Adhesive universal connections in the LS-DYNA environment

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

• ELEMENT_SOLID(8) elements represent the adhesive connection.

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

Defining the adhesive connection and generating the elements

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

• You can either use the Automatic Elements or Connection Elements commands to generate the actual adhesive elements from the connection definitions.If you use the Automatic Elements command, the software uses default values to create the adhesive elements.Note: You can use options on the Adhesive 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 Adhesive Element dialog box to control how the software creates the adhesive elements, such as how many layers of solid elements that the software creates across the width of the adhesive connection. For more information, see Controlling the number of layers across the width of adhesive connections.

Meshing LS-DYNA adhesive connections

The software always creates ELEMENT_SOLID(8) elements to mesh adhesive connection definitions in the LS-DYNA environment.

If you change the specified solver environment to either Nastran or Abaqus after you generate the adhesive 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_TIED_NODES_TO_SURFACE	CHEXA+RBE3 Spider(s)	C3D8+DCOUP3D Spider(s)

Mesh associated data for LS-DYNA adhesive elements

When you generate the adhesive 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_TIED_NODES_TO_SURFACE. This keyword constrains the translational degrees of freedom of the nodes associated with the physical property tables for the flanges.

• 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.If you define all adhesive connections with the same material but the adhesive definitions connect different flanges, the software writes out the *CONTACT_TIED_NODES_TO_SURFACE keyword to reference all connected flanges. During the solve, LS-DYNA determines the appropriate flange-adhesive interaction through the defined contact.

• 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 Adhesive Element dialog box. For more information on these contact-specific options, see Specifying additional LS-DYNA contact properties.

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

• Sets the material to use for the adhesive. 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 adhesives. The SECTION_SOLID option corresponds to the *SECTION_SOLID keyword.

LS-DYNA adhesive elements in the Simulation Navigator

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

Mesh for LS-DYNA adhesive elements in the Simulation Navigator

Solver syntax for LS-DYNA adhesive elements

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

$ ------------------- ELEMENTS -------------------$*ELEMENT_SOLID$    eid     pid$     n1      n2      n3      n4      n5      n6      n7      n8      n9     n10    2024      10    2138    2139    2135    2134    2140    2141    2137    2136    2025      10    2142    2143    2139    2138    2144    2145    2141    2140    2026      10    2146    2147    2143    2142    2148    2149    2145    2144    2027      10    2150    2151    2147    2146    2152    2153    2149    2148 *SET_PART         1        10*SET_PART         2         1         2*CONTACT_TIED_NODES_TO_SURFACE_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                                                                                $$ ------------------- NODES -------------------$*NODE$    nid               x               y               z      tc      rc    2134 1.501380773E+01 9.827668252E+00-2.400000000E+01       0       0    2135 1.488122518E+01-1.714528028E-01-2.400000000E+01       0       0    2136 1.501380773E+01 9.827668252E+00-3.000000000E+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	Adhesive Connection Connection Elements Automatic Connection Elements

Adhesive universal connection customer defaults

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

Learn more

Adhesive universal connections in the Nastran environment

Controlling the number of layers across the width of adhesive connections

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Adhesive 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 } });