Hello, I´m performing dynamic buckling analysis in a composite shell. I´m using Nastran SOL129, but I´m facing some difficulties in the analysis. I have enabled large displacements in order to appreciate the buckling. I get perfectly the buckling shape, so it works pretty well in that way, but I´m not able to recover ply stresses or failure indices. Time ago I heard that was not possible to recover these stresses in a non linear transient analysis of composites. Bearing this in mind, I have used the PSHELL+MAT2 equivalent anisotropic elements in order to get the stress tensor of these elements (just for have some information of stresses). As I supposed, displacements are exactly the same than using PCOMP+MAT8, but I´m neither able of recovering the stress tensor.

Therefor it seems that in a nonlinear transient analysis of a model built in anisotropic elements you are not able to recover any kind of stresses. I´ve been trying to solve this issue several days and I´m becoming crazy. I´ve read almost all commands in the Quick Reference Guide, and I´ve done a lot of test without positive results.

So I´m looking to a solution (some command or parameter that I can have overlooked) or someone that tells me that this simply not possible. If it´s not possible, I would also like to know where can I find that issue in order to refer it in my report.

Thank you very much

I forgot to mention that I´m using MSC Nastran 2012

Here are my suggestions

1) Contact mscnastran.support@mscsoftware.com for direct support.
2) Switch to SOL 400, if you have it. Here is a tutorial on how to do exactly what you want with SOL 400.
http://www.scribd.com/doc/95800391/Ws-04-Buckling

You can run a second linear analysis with imposed displacement by first analysis. Remember to live almost one grid point with no imposed displacement to leave something to solve to nastran.
Ask on the linear analysis the stress or directly the ply by ply stress and strain. The model shall be exactly the same, with same stiffness on elements.
The mean is just to overcome the problem of stress recovery.
regards
Onda

Hi, first at all, thank you very much for your answers. I´ve been quite bussy these days, so I haven´t been able to answer you.

@ZeroExperience: Maybe I´ll have a answer from MSC support, I´m trying to get in contact with them. I´ve been told that SOL400 should work, but I haven´t been able of getting results.

@Onda: Thank you very much for your proposal, but it would be quite hard to perform your solution. The model has several thousand of grid points, and there are hundreds of time steps, so apply all displacements seems pretty hard (correct me if I´m wrong, please).

Anyway, if someone knows that this simply can´t be done, please, tell me.

Thanks!

Hi Databor,
for sure, run a linear for each time step will be impossible. but you can run for the last or for few time step of interest.
The fact that you have many grid points isn't an issue. Using patran you can create a new load case with the deformation from a previous analysis. So is just some minutes of work.
just create spatial FEM field discrete (vector) when displaying translational displacement. and another field when displaying rotational displacement (remember to load rotational grid point results!).
use the two field to create a nodal displacement load.
Remember to do not constrain all grid points as the analysis will not run. So live almost one grid point free.
Onda

Hi, first at all, thank you very much for your answers. I´ve been quite bussy these days, so I haven´t been able to answer you.

@ZeroExperience: Maybe I´ll have a answer from MSC support, I´m trying to get in contact with them. I´ve been told that SOL400 should work, but I haven´t been able of getting results.

@Onda: Thank you very much for your proposal, but it would be quite hard to perform your solution. The model has several thousand of grid points, and there are hundreds of time steps, so apply all displacements seems pretty hard (correct me if I´m wrong, please).

Anyway, if someone knows that this simply can´t be done, please, tell me.

Thanks!

Hi Onda, sorry for the repeated post, I have sent it twice.

Well, as you said it doesn´t seem so hard, I will try it and I will tell you how it goes. Anyway I don´t know if my superior will accept it as stresses are taken from a linear analysis. I really have no too many options.

I have used another solution, SOL600. Well, this is whole differente world man. It´s a Marc solution, and at least I´ve been able of recovering strains in a transient analysis. But in my model I have to apply several time dependant loads using several TABLEDi, and the internal Marc translator it´s not able to handle more than one TABLEDi, so it simply use the first one and ignore the rest of TABLEDi.

Any idea about this other problem?


PS: If I must made a new post with the SOL600 problem, please, tell me. Thanks!

If nonlinearity are geometrical and not material dependent I don't see the problem to recover stress from a linear analysis. the fact is that you recover stress from a deformed shape, until hooke's law is valid your recover stress is correct. You run a non linear analysis to obtain the correct deformed shape. once you have it, you can impose the displacement to a model and recover stress obtained by the displacement imposed.
Cannot help on sol 600. sorry.
regards

Hi Onda, I´ve been a trying to create the displacements vector but I´m not able to do it. I follow all steps in Patran. I attach the results file, I make a quick plot of displacements translational, I go to Fields and select:

Action: Create
Object: Spatial
Method: FEM
FEM Field Definition: Discrete
Feld Type: Vector
Entity Type: Node
Input Data: => I select all nodes of the model, and a column of nodes is created, but there is nothing in the values column.

What I´m doing wrong?

Thanks!

Sorry, a couple of imprecision on my previous post.
The field shall be continuous not discrete. And to make a vector field you shall display a marker vector, not a fringe, good for a scalar field.
in this way is very easy to make the field and use it for input in a displacement.
regards
onda