Beam stresses

Structural FE solvers do not output a complete stress tensor for beam elements. This means that stress displays using solver stress output are incomplete, and derived results such as von Mises stress may be inaccurate.

When you first open your results in the Post Processing Navigator, if you expand the Stress – Element-Nodal or Strain – Element-Nodal nodes in the solution, all component and derived stresses are listed. This is to ensure consistent presentation of results across element types. Many components are empty; the mapping of solver stress output to Post Processing Navigator components may vary depending on the solver and element formulation. For complete and accurate stress tensor components, the software can calculate stress tensors from element forces and beam geometry.

To verify your model prior to calculating complete beam stresses, examine your model's Beam Resultants.

To calculate stress tensor components, on the Result dialog box, select the Calculate Beam Results from Forces and Beam Geometry check box. You can then use the Post Processing Navigator or the Result dialog box to navigate among complete and accurate stress or strain components and derived results. Beam stresses are also calculated automatically when you create a cross-section view.

Example: Comparing CBEAM .op2 stress results to calculated stresses

For example, the following table summarizes the stress components available for beam components for Simcenter Nastran output and stresses calculated in Post-processing. All components are in the element (local) coordinate system.

Displayed in navigator	Description	.op2 results	Calculated stresses
XX	X normal stress	Axial plus bending stress; the stress in the axial direction.	Axial plus bending stress; the stress in the axial direction.
YY	Y normal stress	No result	No result
ZZ	Z normal stress	No result	No result
XY	Shear stress on the X face in the Y direction, or shear on the Y face in the X direction	No result	Calculated results
YZ	Shear stress on the Y face in the Z direction, or shear on the Z face in the Y direction	No result	Calculated results
ZX	Shear stress on the Z face in the X direction, or shear on the X face in the Z direction	No result	Calculated results

Stress calculation process

When you request calculated beam stresses, the software:

1. Queries the results file for material properties (Young’s modulus and Poisson’s ratio) and section definition.If that information is not available in the results file, and the associated Simulation is loaded, the software queries the model for that information.If either property is temperature-dependent, it is evaluated at the ambient temperature.

2. Retrieves element force results from the current load case or iteration.

3. Generates an adaptive mesh on each section, and then computes the stress tensor at each node in the mesh. Derived components such as von Mises are also calculated for each node.For more information about how derived components for tensor data are calculated, see Vector and tensor components and invariants.

4. Retains tensors at nodes closest to the original stress recovery points.

A progress bar is displayed in the Status line while the calculation takes place. For large models containing many section definitions, the calculation may take a few moments.

How do I

Calculate beam stresses from element forces and geometry

Specify a stress recovery point

Set up a cross-section view

Learn more

Beam post-processing

Displaying results on beam sections

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Beam stresses, 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 } });