Margin of safety overview

Simcenter 3D Margin of Safety is a solution process that allows you to use the results of a Simcenter Nastran linear static structural analysis to evaluate structural integrity on the basis of margin of safety. The Simcenter Nastran linear static structural analysis solution sequences whose results can be used in a margin of safety analysis include:

• SOL 101 linear static analysis

• SOL 144 static aeroelastic response analysis

Note:

SOL 144 static aeroelastic response analysis results can be used because the underlying structural model is linear static.

Margin of safety, MS, is defined as:

MS = \left( {\frac{{{P_f}}}{{{P_w}}}} \right) - 1

where Pf is the load at which failure initiates, and Pw is the corresponding working load.

The load at which failure initiates and the corresponding working load can be any type of result obtained from the linear static solution such as force, moment, stress, strain, deflection, and so on. For example, in a linear static solution, stress varies linearly with respect to the applied load. Thus, a valid calculation for the margin of safety is:

MS = \left( {\frac{{{\sigma _f}}}{{{\sigma _w}}}} \right) - 1

where σf is the stress at which failure initiates, and σw is the working stress.

Note:

For an example of calculating the margin of safety for results that do not vary linearly with respect to the applied load, see Custom method example.

Load at which failure initiates

The load at which failure initiates, Pf, is obtained from the following:

• A failure criterion.Failure criteria are referred to as methods. You can select from built-in methods, or you can create and use your own. The built-in methods represent a single failure mode, such as methods that predict yielding of ductile materials, buckling of columns, plates, and shells, and fastener-related failures. Methods that you create can include multiple failure modes.You select the method when you create a calculation. For more information, see Margin of safety calculations.For information on how to create and use your own methods, see Custom methods.

• Given the selected method, a definition of the value of the load at which failure initiates.For example, when you use the Tresca plane stress method, you directly define the allowable shear strength for the material. When you use Euler column buckling, you directly define the length, cross-sectional properties, end fixity, and elastic modulus for the column, which indirectly defines the critical load for the column.When you define a material property, physical dimension, or other parameter for a method, you can define it as a constant, or you can use an expression or field to define it as a function of temperature, strain, and so on.

Working load

The working load, Pw, is obtained in one of the following ways:

• From the analysis results.

• From values that you manually enter. For information, see Manual load extraction.

• From nodal force report results. For information, see Nodal force report extraction.

When you use the software to obtain a set of analysis results, the software requires the following:

• Load case sets created from the linear static subcase results. Each subcase represents a load and constraint combination for which you want to evaluate the margin of safety. For information, see Load case sets (margin of safety).

• The result type and, if applicable, the component to use.Note: The software retrieves the results from the post-processor. The post-processor reads the components of stress, force, displacement, and so on directly from the Nastran .op2 file. The post-processor calculates any derived values like von Mises stress, principal stresses, magnitude of force, magnitude of displacement, and so on from the components.

• The nodes or elements for which to retrieve the results.

From the set of results, the software extracts a single value for Pw based on options that you select. For information on how the software applies these options, see Extracting a single value from the set of results (margin of safety).

Viewing margin of safety results

When the margin of safety calculation is completed, you can examine the margin of safety results in the following ways:

• View the results in a table in the Margin of Safety dialog box.

• View annotations that display the results in the graphics window.

• View results for a specific calculation in the calculation log.

For more information, see Margin of safety results.

Margin of safety solution in the Simulation Navigator

Margin of safety solutions and their corresponding load set cases and calculations are listed in the Simulation Navigator and are associated with a parent Simulation file. Margin of safety results are stored in the parent Simulation file. When you open the parent Simulation file, any associated margin of safety solutions open as well. When you make changes to the parent Simulation file that cause the linear static analysis results to change, you must rerun the margin of safety solution so that the margin of safety results reflect the changes.

Note:

Margin of safety solutions create links to results. After you rerun a linear static solution from which you renamed or deleted subcases that the margin of safety solution uses as load cases, and you rerun the margin of safety solution, the links break. Thus, the software can no longer access the results it needs to calculate the margin of safety for these load cases. For more information on such a situation, see Orphan load cases (margin of safety).

Where do I find it?

Application	Pre/Post
Simulation Navigator	Right-click the Simulation file→New Solution Process→Margin of Safety

How do I

Create a margin of safety solution

Learn more

Margin of safety workflow

SOL 101 setup for margin of safety

Critical margin of safety expressions

Margin of safety results

Margin of safety reports

Terminating margin of safety solves

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Margin of Safety methods documentation

Margin of safety overview, 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 } });