3D Swept Mesh dialog box

Type
Type	Controls how the software sweeps the mesh through the selected bodies.Select Multi Body-Infer Target to sweep a mesh through a solid body. With this option, the software sweeps the mesh from a selected source face to a target face that the software determines for you. With this option, you can select source faces in separate bodies simultaneously. However, the software sweeps the mesh through each individual body. Select Until Target to sweep a mesh through a solid body, from a source face in one body to a target face in another body. The intervening bodies must be contiguous.Select Automatic Between to have the software automatically sweep a structured mesh between two solid meshes. With this option, the software tries to determine the edge and loop correspondence between the source and target faces. This method only works if the source and target faces are parallel and are positioned closed to each other.Select Manual Between to have the software manually sweep a structured mesh between two sets of faces or meshes. With this option, you manually define the edge and loop correspondence between the source and target faces.You can also use the Manual Between option to:Sweep a mesh between source and target faces in the same body, such as to fill a void space with structured elements. For more information, see Manually sweeping a mesh through a void in a body.Create a single layer of cohesive elements between the source and target faces in the Simcenter 3D Multiphysics, Samcef environments, or a single layer of interface elements in the ANSYS environment. For more information, see Cohesive elements and Modeling cohesive zones with ANSYS interface elements.See Selecting the type of swept mesh to create for more information.
Mesh Name
Mesh Name	Lets you specify a name for the mesh.
Objects to Mesh
Select Source Face	To create a swept mesh, you can select a source face that is either unmeshed or meshed:If the face you select is unmeshed, the software generates a quadrilateral mesh on the source face. It then uses those quadrilateral elements to sweep a hexahedral mesh through the solid.If the face you select is meshed, the software uses the existing elements to sweep a mesh through the solid.
Select Target Face	Available if Type is set to Until Target, Automatic Between, or Manual Between.If you select Until Target from the Types list, lets you select the target face. The software terminates the swept mesh at the target face.
Wall SelectionAvailable if Type is set to Manual Between.
Select Wall Face	Lets you manually select the wall faces.
Dynamic Wall Selection	Select this option to have the software select the wall faces automatically. With Dynamic Wall Selection, the software selects all faces that share edges with both the source and target faces.
Element Properties
Mesh Type	Lets you choose the type of elements to use in the swept mesh. The available options depend on the specified solver and type of analysis you are performing as well as on the type of mesh (if any) on the source face.If the source face is either unmeshed or meshed with quadrilateral shell elements, you can choose linear or parabolic hexahedral elements.If the source face is meshed with triangular shell elements, you can choose linear or parabolic wedge elements.To specify an alternative formulation of an Abaqus element, such as a hybrid, click Edit Mesh Associated Data .
Source Mesh Parameters
Source Element Size	Enter the desired source element size. Alternatively, you can click to have the software estimate an element size for the currently selected geometry.If you select a surface mesh to use as a seed mesh, the source element size is the size of the selected mesh, and you cannot modify this value. 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.Examines the selected geometry and calculates an estimated element size. The Overall Element Size field updates to show this element size.
Automatic Element Size	Examines the selected geometry and calculates a suggested overall element size. The Source Element Size field updates to show the suggested element size.Note: The element size calculated by Auto 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 for more information.
Attempt Free Mapped Meshing	Available if Type is set to Multi-Body Infer Target or Until Target.For unmeshed source faces, controls whether the software creates a mapped-like mesh on the source face.Select Attempt Free Mapped Meshing to have the software try to create a mapped (structured) mesh on the source face. See Understanding free mapped meshes for more information.Clear the Attempt Free Mapped Meshing check box to have the software create a free (unstructured) mesh on the source face.
Attempt Quad Only	Controls whether the mesh on the source face contains only quadrilateral elements. Having an all quadrilateral mesh on the source face ensures that the swept mesh through the volume will not contain any wedge 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.On - Single Triangle: The software creates a mesh that contains, at most, a single triangular element per selected face. With this option, the software only inserts a triangular element if it cannot establish nodal parity (an even number of nodes) along the boundary of a face.For more information, see Quadrilateral only meshing.
Make Mesh Non-Associative	Controls whether the software associates the resulting solid mesh to the geometry.If you do not want to associate the new nodes and elements with any of the source geometry, select the Make Mesh Non-Associative check box. The resulting mesh is FE-based. The software does not update this mesh if it updates any neighboring meshes. You cannot modify a non-associative mesh.To associate the new nodes and elements with the source geometry, clear the Make Mesh Non-Associative check box. The software creates a mesh recipe for the resulting mesh in the Simulation Navigator. Use this recipe to modify the swept mesh. The software also uses this mesh recipe to update the manual swept mesh when changes occur to adjacent meshes or to the underlying geometry.Note: With meshes that you create with the Manual Between option, the interior nodes are always not associated with the geometry.
Wall Mesh Parameters
Use Layers	Controls the number of layers of elements that the software generates between a source face and a target face. This also allows you to control the size of the elements that the software sweeps through the volume.You can specify the number of layers as an integer value, or you can specify the number as an expression. See Expressions for more information.
Number of Layers	If you select Use Layers, lets you specify the number of layers to create between the source and target faces.
Edge Mapping	Available if Type is set to Multi-Body Infer Target or Until Target.Projects vertices along the boundaries of the source face or faces to the target face. This allows you to control the appearance of the mesh along the wall faces. See Projecting vertex locations in mapped meshes for more information.
Target Mesh ParametersAvailable if Type is set to Multi-Body Infer Target or Until Target.
Smooth Nodes	Controls whether the software smooths the nodes in the mesh on the target face. If you select the Smooth Nodes check box, the software makes minor modifications to the position of the nodes on the target face to achieve a more regular mesh. However, the resulting mesh on the target face will not exactly match the mesh on the source face.
Destination Collector
Destination Collector	Controls the mesh collector in which the current mesh is stored.Select Automatic Creation to have the software automatically create a new collector for the mesh. The automatic mesh collector uses the default physical properties and inherits the material properties of the idealized part.Clear the Automatic Creation check box to select a mesh collector. You can select an existing mesh collector from the Mesh Collector list or click New Collector to create a mesh collector.
Preview
Show Result	Previews the swept mesh. The preview is based on the options you selected in the 3D Swept Mesh dialog box, any existing the mesh mating conditions, and the mesh attributes on the body's boundary edges.

Learn more

Multi Body-Infer Target and Until Target meshes

Criteria for sweepable bodies

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

3D Swept 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 } });