Rahul Ponginan 279 Report post Posted February 19, 2015 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 Quote Share this post Link to post Share on other sites

Rahul Ponginan 279 Report post Posted February 19, 2015 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 Quote Share this post Link to post Share on other sites

narasimhamurthy 0 Report post Posted June 11, 2015 Hi, can we do nonlinear buckling analysis in optistruct. i didnt get any optistruct tutorials on nonlinear buckling analysis. so.. thank you Quote Share this post Link to post Share on other sites

Guest Report post Posted June 11, 2015 Hi NarasimhaMurthy, You can use RADIOSS (Block) to solve Non linear buckling problems. Please refer to RADIOSS Example 38 - Buckling of L-Shaped Beam Quote Share this post Link to post Share on other sites

Rahul R 336 Report post Posted June 11, 2015 Hi, Currently Optistruct uses Radioss implicit features to carry out nonlinear buckling analysis.Please find attached examples of the same. RegardsRahul RPost_Buckling.zip Quote Share this post Link to post Share on other sites

msc 1 Report post Posted June 6, 2016 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? Quote Share this post Link to post Share on other sites

Rahul R 336 Report post Posted June 7, 2016 see reply in below post. Quote Share this post Link to post Share on other sites

Brian DO 0 Report post Posted May 15 So, How to do nonlinear buckling or post buckling analysis in Optitruct ? Thanks advanced Quote Share this post Link to post Share on other sites

Simon Križnik 335 Report post Posted May 15 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. Buckling.pdf1.46 MB · 130 downloads 2_2_snap_roof___implicit.pdf663.71 kB · 105 downloads 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 RD-T_ 3030 Buckling of a Tube Using Half Tube Mesh.pdfUnavailable RD-T_ 3530 Buckling of a Tube Using Half Tube Mesh.pdfUnavailable RD-E_ 0300 S-Beam Crash.pdfUnavailable Brian DO likes this Quote Share this post Link to post Share on other sites

Brian DO 0 Report post Posted May 21 On 5/16/2020 at 2:50 AM, Simon Križnik 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. Buckling.pdf1.46 MB · 130 downloads 2_2_snap_roof___implicit.pdf663.71 kB · 105 downloads 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 RD-T_ 3030 Buckling of a Tube Using Half Tube Mesh.pdfUnavailable RD-T_ 3530 Buckling of a Tube Using Half Tube Mesh.pdfUnavailable RD-E_ 0300 S-Beam Crash.pdfUnavailable Thanks Simon Križnik I will do it with your guide. Quote Share this post Link to post Share on other sites

Adriano A. Koga 82 Report post Posted June 3 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). Simon Križnik likes this Quote Share this post Link to post Share on other sites