Meshing LS-DYNA bolt connections with rigid body elements

In the LS-DYNA environment, when you generate bolt elements from bolt universal connection definitions, you can select the CONSTRAINED_NODAL_RIGID_BODY Spider(s) option to model the bolts with rigid body elements.

Meshing a bolt connection with the CONSTRAINED_NODAL_RIGID_BODY Spider(s) option

When you generate bolt elements with the CONSTRAINED_NODAL_RIGID_BODY Spider(s) option, the software creates spider-like rigid body elements and connects the legs of the elements to the nodes on the target flanges. When you export the solution, uses the *SET_NODE keyword to write out the pairs of connected nodes.

The following example shows a bolt with CONSTRAINED_NODAL_RIGID_BODY Spider(s) option that connects three parallel plates meshed with 2D elements. The CONSTRAINED_NODAL_RIGID_BODY Spider(s) elements connect to the nodes around the bolt hole on each plate.

Bolt meshed with the CONSTRAINED_NODAL_RIGID_BODY Spider(s) option	Side view of the CONSTRAINED_NODAL_RIGID_BODY Spider(s) bolt element

Mesh associated data for the CONSTRAINED_NODAL_RIGID_BODY Spider(s) option

When you generate bolt connection elements, the software automatically defines the mesh associated data for the elements. In the Mesh Associated Data dialog box, the software sets the Displacement Release Flag (DRFLAG) and Rotational Release Flag (RRFLAG) options to (0) Off for rigid body behavior.

You can edit the mesh associated data to modify these values or to select additional options. For example, you can use the Optional Properties list to specify a Constrained Nodal Rigid Body Optional modeling object to define optional properties for the rigid body, such as inertia properties, or to select a node to use for post processing rigid body results.

CONSTRAINED_NODAL_RIGID_BODY elements in the Simulation Navigator

The software stores the bolt connection elements as a new mesh in a CONSTRAINED_NODAL_RIGID_BODY Collector entry in the 1D Collectors node in the Simulation Navigator.

Meshes for LS-DYNA bolt elements (CONSTRAINED_NODAL_RIGID_BODY Spider(s) option) in the Simulation Navigator

Solver syntax for CONSTRAINED_NODAL_RIGID_BODY elements

When you export an LS-DYNA solution, the software uses the *CONSTRAINED_NODAL_RIGID_BODY and *SET_NODE keywords to write out the data for CONSTRAINED_NODAL_RIGID_BODY elements. For example:

$ ------------------- ELEMENTS -------------------$$$ -------------- CONSTRAINED KEYWORDS (from FEM) --------------*SET_NODE         4      2128       404       405       406       407       408       409       410       414       415       416       417       418       419       492       493       494       495       496       497       498       499       500       501       502       503       504       505       506       507       945       946       947       948       949       950       951       952       953       954       955       956       957       958       959      1345      1346      1347      1348      1349      1363      1364      1365      1366      1487      1488      1489      1490      1491      1492      1493      1494      1495      1496      1497      1498      1499      1500      1501      1502      1503      1504      1505      1506      1507      1508      1627      1697      1716      1755      1756      1762      1763      1804      1805      1806      1807      1808      1809      1855      1856      1857      1858*CONSTRAINED_NODAL_RIGID_BODY_TITLEBolt Element(12)$Card1 pid       cid      nsid     pnode      iprt    drflag    rrflag         4         0         4         0         1         0         0$

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	Universal Bolt Connection Connection Elements Automatic Connection Elements

Bolt universal connection customer defaults

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

How do I

Simulate a bolt preload in ANSYS using universal bolt connections

Create large quantities of bolts in one connection

Learn more

Bolt universal connections

Override the length of bolt shanks

Extending the legs of spider elements in bolt connections

Bolt universal connections in the Nastran environment

Bolt universal connections in the LS-DYNA environment

Meshing LS-DYNA bolt connections rigid body and beam elements

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Meshing LS-DYNA bolt connections with rigid body elements, 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 } });