Bolt pre-loads with ANSYS

If you are working with the ANSYS solver, you can use the Bolt Pre-Load command to apply a load to a bolt (or fastener).

Creating an appropriate mesh for analyzing pre-loaded bolts

In ANSYS, axial pretension within the bolt shank can be modeled with the PRETS179 pretension element. To solve a model in ANSYS that contains pre-loaded bolts, the regions of the model that are connected by the PRETS179 elements must have matching meshes with coincident nodes.

In Pre/Post, you can use the Mesh Mating Condition command with the Free Coincident type to ensure that the meshes to connect with the PRETS179 elements match. With the Free Coincident type, the software aligns the meshes but does not generate any connection elements. You can then use the 1D Mesh to generate PRETS179 elements between the pairs of coincident nodes.

Note:

If you use the Split Body command to divide the bodies in your model, the software automatically creates a Glue Coincident type mesh mating condition at the location of the split.

Key ANSYS bolt pre-load concepts

With ANSYS, you apply bolt pre-loads to your model across defined “pre-tension sections.” In ANSYS, a pre-tension section is specified with the SECDATA command (using the PRETENSION type option) in an ANSYS input file. It defines the portion of the model across which the software applies the pre-load. A pre-tension section is comprised of:

• The PRETS179 elements that define the bolts or fasteners themselves.

• A “pre-tension” node that the software uses to control and monitor the total tension loads.

In ANSYS, loads are then applied to the pre-tension section with the SLOAD command.

Defining the pre-tension section options

In Pre/Post, you specify the options for the SECDATA command that defines the pre-tension section in the physical property table for the PRETS179 elements that define the bolt. The options in the Pretension Node (SECDATA) group in the Mesh Associated Data dialog box let you select both a pre-tension node and define a vector that controls the direction in which the software applies the load.

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. However, the pre-tension node must use the global Cartesian coordinate system as its nodal coordinate system. For more information on ANSYS pre-tension nodes, see the PRETS179 topic in the ANSYS Element Reference manual.

Defining the bolt pre-load options

In Pre/Post, you can specify the options for the SLOAD command in two different places:

• In the Pretension load (SLOAD0 group in the PRETS179 physical property table dialog box.

• In the Bolt Pre-Load dialog box.

The PRETS179 physical property table dialog box gives you access to a slightly expanded set of SLOAD options than the Bolt Pre-Load dialog box. The key differences are:

• With the Bolt Pre-Load dialog box, the software always applies the defined load to the active load step. With the PRETS179 physical property table dialog box, you can use the LSLOAD option to specify the load step to which the software applies the load.

• With the Bolt Pre-Load dialog box, if you choose LOCK as the KINIT option, the software automatically applies the lock to the next load step. With the PRETS179 dialog box, you can use the LSLOCK option to specify the load step in which the software locks the value of the load.

Though the PRETS179 dialog box lets you specify more options for the ANSYS LSLOAD command, it only allows you to create a single LSLOAD command for a given set of PRETS179 elements. That means you can only use it to apply a single bolt-preload to a given set of elements within a given load step. The Bolt Pre-Load dialog box, in contrast, allows you to apply either a single LSLOAD command or multiple LSLOAD commands to the same set of PRETS179 elements. This is helpful if you want to define multiple sequences of bolt pre-loads within a single analysis.

Note:

If you use both the LSLOAD options on the PRETS179 dialog box and the Bolt Pre-Load dialog box to define a bolt pre-load for the same set of PRETS179 elements, the load defined with the Bolt Pre-Load takes precedence.

For more information, see Defining Pretension in a Joint Fastener in the ANSYS Basic Analysis Guide and LSLOAD in the ANSYS Commands Reference manual.

Types of pre-loading supported

When you are working in the ANSYS environment, you create two different kinds of bolt pre-loading conditions: either a force or a length adjustment (displacement). If you define the bolt pre-load from the PRETS179 dialog box, the KFD option controls whether the pre-load is a force or a displacement. If you define the bolt pre-load from the Bolt Pre-Load dialog box, the Type option controls whether the pre-load is a force or displacement.

• The Force on 1D elements type lets you apply a concentrated load (force) to the bolt. In ANSYS, this sets the KFD option on the SLOAD command to FORC.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 PRETS179 element. ANSYS applies the Force on 1D elements type as a “ramped” type load in which the load value for a given substep is linearly interpolated from the values of the previous load step.

• The Adjustment on 1D elements type lets you apply a tightening adjustment to the bolt. In ANSYS, this sets the KFD option on the SLOAD command to DISP.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. ANSYS applies the Adjustment on 1D elements type as a “stepped” type load. With a stepped load, the software step changes the load at the first substep of the load step to the values of the current load step (i.e., the software uses the same values for all substeps).

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)

Pre-loaded bolts modeled with beam elements (Abaqus)

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Bolt pre-loads with ANSYS, 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 } });