Add element-associated data

1. Display the FEM.

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

3. From the Type list, select the type of element to which you want to add attributes data. For example, select Shell / Plane Stress / Chocking for 2D elements or Beam / Bar for 1D beam or bar elements.

4. In the graphics window, select the element(s) to which to add attributes data.Note: Alternatively, you can select the elements in the graphics window first and then open the Element Associated Data dialog box. If you select multiple elements of different types, the software only processes the type of element you selected first.

5. In the Element Associated Data dialog box, click next to the type of element-associated data you want to add and select Set from the menu that appears.Note: For shell elements, if you had previously defined either material orientation or corner node thickness and you are now adding the other, select No change next to the associated data that you want to leave unchanged and select Set next to the associated data you want to add.

6. Define the associated data. Different types of data are available depending on the element type and the selected solver.Material Orientation (shell elements)—Select Coordinate System to use the X-axis of the selected coordinate system as the material orientation vector. The software projects that vector onto the plane of the selected element to determine the material coordinate system. Or, select Vector Projection to specify a vector; the software projects that vector onto the plane of the selected element to determine the material coordinate system (the vector becomes the X-axis). For more information, see Material orientation.Corner Node Thickness (shell elements)—Enter the thickness as a constant value or expression. This option lets you override the overall thickness defined at the physical property table level. For more information, see Shell thickness.Corner Node Gap (chocking elements)—Enter the size of the gap at each corner node as a constant value. This option lets you override the gap thickness value defined as mesh associated data.Z Offset (shell elements)—Enter the distance from the element surface of nodes to the element reference plane (mid-plane or neutral axis). Section Orientation (beam and bar elements)—For information about defining the beam section orientation, see Define cross section orientation. End A/End B Offsets—Enter X, Y, and/or Z offsets for the beam section. For more information about defining the offsets, see Offset a cross section.Pin Flags/End Releases (beam and bar elements)—If necessary, use the DOF1–DOF6 options to remove connections between a node and the selected degrees of freedom (in the element coordinate system). For more information about end releases, see End releases for 1D elements.Mass (lumped mass elements)—Enter the mass as a constant value or expression. Stiffness (spring elements)—Enter the translational and/or rotational spring stiffness as a constant value or expression.Viscous Damping (damper elements)—Enter the translational and/or rotational viscous damping constant as a constant value or expression.Orientation (spring-damper elements, gap elements, and kinematic joint)—Define the orientation by defining a vector, coordinate system, or by selecting a reference node.Properties (all elements but lumped mass and constraint equation)—Assign a physical property table to define associated properties. The available physical property tables depend on the element type and selected solver.

7. Click OK or Apply to add the associated data.

If you want this element-associated data to override the mesh-associated data, make sure Use Element Associated Data is selected in the Mesh Associated Data dialog box (for the mesh in which the element resides).

Note:

All element-associated data for a given mesh is lost when you update the mesh.

How do I

List and show element-associated data for a mesh

Remove element-associated data

Add mesh-associated data

Modify the properties of multiple meshes

Edit the mesh associated data for multiple meshes

Create an ANSYS KEYOPT table

Override element attributes

Learn more

Element and mesh attributes

Element-associated data

Managing element-associated data

End releases for 1D elements

Mesh-associated data

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Add element-associated data, 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 } });