Correct way to perform nonlinear buckling analysis

[Facundo L. Pfeffer]

Hello, thanks in advance for your time.
I am trying to obtain the 'load multiplier' that will cause a structure to become unstable, using nonlinear buckling analysis with no geometrical imperfections.

I am using COMSOL software which to my knowledge does not possess this option, and I want to know if I am using the correct workaround:

- I first defined a 'load multiplier A' that applies to the stationary loads.
- I run a nonlinear static analysis using the amplified load.
- I run a linear buckling analysis on the deformed structure obtained in the previous step. Then I obtain 'load multiplier B' by solving the eigenvalue problem.
- Finally, the 'load multiplier' is obtained by multiplying 'load multiplier A' by 'load multiplier B'.

I do repeat these steps using different values of 'load multiplier A', until the final value converges.

Is my approach correct? Or am I missing some important theoretical concepts here?

Any input is much appreciated!

Extra context on how the program works can be found at

https://doc.comsol.com/6.1/doc/com.comsol.help.sme/sme_ug_modeling.05.157.html,

but the keynotes are:

The study in COMSOL is being done by first resolving and stationary step that considers geometric nonlinearity:

Then, this initial deformation is used in the formulation of the linear buckling analysis, and the eigenvalue problem solved is:

 

[FEA way]

COMSOL is definitely not a good software for that but if you don't have a choice... I would just use free and open-source CalculiX if I had no access to better software though.

Anyway, in COMSOL, as well as in other software, nonlinear buckling analyses are performed using regular static or dynamic procedures (not the eigenvalue/linearized buckling one) with geometrical nonlinearity enabled. The problem with COMSOL is that you normally can't trace the load increments. However, the parametric continuation solver should be able to help with this. Check the article "Buckling, When Structures Suddenly Collapse" on their blog for more details.

The above applies mostly to older COMSOL versions. If you have COMSOL 6.0 or above, there should be some significant improvements in this regard. They are described in the following blog article: "New Functionality for Buckling Analysis in COMSOL Multiphysics".

 

[Facundo L. Pfeffer]

Thank you for your reply.
Unfortunately, I need to keep using COMSOL since all previous work on this project is there and it would take quite some time to migrate.

Yes, the blogs you cited did help me understand the nature of the problem. However, they seem to focus on modeling imperfections or obtaining the force-displacement graph of a nonlinear problem, which is not exactly what I want to achieve.

From a theoretical viewpoint, do you think what I stated could work? Will the solution be mathematically accurate?

Again, thank you

 

[centondollar]

I am using COMSOL software which to my knowledge does not possess this option, and I want to know if I am using the correct workaround:

- I first defined a 'load multiplier A' that applies to the stationary loads.
- I run a nonlinear static analysis using the amplified load.
- I run a linear buckling analysis on the deformed structure obtained in the previous step. Then I obtain 'load multiplier B' by solving the eigenvalue problem.
- Finally, the 'load multiplier' is obtained by multiplying 'load multiplier A' by 'load multiplier B'.

As far as I know, Comsol can do non-linear buckling analysis, including snap-through (with displacement control) and even snap-back ever since they implemented a Rik's method solver. It's in one of the examples which can be found by googling.

The steps are straightforward:
1. Run a linear analysis (or a non-linear one, if the structure is e.g., a cable, which is always non-linear).
2. Run a linearized buckling analysis (eigenvalue problem, formulated with the second equation if the basic static solution involves geometrically non-linear effects).
3. Use a scaled buckling mode as an intial imperfection.
4. Run a non-linear analysis (geometry, material or boundary conditions).

The study in COMSOL is being done by first resolving and stationary step that considers geometric nonlinearity:

Incorrect. That equation describes the reference load case stiffness (K_L) and the geometric stiffness from reference load case (K_NL), which in a beam analysis would be the geometric stiffness (compression reduced bending stiffness and vice versa). The equation describes the linear buckling eigenvalue problem, which is then solved to yield multipliers of the normal forces / bending moments that cause eigenvalue buckling.

Example: you have a column with axial force P = 1 kN. Run the elastic analysis to get a normal force (P=1 kN in this case), then solve the eigenvalue problem to get "P*lambda", where lambda=eigenvalue. This calculation can be done by hand for simple columns.

 

[centondollar]

"Yes, the blogs you cited did help me understand the nature of the problem. However, they seem to focus on modeling imperfections or obtaining the force-displacement graph of a nonlinear problem, which is not exactly what I want to achieve."

I suggest you re-read the blogs. The result you want is precisely a force-displacement graph of a non-linear problem, considering only geometric non-linearity (and possibly including scaled imperfections) or geometric and material non-linearity, or geometric, material and boundary condition non-linearity.

If the loading is rapid or transient, you may also want to include inertia and damping, in which case you would also need to integrate the solution through time.

 

[Facundo L. Pfeffer]

Hello centondollar, thank you for your response.

This might be a limitation in my understanding, so please forgive me if my question is off track:

"The result you want is precisely a force-displacement graph of a non-linear problem."

I understand that such a graph can indicate the force value at which the structure becomes unstable. However, my structure is a 50-diameter API650 tank, and relying on the displacement of a single point or an integration of displacements might not accurately predict overall shell buckling.

My goal is to determine the load multiplier at which the structure will first buckle, considering geometric nonlinearity but assuming an initially perfect geometry. Essentially, I am looking for a single number that represents this critical load multiplier.

Thank you for your assistance.

 

[centondollar]

I understand that such a graph can indicate the force value at which the structure becomes unstable. However, my structure is a 50-diameter API650 tank, and relying on the displacement of a single point or an integration of displacements might not accurately predict overall shell buckling.

There exist simple formulas for cylindrical shell buckling with an appropriate knockdown factor. I suggest you compare that result to FEA. These formulas are probably referenced in API650. Simple formulas also exist for evaluating tank shell plate thickness for stresses due to hydrostatic pressure.

The force-displacement graph is just a simplified way of describing system-level instability. Instead of looking at a graph of force and displacement of a node, you would of course want to animate the whole structure at the end of each load step, and possibly extract force-displacement graphs from several nodes (say, 1 to 1000 or 10 000, depending on your needs) to find the failure point.

My goal is to determine the load multiplier at which the structure will first buckle, considering geometric nonlinearity but assuming an initially perfect geometry. Essentially, I am looking for a single number that represents this critical load multiplier.

A geometrically non-linear analysis will not give you an exact buckling load (material non-linearity and inertia of contents and the shell may be critical for liquid tank), but for the sake of argument, consider this:
1. There are several cases to investigate. For example:
- empty tank, wind
- empty tank, seismicity
- empty tank,
- full tank, wind
- full tank, seismicity
- tank with 1-99% liquid and wind or seismicity
- tank with 1-99% liquid and sloshing and wind or seismicity
etc.

For each case, you will receive a different buckling factor (either from an eigenvalue analysis or from a non-linear analysis), and the smallest one is the critical one. Consider also that seismicity and sloshing require consideration of the inertia of the tank and liquid. Consider also that failure to converge does not necessarily indicate failure - it can also mean that the solver cannot handle snap-through or snap-back.

I suggest you reach out to a colleague who is familiar with design of tanks in your region of the world.