Learning Forum

[Ana Pereira]

Hi,

I have noticed that depending on the input for the Max modes to find in the eigenvalue buckling analysis setting, the results vary. Why is this the case?

Also, I have tried accessing the help link mentioned in this other post: How ANSYS translates the eigenmodes to displacement or stress values? When one change the unit system (say from m to mm) for the modal analysis, the displacement values change to a value that's unrelated between the two unit-systems. - Ansys Knowledge but was not able to access any of the information.

 

Thanks in advance!

[peteroznewman]

Hi Ana,

Please reply with your specific example, what inputs did you use for Max modes, what results were returned and how did the results change with different inputs.

I don’t see any help link in the other post, but that post is for Modal and not for Buckling.

[Ana Pereira]

 

Hi,

Thanks for the reply!

I am doing a structural analysis of a stiffened panel, you can see the main details in this screenshot:

The bottom right shot is for the 5th eigenmode, although, the first eigenmode for such analysis can be found on the following figure:

The result above was shown when I selected “5” as the Max modes to find. Although, when I change this input to the value 1, these are the results I get:

So -8.6327e-04 is quite different from -1.2934e-05. What might be the reason?

In addition, I understand that the buckling results are load multipliers and therefore must be multiplied by the applied load. Following this logic, and after having seen the Ansys Tutorial about eigenvalue buckling, I don’t undertsand how the buckling patterns change depending on the magnitude of the applied load, since this analysis is described as being “load independent”. In the figure below, we can see the tremendous change in buckling behaviour between applying a line pressure of 5000 N/mm and 7500 N/mm.

Any guidance you might offer for any of these cases? I’m sorry in advance for such a long response but these are doubts about my master’s thesis that I haven’t been able to get any help with.

Thank you so much for your help!

 

 

[peteroznewman]

Hi Ana,

When the Load Multiplier is 1e-4, multiply the load by 1e-4 then rerun the analysis, you will get a more accurate estimate of the critical buckling load when the Load Multiplier is closer to 1.0

You have a panel with many flat rectangular membranes surrounded by ribs. Small loads buckle those membranes out of plane. Since there are hundreds of membranes, there are hundreds of closely spaced buckling modes. This is a local buckling mode. You may be more interested in a global buckling of the entire panel. For that, you will need to find a buckling mode that is much higher than those local buckling modes.

Is there a pressure load on the face of the panel? If so, a nonlinear Static Structural analysis (large deflection On) run upstream of the Eigenvalue Buckling would cause the membranes to be deflected slightly out of plane by the face pressure. Then the buckling caused by the line pressure on the top edge may generate higher Load Multipliers so you can more easily find the global panel buckling mode.

 

[Ana Pereira]

Thanks for all the suggestions!