Seam weld universal connections in the Nastran environment

In the Nastran environment, you can use the universal connection commands to define and mesh seam weld connections between components.

Defining the seam weld connection and generating the elements

• You can use the Seam Weld Connection command to specify the definition for the seam weld connection. For example, you specify the parts (flanges) to connect, the locations of the connections, tolerance values for creating the connections, and properties of the connection such as the width and height of the welds and the weld material.

• You can use either the Automatic Elements or Connection Elements commands to generate the actual seam weld elements from the connection definitions.If you use the Automatic Elements command, the software uses default values to create the seam weld elements.Note: You can use options on the Seam Weld Element page of the Universal Connections customer defaults to control those default values.If you use the Connection Elements command, you can use options in the Seam Weld Element dialog box to control how the software creates the seam weld elements.

Meshing Nastran seam weld connections

You can use the Type option in the Seam Weld Element dialog box to specify the type of elements to use to mesh seam weld connection definitions in the Nastran environment.

• Select RBE2 to use RBE2 rigid body elements to model the seam weld.

• Select RBE2+RBE2 spider(s) to use RBE2 rigid body elements to model the seam weld and RBE2 elements in a spider configuration to model the interaction between the weld and the connected flanges. If you select this option, you can use the DOF Selection options to specify the dependent degrees of freedom for all the RBE2 elements.

• Select CBAR+RBE3 spider(s) to use a CBAR element to model the weld and RBE3 interpolation elements to model the interaction between the seam weld elements and the connected flanges. The CBAR+RBE3 spider(s) option more accurately models the tension and compression, torsion, bending in two perpendicular planes, and shear in two perpendicular planes that might occur in the seam weld.

Mesh associated data for Nastran seam weld elements

When you generate the seam weld connection elements, the software automatically defines the mesh associated data for the elements.

• For CBAR elements, the software automatically defines the orientation vector and end offsets. You can edit the mesh associated data to modify these options and to set other options, such as the pin flags for ends A and B of the bar element.

• For RBE2 elements with the RBE2+RBE2 spider(s) option, the software automatically sets the degrees of freedom for the core node and the leg nodes to On.

• For RBE3 elements, the software automatically sets the degrees of freedom for the core node and the leg nodes. These default settings differ depending on whether the connected flanges are meshed with 2D or 3D elements.For RBE3 elements that connect flanges meshed with 2D elements, the software sets all degrees of freedom for both the core node and the leg nodes to On.For RBE3 elements that connect flanges meshed with 3D elements, the software sets the translational degrees of freedom (DOF1-DOF3) for the core and leg nodes to on and sets the rotational degrees of freedom (DOF4-DOF6) to Off.

To modify mesh associated data, right-click the mesh in the Simulation Navigator and select Edit Mesh Associated Data.

Weighting factors for RBE3 leg nodes

During the meshing process when the element type is set to CBAR+RBE3 spider(s), the software automatically sets the weighting factors for the leg nodes of the RBE3 elements. For example:

------------------------------------------------------------ ELEMENT ASSOCIATED DATA INFORMATION ------------------------------------------------------------     Label                               : 719    Element Type                        : RBE3    Mesh Name                           : Seam Weld Element(3)    DOF Weights for Independent Nodes   :    Node                                : 259        DOF Weights DOF 1-6             : 0.0001  0.0001  0.0001  Null  Null  Null     Node                                : 260        DOF Weights DOF 1-6             : 1  1  1  Null  Null  Null     Node                                : 339        DOF Weights DOF 1-6             : 0.0001  0.0001  0.0001  Null  Null  Null     Node                                : 340        DOF Weights DOF 1-6             : 0.0001  0.0001  0.0001  Null  Null  Null

You can use the Interpolation option in the Element Associated Data dialog box to modify the weighting factors and UM data for selected RBE3 elements. For more information, see RBE3 in the Simcenter Nastran Quick Reference Guide.

Physical property data for Nastran seam weld elements

If you select the CBAR+RBE3 spider(s) option, during the meshing process, the software also creates a PBAR physical property table that defines the properties for the CBAR elements that represent the seam weld. The PBAR physical property table defines options, such as:

• The material to use for the CBAR elements.

• The nonstructural mass value for the CBAR elements.

• A circular Beam Section cross section that defines the shape and radius for the Fore Section of the beam element. The software sets the D1 radius value to ½ the Width value that you specify on the Weld Properties page of the Seam Weld Connection dialog box.

The options in the PBAR dialog box correspond to the fields on the PBAR bulk data entry. For more information, see PBAR in the Simcenter Nastran Quick Reference Guide.

Nastran seam weld elements in the Simulation Navigator

The software stores the seam weld connection elements as a new mesh or meshes in the appropriate collectors in the 1D Collectors node in the Simulation Navigator.

• CBAR elements are stored in a single mesh in the Bar Collector container.

• RBE2 elements are stored in RBE2 Collector container.

• RBE3 elements are stored in RBE3 Collector containers. RBE3 elements that connect 2D meshes and RBE3 elements that connect 3D meshes are stored as separate meshes because of the differences in how their degrees of freedom are defined by default.

Where do I find it?

Application	Pre/Post
Prerequisite	A FEM or assembly FEM file as the work part and displayed partSimcenter Nastran or MSC Nastran as the specified solver
Command Finder	Seam Weld Connection Connection Elements Automatic Connection Elements

Seam weld universal connection customer defaults

Menu	File→Utilities→Customer Defaults
Location in dialog box	Simulation→Pre/Post→Universal Connections→ Seam Weld tab

Learn more

Seam weld universal connections in the LS-DYNA environment

User defined seam weld fine models

Seam weld visualization

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Seam weld universal connections in the Nastran environment, 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 } });