Transient events

You create a transient durability event to perform a durability analysis on a model for which you have transient stress or strain results.

A transient durability event references the stress or strain history results from the transient solutions. The loading history is defined as an input to the solution.

For each transient durability event, you must specify the following durability settings:

• Strength criterion

• Fatigue life criterion

• Number of cycles

• Primary loading direction

• Durability analysis time range

You specify these settings in the durability objects that are referenced by the transient event.

Transient event solution support

A transient event references stress or strain results from the following Simcenter Nastran and MSC Nastran solution types:

• SOL 103 Flexible Body (Simcenter Nastran only)

• SOL 106 Nonlinear Statics — Global Constraints

• SOL 106 Nonlinear Statics — Subcase Constraints

• SOL 109 Direct Transient Response

• SOL 112 Modal Transient Response

• SOL 129 Nonlinear Transient Response

• SOL 401 Multi-Step Nonlinear (Simcenter Nastran only)

• SOL 601,106 Advanced Nonlinear Statics (Simcenter Nastran only)

• SOL 601,129 Advanced Nonlinear Transient (Simcenter Nastran only)

• SOL 701 Explicit Advanced Nonlinear Analysis (Simcenter Nastran only)

From the Response Dynamics solution process, a transient event references one of the following:

• Linear stress or strain results stored in RS2 files.

• Modal response results stored in EEF files.

Notes on Response Dynamics solution process and durability

Creating, editing, and solving transient events based on Response Dynamics solution process with large number of iterations could result in slow performance. On a 32-bit machine with less than 8 GB of RAM, you can get out-of-memory errors.

For the Response Dynamics solution process, you can save geometry information with the results in the RS2 file. To do this, select the Save Geometry with Event Results check box in the Settings group in either the New Event dialog box or the Edit Event dialog box.

When a transient event references an RS2 file that does not contain geometry information, the durability analysis is performed over all iterations of the stress or strain histories. The Output Start Time and Output End Time boxes on the Data Control tab in the Transient Durability Event dialog box, are unavailable.

When you edit pre-NX 7.5.2 durability transient events based on Response Dynamics events whose RS2 file also contains geometry, the software does not automatically retrieve the time domain of the Response Dynamics event. You need to specify valid Start Time and End Time values on the Data Control tab in the Transient Durability Event dialog box.

When you perform a durability analysis on modal response results from a Response Dynamics solution process event, the durability solver computes the stress or strain histories using the following:

• The modal response from the EEF file.

• The stress or strain modes from the SOL 103 Response Dynamics OP2 file. The OP2 file stores the results from the parent solution of the Response Dynamics solution process event.

For some models, performing a durability analysis on modal response results is faster than directly reading the stress or strain histories from the RS2 file.

Flexible multibody durability analysis

In the Solution dialog box, on the Case Control page, from the Flexible Body Solution Type list, you can select:

• Recover to create a Simcenter Nastran SOL 103 Flexible Body solution with recovery option.

• Export to create a Simcenter Nastran SOL 103 Flexible Body solution with export option.

The OP2 file size for solutions with recovery option is larger than for solutions with export option.

When you select a Simcenter Nastran SOL 103 Flexible Body solution for your transient durability event:

• If the solution has the recovery option, the OP2 file contains all the necessary stress or strain histories that are required to perform the durability analysis directly.

• If the solution has the export option, the OP2 file contains only mode shapes. The modal displacement history results from the multibody dynamics solver are stored in the MDF file. You must specify the MDF file in the Transient Durability Event dialog box.For each element node, the durability solver recovers stress and strain histories by scaling the modal displacement histories with mode shapes. The computed stress and strain histories are then used to perform the durability analysis.

Where do I find it?

Application	Pre/Post
Prerequisite	A transient structural solution
Command Finder	Transient Event
Simulation Navigator	Right-click the Durability solution process node→New Event→Transient

How do I

Create a transient durability event

Learn more

Durability objects

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Transient events, 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 } });