Define a bolt pre-load for a bolt modeled with beam elements (Abaqus)

1. With the FEM file active, use the Bolt Connection command to model the bolted connection. With an Abaqus model, Bolt Connection defines the shank of the bolt as a 1D element, such as a B31 or B21 element. Bolt Connection uses Abaqus *KINEMATIC COUPLING constraints to connect the 1D element to the mesh on the surrounding part. For more information, see Modeling bolted connections and *KINEMATIC COUPLING in the Abaqus Keywords Reference Manual.

2. Switch to the Simulation file and make the appropriate solution active.

3. Choose Home tab→Loads and Conditions group→Bolt Pre-Load .

4. In the Bolt Pre-Load dialog box, select the type of bolt pre-load to create. Select Force on 1D elements to apply a concentrated load (force) to the bolt.Select Adjustment on 1D elements to apply a tightening adjustment to change the length of the bolt.

5. In the Model Objects group, click Select Object and select the elements or curves on which to create the pre-load.

6. (Optional) In the Node group, click Pre-Tension Node to select a node that is not attached to any elements in your model to serve as the pre-tension node. If you do not explicitly select a pre-tension node, the software assigns one for you automatically when you solve your model. For more information, see Defining a pre-tension node.

7. In the Magnitude group, define the pre-load force or the tightening adjustment in one of these ways:Select Expression to use a constant value or expression to define the magnitude. For more information, see Expressions. Select Field to define magnitude that varies with frequency, time, or temperature. For more information, see Using fields and expressions to define boundary conditions.

8. (Optional) Select the method to use to define the Section Normal for the bolt pre-load. The section normal controls the direction in which the software applies the bolt pre-load.Select Along Element to apply the load from the first node to the last node in the beam element's connectivity.Select User Defined to use a vector command to specify a different vector to use as the normal. For more information, see Vector dialog box.

9. Click OK.The software applies the load to the model.

How do I

Define a bolt pre-load (ANSYS)

Learn more

Bolt pre-load

Bolt pre-loads with Simcenter Nastran and Simcenter 3D Multiphysics

Pre-loaded bolts modeled with beam elements (Nastran)

Pre-loaded bolts modeled with solid elements (Nastran)

Bolt pre-loads with Abaqus

Constraining bolts to their pre-loaded lengths (Abaqus)

Pre-loaded bolts modeled with solid elements (Abaqus)

Pre-loaded bolts modeled with beam elements (Abaqus)

Bolt pre-loads with ANSYS

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Define a bolt pre-load for a bolt modeled with beam elements (Abaqus), 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 } });