Modeling spot welds for LS-DYNA

In the LS-DYNA environment, you can manually create spot weld connections between parts (sets of 2D elements). In LS-DYNA:

• You use the *CONTACT_SPOTWELD keyword to model spot weld connections between two or more layers, typically sheet metal layers. The layers should be parallel or nearly parallel.

• You can use the *MAT_SPOTWELD keyword to define the material properties for the spot weld.

Modeling the spot weld connection

You can use the *CONTACT_SPOTWELD keyword to define a contact pair between 2D elements, which define the master part, and 3D elements or 1D elements, which define the slave part. You can use different configurations of solid elements to create the spot weld connection. For example:

• A spot weld represented by multiple solid elements, such as a cluster of four hexagonal elements (ELEMENT_SOLID(8)), that share nodes with the shell elements on the slave part.

• A spot weld represented by multiple solid elements, such as a cluster of four hexagonal elements (ELEMENT_SOLID(8)), that does not share nodes with the shell elements on the slave part.

• A spot weld represented by a single solid element that does not share nodes with the shell elements on the slave part.

• A spot weld represented by one or more 1D beam elements (ELEMENT_BEAM).

Defining the parts to connect with the spot weld (master parts)

The master parts are the parts connected by the spot weld. The spot weld is the slave part in the contact definition.

To define the master parts to connect, you can create the 2D meshes and associate them with a PART (shell) or a PART (laminate shell) physical property table.

• The Label field corresponds to the ID of the *PART or *PART_COMPOSITE keyword.

• When you export or solve the solution, the software uses the*SET_PART keyword to group the physical property tables referenced by the *CONTACT_SPOTWELD keyword.

Defining the spot weld connection (slave part)

To define the slave part that represents the spot weld, you create a 3D mesh or a 1D mesh.

• In the Mesh Associated Data dialog box for the 3D mesh or 1D mesh, select CONTACT_SPOTWELD from the Connection Options list. Then use the LS-DYNA Parts for masters option to select the PART (shell) or a PART (laminate shell) physical property tables to connect. When you export or solve the model, Pre/Post writes out the *CONTACT_SPOTWELD keyword. You can also use the CARD2/CARD3, CARDA/CARDB (optional), and Massively Parallel Processing Option (MPP) options to define additional contact properties for the solution. For more information, see Specifying additional LS-DYNA contact properties.

• You must associate the 3D mesh with a PART (solid) physical property table or the 1D mesh with a PART (beam). physical property table. The Label field corresponds to the ID of the *PART keyword.

• When you export or solve the solution, the software writes out one *CONTACT_SPOTWELD keyword for each PART (solid) or PART (beam) label (ID) in the model. If a single PART (solid) or PART (beam) table is referenced in multiple mesh collectors, the software exports multiple *CONTACT_SPOTWELD keywords with the same slave part ID.

Defining the material for the spot weld

In LS-DYNA, you use the *MAT_SPOTWELD keyword to define the material properties of the spot weld. In Pre/Post:

• In the Isotropic Materials dialog box, you can select **LS-DYNA MAT_SPOTWELD (MAT_100) from the Property View filter to display only the relevant, supported material properties for the *MAT_SPOTWELD keyword.

• In the Part (Solid) or Part (Beam) physical property table dialog box for the spot weld elements, you use the Material Option options to assign the material to the physical property table dialog box, specify the keyword to use to export the material properties, and also define additional properties for the *MAT_SPOTWELD keyword. Select the Use Pre/Post Material check box .Select the material that you created in the Isotropic Materials dialog box from the Pre/Post Material list.Select **MAT_SPOTWELD (MAT_100) from the Material Type list to have the software write out the material properties to the *MAT_SPOTWELD keyword during the export process.Use the *Additional MAT_SPOTWELD Properties option to specify specific material properties for the *MAT_SPOTWELD keyword that are not supported in the Isotropic Materials dialog box, such as the Axial force resultant (NRR) value.Note: Pre/Post does not currently export the DAMAGE-FAILURE option for the *MAT_SPOTWELD keyword.For more information on materials and material properties for LS-DYNA, see Defining material properties for LS-DYNA materials.

Where do I find it?

Mesh Associated Data command

Application	Pre/Post
Prerequisite	A FEM file as the work part and displayed partLS-DYNA as the specified solver
Command Finder	Mesh Associated Data

Physical Properties command

Application	Pre/Post
Prerequisite	A Simulation file as the work part and displayed partLS-DYNA as the specified solver
Command Finder	Physical Properties

Modeling Objects command

Application	Pre/Post
Prerequisite	A FEM or Simulation file as the work part and displayed partLS-DYNA as the specified solver
Command Finder	Modeling Objects

Look up more details

LS-DYNA elements

Defining constrained joint connections for LS-DYNA models

Manually creating connections in LS-DYNA models

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Modeling spot welds for LS-DYNA, 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 } });