Non-Linear Analysis on an imperfect structure 1

[ThomasH]

Hi
I am currently using non-linear analysis to find the load capacity on structures.

The workflow is as follows:

1. Linear buckling analysis (Nastran)

2. Use the buckling shape and scale it to create a deformed structure (preprocessor Femap).

3. Run a non-linear analysis to find the load capacity (Nastran).

My question is, could this be done directly in Nastran using subcases and different analysis types?

Kind regards

Thomas

 

[karachun]

For simple beam structures you may replace imperfections with distributed and concentrated loads. Then you need only one nonlinear solution.
Here is picture from Eurocode 3.

 

[ThomasH]

karachun

My problem is that I am not working with a simple beam structure. And I would like to do this inside Femap/Nastran within a single model.

Thomas

 

[klaus.]

It is a long time ago since I used Femap Nastran the last time ...but yes I think you can do that within the Program... but don't ask me how to do it ..

 

[BlasMolero]

Dear Thomas,
The way to proceed is what tells you Karachun: take note of the linear buckling shape and apply an small load that cause this type of deformation, and run the nonlinear analysis.
This is one fast way to account for geometric imperfections.

Please note the above is necessary only when you are studying a simply beam column, perfect in geometry, with a compression load only, not any lateral loading or lateral moment, but in real life with complex structures you will have loads in many directions, then the nonlinear analysis directly will give you the correct solution, OK?.
Best regards,
Blas.

~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director

IBERISA
48004 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/

 

[ThomasH]

Dear Blas,
I am currently working with a fairly complex structure and I need to implement imperfections into the analysis. If you look in Eurocode 1993-1-5, Annex C there is a description of the general approach. I use it regularly for steel.

To use loads as a way of creating the buckled shapes I need is probably more complex that the method I currently apply. I simply deform the mesh using a scale factor in Femap. But I would like to use the buckling shape as basis for a deformation directly inside Nastran.

I am sure it is possible, but I have not managed to figure it out yet . On the other hand, I have a working method so I have prioritized it either .

Thank you

Thomas

 

[BlasMolero]

Dear Thomas,
Take a look to the blog of my friend Lukasz from Poland, he is an expert in Nonlinear Analysis with FEMAP and Simcenter Nastran, and he explain how to apply imperfections and solve the buckling problem:
He say: "Using deformations from linear buckling as imperfections in nonlinear buckling case is the most common approach. I will use a simple example to prove that this is not always the best idea. Proper selection of imperfections is a very complicated process – I hope to shed some light on this matter."

https://enterfea.com/imperfections-in-buckling-design/

Best regards,
Blas.

~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director

IBERISA
48004 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/

 

[karachun]

The main problem - you need some API to automate this operations. The only way to move nodes to create imperfections (without any additional steps like additional loads) is to use Custom Tools-> PostProcessing->Node Move by Deform with option. This is possible only inside Femap GUI.

 

[ThomasH]

@BlasMolero and karachun,

Thak you för your interest. The problem I have is not with the imperfections specifically. I know that you may need to vary them but in this case the first buckling mode has proven to be a valid starting point.

The problem is that for each analysis I create a deformed mesh, run a nonlinear analysis and get results. And the model with the deformed mesh is then "dead". I don't se any way to get the undeformesd mesh back.

Instead I use a copy of undeformed model, create a new imperfection, nonlinear analysis, results and another "dead" model.

I have it more or less automatic but all the "dead" models annoy me. There must be a more elegant approach .

Thank you

Thomas

 

[karachun]

You may use Node Move by Deform with option and set negative scale factor to "unbend" mesh to previous state.
This still requires some discipline - always keep in mind what result you use to deform mesh and what is actual status of mesh (deformed or not).
I use this trick a couple of times when performing modal analysis with nonlinear pretension in SOL401 (problems like normal modes of fishing rod, with large displacements).

 

[ThomasH]

@karachun
My apologies for a very late reply. I did not believe in your suggestion with a negative scale factor, but now I have used it and it works fine.

Thank you.

Thomas

 

[dmapguru]

Take a look at MSC Nastran V2020; a new capability called "Geometric Imperfection" was added at version 2020 and does exactly what you asked.

DG