Solid from Shell meshing

Use the Solid from Shell Mesh command to create a 3D mesh from an existing 2D mesh of triangular or quadrilateral elements. This command is useful when you want to use elements, rather than polygon geometry, to define the enclosed surface of a volume.

You can use the Solid from Shell Mesh command in a variety of workflows, such as to:

• Model an acoustic fluid in a Simcenter Nastran FEM acoustic or vibro-acoustic analysis. For example, you can use Solid from Shell Mesh to create a 3D acoustic fluid mesh. You can use Solid from Shell Mesh to create the fluid mesh between a 2D mesh that represents the inner boundary of the fluid and a mesh created with the Convex Mesh command that represents the outer boundary of the fluid. For more information, see Meshing for FEM acoustic analysis.

• Model the fluid body inside a solid enclosure, possibly with other solid bodies acting as a barrier to the flow.

• Create a solid mesh inside a closed volume of 2D elements in a FEM file that does not contain any geometry, such a model that you imported from a Nastran bulk data file.

Example: Creating solid meshes from shell meshes

The following graphics show an example of how you can use Solid from Shell Mesh to generate a mesh of tetrahedral elements from an existing, enclosed volume of 2D triangular elements.

A 2D triangular mesh of an interior cavity. Here, the nodes are displayed as asterisks for clarity.	2D triangular mesh of a bounding box. Together, these two meshes create an enclosed volume.

A 3D tetrahedral mesh created from the selected 2D meshes. Note the distribution of interior nodes.

Element size in the 3D mesh

The source mesh of 2D elements controls the size of the 3D elements that the software creates. The software uses the length of the elements in the 2D source mesh as the initial element length for the tetrahedral mesh. You can use the Internal Mesh Gradation option in the Solid from Shell dialog box to control whether the software can gradually enlarge this size as it creates elements through the volume.

Note:

If you do not want the size of the elements to change, specify a value of 1.0 in the Internal Mesh Gradation box.

Element type in the 3D mesh

You can select either linear or parabolic 2D source meshes, or a mix of linear and parabolic 2D source meshes, and then select an option in the Type list to create either a linear or parabolic 3D mesh. Selecting a mix of linear and parabolic 2D source meshes allows you to reuse existing midnodes and preserve the original mesh accuracy. For example, when you need to generate a mesh in an enclosed domain between a 2D parabolic mesh and a 2D linear mesh, the Solid from Shell Mesh command reuses the midnodes of the 2D parabolic mesh and preserves the accuracy of that mesh in the 3D mesh.

The example below shows the original parabolic 2D mesh and the linear 2D convex mesh that is created to envelope the original mesh. The Solid from Shell Mesh command is then used to create parabolic tetrahedral elements to fill the space between the two 2D meshes.

Parabolic 2D Mesh	Linear 2D Convex Mesh	Parabolic 3D Tetrahedral Mesh

If you select a source mesh of quadrilateral elements and the clear the Transition with Pyramid Elements check box, the software automatically splits each element into two triangular elements before it creates the tetrahedral elements.

Note:

Use caution when generating a solid mesh from parabolic shell elements. Unless the parabolic triangular shell elements have straight edges, the resulting parabolic tetrahedral mesh may contain elements that fail Jacobian quality checks.

2D mesh must form a closed volume

The 2D mesh or meshes that you select with the Solid from Shell Mesh command must form a completely enclosed volume. If they do not, the software cannot generate the tetrahedral mesh.

Tip:

Use the Element Edges command to find unconnected elements within the 2D mesh. This lets you see whether there are any gaps from missing or unconnected elements in the boundary of the volume. See Checking for free and non-manifold element edges for more information.

Additionally, the source 2D meshes should not contain any coincident elements.

Tip:

Use the Duplicate Nodes command to identify duplicate nodes. Identifying duplicate nodes can help you locate coincident elements. For more information, see Checking for duplicate elements and nodes.

Separate 3D meshes in interior volumes

In the Solid from Shell dialog box, use the Mesh Interior Volumes option to control whether the software creates a separate solid mesh within the interior of the volume. If you select this option, the software generates one 3D mesh for each 2D mesh that defines the outer boundary of the volume and a separate 3D mesh for the interior volume. This option is useful for modeling thermal or flow problems, in which the interior volumes would typically represent a heat sink or source, or a flow obstacle.

Creating pyramid element transitions

Use the Transition with Pyramid Elements check box to control whether the software creates pyramid elements in addition to tetrahedral elements when the source 2D mesh contains quadrilateral elements.

• Select the Transition with Pyramid Elements check box when the source 2D mesh contains quadrilateral elements that you want to retain.

• Clear the Transition with Pyramid Elements check box if you want the software to create a mesh of tetrahedral elements only.

2D source meshes with triangular and quadrilateral elements	Solid from shell mesh with tetrahedral and pyramid elements
Solid from shell mesh with only pyramid elements displayed

The software stores the pyramid elements and the tetrahedral elements in different meshes in the Simulation Navigator:

Note the following considerations for creating pyramid elements:

• You can select the Transition with Pyramid Elements option only when the elements in the source 2D meshes are of the same order (linear or parabolic).

• You cannot select the Transition with Pyramid Elements option if you select the Mesh Interior Volumes check box.

• You can only select the Transition with Pyramid Elements check box in solver environments that support pyramid elements, such as Simcenter Nastran and ANSYS.

Solid mesh associativity

The 3D mesh that the Solid from Shell Mesh command creates is not associated with either the source 2D mesh or with any geometry. Additionally, you cannot modify a 3D mesh that you create with the Solid from Shell Mesh command. If you want to change the mesh, such as specify a different element size, you must delete the mesh and then use the Solid from Shell Mesh command to recreate the 3D mesh with different options.

Where do I find it?

Application	Pre/Post
Prerequisite	A FEM file or a component FEM within an assembly FEM file as the work part and displayed part
Command Finder	Solid from Shell Mesh
Menu	Insert→Mesh→Solid from Shell Mesh

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Solid from Shell meshing, 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 } });