Pre-loaded bolts modeled with solid elements (Nastran)

In the Bolt Pre-Load dialog box, you can use the Force on 3D elements option to define a pre-load on a bolt that is modeled with CHEDA, CPENTA, or CTETRA type of solid elements.

Selecting the nodes that define the cross section on the bolt

With the Force on 3D Elements option, you must select a series of nodes that define a cut through the bolt at any location (1) on the interior of the bolt. You then specify a coordinate system and axis that Simcenter Nastran uses to define the axis of the bolt (2).

Note:

If you select one or more polygon faces to define the cut through the bolt, the software uses all of the nodes associated with those faces to define the cut.

• You cannot use the Pressure command to apply a pressure to the face of an element if the connectivity of the element includes any of the nodes you select to define the Force on 3D Elements option.

• The nodes that you select to define the Force on 3D Elements cannot be used to define the connectivity of solid composite elements.

Understanding the bolt pre-load calculation process for solid elements

• Simcenter Nastran first splits the mesh on the bolt by:Duplicating each node you selected to define the Force on 3D Elements option. The labels (IDs) for the duplicated nodes start at the highest user-defined node label in the model plus one and continue sequentially higher.Modifying the element connectivity on one side of the cross section to use the new duplicate nodes.Note: Simcenter Nastran writes the new nodes and updated element connectivity are written to the .op2 file. Additionally, these are visible when you post- process the results.

• Simcenter Nastran adds a weak spring between each pair of nodes with stiffness in the bolt’s axial direction. The spring stiffness is calculated as EA/(LBOLTFACTN), where E is the modulus of the bolt material, A is the projected area of the bolt cut, L is an approximate bolt length, BOLTFACT is a parameter, and N is the number of nodes you selected to define theForce on 3D Elements option.Note: In Pre/Post, you can modify the value of the BOLTFACT parameter through the Solution Parameters modeling object. From the Modeling Object Manager dialog box, select Solution Parameters from the Type list. In the Solution Parameters dialog box, expand the A-B group and then scroll down to the BOLTFACT parameter.

• Simcenter Nastran determines the projected area of the solid elements using the nodes, coordinate system, and axis you selected in the Bolt Pre-Load dialog box. Simcenter Nastran uses this area to apply the equivalent bolt pre-load as two equal and opposite face tractions in the bolt axial direction.

• Simcenter Nastran runs an initial solution with only these face tractions applied to obtain the deflection at the bolt’s cross section due to the bolt pre-load. Simcenter Nastran uses these deflections to calculate the initial strain in the bolt.

• Simcenter Nastran then runs a second solution with:The initial strain applied.The springs removed.The service loads applied (if you have included any service loads in the analysis).

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)

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

Pre-loaded bolts modeled with solid elements (Nastran), 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 } });