Post-buckling analysis workflow (SOL 401)

Step	Summary	Detailed help topic
1.	Create the FEM and Simulation	In the New FEM and Simulation dialog box, set the solver to Simcenter Nastran and the analysis type to Structural.
2.	Specify the Simcenter Nastran solution	In the Solution dialog box, set the solution type to SOL 401 Multi-Step Nonlinear.
3.	Specify large displacement/small strain analysis	In the Solution dialog box, in the Bulk Data tab, select Large displacements (LGDISP).
4.	(Optional) Specify plasticity analysis	In the Solution dialog box, in the Bulk Data tab, select Material Nonlinearity (MATNL).
5.	Specify dependency between post-buckling solution step and the previous solution step	In the Solution Step dialog box, in the Properties group, from the Sequential Dependency on Previous Subcase list, select Yes to use the prevailing loads at the end of the previous nonlinear solution step in the post-buckling solution step. Select No to make the post-buckling solution step independent of any other solution steps.
6.	Specify arc-length method	In the Solution Step dialog box, in the Properties group, create and edit an arc-length parameters modeling object.Note: As a best practice, specify problem-specific values for initial load factor and maximum number of increments.	Nonlinear buckling in the Simcenter Nastran Multi-Step Nonlinear User's Guide
7.	(Optional) Specify contact parameters and output requests	In the Solution Step dialog box, in the Properties group, create and edit contact parameters and output request modeling objects.
8.	Specify the time for the post-buckling subcase	In the Solution Step dialog box, in the Time Step Definition group, specify the time for the post-buckling subcase.If the post-buckling subcase is the first subcase, in the End Time box, type 0.If the post-buckling subcase is not the first subcase, in the End Time box, type the end time of the subcase that immediately precedes the post-buckling subcase.Note: The Number of Increments setting is ignored in the post-buckling subcase.	Nonlinear buckling in the Simcenter Nastran Multi-Step Nonlinear User's Guide
9.	Construct the FE model	Define the material properties, meshes, loads, constraints, and so on as you would for other structural solution types.Note: Specify all loads at their maximum value.
10.	(Optional) Define initial imperfections to the geometry	In the Home tab, in the Loads and Conditions group, from the Load Type list, select Initial Imperfection . Use the options in the Initial Imperfection dialog box to perturb the locations of selected nodes.	Modeling initial imperfections
11.	Solve the model	The Solution Monitor contains information about the status of your solution, and the Simcenter Nastran .f06 output file contains the requested results from your analysis.To locate the Simcenter Nastran .f06 file, right-click the solution and select Browse.
12.	Post-process the results	Use the Post-Processing Navigator and the Results tab to manage and view the results.Note: As a best practice, if the model contains contact, set the deformation scale to 1.0. Otherwise the results may show penetration between objects.
13.	Determine the buckling load	Graph load factor vs. displacement to determine the load factor at which buckling occurs.	Graph load factor vs. displacement

How do I

Model an initial imperfection

Graph load factor vs. displacement

Learn more

Post-buckling analysis (SOL 401)

Modeling initial imperfections

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Post-buckling analysis workflow (SOL 401), 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 } });