Interpretation of results (buckling analysis) 1

[jeram123]

Hi,
I have tried to perform a buckling analysis for a simple hollow box (1000*450*300mm)using PATRAN. One end of the box is fixed and other end is loaded giving a transverse load 0f 900 kg (450 each at the ends of top and bottom panel)from down side. I got a value nearer to .06 through eigen value analysis.The buckling mode runs upto a length of 600mm and stops.
How can i verify the credibility of my FEA results.Please help me to sort out this problem.

 

[rb1957]

shear buckling of the flat faces ?

 

[jeram123]

The load is applied in such a way that the hollow box's top panel will go for compression and bottom panel will be in tension.. the top panel is displaying buckling deformation nearly half of the whole span.. The load causing buckling is compressive only...

 

[SWComposites]

compression causes bucking ....yep.... what is the issue/question?

have you calculated by hand the stress in the top panel and calculated the buckling stress using a closed form classical plate buckling equation?

can you post a picture of your part, loading and buckle pattern?

 

[jeram123]

Thank you for your immediate response. A picture of my problem is attached with this post.

My question is how to perform hand calculation for this.

 

[rb1957]

the top panel is in compression, it looks like your load is up.

the sides are shearing load into the top panel, so that the compression is increasing as you get closer to the support.

you can see how the panel is buckling, more than one crest = more than 1 mode.

From this result, i'd consider the top panel as a simple panel in compression, the wide is dfined (yes?), the length would be the length to the undeformed panel between the crest and the trough (yes?), constant compression = the stress at teh crest position (figuring that this is 1/2 the length of the assumed panel), simply supported on 4 sides, = text book solution.

 

[jeram123]

Thanks a lot rb1957.....

I am getting you. But if you have time,please help me to clear the following doubts

1. When one end of the box is fixed how come you can take 4 end simply supported condition?

2.How can i calculate the compression load that should be used for text book formulas.

3.which length i should consider for the panel calculations? the length through out which buckling deformation is found or just the length of first two modes?

 

[rb1957]

1) if the suppor end is turly fixed, assume 3 sides SS, one loaded side fxd (a not so quite standard problem). assuming loaded end SS would be slightly conservative.

2) once you determine the length of the panel (the length of the frist buckle), then use the stress at the mid-length position (ie 1/2 a buckle from the end) ... yes?

3) the panel is buckling up then down. somewhere between it isn't displacing out of plane. this'll define the length ... yes?

you could investigate how an eigenvalue solution (depending on your FE code) will help you determine an allowable load.

 

[jeram123]

thanks rb1957. but i want to know whether validation of my model through SOM approach is possible or not?
For that how can i find out the load?

 

[jeram123]

Hi friends,
I have a new topic to discuss with those who are interested in buckling analysis.
ie. will the eigen factor ever becomes negative?

( I did the hollow box problem which i described above keeping an uniform thickness everywhere. PATRAN shows a buckling at tension side. why it is happening?)

Please refer the pic posted with this.

 

[jeram123]

The load application is same as that in the the pic posted first in this thread.

 

[Taz99]

A negative Eigenvalue indicates that the direction the the load is applied has to be reversed for this buckling mode to occur.
From what I see in you model you should expect the next mode to be approximately the same magnitude but have a positive value and occur on the opposite face.

If you only what to see positive Eigenvalues you need to modify the EIGRL entry in your .bdf file. for example
EIGRL 10 0.001 15
Where 10 = the value of your METHOD card (look a few lines above) i.e METHOD=10
0.001 is the lowest eigenvalue that will be reported
15 is the largest eignevalue that is reported.
Check the EIGRL in the nastran quick reference quide for more information.

 

[rb1957]

if your constraint is fully fixed, then the reactions will include moments, the panel will be bending at the support, there'll be moment in the panels, there'll be out-of-plane deflections; try running with XYZ constraints only.

-ve eigen values interpreted above.

"SOM methods" ?

 

[jeram123]

thanks rb1957 & Taz for spending your valuable time here.

I will try the problem with your suggestions and let you know the result.

@ rb1957, By using the term 'SOM',i mean Strength of materials related calculations/the simple 4 side boundary condition buckling calculations

 

[rb1957]

that's what i was describing (i thought) a flat rectangular panel uner constant compression, with "simple" boundary conditions (4 sides SS or 3 SS/1 Fxd)

 

[jeram123]

hi friends,
thanking you a lot for your useful suggestions.
Patran is giving negative eigen factor just because of it's coding only(FEA engineer has nothing to do with that).
Never mind for the sign,just see for the deformation followed by the structure.

I would like to know your opinion about post buckling analysis with nastran. will it give fine results?

Can anyone give some idea about Post buckling analysis in PATRAN 'n' NASTRAN?

 

[rb1957]

don't know i'd say "never mind the sign" ... the indicates the direction of the critical load.

the question in my mind is "why -ve ?" ... you have a simple looking box beam with one face loaded in tension and the other in compression. why is the +ve not as critical as the -ve loading ? assuming the faces are the same thickness, they should be the same criticality ??

 

[jeram123]

Even i dont have much idea.... but i feel like the length to width ratio is having some role on making the eigen factor negative.

 

[Taz99]

Jeram you should get matching positive and negative eigenvalues when the model and loading has a plane of symmetry, as your model does.
I would guess that the negative eigenvalue is slightly more critical than the positive one and that is why it is listed as the first eigenvalue.

Your statement "the length to width ratio is having some role on making the eigen factor negative" - is incorrect, this is not what is happening please understand that a negative eigenvalue mean that the direction of the applied load must be reversed for this buckling mode to occur in reality.

 

[jeram123]

yea...you are right. But still more clarity is needed. I think i should work more to see what is the real reason. May be some highly experienced people from industries can help to connect the result with the practical case