Pre-loaded bolts modeled with solid elements (Abaqus)

In Pre/Post, if you are working with Abaqus as your solver, you can model a pre-loaded bolt using continuum type solid elements. In the Bolt Pre-Load dialog box, use the Force on 3D Elements option on the Type menu to define a pre-load on solid elements.

With Abaqus, you apply a bolt pre-load across pre-tension sections that you define. The software applies the load to a pre-tension node that is associated with the pre-tension section along a vector. The following graphic shows an example of a bolt modeled with solid elements. (A) shows the pre-tension section, (B) shows the pre-tension node, and (C) shows the normal to the pre-tension section.

Figure 13-1. Bolt modeled with solid elements

Supported types of solid elements

In Pre/Post, you can use the following types of solid elements to model the bolt:

Abaqus Element Types	Description	Command Used to Generate Element in Pre/Post
C3D4, C3D4H	4-node linear tetrahedral elements	3D Tetrahedral Mesh
C3D8, C3D8H, C3D8I, C3D8IH, C3D8R, C3D8RH	8-node linear brick elements	3D Swept Mesh
C3D10, C3D10H, C3D10M, C3D10MH	10-node parabolic tetrahedral elements	3D Tetrahedral Mesh
C3D20, C3D20H	20-node parabolic brick elements	3D Swept Mesh

Note:

To specify the hybrid formulation of an Abaqus element, select the general solid element type from the Type list in the 3D Tetrahedral Mesh or the 3D Swept Mesh dialog box, such as C3D4. Then, click Mesh Associated Data and use the Element Formulation list to select Hybrid. When the software generates the mesh, it creates C3D4H elements.

Defining the pre-tension section

For a bolt modeled with solid elements, the pre-tension section is a surface inside the bolt that bisects the bolt. In the Bolt Pre-Load dialog box, with the Force on 3D Elements option, you must explicitly define the pre-tension section by selecting a Region.

When you create a Region for a pre-load definition on Abaqus solid elements, you can either select surfaces from the geometry or element faces to define the pre-tension section.

For more information about regions, see Working with reusable regions.

Note:

As a best practice, you should define the pre-tension section in the middle of the bolt.

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.

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. In general, 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.

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

The software applies the load along a vector that is normal to the pre-tension section. The Section Normal option lets you control how the software computes this vector.

• If you select Average Surface Normal, the software computes an average normal to the section that faces away from the underlying continuum elements.

• If you select User Defined, you can define the vector to specify the normal. This option is useful when the direction in which you want to apply the load is different from the average normal to the pre-tension section.

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.

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 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

Pre-loaded bolts modeled with solid 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 } });