Physical properties and element attributes

When you define a mesh, the available element types depend on the solver language that you selected when you created the FEM or Simulation file. For example, if you selected Simcenter Nastran as your solver, you can create a mesh using CQUAD4 elements.

Depending on the selected solver type and element type, you can specify additional properties for the elements through physical property tables and element attributes. For the ANSYS solver language, you can also define KEYOPT tables.

Creating and applying physical property tables

Physical properties describe the physical qualities and characteristics of an element, such as thickness or nonstructural mass. You can create physical property tables to store these physical properties in the context of a FEM file or a Simulation file. When you create a physical property table with the FEM active, you can assign it to a mesh collector. The meshes (and therefore, the elements in these meshes) that are assigned to the mesh collector then inherit those physical properties. You can also assign a physical property table to element-associated data for certain element types.

If you create a physical property table with the Simulation file active, you can use it to override the physical properties that were assigned to a mesh collector. If you have multiple Simulation files, the overrides enable you to explore how different physical properties affect the solution results. A physical property table created when a Simulation file is active cannot be used when the FEM file is active.

Defining element and mesh attributes

Some element types, such as concentrated mass, rigid links, and springs, do not use physical property tables. Instead of creating a physical property table, you use the Mesh Associated Data or Element Associated Data dialog boxes to define the physical properties for these elements.

Other elements, such as the Simcenter Nastran CQUAD4 element type, have both a physical property table and additional element attributes. For Abaqus elements, you use the Mesh Associated Data dialog box to select the element’s alternative formulation, such as hybrid.

You can define attributes for all elements in a mesh (mesh-associated data) or for individual elements (element-associated data). You can also specify that an element's associated data override the mesh's associated data, which allows you to place similar elements in the same mesh and then capture any differences (such as a different material orientation) in the element-associated data.

For more information about mesh-associated data, see Mesh-associated data. For more information about element-associated data, see Element-associated data. For a list of all supported element-associated data and mesh-associated data by solver, see Element and mesh attributes.

Defining ANSYS element attributes

ANSYS elements may use options which are controlled with switches called KEYOPTS. In Pre/Post, you can create modeling objects to define ANSYS KEYOPT tables for elements. The KEYOPT table is assigned to elements through the Mesh Associated Data dialog box. For more information, see Create an ANSYS KEYOPT table.

Like the elements for other solver types, ANSYS elements also use physical property tables, which are assigned to mesh collectors. A physical property table in Pre/Post is equivalent to an ANSYS real constant table.

Defining LS-DYNA physical properties and element attributes

You describe an LS-DYNA model's physical and material properties using the physical property named PART and the modeling objects named SECTION and HOURGLASS.

• PART lets you choose the Pre/Post material or enter the ID of an external LS-DYNA material.

• SECTION lets you define physical properties such as shell thickness, element formulation, nonstructural mass, and so on.

• HOURGLASS lets you specify an external hourglass control ID or define the hourglass control in the HOURGLASS modeling object.

Note:

The LS-DYNA Equation of State object is not supported; the ID is set to 0.

With LS-DYNA, you can define element attributes at either the element level or the mesh level. If you select Use Element Associated Data for the mesh, and not all elements have material orientations defined, those elements are written to the keyword file as *ELEMENT_SHELL (that is, the same as selecting None for the Keyword Option).

For a list of supported LS-DYNA elements, see LS-DYNA elements.

Where do I find it?

To create a physical property table:

• Choose Home tab→Properties group→Physical Properties .

• Choose Insert→Physical Properties.

To apply a physical property table to a mesh collector:

• In the Simulation Navigator, right-click the mesh collector and choose Edit.

To define element attributes:

• In the Simulation Navigator right-click the mesh node and choose Edit Mesh Associated Data.

• Choose Home tab→Properties group→Mesh Associated Data .

• Choose Nodes and Elements tab→Elements group→Associated Data .

To create an KEYOPT table when ANSYS is the solver type:

• Choose Home tab→Properties group→Modeling Objects .

• Choose Insert→Modeling Objects.

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Physical properties and element attributes, 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 } });