Pre-loaded bolts modeled with beam elements (Abaqus)

In Pre/Post, if you are working with Abaqus as your solver, you can model a pre-loaded bolt using B31 type beam elements. With Abaqus, you apply bolt pre-loads to your model across defined pre-tension sections. In Abaqus, a pre-tension section (specified with the *PRE-TENSION SECTION keyword in an Abaqus input file) defines the portion of the model across which the software applies the pre-load. For a bolt that you model with B31 type beam elements, the pre-tension section is comprised of:

• the beam element that defines the shank of the bolt

• a pre-tension node, which you can either select or have the software generate for you

With a B31 element, the solver reduces the pre-tension section to a point. Abaqus assumes that the pre-tension section itself is located at the last node of the element (node N2 in the graphic below) as defined by the element's connectivity. The following graphic shows an example of a bolt modeled with a beam element. (A) shows the pre-tension section, and (B) shows the pre-tension node.

Bolt modeled with a beam element

In Pre/Post, when you define a bolt pre-load for a model in which Abaqus is the specified solver, you do not explicitly create a pre-tension section. When you solve your model, the software uses the beam element and a pre-tension node to create a pre-tension section in your Abaqus input file.

For more information on pre-tension sections, see the Prescribed assembly loads topic in the Abaqus Analysis User's Manual or the *PRE-TENSION SECTION topic in the Abaqus Keywords Reference Manual.

Pre-load is applied along the normal for the pre-tension section

When you solve your model, Abaqus applies the specified bolt pre-load to the pre-tension section along the defined normal for the pre-tension section. The Section Normal option in the Bolt Pre-Load dialog box lets you control the direction of the normal for the resulting pre-tension section.

• If you select Along Element, the software computes the normal as the vector from the first node to the last node in the beam element's connectivity.

• If you select User Defined, you can use a vector command to specify a different vector to use as the normal for the pre-tension section.

Defining a pre-tension node

Abaqus uses a pre-tension node to transmit the bolt pre-load across the pre-tension section. The pre-tension node can be any node that is not connected to any element in your model. The coordinates of the pre-tension node are not important. As a best practice, however, you should allow the software to assign a pre-tension node for you. This ensures that the node meets the Abaqus criteria for a pre-tension node.

When you use the Bolt Pre-Load dialog box to define a bolt pre-load for an Abaqus analysis, you can choose to explicitly select a pre-tension node. If you do not select a pre-tension node, the software creates a new node when it writes out the Abaqus input file to serve as the pre-tension node. The software creates the new node with coordinates of (0,0,0) and assigns it a label that is equal to the current maximum node ID +1.

Constraining the pre-tension node

The pre-tension node has only one degree-of-freedom to represent the relative displacement with the pre-load in the direction of the specified vector. The software fully constrains all DOF of the pre-tension node in subsequent steps of the analysis. This allows you to maintain the initial adjustment of the bolt (pre-tension section) at their current values once the initial pre-tension has been applied. With this technique, the load across the bolt (pre-tension section) changes according to the externally applied loads to maintain equilibrium.

If you use the Bolt Pre-Load dialog box to manually designate a pre-tension node, you must ensure that the node and your model is appropriately constrained by a load or boundary condition. If you do not apply a constraint to the pre-tension node, then you must ensure that your model is constrained kinematically. If it is not, rigid body modes may occur.

Types of pre-loading supported for beam elements

• The Force on 1D elements type lets you apply a concentrated load (force) to the bolt. With the Force on 1D elements type, the software applies a concentrated load to the pre-tension node. The load is the self-equilibrating force carried across the pre-tension section. The force acts in the direction of the specified normal for the pre-tension section on the specified beam element. With this type, when you solve your model, the software uses the *CLOAD keyword to define the bolt pre-load in your Abaqus input file.For more information on the *CLOAD keyword, see the *CLOAD topic in the Abaqus Keywords Reference Manual.

• The Adjustment on 1D elements type lets you apply a tightening adjustment to the bolt. With the Adjustment on 1D elements type, the software applies a tightening adjustment of the pre-tension section by using a nonzero boundary condition at the pre-tension node. This corresponds to a change in the length of the selected beam element (bolt) in the direction of the specified normal for the pre-tension section. With this type, when you solve your model, the software uses the *BOUNDARY keyword to define the bolt pre-load in your Abaqus input file.For more information on the *BOUNDARY keyword, see the *BOUNDARY topic in the Abaqus Keywords Reference Manual.

How do I

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

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)

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

Pre-loaded bolts 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 } });