Explanation of Buckling

Question

Hello,
Someone he already made simulations of buckling.
Because I do not understand the result in buckling of a rod with several ( BLF) bending load factor , I still get
the same scale of displacement, with a maximum displacement of 1 [mm] .
I made several simulations of various shapes and load and I have always the same result, a displacement of 1 [mm] .

To view the buckling, we have to go through a static simulation model with all the stress conditions and charges
before proceeding to the simulation of buckling which includes the previous results of the static simulation.
Where I think the actual load must be important.

In the knowledge base PTC it is written :
For the stresses and displacements of the structure at the critical buckling load , the greater the BLF must be multiplied
by the initial compression load used in the static analysis . The initial load shall be changed
this value and static analysis restarted. Pro / SIMULATE not calculate the stresses due to buckling ,
because it is the field of nonlinear large deformation calculations .

If you have an idea , it will be welcome or a sample file .
Cordially.
Denis .

This thread is inactive and closed by the PTC Community Management Team. If you would like to provide a reply and re-open this thread, please notify the moderator and reference the thread. You may also use "Start a topic" button to ask a new question. Please be sure to include what version of the PTC product you are using so another community member knowledgeable about your version may be able to assist.

sdensberger · Answer

As Charles pointed out, the buckling analysis in Creo Simulate (Pro/Mechanica) is solving an eigenvalue problem (same as a modal analysis), where your eigenvalues are the Buckling Load Factors (the factor of the applied load "needed" to cause buckling) and the eigenvectors are the buckling mode shape. For an eigenvalue problem, Mechanica will always normalize the results (i.e. the largest "displacement" is 1).

Now, all that being said, it's very important to keep in mind that last sentence from the knowledge base: "Pro / SIMULATE not calculate the stresses due to buckling, because it is the field of nonlinear large deformation calculations."

The analysis you're doing is sometimes called a linear bucking analysis, because the solution is a linear perturbation of the intial change in the structures stiffness due to the base static analysis. There are two very important points about a linear buckling analysis that must be kept in mind:

There is a unknown amount of error between the linear and non-linear buckling solution.
The linear buckling solution is unconservative (i.e. the calculated buckling load is higher than the true buckling load).

The implication of these two points (particularly the last one) means that you need to be very careful how you use the results from a linear buckling analysis. Realistically, a linear buckling analysis should only be used for preliminary comparisons (what type of buckling mode could exist, and how design changes effect the trend of the BLF). If the results are used for anything else, then a high factor of safety is needed. More accurate results can be obtained by running a non-linear analysis with large-displacement formulation and a non-linear material property. If you do this, be sure to include some eccentricity in your model (whether load or geometric).

Sign up

Please use your PTC eSupport account.

Welcome to the PTC Community

Please use your PTC eSupport account.

Scanning file for viruses.

This file cannot be downloaded