Hello to everybody,
First I will explain my problems I think that is much easier than to write question immediately to you
In attachments you can see the six pictures.
Model is plate thickness=8mm, high=1500mm, width=25000mm. There is one horizontal rib to make stiffer main plate according to buckling. Vertical ribS I omitted and change it with constrains in Tx direction in the middle of plate and on edge with dependent nodes of RBE2.Also I put constrains in nodes and I have simply girder SEE Picture 3
I analysed only 3000 mm in the middle of the span the rest of plate I put as rigid virtual body RBE2 elements SEE Picture 2
The upper zone (area) is subjected (expose) to pressure stress.In the lower zone (area) bellow of neutral line we have tensile stress.
Everybody will agree that we will have buckling only in zone where is pressure stress.We expect that buckling will happened in upper zone
The force are on distance of 1600mm .Every force is 30000N.
On Picture 6 buckling occur (appear) in lower zone where we have tensile. And Eiginvalue factor is negative -0.23 buckling will happened
Always when I got negative Eigenvalues I got buckling in opposite area where I do not expect buckling
IN CATIA SOFTWARE ALSO HAPPENED THIS than I change direction of force and I got buckling where I expect
FINALLY QUESTION: HOW TO CHANGE BUCKLING AREA APROPOS THAT NASTRAN SHOW IN AREA WHERE IS NORMAL TO OCCUR. WHY NASTRAN AND OTHER PROGRAMS DO THAT
THANK YOU IN ADVANCE
Negative eigenvalues mean that buckling is possible with a reversed load. If a reversed load is not physically possible, or is not of interest, then the only change required is to set the range of eigenvalues to search for. Instead of just asking for just 1 or more eigenvalues, set the lower limit to 0.001 and Nastran will not search for any negative eigenvalues. The settings below will return the lowest 5 eigenvalues above 0.001(all positive)
Hello Mark I send the picture of succsseful finish the calculation.
The buckling happened in upper area where is expect to be.
I have only one more question. Eigenvalue factor is critical force / force
In this case Force which subjected the plate is to much bigger of critical buckling force why is Top Von Meases Stress are 54 N/mm2 Buckling will happened
I edit thickness from 8mm to 10 mm and put lower forse Than buckling is escape. Total deformation is 1 Can you explain me why Nastran can not give the real deformation
How to explain that values
Buckling analisys is like eigenvalue analisys - you have buckling factor and shape of buckling, but translations, stresses and other resauts scaled by some factor and you can not use it. They are meaningless, but they represetnt deformed shape. If you want to see stresses - make nonlinear analisys.
A linear buckling analysis in Nastran consists of 2 subcases. The first subcase is just a linear static analysis using the load you specified. The results of this case are correct for this static loading and can be used.
The second subcase is the buckling case and is an eigenvalue extraction using the differential stiffness based on the static loading of the first subcase. In general the only useful results from this case are the deformed shapes(buckling mode shapes) and the actual eigenvalues. Any stress or other results are created from the deformations of these buckling modes and therefore not usually meaningful.
One important check to make from a linear buckling analysis like this, if you multiply the eigenvalue by the maximum stress in the first subcase, you must still be below the yield stress of the material, otherwise you have violated the basic assumption of linear buckling analysis.
For more details on linear buckling analysis in Nastran, see the Nastran User's Guide which you can find under Femap/Help/Nastran