buckling - post process

[minny]

Hy
I must check if a structure under applied load goes in buckling with f.e.a. nastran.
I did a long time back, so I need help to remember the right way to post-process the results.
The f.e.m. is very complex, I have the complete wing.
The major problem that I have is to understand in the case that I have an eigenvalue minor than 1, which part of the structure is in buckling, if I remeber well I did two thinks:
1) look at the deformed shape
2) I seached the node that had the eigenvector equal to 1.00 (if it's true what I need to write as output request? what I need to plot in Patran: eigenvector magnitude or component?)

please, help me

 

[rb1957]

print the f06 file (output to postprocess and print)

then you should be able to see the element(s) < 1.

you applied limit load or ultimate ?

 

[ESPcomposites]

A few comments:

- you always want to look at the deformed shape to make sure it is a real, meaningful mode.

- you seem to be confusing an eigenvalue with an eigenvector. An eigenvalue of 1.0 would indicate the applied load is the buckling load.

- the magnitude of the eigenvector is meaningless. It's value is that it provides the deformation of the part with respect to itself. Therefore, you can determine if the shape is as expected and that boundary conditions are proper, etc.

If you can improve your post with this in mind, it will ne easier to provide further help.

Brian

http://www.espcomposites.com

 

[minny]

An eigenvalue of 1.0 indicates the applied load is the buckling load. It's absolutely true.

I have in output numerour eigenvalue minor than 1 (numerous mode).
In mine complex structure, for a single mode, I have in output numerous wave in different locations. I need to select the wave of a really buckled part.

I'll use the F06 to see the NODE with eigenvector translational equal to 1, but what do I have to type as output request in Nastaran input file? which of the eigenvector componet X,Y and Z has to be equal to one?
Does the Patran show that eigenvector component?

help me to find the right way to select the buckled part of mine complex structure.

thanks

 

[ESPcomposites]

Minny,

Oh, I see. Your original post does make sense I think, provided NASTRAN normalizes the eigenvector such that the max displaced magnitude is 1.0. I suppose this statement tripped me up a bit:

"2) I seached the node that had the eigenvector equal to 1.00 (if it's true what I need to write as output request? what I need to plot in Patran: eigenvector magnitude or component?)"

The eigenvector is a collection of values for all nodes. The maximum value within the set would indicate the location of max displacement, and probably your area of interest.

I am not sure how NASTRAN normalizes the eigenvector, but why not just plot the magnitude and components and see which gives you 1.0? I would assume it normalizes it by magnitude. Normalizing it by a component would seem arbitrary (I suppose the counter to that is the eigenvector is arbitrary anyhow).


Brian

http://www.espcomposites.com

 

[rb1957]

isn't the eigenvalue the reserve factor for buckling ? ie apply 1000 lbs compression on a column, get eigenvalue = 4. critical load for the column is 4000 lbs. yes? no?

i though nastran would calculate the lowest eigenvalue and print the stresses and deflections for that mode. i think the node with deflection = 1 is the critical area.

i think ESP is right in saying look at the mode, 'cause it might not be particularly "real". it is an elastic solution, and it might be reporting what might be localised plasticity as a hard failure. if there are loadpaths around the plasticity there the structure should hold together, if there aren't then it'll probably collapse.

 

[ESPcomposites]

rb1957,

"ie apply 1000 lbs compression on a column, get eigenvalue = 4. critical load for the column is 4000 lbs. yes? no?"

yes, the buckling load is the eigenvalue x applied load.

"i though nastran would calculate the lowest eigenvalue and print the stresses and deflections for that mode. i think the node with deflection = 1 is the critical area."

NASTRAN will give you as many modes as you request. The first mode may not necessarily be the mode of interest though. That is why is it common to request several modes and manually identify the proper mode via inspection. As far as stresses go, they would be meaningless. The deflections are only meaningful in their relationship to the other nodes. The magnitude is is just a normalized value with no particular meaning.

"i think ESP is right in saying look at the mode, 'cause it might not be particularly "real". it is an elastic solution, and it might be reporting what might be localised plasticity as a hard failure. if there are loadpaths around the plasticity there the structure should hold together, if there aren't then it'll probably collapse."

A few reasons to survey the deflection:

- There may be rigid body modes, depending on the constraints.

- Determine if the mode is local (panel) or global buckling.

- To check that the deformation is as expected and the boundary conditions are correct.

- I remember having problems with certain higher order elements and the displacements were clearly erroneous. That may have been fixed, but the point being that finite elements are not perfect either and neither are their element formulations.

- Certain model "fictitious" entities can create undesired modes. For example, I may use soft springs to help balance models or other connections, etc. They can have associated modes that are not relevant to elastic buckling.

Brian

http://www.espcomposites.com

 

[Burckan]

If you have Eigen Value in Negative, Buckling will occur, if you reverse the Loading Direction.