Displaying results on beam sections

You can display stress and strain contours on selected beam cross sections.

Note:

To display stress contours on beam sections, you must have beam resultants in your results file. To calculate beam resultants, be sure to include an element force request in your solution output requests. For more information, see:

• Requesting output for Nastran analyses

• Requesting output for Abaqus analyses

Note:

You cannot create beam section displays for Simcenter Samcef analyses.

Before you can create a cross-section view, you must create a contour display of your beam model. You then select an element end from this post view to generate the cross-section view.

Tip:

As a best practice when creating beam section displays, you should set up a layout of multiple viewports, with a standard post view of your beam model in one viewport and your cross section display in another. In this way, you can interactively select different beam elements to update the cross-section view. If you have multiple post views of your model display, you select elements for cross-section displays from the Master post view. For more information, see Layouts and viewports.

You can select element ends graphically or by specifying an element ID and the fore or aft end. If your beam model contour display is of a stress or strain component, that component is used to generate the cross-section view. Otherwise, you can specify the stress or strain component using the Select Results dialog box (the title of the dialog box changes depending on the type of display selected for your cross-section view).

Tip:

When selecting element ends graphically, use the Preview check box before generating the cross-section view to quickly and efficiently interrogate your model. You can resize the Preview window as needed, and the displayed preview updates automatically as you select different locations in your model.

To generate the cross-section view, the software automatically generates an adaptive mesh on the beam section geometry and calculates stresses from element forces, material properties, and beam geometry. For more information, see Beam stresses.

The beam section mesh is displayed in the selected viewport with a standard contour display of the calculated results in the element (local) coordinate system.

Tip:

By default, the edge display in the cross-section view is set to Feature. To examine the automatically generated mesh on your beam section, in the Cross-Section View dialog box, click the Edges & Faces tab. From the Edges list, choose Wireframe.

Adding fillets to the beam section

In the Select Results dialog box for your cross-section view, you can select Add Fillets to add fillets to interior corners of your beam section geometry. To determine the fillet radius, the software multiplies the Fillet Radius Scale Factor by the minimum beam wall thickness. For example, consider the following beam section:

The minimum beam wall thickness at the interior corner is 10 mm. If the Fillet Radius Scale Factor is 0.5, the resulting fillet will have a radius of 5 mm.

The software then modifies the section geometry and remeshes the section. Adding fillets can reduce artificial stress concentrations at interior corners.

Top: Section view without fillets. Note stress concentrations at arrows. Bottom: Section view with added fillets. Artificial stresses are reduced.

Where do I find it?

Application	Pre/Post
Prerequisites	A structural analysis of a model containing beam elementsA force output request in your structural beam solution
Command Finder	Cross-Section View
Menu	Tools→Result→Cross-Section View

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

Beam stresses

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Displaying results on beam sections, 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 } });