Spot weld universal connections in the LS-DYNA environment

In the LS-DYNA environment, you can use the universal connection commands to define and mesh spot weld connections between components. Pre/Post uses:

• ELEMENT_SOLID(8) type elements to represent the spot weld connection.

• The LS-DYNA *CONTACT_SPOTWELD keyword to model the interaction between the spot weld elements and the connected components.

Defining the spot weld connection and generating the elements

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

• You can use either the Automatic Elements or Connection Elements commands to generate the actual spot weld elements from the connection definitions.If you use the Automatic Elements command, the software uses default values to create the spot weld elements.Note: You can use options on the Spot Weld 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 Spot Weld Element dialog box to control how the software creates the spot weld elements, such as whether the software uses a single ELEMENT_SOLID(8) element to represent the weld or a cluster of eight ELEMENT_SOLID(8) elements.

Specifying how to model the spot weld

In the Spot Weld Element dialog box, you can use the Representation option to control whether the software represents the spot weld with one or more ELEMENT SOLID(8) elements.

Option	Description	ELEMENT SOLID(8) representation
Single Element	Creates one, linear hexahedral (solid) element.The area of the element's face is equivalent to the circular area of the spot weld.This option reduces the overall solve time compared to the Cluster 8 option.
Cluster 8	Creates a cluster of eight, linear hexahedral (solid) elements in the shape of trapezoids. Three sides of the trapezoids are equal in length, and the adjacent elements share common faces.The area of the element's face is equivalent to the circular area of the spot weld.This option increases the overall solve time compared to the Single Element option. However, this option better represents spot weld behavior and results in more refined post-processing.

If you change the specified solver environment to either Nastran or Abaqus after you generate the spot weld elements, the software converts the ELEMENT_SOLID(8)+CONTACT_SPOTWELD elements as shown below when you use the Update Finite Element Model command.

LS-DYNA	Nastran	Abaqus
ELEMENT_SOLID(8)+CONTACT_SPOTWELD	CHEXA+RBE3 Spider(s)	C3D8+DCOUP3D Spider(s)

Mesh associated data for LS-DYNA spot weld elements

When you generate the spot weld connection elements, the software automatically defines the mesh associated data for the elements. In the Mesh Associated Data dialog box, the software automatically:

• Sets the Connection Options list to *CONTACT_SPOTWELD.

• Uses the LS-DYNA Parts for masters option to select the physical property tables, such as a PART (shell) or a PART (solid) table that are associated with the flanges to connect.

• Sets the CARD2/CARD3, CARDA, CARDB (optional), and Massively Parallel Processing Option (MPP) options to select the related modeling objects that you specified in the Spot Weld Element dialog box. For more information on these contact-specific options, see Specifying additional LS-DYNA contact properties.

Physical property data for LS-DYNA spot weld elements

During the meshing process, the software also creates a PART (solid) physical property table that defines the properties for the solid elements that represent the spot welds. In the PART(solid) dialog box, the software automatically:

• Sets the material to use for the spot weld connection. The software selects the Use Pre/Post Material check box in the Material Option group, sets the Material list to the material that you specified in the Adhesive Connection dialog box and sets the Material Type, which controls how the software exports the material property data to the LS-DYNA input file to Defined by Pre/Post.

• Specifies the SECTION_SOLID modeling object to use. During the meshing process, the software creates a SECTION_SOLID modeling object with default settings that you can modify, such as the element formulation to use for the solid elements that represent the spot welds. The SECTION_SOLID option corresponds to the *SECTION_SOLID keyword.

LS-DYNA spot weld connections in the Simulation Navigator

The software stores the spot weld connection elements as a new mesh in the appropriate PART (solid) entry in the 3D Collectors node in the Simulation Navigator. If your model contains multiple spot weld connection definitions that use different materials, the software places the elements into separate meshes in different PART (solid) entries, as shown below.

Meshes for LS-DYNA spot weld elements in the Simulation Navigator

Spot weld connections in the LS-DYNA input file

When you export an LS-DYNA solution, Pre/Post writes out the spot weld element information to the LS-DYNA input file using the *ELEMENT_SOLID, *CONTACT_SPOTWELD, and *SET_PART keywords. For example:

$ ------------------- ELEMENTS -------------------$*ELEMENT_SOLID$    eid     pid$     n1      n2      n3      n4      n5      n6      n7      n8      n9     n10      27       6      59      60      61      62      63      64      65      66      28       6      67      68      69      70      71      72      73      74*SET_PART         1         6*SET_PART         2         1         2*CONTACT_SPOTWELD_ID         1 PART (solid)1$Card1 ssid     msid     sstyp     mstyp    sboxid    mboxid       spr       mpr         1         2         2         2                             0         0$Card2  fs        fd        dc        vc       vdc    penchk        bt        dt                                                                                $Card3 sfs       sfm       sst       mst      sfst      sfmt       fsf       vsf

Where do I find it?

Application	Pre/Post
Prerequisite	A FEM or assembly FEM file as the work part and displayed partLS-DYNA as the specified solver
Command Finder	Universal Spot Weld Connection Connection Elements Automatic Connection Elements

Spot weld universal connection customer defaults

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

Learn more

Spot weld universal connections

Seam weld universal connections in the Nastran environment

Importing and exporting spot weld connections using wcd format

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Spot weld universal connections in the LS-DYNA 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 } });