual face. The software uses the name that you specify in the Mesh Name field in the 2D Mesh dialog box as the base name for the element collectors and then increments each name by a value of 1.Select On - For Each Body to create a separate mesh for each selected polygon body. The software creates a parent mesh recipe that contains separate element collectors for the mesh on each body. The software uses the name that you specify in the Mesh Name field in the 2D Mesh dialog box as the base name for the element collectors and then increments each name by a value of 1.Because materials are often assigned to bodies in a CAD model, the On - For Each Body option helps ensure that each mesh inherits the correct material.For more information, see Creating a separate mesh for each face or polygon body.
Mesh Quality Options
Midnode Method	Available when Type is set to a parabolic element type.For parabolic elements, specifies how their midnodes are projected onto geometry: Mixed: The midnodes on an element are projected to the geometry unless this causes the element's Jacobian value to exceed specified the Jacobian threshold.Curved: All midnodes are projected to the geometry regardless of the resulting element quality.Linear: All midnodes are positioned in a straight line between the two corner nodes.
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. If the distance between a midnode and the associated edge or face is greater than this distance, the software automatically remeshes the edge or face.For more information, see Midnode placement for parabolic elements.
Target Maximum Element Length	Controls whether the software attempts to ensure that the mesh does not contain any elements that have an edge length longer than the specified Maximum Element Length value.
Maximum Element Length	Available if you select the Target Maximum Element Length check box.Lets you specify the maximum element edge length for the mesh. The software tries to ensure that it does not generate an element with an edge longer than this value.Note: The Maximum Element Length value must be larger than 1.7 times the specified global Element Size.
Target Minimum Element Length	Available when you create a mesh of quadrilateral elements only.Controls whether the software attempts to ensure that the mesh does not contain any elements that have an edge length smaller than the specified Minimum Element Length.
Minimum Element Length	Available if you select the Target Minimum Element Length check box.Controls whether the software attempts to ensure that the mesh does not contain any elements that have an edge length smaller than the specified Target Minimum Element Length value.You cannot set this value to greater than 50% of the specified global Element Size.Note: You should use caution if you specify a Minimum Element Length value that is larger than the Small Feature Tolerance value as doing so may negatively impact element quality.
Attempt to Fix Failed Elements	If selected, the software uses smoothing to modify elements that fail the Jacobian and Max Included Angle and Min Included Angle checks. If the mesh contains a small number of elements that the software cannot fix with smoothing, the software splits any quadrilateral elements into triangular elements that pass those checks.Tip: The Attempt to Fix Failed Elements option works best if you also select the Move Nodes Off Geometry check box.
Move Nodes Off Geometry	Available if you select the Attempt to Fix Failed Elements check box.Controls whether the software addresses quality issues by either moving nodes off the geometry or by abstracting the geometry.If you select this check box, the software can correct element quality issues by moving nodes a small distance off the polygon geometry to fix the following types of quality issues:Elements that are smaller than the specified Minimum Element Length value.Elements that violate the specified Jacobian and Warp values.Elements whose minimum or maximum included angles are larger or smaller than the specified threshold values.Note: Before you select this option, you should first clear the Project Nodes to CAD check box in the Meshing Preferences dialog box. If you do not, the software is unable to move nodes off the geometry.If you clear this check box, the software abstracts the geometry to address quality issues. During this process, the software may, for example, modify the geometry of faces in very narrow regions.
Max Warp Threshold	Available if you select the Attempt to Fix Failed Elements check box.For quadrilateral elements, controls the maximum angle allowed in the planar surface of the element.
Jacobian	Available if you select the Attempt to Fix Failed Elements check box.Specifies 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 software does not project an element's midnodes to the associated geometry.
Jacobian Ratio	Available when the Context list in the Meshing Preferences dialog box is set to Crash Analysis and if you select the Attempt to Fix Failed Elements check box.Specifies the ratio of the largest Jacobian determinant to the smallest in accordance with how LS-DYNA computes Jacobian values. Specify a value between 0.0 and 1.0.This ratio provides you with an idea of the overall distortion of an element You can use the Jacobian Ratio check to identify when an element’s interior corner angles deviate too much from 90°. A Jacobian ratio close or equal to 1.0 is desired. The lower the ratio, the worse the quality of the element. For quadrilateral elements, the Jacobian threshold is expressed as a ratio of the worst to the best Jacobian value computed at the element's Gauss points. For example, for a linear quadrilateral element, the software computes the Jacobian determinant at four Gauss points. The Jacobian ratio for an element is the lowest Jacobian determinant/the highest Jacobian determinant. A square element has a Jacobian ratio of 1.0 as all values are equal.
Taper	Available if you select the Attempt to Fix Failed Elements check box.For quadrilateral elements, lets you specify the maximum acceptable taper value for the elements in the mesh.Note: This option is available in the Nastran and Simcenter 3D Multiphysics environments only.
Skew	Available if you select both the Attempt to Fix Failed Elements and the Move Nodes Off Geometry check boxes.For quadrilateral elements, lets you specify the maximum acceptable skew angle value for the elements in the mesh.
Aspect Ratio	Available if you select the Attempt to Fix Failed Elements check box and the selected element type is a quadrilateral element.Lets you specify the maximum ratio of the element's shortest and longest sides. Use this option to prevent the software from generating overly long or thin elements. Specify a value between 3.0 – 500.0.
Max Included Angle (Quad) Min Included Angle (Quad) Max Included Angle (Tria) Min Included Angle (Tria)	Available if you select the Attempt to Fix Failed Elements check box.Lets you specify the maximum and minimum acceptable interior angle values for quadrilateral and triangular elements.For quadrilateral elements, the ideal interior angle value is 90°, with typical acceptable values ranging from a minimum of 40° to a maximum of 150°.For triangular elements, the ideal interior angle value is 60°.You can specify a Min Included Angle (Tria) value between 0 and 40 degrees.You can specify a Max Included Angle (Tria) value between 120 and 180 degrees.For more information, see Fixing triangular element interior angle quality issues.
Model Cleanup Options
CAD Curvature Abstraction	Uses a curvature analysis methodology to preserve the representation of part features during the geometry abstraction process. In general, this option improves quadrilateral meshes on relatively thin-walled parts with curvature, such as automotive body panels.The software merges groups of adjacent faces that have similar curvature. For smaller, sliver faces within the model, such as tiny faces along fillets, the software merges those faces with adjacent faces. This process aims to preserve the boundaries of features while eliminating very small faces that are interior to features. This methodology results in fewer small elements in the mesh that violate the specified Minimum Element Length value.For more information, see About CAD curvature abstraction.
Small Feature Tolerance	Available when the CAD Curvature Abstraction check box is cleared.Specifies the percentage of the element size that the software uses to determine which small 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. You can specify a percentage of the target Element Size between 0 and 50%. If you specify 0, 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 faces, that are 1 mm or less in size.For more information, see Understanding the geometry abstraction process.
Minimum Element Length (Read Only)	Displays the length of the shortest element edge in the model. You can modify this value only when the CAD Curvature Abstraction check box is selected.
Suppress Hole	Controls whether the software automatically suppresses holes in sheet bodies during 2D meshing. Use this option to remove holes from sheet bodies, such as midsurface sheet bodies, during the meshing process. The software removes all holes whose diameter is less than the threshold value you specify.You can remove:Holes contained within a single face.Holes that span multiple faces.Circular and non-circular holes.
Hole Diameter	Lets you specify the size of the holes you want to suppress. When you click OK or Apply, the software suppresses all holes whose diameter is smaller than this value.
Point Creation	Controls whether the software creates a point at the center of the suppressed hole.Select None if you do not want the software to create a point at the center of the suppressed hole.Select Point if you want the software to create a CAD point at the center of the suppressed hole. During meshing, the software does not create a node at the location of CAD points.Select Mesh Point if you want the software to create a mesh point at the center of the suppressed hole. During meshing, the software creates a node at each mesh point location.You may want to create a mesh point at the hole’s center, for example, so you can later create an FE-based connection element, such as an RBE2 at that location.
Merge Edges	Controls whether the software removes unnecessary vertices and then merges the associated edges. This prevents the software from generating a node at that location during meshing.Select Merge Edges to have the software remove a vertex if it connects two or fewer edges and if the angle between those edges is less than or equal to the threshold value you specify in the Vertex Angle box.Clear the Merge Edges check box if you do not want the software to merge edges during meshing.
Vertex Angle	Lets you specify the threshold value the software uses for removing vertices. The Vertex Angle is the angle between two separate edges that are joined at a vertex along the boundary of a face.
Match Edges	If you are meshing multiple sheet bodies, controls whether the software matches the nodes on the edges of the different sheet bodies to generate a continuous mesh. If you want the software to generate a continuous mesh across multiple sheet bodies, the edges and ends of edges of the different sheet bodies must be within the specified Match Edge Tolerance.If you are not satisfied with how the software matches the edges on the sheet bodies, you must first delete the meshes being matched. Then, you can recreate the meshes and either clear the Match Edges check box or reduce the Match Edge Tolerance value.
Match Edge Tolerance	If you select Match Edges, lets you specify the distance within which the software matches nodes on edges.
Destination Collector
Automatic Creation	Select the Automatic Creation check box 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. For more information, see Mesh collectors.
Show Result	Click Show Result to preview the mesh based on your current selections.

How do I

Create a 2D free mesh

Learn more

2D free meshing

Understanding the 2D meshing methods

Understanding free mapped meshes

Understanding free mesh generation

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

2D 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 } });