Buckling non lineare

[guido84]

Bye to all,

My problem is as follows:
I have a model for which I need to do a buckling analysis. the model has gaps, so I thought I'd make a buckling with a sol 106 inserting the param buck=2
the problem is that by doing test runs on a simple structure (a plate loaded with a pressure and stuck on the whole contour), I expected to get with the sol 106 and with the 105 the same results, but so it was not. is it right to have different solutions (although in fact the model is linear)?
in the run with the sol 106 two subcases, like in the sol 105? I limited myself to adding the param buck=2

Thank you.

 

[Onda]

Hi.
First of all I recommend you to do a test with a framed / hinged rod, so you can calculate the analytical solution easily and carry out a verification.
Secondly, with the sol105 calculates the eulero load while with the sol 106 without param buckle, you should get to the load beyond which you no longer have convergence. That is the load of non-linear buckling.
if you activate the param buckle, do a buckling analysis of the structure deformed by the non-linear, which is still a different thing.
serves when the structure has non-linear behaviors (geometries or materials) and therefore the linear deformity is shaken by the non-linear deformity.
If I understand your problem, I suggest you do a sol 106 with a load large enough not to be straight from the structure. the last load value to which the solutor has reached convergence is the nonlinear load value.
you can activate the arc length method that changes the load increase value according to the solution convergence.
consult the qrg because I don't remember how to do it.
the load value found is often lower than the load of the sol 105 which is theoretical.
Anyway, do some evidence with a tip-loaded beam.
Keep in mind that the sol 106 needs a small destabilizing load (typically a 90° load in the middle of the auction) to develop instability.
wave

 

[guido84]

thanks to the delucidazione,
In fact the area for which I am interested in calculating the buckling is constituted by a plate subject to pressurization, hence the choice to use as a test a pressurized plate.

By activating the param bukle I get a greater self-value than that obtained with the sol 105, this, if I understand how much you wrote me, is precisely because by activating this param I go to consider the membrane behavior of the quads.
A question arises at this point: if I activate param lgdisp what would I get?

guide

 

[Onda]

I don't know your problem, but so feeling, if it's under pressure, a plate, working as you say like a membrane, it doesn't go in buckling.
How is the deformed of the 105 self-value? Does that make sense?
are there other structures (costoles etc) going in buckling?
or are there pressurization loads and compression loads together?
because if you do not have compression or shear it is difficult for you to have buckling

 

[guido84]

the structure and the applied load are quite complex, from the sol 105 of the whole structure was to go in buckling the plate on which I then began to make some radiance.

deformed both of 105 and 106 are "clean"

the sol 105 of the plate isolated from a value of 1.7, while the one obtained with 106 and param buck is equal to 19.

by comparing the level of stress obtained with the 101 and the one obtained with a 106 lgdisp I have with the latter a reduction of the stress of about 2/3; so I am led to think that membrane behavior is fundamental.

I apologize if I insist, but doing a sol 106 with param buck and param lgdisp what I would get

 

[Onda]

you have to do 106 with the load up to 1 (total load value). with lgdisp you upgrade the matrix of stiffness with the new position of the knots, also enable the follower force. from my point of view when I use 106 I always use lgdisp. Surely if you have a membrane behavior and great deformations it is better than you skill it.
Of course the difference seems very high!

 

[f.pelizza]

hi drive 84,
if you have entered
param,buckle,2 and
method
where x is the id of the eigb call (or eigrl) goes well and you don't need anything else. the reason you find self-value =19 is because the self-value refers to the last load increase. to make an example if you have divided the load into 20 increments (in nl mean), with autovalue 19 you have the following:
buckling load = 1+ (1/20*19)=1.95.

second thing. never use arc length unless you're looking for post buckling phenomena, but I don't think it's your case.

I hope I've helped you.
france

 

[alessandro pani]

Good morning,
I add to the discussion.
My model is a simple point-loaded notebook with a small transversal instabilizing force (I also tried different strategies such as the introduction of a geometric imperfection).
I created two loadcases of which one static nonlinear sol106 normal, the other with buckling .
the point load value is lower than the critical load.
If I don't impose any bounds, I always get the error:

*** system fatal message 3034 (lnnherr)
     internal failure in the lanczos procedure:
     m-orthogonal qr procedure failed to converge.  probable cause:
     mass matrix is indefinite (modes) or stiffness matrix is indefinite (buckling).
     user action: contact msc client support

otherwise if imposed as lower bound -1 (as they advised somewhere)
I get:

*** user warning message 6636 (lnnrigl)
      no modes exist in the interval specified (-1.5915494e-01 to  1.5915494e+18 hz).
1    msc.nastran job created on 29-may-14 at 10:15:14   **student edition*      may  29, 2014  msc.nastran  7/ 6/12   page    42
                                                                                                                                    
0                                                                                                                                   
0                                                                                                                                   
                                                                                                                                    
                                                                                                                                    
 *** user fatal message 4405 (prtprn)
     no eigenvectors computed for component mode synthesis or system solution.

If instead I try to overcome the critical load, clearly I can get the data from the increase of load, but in this case the solution ends without lanzos leaving.
I know I'm probably getting a little confused, could you roam me?
Thank you very much!:finger: