Element Associated Data dialog box

For a list of all element attributes supported by each solver, see Element and mesh attributes.

Type
Type list	Specifies the type of elements you can select for which to define associated data.
Elements
Select Elements	Lets you select one or more elements on the model where you want to define element associated data.
Element Labels	Lets you add elements to the selection.Use a space or comma to separate your entries.Use a colon or a dash to add a range of element labels.For example, enter 1:10 or 1-10 to add all the element labels from 1 to 10.Use colons to add an incremented range of element labels.For example, enter:1:9:2 to add element labels 1, 3, 5, 7, 9.1:10:2 to add element labels 1, 3, 5, 7, 9, 10.10:1:-2 to add element labels 10, 8, 6, 4, 2, 1.Press enter or click Select to add your entries.To edit your selection, click Edit Element Selection .
Set No change Clear	Determines the editing action for the associated data when you click OK.Set—Adds a new associated data to the selected element(s). If this type of associated data was already defined on this element, selecting Set discards the existing associated data.No change (Shell elements only)—Leaves any existing associated data unchanged. Clear—Deletes any previously defined associated data from the selected element(s).

Lumped Mass

Mass
Mass	Enter the mass as a constant value or expression.

Spring options

Properties
Physical Property	Select a physical property table from the list to define properties.For information about creating a physical property table, see Define physical properties.
Stiffness
Translational****Rotational	Defines the translational and/or rotational spring stiffness as a constant value or expression.
Component End A/Component End B
Translational****Rotational	Defines the direction of translation and rotation at the ends.

Shell / Plane Stress / Chocking options

Properties
Type	Specifies the type of physical property table to use to define the properties. The types available depend on the selected solver. For information about creating a physical property table, see Define physical properties.
Physical Properties	Select a physical property table from the list to define properties.For information about creating a physical property table, see Define physical properties.
Material Orientation
Definition method	Lets you select whether to define the material orientation by selecting a coordinate system, defining a coordinate system by selecting its type and specifying points, or by specifying a vector.For more information about material orientation, see Material orientation.
Specify CSYS	Available when the definition method is Coordinate System.Lets you use the standard coordinate system tools to define the material orientation based on a local coordinate system. The software uses the X-axis of the selected coordinate system as the material orientation vector. That vector is projected onto the plane of the selected element to determine the material coordinate system. For more information about the CSYS dialog box, see CSYS dialog box.
Coordinate System Data	Available when the definition method is Coordinate System Data.Select the type of coordinate system that you want to create, such as Cartesian, and then specify the origin and two points to define the coordinate system.
Specify Vector	Available when the definition method is Vector Projection.Lets you use the standard vector tools to define the material orientation by specifying 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 about the Vector dialog box, see Vector dialog box.
Reverse Direction	Reverses the direction of the vector.
Corner Node Thickness
Thickness	Defines the thickness at all of the element's corner nodes (the value is applied to each corner node). Use this option to override the shell thickness defined at any other level (at the physical property table level, mesh-associated data level, or mesh level, depending on the selected solver). For more information, see Shell thickness.For more information about using an expression or constant value, see the description in Mass above.
Define Thickness for Selected Nodes Only****Select Node	Applies the value specified in Thickness only to the nodes you select. If you do not select any nodes, the Thickness value applies to all corners of the element and defines a uniform thickness. In the example below, only two corners of the shell element were selected for the thickness definition.
Node Labels	Lets you specify nodes for which to define thickness by node label.Use a space or comma to separate your entries.Use a colon or a dash to add a range of node labels.For example, enter 1:10 or 1-10 to add all the node labels from 1 to 10.Use colons to add an incremented range of node labels.For example, enter:1:9:2 to add node labels 1, 3, 5, 7, 9.1:10:2 to add node labels 1, 3, 5, 7, 9, 10.10:1:-2 to add node labels 10, 8, 6, 4, 2, 1.Press enter or click Select to add your entries.To edit your selection, click Edit Node Selection .
Corner Node Gap
Gap	Defines the gap size at each of the element's corner nodes. Use this option to override the gap thickness value defined in the Mesh Associated Data or Chocking Property dialog boxes. For more information, see Chocking elements.
Define Gap for Selected Nodes Only****Select Node	Applies the Gap value only to the nodes you select. If you do not select any nodes, the Gap value applies to all corners of the element and defines a uniform gap size.
Node Labels	Lets you specify nodes for which to define the gap value by node label.Use a space or comma to separate your entries.Use a colon or a dash to add a range of node labels.For example, enter 1:10 or 1-10 to add all the node labels from 1 to 10.Use colons to add an incremented range of node labels.For example, enter:1:9:2 to add node labels 1, 3, 5, 7, 9.1:10:2 to add node labels 1, 3, 5, 7, 9, 10.10:1:-2 to add node labels 10, 8, 6, 4, 2, 1.Press enter or click Select to add your entries.To edit your selection, click Edit Node Selection .
Z Offset
Z Offset	Lets you offset the element by specifying the distance from the element surface of nodes to the element reference plane (mid-plane or neutral axis).

Beam/Bar options

Properties
Type	Specifies the type of physical property table to use to define the properties. The types available depend on the selected solver.
Physical Properties	Select a physical property table from the list to define properties.For information about creating a physical property table, see Define physical properties.
Section Orientation
Method	Specifies the method used to define the cross section orientation:Vector—Lets you orient the Y-axis or Z-axis (n1 or n2 axis for Abaqus) of the cross section by specifying a vector in either the absolute coordinate system or nodal displacement coordinate system.Node—Lets you orient the cross section using a third node that, along with the first and second nodes of the element, defines the orientation vector for the section. These methods work similarly to the Orientation Vector and Orientation Node methods used to define the orientation of the 1D mesh in the Mesh Associated Data dialog box. For steps, see Define cross section orientation.
Define Element Axis	Available when Method is set to Vector.Specifies the axis of the cross section to orient (either the Y-axis or Z-axis).
Orientation CSYS	Available when:The selected solver is Simcenter Nastran, Simcenter 3D Multiphysics, or MSC Nastran.Method is set to Vector.Defines the coordinate system used to orient the axis of the cross section:Absolute—Lets you orient the axis of the cross section by specifying a vector in the absolute coordinate system.Nodal Displacement—Lets you orient the axis of the cross section by specifying a vector in the nodal displacement coordinate system.
Specify Vector to project	Available when:Method is set to Vector.Orientation CSYS is set to Absolute.Lets you define the orientation of the cross section by specifying a vector in the absolute coordinate system.For more information about the Vector dialog box, see Vector dialog box.
DOF1/DOF2/DOF3	Available when:The selected solver is Simcenter Nastran, Simcenter 3D Multiphysics, or MSC Nastran.Method is set to Vector.Orientation CSYS is set to Nodal Displacement.Lets you define the orientation of the cross section by specifying a vector in the nodal displacement coordinate system.
Reverse Direction	Reverses the direction of the vector.
Select Node	Available when the definition method is set to Node.Lets you select a node (typically a node you create specifically for this purpose) to use in defining the orientation. The X-Y plane of the cross section orientation is defined by the vector from the first node in the 1D element to the orientation node.In the example, is the first node in the 1D element and is the orientation node.
End A/End B Offsets
Available when Type is set to Beam / Bar.
Offset CSYS	Defines the coordinate system used to offset the cross section at end A/end B:Nodal Displacement—Lets you offset the cross section from the ends of the 1D element by specifying a vector in the nodal displacement coordinate system defined at end A/end B.Elemental—Lets you offset the cross section from the ends of the 1D element by specifying a vector in the element coordinate system.For more information on the CBAR element coordinate system, see CBAR Element Coordinate System and Orientation.For more information on the CBEAM element coordinate system, see CBEAM Coordinate System.
Offset Along ElementOffset Along Section Y-axisOffset Along Section Z-axis	Available when:The selected solver is Simcenter Nastran, Simcenter 3D Multiphysics, or MSC Nastran.Offset CSYS is set to Elemental.Lets you define the offset of the cross section from the ends of the 1D element by specifying a vector in the element coordinate system.Offset Along Element—Lets you specify an offset along the element X-axis.Offset Along Section Y-axis—Lets you specify an offset along the element Y-axis.Offset Along Section Z-axis—Lets you specify an offset along the element Z-axis.
DOF1 Offset to Shear CenterDOF2 Offset to Shear CenterDOF3 Offset to Shear Center	Available when:The selected solver is Simcenter Nastran, Simcenter 3D Multiphysics, or MSC Nastran.Offset CSYS is set to Nodal Displacement.Lets you define the offset of the cross section from the ends of the 1D element by specifying a vector in the nodal displacement coordinate system.
Component 1Component 2Component 3	Available when the selected solver is Abaqus or ANSYS.Lets you define the offset of the cross section from the ends of the 1D element by specifying a vector in the element coordinate system.Component 1—Lets you specify an offset along the element X-axis.Component 2—Lets you specify an offset along the element Y-axis.Component 3—Lets you specify an offset along the element Z-axis.(1) cross section origin; (2) Component 2 offset; (3) Component 3 offsetNote: When ANSYS is the selected solver and no offset is specified, the beam element is placed at the cross section origin.Component 1 is not used (ANSYS does not support offset along the element X-axis).

Spring Damper / Kinematic options

Properties
Type	Specifies the type of physical property table to use to define the properties. The types available depend on the selected solver.
Physical Properties	Select a physical property table from the list to define properties.For information about creating a physical property table, see Define physical properties.
Orientation
Orientation method	Specifies the method to use to define the orientation:Vector—Lets you orient the element to an axis of the global coordinate system or to a direction inferred from geometry. Node—Lets you orient the element using a third node that, along with the first and second nodes of the element, defines the orientation of the element. Coordinate System—Lets you orient the element using a coordinate system that you specify.Select the type of coordinate system that you want to create, such as Cartesian, and then specify the origin and two points to define the coordinate system.

Gap options

Properties
Type	Specifies the type of physical property table to use to define the properties. The types available depend on the selected solver.
Physical Properties	Select a physical property table from the list to define properties.For information about creating a physical property table, see Define physical properties.
Elements
Orientation	Specifies the method to use to define the orientation:Vector—Lets you orient the element to an axis of the global coordinate system or to a direction inferred from geometry. Coordinate System—Lets you orient the element using a coordinate system that you specify.Node—Lets you orient the element using a third node that, along with the first and second nodes of the element, defines the orientation of the element.

Damper options

Properties
Type	Specifies the type of physical property table to use to define the properties. The types available depend on the selected solver.
Physical Properties	Select a physical property table from the list to define properties.For information about creating a physical property table, see Define physical properties.
Viscous Damping
Translational Rotational	Specifies the amount of viscous damping in the translational and rotational directions.
Component End A/Component End B
Translational****Rotational	Defines the direction of translation and rotation at the ends of the damper element.

Rigid options

DOFs
DOF1-DOF6	Lets you constrain the degrees-of-freedom in the translational and rotational directions.

Constraint Equation options

Dependent DOF
Component Number	Lets you specify the degree-of-freedom in the dependent node to constrain.
Coefficient	Lets you specify a coefficient to apply to the constrained degree-of-freedom.
Independent DOF Coefficients
Node ID column	Lists the nodes in the constraint equation.The first row in the table is the dependent node in the equation. You cannot specify coefficients for the degrees-of-freedom for the dependent node.The subsequent rows in the table list the independent nodes in the equation. For each node, you can specify coefficients for the degrees-of-freedom for these nodes.

Interpolation Element options

DOF Weights for Independent Nodes
Node ID	Lists the node ID.
DOF1-DOF6	Lets you specify the weighting factors for the degrees-of-freedom for each independent node.
UM Data
Node ID	Lists the node ID.
Component Number	Lets you specify which degrees of freedom belong to the M set. For more information, see RBE3 in the Simcenter Nastran Quick Reference Guide.

Solid Element options

Properties
Physical Property	Select a physical property table from the list to define properties.For information about creating a physical property table, see Define physical properties.

How do I

Add element-associated data

Edit the mesh associated data for multiple meshes

Remove element-associated data

List and show element-associated data for a mesh

Add mesh-associated data

Create an ANSYS KEYOPT table

Override element attributes

View material orientation graphically

Define Nastran 2D element material orientation

Define Nastran 3D element material orientation

Define Abaqus 2D element material orientation

Define Abaqus 3D element material orientation

Define ANSYS 2D element material orientation

Define ANSYS 3D element material orientation

Define LS-DYNA 2D element material orientation

Define LS-DYNA 3D element material orientation

Define 2D element material orientation (Simcenter 3D Thermal/Flow, Electronic Systems Cooling, and Space Systems Thermal)

Define 3D element material orientation (Simcenter 3D Thermal/Flow, Electronic Systems Cooling, and Space Systems Thermal)

Learn more

Element-associated data

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Element Associated Data 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 } });