Clinch universal connections in the LS-DYNA environment

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

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

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

Defining the clinch connection and generating the elements

• You can use the Clinch Connection command to specify the definition for the clinch 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 diameter of the connection and the clinch material.

• You can use either the Automatic Elements or Connection Elements commands to generate the actual clinch elements from the connection definitions.If you use the Automatic Elements command, the software uses default values to create the clinch elements.Note: You can use options on the Clinch 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 Clinch Element dialog box to control how the software creates the clinch elements, such as the CARD2/CARD3 modeling object to use to specify required contact properties for the connection.

Generating the clinch connection elements

When you generate the clinch elements from the Clinch Connection definition, the software uses one or more ELEMENT SOLID(8) elements to represent the connection.

If you change the specified solver environment to Nastran 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
ELEMENT_SOLID(8)+CONTACT_SPOTWELD	CHEXA+RBE3 Spider(s)

Mesh associated data for LS-DYNA spot weld elements

When you generate the clinch 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 (solid) 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 Clinch Element dialog box. For more information on these contact-specific options, see Specifying additional LS-DYNA contact properties.

Physical property data for LS-DYNA clinch 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 clinch connections. In the PART(solid) dialog box, the software automatically:

• Sets the material to use for the clinch 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 clinch connections. The SECTION_SOLID option corresponds to the *SECTION_SOLID keyword.

LS-DYNA clinch connections in the Simulation Navigator

The software stores the clinch 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 clinch connection definitions that use different materials, the software places the elements into separate meshes in different PART (solid) entries.

Meshes for LS-DYNA clinch elements in the Simulation Navigator

Clinch connections in the LS-DYNA input file

When you export an LS-DYNA solution, Pre/Post writes out the clinch 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    2063      12    2234    2235    2236    2237    2238    2239    2240    2241*SET_PART         1        12*SET_PART         2         1         2*CONTACT_SPOTWELD_ID         1 PART (solid)2$Card1 ssid     msid     sstyp     mstyp    sboxid    mboxid       spr       mpr         1         2         2         2                             0         0$Card2  fs        fd        dc        vc       vdc    penchk        bt        dt                                                                                $Card3 sfs       sfm       sst       mst      sfst      sfmt       fsf       vsf                                                                                $$ ------------------- NODES -------------------$*NODE$    nid               x               y               z      tc      rc    2234 3.675313118E+01 5.396685902E+01-2.400000000E+01       0       0    2235 3.409445040E+01 5.396685902E+01-2.400000000E+01       0       0    2236 3.409445040E+01 5.662553980E+01-2.400000000E+01       0       0    2237 3.675313118E+01 5.662553980E+01-2.400000000E+01       0       0    2238 3.675313118E+01 5.396685902E+01-3.000000000E+01       0       0    2239 3.409445040E+01 5.396685902E+01-3.000000000E+01       0       0    2240 3.409445040E+01 5.662553980E+01-3.000000000E+01       0       0    2241 3.675313118E+01 5.662553980E+01-3.000000000E+01       0       0

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	Clinch Connection Connection Elements Automatic Connection Elements

Clinch universal connection customer defaults

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

How do I

Realize (mesh) universal connections

Create and edit universal connections

Learn more

Universal connections

Managing element-associated data for universal connections (Abaqus)

Local spider element targets in universal connections

Bearing universal connection for rotor dynamics (SOL 414)

Using bushing universal connections in rotor dynamics (SOL 414)

Look up more details

Universal connection elements

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Clinch 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 } });