turn on suggestions

Auto-suggest helps you quickly narrow down your search results by suggesting possible matches as you type.

Showing results for

- Navigation
- Simcenter
- Forums
- Blogs
- Knowledge Bases

- Siemens PLM Community
- Simcenter
- 3D Simulation - Simcenter 3D Forum
- Non-linear buckling

Options

- Subscribe to RSS Feed
- Mark Topic as New
- Mark Topic as Read
- Float this Topic for Current User
- Bookmark
- Subscribe
- Printer Friendly Page

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Highlight
- Email to a Friend
- Report Inappropriate Content

11-16-2016 07:42 AM

Hi all,

I faced some problem with non-linear analysis.

What is the backround: I performed linear buckling analysis (SOL 105) where I got the shape and place of predicted stability failure for certain plate. Now for this specific failure mode I would like to perform non linear investigation and check what will happen when the 'buckled' structure will be loaded with nominal loads.

What I did:

for the mentioned plate I exported the field of displacements and applied it in non-linear analysis as enforced displacement in order to obtain 'initial deformation' of the structure, which later I want to load (in next subcase) with nominal loads.

What is the problem:

This initial deformation, according to Eurocode 3 has to be multiplied by the factor that depends on the plate main dimensions and it looks that the local deformation of the plate that I have to apply is equat to 3.7mm, which seems to be too much, becasue Nastran gives me an error that the load increment shall be reduced. In this moment increment is set to 1% so it should be small enough.

When I start the similuation (SOL 106) subcase 1: wich contains only the inintial deformation of the structure, the solution crashes.

REDUCE THE LOAD INCREMENT BY A FACTOR OF 5.93 FOR BETTER SOLUTION . *** USER WARNING MESSAGE 4675 (NMEPD) EXCESSIVE INCREMENTAL LOAD IS APPLIED IN ELEMENT ID = 230971 REDUCE THE LOAD INCREMENT BY A FACTOR OF 2.55 FOR BETTER SOLUTION . *** USER FATAL MESSAGE 4676 (NMEPD) ERROR EXCEEDS 20.00 PERCENT OF YIELD STRESS IN ELEMENT ID= 230971

And now the questions:

- is enforced displacement a good idea in order to obtain initial deformation of the structure when performing non-linear buckling? Are there any predefined functions of applying such deformations?

- do you have any tips and tricks of doing non-linear buckling analysis? I would really appreciate them.

- I can see that for each subcase in SOL106 I can set the buckling analysis. Is this what I am looking for ?

Best Regards

Tomasz.

Labels:

8 REPLIES

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Highlight
- Email to a Friend
- Report Inappropriate Content

11-19-2016 07:46 AM - edited 11-19-2016 09:18 AM

Hi again,

Above problem makes me frustrated, so I prepared an example.

The model is as follows:

- tower made of CBEAM elements

- elastic - perfectly plastic material is used for all the elements (S235)

- fixed on the bottom

- loaded vertically on the top

- 2 analysis are set up: SOL105 and SOL106.

According to this video all should be ok and indeed, for SOL106 the output is:

No errors or warnings found in NASTRAN output file.

For Linear buckling, Nastran calculates factof for buckling (first critical) = 0.6151

When the same load is applied to SOL106, nothing happens, all 10 increments are passed throuh and buckling seems to to be a problem. What I miss in the non linear solution setup?

And second question. In nonlinear solution subcase there is Eigenvalue Analysis option where buckling can be selected. What is this for and what's the difference between SOL105 ?

What is the most strange, even if the load is increased and beams should plastify, such effect is not take into account, meaning none nonlinear stress are visible in the results.

What is wrong ?

When it comes to the first post, I managed to do second example with applicaiton of initial deformation for non-linear analysis, however need another solution.

For some plates of the structure (marked below) I applied enforced displacement (which were an output from the linear buckling solution), which are scaled according to EN 1997-5-1. But such approach seems to be not correct, since when the 'innitial deformations' are applied, later they are 'not changeable' meaning, I am not able to deform them more by appplying nominal loads. As you can see on the upper part of the screenshot, the deformations on the 'part under consideration' can not be later 'deformed', so there is a clear border where the influence of the 'initial deformation' and external load acts.

So then, how to use such fieled of dislpacement in further analysis together with external loads in a way that they can 'work together' on all the structure?

Please help.

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Highlight
- Email to a Friend
- Report Inappropriate Content

11-21-2016 03:55 AM

Hi,

maybe the "__enforced__ displacements" are the problem? Shouldn't you rather work with "__initial__ displacements"?

The linear buckling simulation gives you deformations how the structure might buckle (with unknown amplitudes of the buckling modes and unknown orientations of the modes). Are you "enforcing" these displacements by prescibing them? This would make the structure "rigid" as all displacements are prescribed.

I rather propose to __modify the initial geometry__ in the nonlinear case with the appropriatley scaled buckling modes shapes and then run a nonlinear analysis in a single load case!

The reason why this is done is to convert a "branching" of the load-deflection-curve which often yields to non-convergence into a numerically more friendly analysis without branching by guing the analysis into a certain load-deflection branch.

Hope this helps!

Another problem can happen if the plasticity occurs in the nonlinear analysis already before the "linear" buckling load is reached. That would make the linear buckling load and mode shapes meaningless.

Best regards.

Martin

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Highlight
- Email to a Friend
- Report Inappropriate Content

11-21-2016 08:09 AM

I understand your point. that's true that enforced displacemenet makes my structure 'rigid' and non-deflectable. So the question is how to do it another way ?

If I will modify my initial geometry I will loose the internal forces in the structure, that will occur in the structure before achieving desired linear buckling mode (appropriately scaled shape). That's why I need some solution, how in SOL_106 deflect the structure to desire shape and further load it and see what will happen with it when the nominal load will still act. Whether plastic hinges will occur or not?

And second thing, is there something wrong with setup of the 'tower example', why it does not buckle in SOL106 and on example from femap (video linked above) it works ?

As far as I know, the NX Nastran is the same in both programs, so there should be no limitation in NX.

Any Ideas ?

Thanks for help

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Highlight
- Email to a Friend
- Report Inappropriate Content

11-21-2016 09:46 AM

Hi,

try "initial imperfection" for the buckling modes instead of using presribed displacements. You will not have internal forces in the structure initially as you do not need those. By the initial imperfection you change the buckling problem from a bifurcation problem into unique solution problem. After the buckling occurs you might need the arc length method for convergence reasons.

Best regards.

Martin

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Highlight
- Email to a Friend
- Report Inappropriate Content

11-21-2016 02:08 PM

I will try this, but can you advise me some quick procedure how to do this ?

Only one thing I have on my mind of doing this is to export the deformed mesh grid ? But then I will loose association of the loads with geometry.

I will really appreciate if you can help me with this. Hope it will be helpful for others too.

Best regards, Tomek

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Highlight
- Email to a Friend
- Report Inappropriate Content

11-22-2016 05:16 AM

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Highlight
- Email to a Friend
- Report Inappropriate Content

01-04-2017 10:19 AM

Good day to you. I have still some questions related to this thread and hopefully someone can help me.

In this thread figured out how to initially deform the mesh for Non-Linear solution by means of using Grid Point Forces from SOL105, but how in the easiest way can I get deformed mesh from Linear Buckling solution so I can use it in SOL106 as you wrote? I mean to get only the mesh that will not have any initial stress and will be just deformed ?

Is there some quick way of doing it in NX?

Thanks and wish you Happy New Year

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Highlight
- Email to a Friend
- Report Inappropriate Content

02-23-2017 09:42 PM - edited 02-23-2017 10:00 PM

First steputput the displacement results to .csv file with the Identify Results

Change to the FEM model , then choose nodal translate , change the Translation Method to By Field

In the Field , choose the .csv file you created in Step 1 and choose proper Scale factor and Click OK.

Then you get the deformed mesh.

Also the method you mentioned in another article is not proper for nonlinear buckling analysis as using nodal force , addational stresses are introduced.

For nonliear buckling , both SOL106 and SOL601 can be used and in both solver arc length method can be used to track the post buckling performance.

In the example manual , there is an example called "Lee Frame" shows the application of arc length method in SOL106.

Follow Siemens PLM Software

© 2017 Siemens Product Lifecycle Management Software Inc