Linear Buckling Analysis

Rahul_P1

Hello,
We are new to that topic and want to make a linear buckling analysis, but we don’t know, how to interpret the results in hyperview. Is it critical, when the magnitude of the buckling mode is higher than one? How can we figure out the safety factor?
What does the number at “Mode 1 – F = 2.519563E+00” or “Mode 2 – F = 2.655379E+00” in the dropdown on the left mean?
Thank you for your help

Rahul_P1

Hello,

the number of the mode can be interpreted as a safety factor vs. buckling. So a value of 2.5 means, that 2.5 times the applied load will lead to buckling failure. You can look up 'Linear Buckling Analysis' in the OptiStruct help for a more detailed explanation.

Jan

narasimhamurthy

Hi,

 

can we do nonlinear buckling analysis in optistruct. i didnt get any optistruct tutorials on nonlinear buckling analysis. so..

 

 

 

 thank you

Altair Forum User

Hi NarasimhaMurthy,

 

You can use RADIOSS (Block) to solve Non linear buckling problems.

 

Please refer to RADIOSS Example 38 - Buckling of L-Shaped Beam

Rahul Rajan_21763

Hi,

 

Currently Optistruct uses Radioss implicit features to carry out nonlinear buckling analysis.

Please find attached examples of the same.

 

Regards

Rahul R

Unable to find an attachment - read this blog

Altair Forum User

Is it possible in OptiStruct to run a linear buckling analysis and to apply selected buckling modes with a scaling factor as initial deformation or imperfection for a non-linear analysis like in Abaqus?

Rahul Rajan_21763

see reply in below post.

 

Brian DO_20786

So, How to do nonlinear buckling or post buckling analysis  in Optitruct ?

Thanks advanced

Simon Križnik

Hi,

 

While nonlinear buckling could be done in Optistruct, it is very is likely the implicit solver will experience convergence difficulties resulting in long run times or even fail due to nonconvergence. Alternatively use Radioss integration to solve your model with the explicit method in Optistruct.

 

Therefore I suggest using Radioss explicit solver instead following this procedure:
1.perform modal analysis in Optistruct
2.in postprocessing create a derived load case>linear superposition>use small scale factor (1e-2 to 1e-3)

3.export the deformed shaped.

4. import the deformed shape into Hypermesh Radioss user profile and set up non-linear buckling analysis.

 

By using the deformed shape obtained from the modal analysis the structure will have geometry imperfection triggering a buckling pattern consistent with modal and linear buckling analysis.

 

Nonlinear buckling analysis is recommended to be performed within Radioss. Post buckling can be solved using nonlinear geometry (Implicit) loadcase. Use any of the Arc-Length methods to solve post-buckling analysis.

 

There are two tutorials and one example on NL buckling: 

• RD-T: 3030 Buckling of a Tube Using Half Tube Mesh (Hypercrash)
• RD-T: 3530 Buckling of a Tube Using Half Tube Mesh (Hypermesh)
• RD-E: 0300 S-Beam Crash

Unable to find an attachment - read this blog

Brian DO_20786

Altair Forum User said:

Hi,

 

While nonlinear buckling could be done in Optistruct, it is very is likely the implicit solver will experience convergence difficulties resulting in long run times or even fail due to nonconvergence. Alternatively use Radioss integration to solve your model with the explicit method in Optistruct.

 

Therefore I suggest using Radioss explicit solver instead following this procedure:
1.perform modal analysis in Optistruct
2.in postprocessing create a derived load case>linear superposition>use small scale factor (1e-2 to 1e-3)

3.export the deformed shaped.

4. import the deformed shape into Hypermesh Radioss user profile and set up non-linear buckling analysis.

 

By using the deformed shape obtained from the modal analysis the structure will have geometry imperfection triggering a buckling pattern consistent with modal and linear buckling analysis.

 

Nonlinear buckling analysis is recommended to be performed within Radioss. Post buckling can be solved using nonlinear geometry (Implicit) loadcase. Use any of the Arc-Length methods to solve post-buckling analysis.

 

There are two tutorials and one example on NL buckling: 

• RD-T: 3030 Buckling of a Tube Using Half Tube Mesh (Hypercrash)
• RD-T: 3530 Buckling of a Tube Using Half Tube Mesh (Hypermesh)
• RD-E: 0300 S-Beam Crash

Thanks  Simon Križnik

 

I will do it with your guide.

Unable to find an attachment - read this blog

Adriano A. Koga

just highlighting a couple enhancements on this, extracted from RElease notes.

OS 2019.0 brought RIKS method for helping these unstable snap-trhu behavior.

 

OS 2019.1

Imperfection

An imperfection can be applied to the model.

Note: Only supported for Nonlinear Analysis.

The IMPERF Bulk Data and Subcase Entries can be used to apply an imperfection. An imperfection can be introduced into the model in the following ways:

• TYPE=H3DRES on IMPERF Bulk Data: An h3d file is referenced which contains previously completed analysis results.
• TYPE=GRID on IMPERF Bulk Data: The perturbation of grids can be directly applied.

 

 

OS 2019.0

 

Snap-thru with Arc-Length method

The Arc-Length method has been implemented to solve snap-thru problems in nonlinear analysis. Solution control is available thru the NLPCI Bulk Entry and three methods (Crisfield, Riks, and Modified Riks).